T-42 T-51 T-65 Multi-Tasking CNC Lathes

Transcription

1 PROGRAMMER S MANUAL TP7878B T-42 T-51 T-65 Multi-Tasking CNC Lathes Equipped with a Fanuc 31i-T Control Revised: March 20, 2015 Original Instructions Manual No. M-504A Litho in U.S.A. Part No. M A February, 2012

2 - NOTE - Damage resulting from misuse, negligence, or accident is not covered by the Hardinge Machine Warranty. Information in this manual is subject to change without notice. This manual covers the programming of Hardinge T-42, T-51, and T-65 Multi-Tasking CNC lathes equipped with a Fanuc 31i-T control. In no event will Hardinge Inc. be responsible for indirect or consequential damage resulting from the use or application of the information in this manual. Reproduction of this manual in whole or in part, without written permission of Hardinge Inc., is prohibited. CONVENTIONS USED IN MANUALS DANGER DANGER indicates a hazardous situation that, if not avoided, will result in death or serious injury. WARNING WARNING indicates a hazardous situation that, if not avoided, could result in death or serious injury. CAUTION CAUTION indicates a hazardous situation that, if not avoided, could result in minor or moderate injury. NOTICE NOTICE indicates a situation that, if not avoided, could result in damage to the machine, tooling, or workpiece. - NOTES - Notes contain supplemental information. 2012, Hardinge Inc. M-504A

3 Table of Contents Offices xvii Machine Description and Intended Use xviii Machine Electrical Operating Range xviii General Warnings and Cautions xix Safety Recommendations xxi CHAPTER 1 - PART PROGRAM LANGUAGE Introduction Programming the Control Data Word Formats and Minimum / Maximum Values T-42 Lathes T-51 and T-65 Lathes Axis Definitions Special Programming Characters Programming Format Programming Sequence Off-Line Programming Sequence Keyboard Programming Sequence Program Number Decimal Point Programming Data Word Descriptions O Word N Word G Word G00 Positioning G01 Linear Interpolation G02 Clockwise Arc G03 Counter-Clockwise Arc G04 Dwell G10 Offset Value Setting G17 Work Plane Selection G18 Work Plane Selection G19 Work Plane Selection G20 Inch Data Input G21 Metric Data Input G22 Stored Stroke Limit Check ON G23 Stored Stroke Limit Check OFF G28 Return to Reference Position G31 Skip Function G32 Threadcutting (Constant Lead) G34 Variable Lead Threadcutting G40 Cancel Tool Nose Radius Compensation G41 Tool Nose Radius Compensation - Workpiece Right of Tool G42 Tool Nose Radius Compensation - Workpiece Left of Tool G50 Maximum RPM Limit G65 Macro Call G70 Automatic Finishing Cycle G71 Automatic Turning Cycle G72 Automatic Facing Cycle M-504A i

4 G73 Automatic Pattern Repeat Cycle G74 Automatic Drilling Cycle (Constant Depth Increments) G75 Automatic Grooving Cycle G76 Automatic Threading Cycle G80 Cancel Machining Cycle G83 Z Axis Drilling Cycle G84 Right-Hand Z Axis Tapping Cycle G85 Z Axis Boring Cycle G87 X Axis Drilling Cycle G88 Right-Hand X Axis Tapping Cycle G89 X Axis Boring Cycle G90 Canned Turning Cycle G92 Canned Threading Cycle G94 Canned Facing Cycle G96 Constant Surface Speed G97 Direct RPM Programming (Constant Surface Speed Cancel) G98 Inches / Millimeter per Minute Feedrate G99 Inches / Millimeter per Revolution Feedrate G107 Cylindrical Interpolation G112 Polar Interpolation G113 Cancel Polar Interpolation X Word U Word Z Word W Word Y Word [Option] V Word [Option] E Word A Word [Option] B Word C Word H Word I Word J Word K Word Circular Interpolation (G02 / G03) Variable Lead Threading (G34) R Word Linear Interpolation (G01) Circular Interpolation (G02 / G03) Tool Nose Radius Compensation (G41 / G42) Defining Tapers P Word Machining Cycles Subprogram Calling Tool Offsets and Work Shift Spindle Selection Q Word F Word S Word T Word ii M-504A

5 M Word M00 Program Stop M01 Optional Stop M03 Main Spindle Forward M04 Main Spindle Reverse M05 Main Spindle Stop / Coolant OFF M07 Sub-Spindle Phase Synchronization with Main Spindle [Option] M08 Coolant ON M09 Coolant OFF M10 High Pressure Coolant ON [Option] M11 High Pressure Coolant OFF [Option] M12 Turret Coolant OFF [Option] M13 Main Spindle Forward / Coolant ON M14 Main Spindle Reverse / Coolant ON M15 Thru-Spindle Coolant ON, Main Spindle [Option] M16 Thru-Spindle Coolant OFF, Main Spindle [Option] M20 Speed Arrival Check ON M21 Main Spindle Collet / Chuck Open M22 Main Spindle Collet / Chuck Close M23 Main Spindle Contouring Mode ON M24 Main Spindle Contouring Mode OFF M25 Main Spindle Part Catcher Retract [Option] M26 Main Spindle Part Catcher Extend [Option] M27 Main Spindle Internal Chucking Mode M28 Main Spindle External Chucking Mode M29 Rigid Tapping Mode M30 End of Program, Auto Door Open M32 Spindle Synchronization [Option] M33 Sub-Spindle Forward [Option] M34 Sub-Spindle Reverse [Option] M35 Sub-Spindle Stop [Option] M36 Air Blast ON [Option] M37 Air Blast OFF [Option] M38 Auto Door Open [Option] M42 No Corner Rounding - Exact Stop M43 Corner Rounding M44 Enable Turret Bi-Directional Index M45 Disable Turret Bi-Directional Index M46 Sub-Spindle Air Blast ON [Option] M47 Sub-Spindle Air Blast OFF [Option] M48 Enable Feedrate and Spindle Override M49 Disable Feedrate and Spindle Override M51 Live Tool Rotational Direction Command [Option] M52 Live Tool Rotational Direction Command [Option] M53 Live Tool Rotational Direction Command / Coolant ON [Option] M54 Live Tool Rotational Direction Command / Coolant ON [Option] M55 Live Tool Stop / Coolant OFF [Option] M56 Sub-Spindle Collet / Chuck Open [Option] M57 Sub-Spindle Collet / Chuck Close [Option] M58 Feed Bar Stock [Option] M59 Cancel Feed Bar Stock [Option] M60 Speed Arrival Check OFF M-504A iii

6 M61 Bar Change [Option] M62 Activate C Axis Spindle Synchronization [Option] M63 Cancel C Axis Spindle Synchronization [Option] M64 Spindle Feedback from Main Spindle M65 Spindle Feedback from Sub-Spindle [Option] M66 Spindle Feedback from Live Tooling [Option] M68 Sub-Spindle External Chucking Mode [Option] M69 Sub-Spindle Internal Chucking Mode [Option] M70 Orient Commands to Sub-Spindle [Option] M71 Orient Commands to Main Spindle [Option] M72 Chamfer OFF M73 Chamfer ON M76 Sub-Spindle Drive OFF [Option] M77 Sub-Spindle Drive Low Torque [Option] M78 Sub-Spindle Drive Normal Torque [Option] M80 Check Part Missing [Option] M81 Check Part Present [Option] M82 E Axis Torque Control Mode ON (Tailstock Programming) M83 E Axis Position Control Mode ON (Tailstock Programming) M87 Tailstock Brake ON M88 Tailstock Brake OFF M90 Part Probe ON M97 Part Counter M98 Subprogram Call M99 Subprogram End M200 Main Spindle Brake ON M201 Main Spindle Brake OFF M202 Sub-Spindle Brake ON [Option] M203 Sub-Spindle Brake OFF [Option] M206 Disable Main Spindle Draw Bar Check M207 Enable Main Spindle Draw Bar Check M208 Disable Sub-Spindle Draw Bar Check [Option] M209 Enable Sub-Spindle Draw Bar Check [Option] M215 Thru-Spindle Coolant ON, Sub-Spindle [Option] M216 Thru-Spindle Coolant OFF, Sub-Spindle [Option] M221 Part Catcher Slide Extend [Option] M222 Part Catcher Slide Retract [Option] M223 Sub-Spindle Contouring Mode ON [Option] M224 Sub-Spindle Contouring Mode OFF [Option] M225 Sub-Spindle Part Catcher Arm Rotate Out [Option] M226 Sub-Spindle Part Catcher Arm Rotate In [Option] M227 Sub-Spindle Part Catcher Gripper Close [Option] M228 Sub-Spindle Part Catcher Gripper Open [Option] M258 Chip Conveyor ON [Option] M259 Chip Conveyor OFF [Option] M300 Series M Codes Diameter Programming General Program Formats Main Spindle Operation Sub-Spindle Operation [Option] iv M-504A

7 CHAPTER 2 - TOOL NOSE RADIUS COMPENSATION Introduction Tool Orientation Number Activating Tool Nose Radius Compensation Entering and Exiting the Workpiece with Tool Nose Radius Compensation Active Switching G41/G42 Code with Tool Nose Radius Compensation Active Axis Reversals with Tool Nose Radius Compensation Active Modes in Which Tool Nose Radius Compensation is Not Performed Multiple Repetitive Cycles with Tool Nose Radius Compensation Active Canned Cycles with Tool Nose Radius Compensation Active G90 Canned Turning Cycle G94 Canned Facing Cycle Tool Moved Away from the Workpiece with Tool Nose Radius Compensation Active Tool Nose Radius Compensation Related Alarms Deactivating Tool Nose Radius Compensation Tool Nose Radius Compensation Programming Rules CHAPTER 3 - LINEAR AND CIRCULAR INTERPOLATION Feedrate Absolute and Incremental Programming Interpolation Linear Interpolation Insert Chamfer or Corner Radius Insert Chamfer Insert Corner Radius Sample Program Alarm Messages for Insert Chamfer/Insert Corner Radius Circular Interpolation G02 Clockwise Arc G03 Counter-Clockwise Arc Programming Notes for Circular Interpolation CHAPTER 4 - WORK SHIFT AND TOOL OFFSETS Work Shift Macro Variable Assignments Storing Work Shift Offsets Loading the Macro Variables from the Part Program Loading a Work Shift Offset from the Macro Variable Registers Tooling and Tool Offsets Tooling Top Plate Configurations Left Hand/Right Hand Tooling Tool Offsets Introduction Tool Nose Radius Value and Orientation Code Storing Tool Offsets from the Part Program Activating Tool Offsets Canceling Tool Offsets M-504A v

8 CHAPTER 5 - WORK COORDINATE SYSTEM How the Control Positions the Slides Rectangular Coordinates Coordinate System Reference Positions Machine Zero Position Turret Axis Reference Position Turret Reference Location Sub-Spindle or Tailstock Axis Reference Position Sub-Spindle or Tailstock Reference Location Position Registers Machine Position Registers Absolute Position Registers CHAPTER 6 - MACHINING CYCLES G90 Canned Turning Cycle Example 1: G90 Straight Turning Example 2: G90 Taper Turning G71/G70 Automatic Multiple Repetitive Rough and Finish Turning G71/G70 Standard Turning Example 3: G71/G70 Standard Turning Cycle G71 Standard Turning Programming Rules G71/G70 Pocket Turning [Option] Example 4: G71/G70 Pocket Turning Cycle G71 Pocket Turning Programming Rules G94 Canned Facing Cycle Example 5: G94 Straight Facing Example 6: G94 Taper Facing G72/G70 Automatic Multiple Repetitive Rough and Finish Facing Example 7: G72/G70 Facing Cycle G72 Programming Notes G73/G70 Automatic Rough and Finish Pattern Repeat Example 8: G73/G70 Pattern Repeat Cycle G73 Programming Notes G70 Automatic Finishing Cycle G70 Programming Notes Automatic Drilling Cycles G74 Constant Depth Increment Automatic Drilling Cycle Block Format Q Word Programming G74 Automatic Drilling Sample Program Variable Depth Increment Automatic Drilling Cycle Block Format Data Word Definitions Positioning the Drill Main Spindle Operation Sub-Spindle Operation Calculating the Drill Pass Increments Macro 9136 without Optional Z Word Sample Part Description Example 1: Main Spindle Example 2: Sub-Spindle vi M-504A

9 Macro 9136 with Optional Z Word Main Spindle Operation Sub-Spindle Operation Sample Part Description Example 3: Main Spindle Example 4: Sub-Spindle G75 Automatic Grooving Cycle Block Format P and Q Word Programming Tool Movement Sequence G75 Automatic Grooving Sample Program Polygon Turning Introduction Spindle Selection Program Entry Manual Data Input Keyboard Entry G Codes Block Format Crowning Selecting the Cutter and Speed Ratio Sample Program Segments Main Spindle Program Segment Sub-Spindle Program Segment Canceling Polygon Turning CHAPTER 7 - THREADING CYCLES Introduction Single Block Threadcutting Establishing a Start Point for Threading G32 Programming Example 1: G32 Straight Threads Example 2: G32 Tapered Threads G92 Canned Threading Cycle Example 3: G92 Straight Threads Example 4: G92 Tapered Threads Plunge Infeed Threading Compound Infeed Threading G76 Automatic Multiple Repetitive Threading Cycle Block Format Example 5: G76 Straight Threads Example 6: G76 Tapered Threads G76 Parameter Line G76 Execution Line G76 Programming Notes G34 Variable Lead Threadcutting Left-Hand Threads Tapping Example Sample Program Segment M-504A vii

10 Rigid Tapping Rigid Tapping with Standard Tooling (Non-Live Tooling) Program Formats for Standard Tooling Turret at the Main Spindle Turret at the Sub-Spindle Rigid Tapping with Live Tooling Program Formats for Live Tooling End-Working Attachment at the Main Spindle Cross-Working Attachment at the Main Spindle End-Working Attachment at the Sub-Spindle Cross-Working Attachment at the Sub-Spindle Thread Milling Introduction Conventional Milling and Climb Milling General Guidelines Work Plane Selection Internal Thread Milling Variable Definitions and Formulas Programming Example Basic Tool Motion Sample Program Segment External Thread Milling Variable Definitions and Formulas Basic Tool Motion CHAPTER 8 - G80 SERIES CYCLES Introduction Canceling Cycles Spindle Orient General Descriptions Drilling Cycles G83 Face Drilling Cycle Data Words Formats Definitions Tool Movement in the G83 Cycle Single Pass Drilling Peck Drilling High Speed Peck Drilling G83 Sample Program Segment G87 Side Drilling Cycle Data Words Formats Definitions Tool Movement in the G87 Cycle Single Pass Drilling Peck Drilling High Speed Peck Drilling G87 Sample Program Segment viii M-504A

11 Tapping Cycles G84 Right-Hand Face Tapping Cycle Data Words Formats Definitions Tool Movement in the G84 Cycle G84 Sample Program Segment G88 Right-Hand Side Tapping Cycle Data Words Formats Definitions Tool Movement in the G88 Cycle G88 Sample Program Segment Boring Cycles G85 Face Boring Cycle Data Words Formats Definitions Tool Movement in the G85 Cycle G85 Sample Program Segment G89 Side Boring Cycle Data Words Formats Definitions Tool Movement in the G89 Cycle G89 Sample Program Segment CHAPTER 9 - MISCELLANEOUS Constant Surface Speed Subprograms Subprogram Call Safe Index Subprograms Introduction Main Spindle Operation Sub-Spindle Operation [Option] Subprogram Descriptions Main Spindle Safe Index Subprogram O Sub-Spindle Safe Index Subprogram O Subprogram Structure Main Spindle Safe Index Subprogram O Sub-Spindle Safe Index Subprogram O Hardinge Permanent Macro Programs Macro 9112: Safe Tool Offset Macro 9136: Variable Depth Increment Automatic Drilling Cycle Macro 9150: Collet Dwell Recommended Settings Setting the Delay M-504A ix

12 Tailstock Introduction Data Word Definitions Tailstock Programming Examples Example 1: Workpiece Held in Collet/Chuck, Live Center in Tailstock Example 2: Machining Between Centers Tailstock Programming Notes Sub-Spindle Part Catcher [Option] Introduction M Codes Interlocks Capacity Programming Sequence for Unloading a Workpiece English / Metric Mode Spare M Codes Outputs Inputs CHAPTER 10 - TOOL LIFE MANAGEMENT Introduction Tool Life Measurement Units Number of Parts Amount of Machining Time Tool Life Management Program Description Bar Feed Operation Programming Tool Life Management Program Program Format Data Word Definitions P Word - Tool Group Number L Word - Tool Life Value Data Word T Word - Turret Station and Offset Number Sample Tool Life Management Program Part Program Tool Commands Sample Part Program Structure using Tool Life Management Combining Tool Commands Programming Notes x M-504A

13 CHAPTER 11 - LIVE TOOLING AND SPINDLE ORIENT Introduction Live Tooling M Codes Determining Rotational Direction C Axis Spindle Orient Programming C Axis Spindle Orient Absolute Orientation Incremental Orientation B Axis Spindle Orient Spindle Orient M Codes Programming B Axis Spindle Orient Direction of Orientation Determining Spindle Orientation Live Tooling Programming Formats Using C Axis Spindle Orient Using B Axis Spindle Orient Deactivating Live Tooling Live Tooling Programming Notes Sample Live Tooling Program Tool Definitions Sample Program using C Axis Spindle Orient CHAPTER 12 - POLAR AND CYLINDRICAL INTERPOLATION Data Word Descriptions Polar Coordinate Interpolation Coordinate Systems Main Spindle Rotation Sub-Spindle Rotation Defining X, C, and A Axis Motion Polar Coordinate Interpolation Guidelines Program Format for Polar Coordinate Interpolation Tool Nose Radius Compensation and Circular Interpolation used with G112 Polar Coordinate Interpolation Main Spindle Sub-Spindle Program Examples Example 1: Square Example 2: Hexagon Example 3: Triangle Example 4: Tongue Example 5: Radius Diamond Cylindrical Interpolation Program Format for Cylindrical Interpolation Cylindrical Interpolation Guidelines Tool Nose Radius Compensation and Circular Interpolation used with G107 Cylindrical Interpolation Main Spindle Sub-Spindle M-504A xi

14 Programming Examples Example 6: Lettering on Part Diameter Example 7: Rectangle Etched on Part Diameter Example 8: Rectangle with Corner Radius Example 9: Worm Gear C Axis Alarms CHAPTER 13 - BLUEPRINT PROGRAMMING Introduction Angle Definitions Blueprint Programming Examples Example 1: Two Points Example 2: Three Points Example 3: Three Points with a Radius Example 4: Three Points with a Chamfer Example 5: Four Points with Two Radii Example 6: Four Points with Two Chamfers Example 7: Four Points with One Radius and Chamfer Example 8: Four Points with One Chamfer and Radius Blueprint Programming Sample Program Blueprint Programming Notes CHAPTER 14 - SUB-SPINDLE [Option] Introduction Travel Specifications Programming Axis Motion Feedrate E Axis Motion E Axis Position Verification X/U Axis Motion Z/W Axis Motion Main Spindle Sub-Spindle Sub-Spindle / Tool Holder Clearance Requirement Sub-Spindle G Codes G02 / G03 Circular Interpolation G41 / G42 Tool Nose Radius Compensation Sub-Spindle M Codes M07 Sub-Spindle Phase Synchronization with Main Spindle M32 Sub-Spindle Synchronization with Main Spindle M33 Sub-Spindle Forward M34 Sub-Spindle Reverse M35 Sub-Spindle Stop M46 Sub-Spindle Air Blast ON [Option] M47 Sub-Spindle Air Blast OFF [Option] M56 Sub-Spindle Collet / Chuck Open M57 Sub-Spindle Collet / Chuck Close xii M-504A

15 M62 Activate C Axis Spindle Synchronization M63 Cancel C Axis Spindle Synchronization M68 External Chucking Mode M69 Internal Chucking Mode M76 Sub-Spindle Drive OFF M77 Sub-Spindle Drive Low Torque M78 Sub-Spindle Drive Normal Torque M215 Thru-Spindle Coolant ON M216 Thru-Spindle Coolant OFF Sub-Spindle Work Shift Tool Offsets Tool Geometry Offsets Tool Wear Offsets X Axis Tool Wear Offsets Z Axis Tool Wear Offsets Spindle Synchronization Sample Programs Sample Program using Standard Collets or Pull Back Systems Sample Program using Dead Length Collets or Chucks Workpiece Transfer Transferring from Main Spindle to Sub-Spindle Bar Job Transfer from Main Spindle to Sub-Spindle Spindle Clearance Requirements Dead Length Collet Not Installed in Sub-Spindle Collet Dead Length Collet Installed in Sub-Spindle Collet Slug Job Transfer from Main Spindle to Sub-Spindle Transferring from Sub-Spindle to Main Spindle Sub-Spindle Sample Program Basic Sequence of Operations Sample Program Sub-Spindle Programming Notes CHAPTER 15 - BASIC Y AXIS PROGRAMMING Introduction Y Axis Programming Formats Main Spindle Operation Sub-Spindle Operation Machining on the Diameter of the Workpiece Sample Program 1 - Drilling Offset Holes Sample Program Sample Program 2 - Milling a Slot G Codes Sample Program Machining the End of the Workpiece Sample Program 3 - Drilling Offset Holes Sample Program Sample Program 4 - Milling a Pocket G Codes Sample Program M-504A xiii

16 APPENDIX ONE Turret Travel Specifications X and Z Axes T-42 Lathe BMT 45 Turret Top Plate A1-1 Hardinge Turret Top Plate A1-2 T-51 and T-65 Lathes BMT 55 Turret Top Plate A1-3 Hardinge Turret Top Plate A1-4 Y Axis [Option] T-42 Lathe A1-5 T-51 and T-65 Lathes A1-6 Tailstock Travel Specifications T-42 Lathe A1-7 T-51 and T-65 Lathes A1-7 Sub-Spindle Travel Specifications T-42 Lathe A1-8 T-51 and T-65 Lathes A1-8 Work Envelopes T-42 Lathe Equipped with Tailstock and BMT 45 Turret Top Plate A1-9 Equipped with Tailstock and Hardinge Turret Top Plate A1-10 Equipped with Sub-Spindle and BMT 45 Turret Top Plate A1-11 Equipped with Sub-Spindle and Hardinge Turret Top Plate A1-12 T-51 and T-65 Lathes Equipped with Tailstock and BMT 55 Turret Top Plate A1-13 Equipped with Tailstock and Hardinge Turret Top Plate A1-14 Equipped with Sub-Spindle and BMT 55 Turret Top Plate A1-15 Equipped with Sub-Spindle and Hardinge Turret Top Plate A1-16 Turret Top Plate Distance to Waycover T-42 Lathe BMT 45 Turret Top Plate A1-17 Hardinge Turret Top Plate A1-18 T-51 and T-65 Lathes BMT 55 Turret Top Plate A1-19 Hardinge Turret Top Plate A1-20 Sample Tooling Layouts T-42 Lathe BMT 45 Turret Top Plate with Static and Live Tooling A1-21 Hardinge Turret Top Plate A1-22 T-51 and T-65 Lathes BMT 55 Turret Top Plate with Static and Live Tooling A1-23 Hardinge Turret Top Plate A1-24 xiv M-504A

17 Spindle Power and Torque Curves Main Spindle T-42 and T-42 Big-Bore Lathes A1-25 T-51 Lathe A1-26 T-65 Lathe A1-27 Sub-Spindle (All Models) A1-28 Live Tooling T-42 Lathe with BMT 45 Turret Top Plate A1-29 T-51 and T-65 Lathes with BMT 55 Turret Top Plate A1-30 APPENDIX TWO G Codes A2-1 M Codes A2-3 DOCUMENT REVISION RECORD M-504A xv

18 - NOTES - xvi M-504A

19 Global Headquarters United States Hardinge Subsidiaries England Germany Switzerland China Taiwan OFFICES Hardinge Inc. One Hardinge Drive Elmira, NY USA Telephone: web site: Jones & Shipman Hardinge Ltd. Murrayfield Road Leicester LE3 1UW England Telephone: +44 (0) website: website: Hardinge GmbH Fichtenhain A 13 c D Krefeld Germany Telephone: (49) L. Kellenberger & Co. AG Heiligkreuzstrasse 28 Postfach Ch-9009 St. Gallen Switzerland Telephone: website: info@kellenberger.net Hardinge Machine (Shanghai) Co. Ltd. Hardinge China Limited No.1388 East Kang Qiao Road Pudong, Shanghai Telephone : web site: Hardinge Taiwan Precision Machinery Ltd. 4 Tzu Chiang 3rd Road Nan Tou City 540 Taiwan, R.O.C. Telephone: M-504A xvii

20 MACHINE DESCRIPTION AND INTENDED USE Applicable Machines: T-42, T-51, and T-65 Lathes These lathes are numerically controlled machine tools designed to shape cold metal by the application of a cutting tool and rotating workpiece capable of performing two or more machining processes (e.g. turning, facing, drilling, grooving and boring) at one set-up of a workpiece and incorporating the following features: Select and change tools from a turret. Change the position of the turret relative to the spindle clamped workpiece. Select and apply spindle speeds and axis feeds. Control auxiliary services (e.g. coolant flow). Tailstock provides added support when machining long parts and reduces part deflection. Optional sub-spindle provides capability of back side tuning. Optional live tooling provides milling capabilities. These lathes are designed to machine non-hazardous metals only. Non-hazardous materials such as Tools Steels, Aluminum, and Brass may be machined. DO NOT machine any flammable, explosive, toxic, or radioactive material. DO NOT machine any material that produces a hazardous residue, dust, or gas. DO NOT use any flammable, explosive, or toxic cutting fluids. In all cases, if in doubt about the content of the material that you wish to machine, contact the material supplier. MACHINE ELECTRICAL OPERATING RANGE Ambient Temperature Range: +5 C to +40 C. Humidity Range: Up to 40% at a maximum temperature of +40 C. Altitude: Up to 1000 meters above sea level (minimum) xviii M-504A

21 GENERAL WARNINGS AND CAUTIONS CHEMICAL WARNING Current laws and regulations require that information regarding chemicals used with this equipment be supplied to you. Refer to the applicable section of the Material Safety Data Sheets supplied with your machine when handling, storing, or disposing of chemicals. BAR FEED WARNING Machine should only be used with a bar feed approved by Hardinge Inc. SPINDLE TOOLING WARNINGS Hardinge HQC (Quick-Change) collets MUST NOT be used in applications where the spindle is rotating without a bar or workpiece in the collet. Rotating the spindle without a bar or workpiece in the collet can result in the collet head being expelled from the spindle. DO NOT exceed the maximum jaw chuck size, as specified in the Operator's Manual (M-505). DO NOT exceed the maximum draw bar force rating of the jaw chuck. DO NOT exceed the maximum rpm rating of the jaw chuck. Refer to the manual supplied with the jaw chuck. Failure to comply with these warnings can result in serious injury or death. ENTRAPMENT WARNING DO NOT climb into the machine guard! You may become entrapped. Due to the compact size of the Hardinge lathes and the provision of side access doors to allow servicing of the machine, it is not necessary to climb into the machine guard. In the unlikely event that this warning is ignored and the main access door is closed, the door will latch shut and cannot be opened from the inside. Another person must release the door lock. Refer to the Operator's Manual (M-505) for information on releasing the door lock. MAIN COOLANT GUARD WARNING The guards provided with the machine are intended to minimize the risks of workpiece ejection and not to eliminate them completely. INTERLOCKED ACCESS PANEL CAUTION Opening an interlocked access panel while the machine is cutting a part will force the control into a dual check speed or position alarm, which can destroy the workpiece and/or tooling. M-504A xix

22 TURRET TOP PLATE ALIGNMENT CAUTION (Live Tool Machines Only) Check the alignment of the turret top plate with the live tool drive shaft in the event that any of the following events have occurred: Static tool breakage Live tool breakage Live tool torque limiter trip Machine crash Refer to the maintenance manual (M-506) for information on checking the alignment of the turret top plate. HIGH PRESSURE COOLANT CAUTION Do not use a high pressure coolant system that can exceed 1000 psi [69 bar]. Damage to the machine will result. xx M-504A

23 SAFETY RECOMMENDATIONS Your Hardinge machine is designed and built for maximum ease and safety of operation. However, some previously accepted shop practices may not reflect current safety regulations and procedures, and should be re-examined to insure compliance with the current safety and health standards. Hardinge Inc. recommends that all shop supervisors, maintenance personnel, and machine tool operators be advised of the importance of safe maintenance, setup, and operation of Hardinge equipment. Our recommendations are described below. READ THESE SAFETY RECOMMENDATIONS BEFORE PROCEEDING ANY FURTHER. Read the appropriate manual or instructions before attempting operation or maintenance of the machine. Make certain that you understand all instructions. Don t allow the operation or repair of equipment by untrained personnel. Consult your supervisor when in doubt as to the correct way to do a job. Wear safety glasses and proper foot protection at all times. When necessary, wear respirator, helmet, gloves, and ear muffs or plugs. Don t operate equipment unless proper maintenance has been regularly performed and the equipment is known to be in good working order. Warning or instruction tags are mounted on the machine for your safety and information. Do not remove them. If a tag comes off, re-attach the tag at the original position. Replace any warning or instruction tag if it becomes unreadable. Refer to the maintenance manual for tag identification. Don t alter the machine to bypass any interlock, overload, disconnect, or other safety device. Don t operate equipment if unusual or excessive heat, noise, smoke, or vibration occurs. Report any excessive or unusual vibration, sounds, smoke, or heat as well as any damaged parts. Reduce spindle speed if vibration occurs. Bar stock straightness will have an effect on vibration and balance of the spindle system. Machining an unbalanced workpiece may create an ejection hazard. Minimize the risk by counter-balancing or machining at reduced speeds. Never operate the machine spindle without a work-holding device if the draw tube is in the spindle. Tighten all draw tube screws before beginning spindle operation. Make certain that the equipment is properly grounded. Consult National Electric Code and all local codes. Disconnect main electrical power before attempting repair or maintenance. M-504A xxi

24 Allow only authorized personnel to have access to enclosures containing electrical equipment. Don t reach into any control or power case area unless electrical power is OFF. Don t touch electrical equipment when hands are wet or when standing on a wet surface. Replace blown fuses with fuses of the same size and type as originally furnished. Ascertain and correct the cause of a control alarm before restarting the machine. Keep the area around the machine well lighted, dry, and free of obstructions. Keep chemical and flammable material away from electrical or operating equipment. Keep chips clear of the work area. Don t use a toxic or flammable substance as a solvent cleaner or coolant. Make certain that proper guarding is in place and that all doors are closed and secured. To remove or replace the collet closer it is necessary to remove the guard door at the left end of the machine. Make certain that the guard door is in place before starting the machine. Don t open guard doors while any machine component is in motion. Make sure chucks, closers, fixture plates, and all other spindle-mounted work-holding devices are properly mounted and secured before starting the machine. Make certain all tools are securely clamped in position before starting the machine. Remove any loose parts or tools left on machine or in the work area before operating the machine. Always check the machine and work area for loose tools and parts especially after work has been completed by maintenance personnel. Remove chuck wrenches before starting the machine. Before pressing the cycle start push button, make certain that proper functions are programmed and that all controls are set in the desired modes. Know where all Emergency Stop push buttons are located in case of an emergency. Check the lubrication oil level and the status of the indicator lights before operating the machine. Make certain that all guards are in good condition and are functioning properly before operating the machine. Inspect all safety devices and guards to make certain that they are in good condition and are functioning properly before the cycle is started. DO NOT power up the machine until the guard door vision panel has been inspected and determined to be in satisfactory condition. Failure to inspect the vision panel can result in unsafe operating conditions. xxii M-504A

25 Check the position of the tool top plate before pressing the Cycle Start push button. Check the position of any load/unload automation before pressing the Cycle Start push button. Check setup, tooling, and security of the workpiece if the machine has been OFF for any length of time. Dry cycle a new setup to check for programming errors. Make certain that you are clear of any pinch point created by moving slides before starting the machine. Don t operate any equipment while any part of the body is in the proximity of a potentially hazardous area. Don t remove chips with hands. Use a hook or similar device and make certain that all machine movements have ceased. Be careful of sharp edges when handling a newly machined workpiece. Don t remove or load a workpiece while any part of the machine is in motion. Don t operate any machine while wearing rings, watches, jewelry, loose clothing, neckties, or long hair not contained by a net or shop cap. Don t operate any machine while under the influence of drugs and/or alcohol. Don t adjust tooling or coolant hoses while the machine is running. Don t leave tools, workpieces or other loose items where they can come in contact with a moving component of the machine. Don t check finishes or dimensions of workpiece near running spindle or moving slides. Don t jog spindle in either direction when checking threads with a thread gauge. Don t attempt to brake or slow the machine with hands or any improvised device. Any machine modification must be reviewed by Hardinge Inc. before implementation. Use caution around exposed mechanisms and tooling especially when setting up. Be careful of sharp edges on tools. Don t use worn or defective hand tools. Use the proper size and type for the job being performed. Use only a soft-faced hammer on tooling and fixtures. Don t use worn or broken tooling on machine. Make certain that all tool mounting surfaces are clean before mounting tools. M-504A xxiii

26 Inspect all chucking devices daily to make certain that they are in good operating condition. Replace any defective chuck before operating the machine. Hardinge high speed spindles are balanced to an ISO G1.0 standard. High speed spindles require a work-holding device balanced to G2.5 or better. Use maximum allowable gripping pressure on the chuck. Consider weight, shape, and balance of the workpiece. Check the workpiece for distortion. Use lighter than normal feedrates and depth of cut when machining a workpiece diameter that is larger than the gripping diameter. Don t exceed the rated capacity of the machine or tooling. Don t leave the machine unattended while it is operating. Don t clean the machine with an air hose. Keep tote pans a safe distance from the machine. Don t overfill the tote pans. Don t let stock project past the back end of the collet closer or machine spindle without being adequately covered and properly supported. Follow each bar feed manufacturer s guidelines. For performance and safe application, size and use feed tube bushings, pushers, and spindle liners according to bar feed information. Make certain that any bar feed mechanism is properly aligned with the spindle. If the bar feed is a floor-mounted type, it must be securely bolted to the floor. During high speed applications, the bar stock must be contained within the collet closer and a bar feed not be used. Hardinge Inc. recommends using a bar loader for feeding bar stock during high speed applications. Bar loaders feed the entire piece of bar stock into the spindle; then, the pusher is disengaged from the bar stock. Unless otherwise noted, all operating and maintenance procedures are to be performed by one person. To avoid injury to yourself and others, be sure that all personnel are clear of the machine when opening or closing the coolant guard door and any access covers. Because there are so many things that either cannot be done or must not be done when using the machine, that is impossible to cover all of them in the documentation. Assume that something is impossible unless the manual specifically states that it can be done. FOR YOUR PROTECTION - WORK SAFELY xxiv M-504A

27 - NOTES - M-504A xxv

28 - NOTES - xxvi M-504A

29 CHAPTER 1 - PART PROGRAM LANGUAGE INTRODUCTION A part program is an ordered set of instructions which define slide and spindle motion as well as auxiliary functions. These instructions are written in a part program language consisting of a series of data blocks. Each data block contains adequate information for the machine tool to perform one or more machine functions. A data block consists of one or more data words, which are treated together as a unit. Each data word consists of a word address followed by a numerical value. A word address is a letter which specifies the meaning of the data word. The value of the number that follows the word address has a format which specifies the number of characters the word contains as well as the range these values must fall within. These formats are listed in the tables beginning on page 1-2. PROGRAMMING THE CONTROL Programming Hardinge lathes requires an understanding of the machine, tooling, and control. Extreme care must be exercised when writing a part program since all machine movements will be executed as programmed. A miscalculation or selection of an incorrect function can result in an incorrect motion. The basic unit for part program input is the BLOCK. Normally, one line or block of information represents one describable operation or several describable operations that are independent of each other. (For example, axis movement and spindle speed changes are independent operations which may be programmed in the same block.) A block may contain any or all of the following: 1. Slash code (/) 2. Sequence number (N Function) 3. Preparatory Functions (G Functions) 4. Axis Movement Instructions (E, X or U, Y or V, and Z or W Functions) 5. Feedrate Command (F Function) 6. Spindle Speed Command (S Function) 7. Turret Station (T Function) 8. Miscellaneous Functions (M Functions) A block MUST contain a valid End of Block character. M-504A 1-1

30 DATA WORD FORMATS AND MINIMUM / MAXIMUM VALUES T-42 Lathes - NOTE - Refer to the table definitions listed on page 1-3. Function (Word) Preparatory Commands INCH MODE (G20) METRIC MODE (G21) Format Minimum Maximum Format Minimum Maximum O (Program #) N (Block #) G (Command) M (Command) P (Block #) P (Dwell) Q (Block #) O4 N4 G3 M3 P4 P8 Q O4 N4 G3 M3 P4 P8 Q E (Coordinate) 1 E (Coordinate) 2 E (Coordinate) 3 E (Coordinate) 4 U (Coordinate) U (Dwell) V (Coordinate) W (Coordinate) X (Coordinate) 5 X (Coordinate) 6 X (Dwell) Y (Coordinate) 7 Z (Coordinate) 8 Z (Coordinate) 9 Z (Coordinate) 10 Z (Coordinate) 11 G00, G01 G00, G01 G00, G01 G00, G01 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 E±2.5 E±2.5 E±2.5 E±2.5 U±2.5 U5.3 V±2.5 W±2.5 X±2.5 X±2.5 X5.3 Y±1.5 Z±2.5 Z±2.5 Z±2.5 Z± E±3.4 E±3.4 E±3.4 E±3.4 U±3.4 U5.3 V±3.4 W±3.4 X±3.4 X±3.4 X5.3 Y±2.4 Z±3.4 Z±3.4 Z±3.4 Z± X (Tool Offset) X (Wear Offset) X (Zero Offset) Y (Tool Offset) 7 Y (Wear Offset) 7 Z (Tool Offset) Z (Wear Offset) Z (Zero Offset) G10 G10 G10 G10 G10 G10 G10 G10 X±2.5 X±0.5 X±2.5 Y±2.5 Y±0.5 Z±2.5 Z±0.5 Z± X±3.4 X±2.4 X±3.4 Y±3.4 Y±2.4 Z±3.4 Z±2.4 Z± I (Circ. Interp.) J (Circ. Interp.) K (Circ. Interp.) K (Lead Change) G02, G03 G02, G03 G02, G03 G34 I±3.5 J3.5 K±3.5 K± I±4.4 J4.4 K±4.4 K± F (per min) F (per rev) F (Thread Lead) G98 G99 G32, G33, G34 F3.2 F1.6 F F4.1 F3.4 F B (Spindle Orient) 12, 13 C (C-Axis) A (C-Axis) B3 C±5.3 A± B3 C±5.3 A± M-504A

31 Function (Word) S (Spindle RPM) 12 G50, G97 S (Spindle RPM) 13 G50, G97 S (Spindle RPM) 14 G50, G97 S (Live Tooling) 15 G97 S (Surface Speed) G96 T (Tool Function) 5 - T (Tool Function) 6 - Preparatory Commands INCH MODE (G20) METRIC MODE (G21) Format Minimum Maximum Format Minimum Maximum S S S S S S S S S S T T T T ,A (Angle),C (Chamfer) R (Radius),R (Radius) G00, G01 G01 G02, G03 G01,A3.5,C2.5 R2.5,R ,A3.4,C3.4 R3.4,R TABLE DEFINITIONS, T-42 LATHE 1. Machine with sub-spindle and 16C main spindle. 2. Machine with sub-spindle and 20C main spindle. 3. Machine with tailstock and 16C main spindle. 4. Machine with tailstock and 20C main spindle. 5. BMT 45 turret top plate. 6. Hardinge turret top plate. 7. Optional Y axis. 8. Machine with BMT 45 turret top plate and 16C main spindle. 9. Machine with BMT 45 turret top plate and 20C main spindle. 10. Machine with Hardinge turret top plate and 16C main spindle. 11. Machine with Hardinge turret top plate and 20C main spindle C main spindle C main spindle. 14. Optional sub-spindle. 15. Live tooling (standard feature with BMT 45 turret top plate). M-504A 1-3

32 T-51 and T-65 Lathes - NOTE - Refer to the table definitions listed on page 1-5. Function (Word) Preparatory Commands INCH MODE (G20) METRIC MODE (G21) Format Minimum Maximum Format Minimum Maximum O (Program #) N (Block #) G (Command) M (Command) P (Block #) P (Dwell) Q (Block #) O4 N4 G3 M3 P4 P8 Q O4 N4 G3 M3 P4 P8 Q E (Coordinate) 1 E (Coordinate) 2 U (Coordinate) U (Dwell) V (Coordinate) W (Coordinate) X (Coordinate) 3 X (Coordinate) 4 X (Dwell) Y (Coordinate) 5 Z (Coordinate) 3 Z (Coordinate) 4 G00, G01 G00, G01 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 E±2.5 E±2.5 U±2.5 U5.3 V±2.5 W±2.5 X±2.5 X±2.5 X5.3 Y±1.5 Z±2.5 Z± E±3.4 E±3.4 U±3.4 U5.3 V±3.4 W±3.4 X±3.4 X±3.4 X5.3 Y±2.4 Z±3.4 Z± X (Tool Offset) X (Wear Offset) X (Zero Offset) Y (Tool Offset) 5 Y (Wear Offset) 5 Z (Tool Offset) Z (Wear Offset) Z (Zero Offset) G10 G10 G10 G10 G10 G10 G10 G10 X±2.5 X±0.5 X±2.5 Y±2.5 Y±0.5 Z±2.5 Z±0.5 Z± X±3.4 X±2.4 X±3.4 Y±3.4 Y±2.4 Z±3.4 Z±2.4 Z± I (Circ. Interp.) J (Circ. Interp.) K (Circ. Interp.) K (Lead Change) G02, G03 G02, G03 G02, G03 G34 I±3.5 J3.5 K±3.5 K± I±4.4 J4.4 K±4.4 K± F (per min) F (per rev) F (Thread Lead) G98 G99 G32, G33, G34 F3.2 F1.6 F F5.0 F3.4 F B (Spindle Orient) C (C-Axis) 6 A (C-Axis) B3 C±5.3 A± B3 C±5.3 A± S (Spindle RPM) 8 S (Spindle RPM) 9 S (Spindle RPM) 10 S (Live Tooling) 11 S (Surface Speed) G50, G97 G50, G97 G50, G97 G97 G96 S4 S4 S4 S4 S S4 S4 S4 S4 S M-504A

33 Function (Word) Preparatory Commands INCH MODE (G20) METRIC MODE (G21) Format Minimum Maximum Format Minimum Maximum T (Tool Function) 3 - T (Tool Function) 4 - T4 T T4 T ,A (Angle),C (Chamfer) R (Radius),R (Radius) G00, G01 G01 G02, G03 G01,A3.5,C2.5 R2.5,R ,A3.4,C3.4 R3.4,R TABLE DEFINITIONS, T-51 AND T-65 LATHES 1. Machine with sub-spindle. 2. Machine with tailstock. 3. Machine with BMT 55 turret top plate. 4. Machine with Hardinge turret top plate. 5. Optional Y axis. 6. Main spindle. 7. Optional sub-spindle. 8. Main spindle, T-51 lathe. 9. Main spindle, T-65 lathe. 10. Optional sub-spindle. 11. Live tooling (standard feature with BMT 55 turret top plate). M-504A 1-5

34 AXIS DEFINITIONS Refer to Figures 1.1 and 1.2. A AXIS (Optional Sub-Spindle) Radial motion around the spindle centerline. C AXIS (Main Spindle) Radial motion around the spindle centerline. E AXIS (Tailstock / Optional Sub-Spindle) Linear motion parallel to the spindle centerline and parallel to the machine bed. X AXIS (Machine Cross Slide) Linear motion parallel to the spindle face and parallel to the machine bed. Y AXIS (Turret) [Option] Linear turret motion parallel to the spindle face and perpendicular to the machine bed. Z AXIS (Machine Carriage) Linear motion parallel to the spindle centerline and parallel to the machine bed. -Z +Z -C +C +A -A +X Main Spindle Viewed from Tailstock/Sub-Spindle -X Sub-Spindle Viewed from Main Spindle Turret Main Spindle Tailstock or Sub-Spindle -E +E TI5662A Figure E, X, and Z Axis Definitions 1-6 M-504A

35 +X +Y -X -Y Spindle Centerline Machine Bed TI5660 Figure X and Y Axis Definitions (Viewed from the Tailstock/Sub-Spindle End of the Machine) M-504A 1-7

36 SPECIAL PROGRAMMING CHARACTERS An End of Record character (%) should be the first and last character in a program which is to be uploaded to the machine control through the RS-232 serial port. If multiple programs are to be loaded from a single punched tape, punch the End of Record character after the last program on the tape. The End of Record character will be followed by an End of Block character. The End of Block character must be used after the last character in each data block of a part program that is to be loaded into the memory of the control. If the End of Block character is omitted from a part program data block, the control will consider the next block to be part of the block missing the End of Block. This may cause undesirable machine behavior. The End of Block character is a Carriage Return character in EIA (RS-224-B) format and a Line Feed character in ASCII (ISO) (RS-358-B) format. When programming from the keyboard, use the End of Block key. This character will be displayed as a semicolon (;) on the control display screen. Operator messages and comments can be included in a part program loaded from tape, provided they are enclosed in parentheses. Any legal ASCII character can be used when writing a comment. The Block Skip (/) code inserted at the beginning of a data block will cause that block of data to be ignored by the control when Block Skip is activated by the machine operator. When Block Skip is not active, the data block will be executed. PROGRAMMING FORMAT Programs to be executed by the control consist of alpha-numeric words that the control recognizes as specific commands. These words consist of one letter addresses and the designated numbers for that address. Words within a block may follow any convenient sequence. However, Hardinge recommends the following sequence: /, N, G, X, Z, U, W, B, C, I, J, K, P, Q, R, A, F, S, T, M The control system is configured to provide inch [.0001 mm] programming resolution. This causes specific data word formats to be applied to the associated values. These formats are listed in the tables beginning on page 1-2. These numbers indicate the maximum number of places allowed to the right and left of the decimal point. A plus sign need not be entered since the control assumes plus if no sign is entered. A minus sign MUST be programmed, if needed. Refer to page 1-55 for the general program formats. The safe index subprograms shown in the program formats are described in Chapter 9 of this manual. 1-8 M-504A

37 PROGRAMMING SEQUENCE Off-Line Programming Sequence 1. Enter an End of Record character (%). 2. Enter program ID code and program number. All programs are identified by the letter O in front of the part program ID number and may have 4 place ID numbers (1-8999). Program numbers 9000 through 9999 are reserved for macro programs. The program ID code and program number are followed by a valid End of Block character. 3. Enter the program. 4. End of Program command (M30) in the last data block. All data blocks must end with a valid End of Block character. 5. Enter an End of Record character (%). Keyboard Programming Sequence Refer to the operator s manual (M-505) for information on entering programs from the control keyboard. M-504A 1-9

38 PROGRAM NUMBER Part programs stored in the control memory must be assigned a part program number. The program numbers are used by the control to identify the various programs and subprograms which are stored in the control memory. The program number MUST be identified by the letter O followed by the program identification number. It is not necessary to program the leading zeros as these are automatically inserted by the control, when needed. The program number must be on the first line of the program. It may be programmed on a line by itself or it may be the first entry in the first data block. The part program numbers range from 1 to However, the following restrictions must be observed when assigning program numbers: 1. Alpha and other miscellaneous characters (such as dashes) are not allowed. 2. Program numbers 9000 through 9999 are reserved for permanent macro programs. These numbers cannot be assigned to other part programs or macros. - NOTE - When entering a program from the keyboard, if the program identification number is omitted, the active part program will be edited according to the data entered when the Insert key is pressed. If one of the 9000 series permanent macro programs is active and no program number is entered, the first program data block will be rejected and the message Write Protect will be displayed on the control display screen. When a tape which does not contain a program identification number is loaded into memory, the control will automatically assign the first programmed sequence number as the program number. Any attempt to store programs having numbers already stored in program memory will cause the message Already Exists to be displayed on the control display screen. This message indicates that the program identification number has already been assigned M-504A

39 DECIMAL POINT PROGRAMMING A decimal point should be used with the following address words: A, C, E, F, I, K, R, U, W, X, and Z. If a decimal point is programmed in a word in which a decimal point is not allowed or if two or more decimal points appear in any one data word, an error message will be displayed. Values with or without decimal points may be commanded in the same data block. Trailing zeros need not be programmed when using decimal point programming. If no decimal point is programmed, the control uses the appropriate data word format to insert leading zeros and properly position the decimal point. Example In Inch mode, the format for the Z word is ±2.5. If Z4. is programmed, the control will assume Z NOTICE The programmer must make certain all decimal points are correctly positioned to prevent undesirable machine behavior. This assumed decimal point is an important concept to keep in mind. There can be a great deal of difference between values with and without decimal points. Example The command X2. sends the cross slide to coordinate X ; however, the command X2" (no decimal point) sends the cross slide to X Be sure the decimal point is programmed when allowed. Besides specifying the location of the assumed decimal point, the word address format also indicates the maximum number of digits which can appear to the left and right of the decimal point. M-504A 1-11

40 DATA WORD DESCRIPTIONS O WORD The O word is used as the letter address for part program numbers and must precede the part program identification number. Refer to Program Number, on page N WORD The N word provides a sequence number consisting of the letter N and up to four digits ( ). It is not required to have a sequence number in any block. When used, they may be placed anywhere in the block; however, it is customary to program them as the first word in the block, except when a Block Delete (/) is programmed. Block Delete codes, when programmed, will be the first character in a block. The N word does not affect machine operation. However, it does give operators a valuable reference should they wish to relate an operation being performed to the program manuscript. The numbering sequence can begin with any number, such as N0001. It is recommended that the programmer assign sequence numbers in intervals of five or ten so that additional blocks can be inserted into the program if necessary. This eliminates the necessity of reassigning sequence numbers after blocks are added to the program. The only exception to this recommendation is that the block starting each operation be assigned the number of the turret station to be used for that operation. For example, when using turret station #6, N6 will be the block number to start the operation. Leading zeros may be omitted. G WORD The G word is a preparatory command which sets up the control for a specific type of operation. It has the word format G3, with a range of 00 to 999. Certain G codes are default codes and are automatically activated by the control under the following conditions: 1. Machine Power-up 2. Reading an End of Program Code (M30) 3. Control Reset 4. Emergency Stop The G codes are of two types: 1. Non-modal G codes are effective only in the block in which they are programmed. 2. Modal G codes remain effective until replaced by another G code in the same group. The chart in Appendix Two lists the G codes that are used with the control by groups. Only one G code from each group is permitted in a data block. If more than one G code from a group is programmed in a data block from the keyboard or tape, the last of the conflicting G codes entered in the data block will be the active G code. G codes containing a leading zero may be programmed without the zero. Example: G01 may be programmed as G M-504A

41 G00 Positioning (Group 1 G Code) This positioning command generates linear motion on one or more axes (E, X, Y, or Z) from the current position to the programmed end points at a rate determined by the Rapid Override switch. The rapid traverse rates are listed below, as inches per minute [millimeters per minute]. Axis Rapid Traverse Rate T-42 Lathe T-51 and T-65 Lathes E 1500 [38100] 1500 [38100] X 945 [24000] 1100 [27940] Y 236 [6000] 375 [9525] Z 1200 [30480] 1500 [38100] - NOTE - The E axis cannot be commanded incrementally. Axis motion can be expressed as E, X, Y, and Z for absolute moves or U, V, and W for incremental moves. A programmed feedrate (F Function) in a G00 block is ignored by the control. When the turret is programmed to move on more than one axis, the axes execute a vectorial move at a traverse rate that is determined by the rapid traverse rate for each of the programmed axes. When a G00 positioning move is programmed and the Rapid Override switch is set to 100%, both axes will move at maximum traverse. The G00 command is modal. A programmed G00 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G00 command. G01 Linear Interpolation (Group 1 G Code) Linear Interpolation generates linear motion on one or more axes (E, X, Y, or Z) from the current position to the programmed end points at a rate specified by a feedrate command in the same block or by an active feedrate from a preceding block. The programmed feedrate is directly affected by the Feedrate Override switch. - NOTE - The E axis cannot be commanded incrementally. Axis motion can be expressed as E, X, Y, and Z for absolute moves or U, V, and W for incremental moves. When multiple axes are programmed for a taper cut, the control will compensate the axis feedrates to produce a vectorial velocity equal to the programmed feedrate. That is, when both axes are programmed, a vectorial move is generated. The G01 command is modal. A programmed G01 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G01 command. M-504A 1-13

42 G02 Clockwise Arc (Group 1 G Code) The arc direction is determined by the rotational direction of the cutting tool when looking downward at the plan view of the workpiece. The G02 command is used with I and K words (arc center offset) or R word (radius) to provide the necessary qualifying dimensions of the arc. The G02 command is modal. A programmed G02 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G02 command. Refer to Circular Interpolation, in Chapter 3. G03 Counter-Clockwise Arc (Group 1 G Code) The arc direction is determined by the rotational direction of the cutting tool when looking downward at the plan view of the workpiece. The G03 command is used with I and K words (arc center offset) or R word (radius) to provide the necessary qualifying dimensions of the arc. The G03 command is modal. A programmed G03 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G03 command. Refer to Circular Interpolation, in Chapter 3. G04 Dwell (Group 0 G Code) A dwell command must be programmed with a X, U, or P word to specify the duration of the dwell in seconds. The range of dwell is.001 to seconds Refer to the tables beginning on page 1-2 for data word formats. The G04 Preparatory Command and its associated X, U, or P word must be programmed together in a data block that does not generate axis motion. - NOTE - Decimal point programming cannot be used when the P word is used to specify the dwell period. The P word specifies dwell in milliseconds. Leading zero suppression format must be used. DWELL IN SECONDS: A dwell of 2.5 seconds may be programmed in any of the following ways: G04 X2.5 G04 U2.5 G04 P2500 The dwell code is non-modal and does not change the status of any modal condition of the control. Following the dwell, the operating mode reverts to the same status as before the dwell. The previous feedrate is reinstated M-504A

43 G10 Offset Value Setting (Group 0 G Code) The G10 command permits entering the Work Shift Offset and Tool Offsets with the part program or as a separate program instead of entering the offset(s) individually from the Manual Data Input keyboard. When offsets are entered as a separate program, this program must be executed prior to part program execution to insert the offset values into the offset registers. As many offsets as needed may be entered from a separate tape. The G10 preparatory command is non-modal and must be programmed in each offset entry block. Refer to Chapter 4 for additional information. G17 Work Plane Selection (Group 16 G Code) The G17 command is used during C axis programming to select the X,C plane as the active work plane. Refer to Chapter 12 for additional information. G18 Work Plane Selection (Group 16 G Code) The G18 command is used during C axis programming to select the X,Z plane as the active work plane. Refer to Chapter 12 for additional information. G19 Work Plane Selection (Group 16 G Code) The G19 command is used during C axis programming to select the Z,C plane as the active work plane. Refer to Chapter 12 for additional information. G20 Inch Data Input (Group 6 G Code) - NOTE - It is recommended that all programs written with inch dimensions have the G20 code at the beginning of the program to ensure the correct format is active in case the previously executed program was in metric mode. Inch mode allows the programmer to program in inch units. The command is modal and can be canceled only by a G21 (metric mode) command. Pressing the Reset key has no affect on G20. If G20 is active when power is turned OFF, it will be active when power is restored. G20 must be programmed in a block by itself. M-504A 1-15

44 G21 Metric Data Input (Group 6 G Code) - NOTE - It is recommended that all programs written with metric dimensions have the G21 code at the beginning of the program to ensure the correct format is active in case the previously executed program was in inch mode. Metric mode allows the programmer to program in metric units. The command is modal and can be canceled only by a G20 (inch mode) command. Pressing the Reset key has no affect on G21. If G21 is active when power is turned OFF, It will be active when power is restored. G21 must be programmed in a block by itself. G22 Stored Stroke Limit Check ON (Group 9 G Code) With G22 active, stored stroke limit #2 is active. G22 is active at power-up regardless of whether it was active when the power was turned OFF. However, a control reset will not return the control to G22 if G23 is active when the control reset is performed. - NOTE - Stored stroke limit #1 is active even if G22 is inactive. When parameter 1300, bit 1, is set to 0", the tool is prohibited from entering the area established by these stored stroke limits. When parameter 1300, bit 1, is set to 1", the tool is prohibited from exiting the area established by these stored stroke limits. G23 Stored Stroke Limit Check OFF (Group 9 G Code) With G23 active, stored stroke limit #2 is inactive. The tool is free to move within the rectangular areas established by these limits. - NOTE - Stored stroke limit #1 is active even if G23 is active M-504A

45 G28 Return to Reference Position (Group 0 G Code) NOTICE Tool offsets and tool nose radius compensation should be canceled BEFORE commanding G28. - NOTE - Refer to the illustrations in Appendix One for the turret reference positions. The Y axis command is only effective on machines equipped with the optional Y axis feature on the turret. The G28 command performs an automatic return of the turret to the reference position for one or more axes. The move can be through an intermediate position or directly to the reference position. The move is performed at rapid traverse for each axis commanded. Move Directly to the Reference Position: G28 U0. ; Move the turret to the X axis reference position or G28 V0. ; Move the turret to the Y axis reference position or G28 W0. ; Move the turret to the Z axis reference position or G28 U0. V0. W0. ; Move the turret to the X, Y, and Z axis reference positions Move through an Intermediate Position: G28 X4. Z12. ; Move the turret to X4. Z12., then to the X and Z axis reference positions G31 Skip Function (Group 0 G Code) The G31 command allows the programmer to command linear interpolation (similar to G01) with the added capability of responding to an external skip signal. If no skip signal is detected, program execution occurs as if G01 has been commanded. If a skip signal is detected, program execution immediately moves to the next data block. The currently being executed is not completed. G31 is non-modal and must be programmed each time it is to be effective. M-504A 1-17

46 G32 Threadcutting (Constant Lead) (Group 1 G Code) The G32 threadcutting command is used when the programmer wishes to maintain complete control over the depth of each cutting pass. Threading may be done in either, or both the X and Z axes. The length of the thread is determined by the distance command for X and/or Z. If a linear thread is to be cut, it requires programming one axis. If a tapered thread is to be cut, it requires both the X and Z axes to be programmed. The lead command is entered as an F word whose value is determined by the distance between each thread. Refer to the tables beginning on page 1-2 for data word formats. Example The command G32 W-6. F.05" will result in a linear thread cutting pass 6 inches long with a.05 inch lead. The Feedrate Override switch is not effective during the threading pass unless it is set to 0%. Setting the Feedrate Override switch to 0% during a threading pass will stop X and Z axis motion. The Feedrate Override switch is active during the return pass. The Emergency Stop push button and Reset key are active during the threading pass. The G32 command is modal. A programmed G32 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G32 command. Refer to Chapter 7 for information on threading cycles. G34 Variable Lead Threadcutting (Group 1 G Code) The G34 variable lead threadcutting command is used if thread lead is to increase or decrease. Threading may be done in either, or both the X and Z axes. The length of the thread is determined by the distance command for X and/or Z. If a linear thread is to be cut, it requires programming one axis. If a tapered thread is to be cut, it requires both the X and Z axes to be programmed. The lead command is entered as an F word whose value is determined by the distance between each thread. The K word specifies the rate per revolution at which the lead increases or decreases. A positive (+) K causes an increasing lead and a negative (-) K causes a decreasing lead. Refer to the tables beginning on page 1-2 for data word formats. The Feedrate Override switch is not effective during the threading pass unless set to 0%. Setting the Feedrate Override switch to 0% during a threading pass will stop X and Z axis motion. The Feedrate Override switch is active during the return pass. The Emergency Stop push button and Reset key are active during the threading pass. The G34 command is modal. A programmed G34 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G34 command. Refer to Chapter 7 for information on threading cycles M-504A

47 G40 Cancel Tool Nose Radius Compensation (Group 7 G Code) Tool Nose Radius Compensation (G41/G42) is canceled by a programmed G40. If G40 is programmed in a block by itself, tool compensation is canceled. If the G40 block contains an axis move, tool compensation is canceled; then, the programmed move occurs without compensation. Tool Nose Radius Compensation will be canceled when the Emergency Stop push button or the Reset key is pressed. Refer to Chapter 2 for additional information. G41 Tool Nose Radius Compensation - Workpiece Right of Tool (Group 7 G Code) Tool Nose Radius Compensation with the workpiece to the right of the tool is established by programming G41. Imagine the operator sitting on the tool facing in the direction of the tool motion. If the workpiece is to the right of the operator, the correct code is G41. G41 may be programmed with or without position data in the same data block. Refer to Chapter 2 for additional information. G42 Tool Nose Radius Compensation - Workpiece Left of Tool (Group 7 G Code) Tool Nose Radius Compensation with the workpiece to the left of the tool is established by programming G42. Imagine the operator sitting on the tool facing in the direction of the tool motion. If the workpiece is to the left of the operator, the correct code is G42. G42 may be programmed with or without position data in the same data block. Refer to Chapter 2 for additional information. G50 Maximum RPM Limit (Group 0 G Code) The G50 command is used with Constant Surface Speed to establish a spindle rpm limit. The following example establishes a spindle speed limit of 4000 rpm. Example: G50 S4000; A Control OFF cancels a G50 rpm limit. Refer to Chapter 9 for additional information on Constant Surface Speed. M-504A 1-19

48 G65 Macro Call (Group 0 G Code) To activate a particular macro and have it executed from the current slide position, program the following macro call command: G65 P ; Where: G65 = Macro Call Command P = Macro Program Number The G65 command is non-modal. After the G65 command block is executed, G65 mode is deactivated. Refer to Chapter 9 for additional information on the G65 Macro Call command. G70 Automatic Finishing Cycle (Group 0 G Code) The G70 command is used in conjunction with canned roughing cycles G71, G72, or G73 to specify the section of the workpiece to be finish contoured. The G70 data block specifies the first and last block in the part program controlling the section to be finish contoured. Refer to the following sections for additional information: G71 Automatic Turning Cycle, in Chapter 6 G72 Automatic Facing Cycle, in Chapter 6 G73 Automatic Pattern Repeat Cycle, in Chapter 6 G71 Automatic Turning Cycle (Group 0 G Code) The G71 canned cycle provides the programmer with the capability to program rough contouring of a workpiece with multiple turning passes. This automatic cycle is usually used in conjunction with the G70 Auto Finishing Cycle. The G71 blocks specify the amount of stock to be removed on each roughing pass, the amount of stock to be left for finish contouring, and the first and last block in the part program controlling the rough contouring. Refer to Chapter 6 for additional information on the G71 Automatic Turning Cycle. G72 Automatic Facing Cycle (Group 0 G Code) The G72 canned cycle provides the programmer with the capability to program rough contouring of a workpiece with multiple facing passes. This automatic cycle is usually used in conjunction with the G70 Auto Finishing Cycle. The G72 blocks specify the amount of stock to be removed on each roughing pass, the amount of stock to be left for finish contouring, and the first and last block in the part program controlling the rough contouring. Refer to Chapter 6 for additional information G72 Automatic Facing Cycle M-504A

49 G73 Automatic Pattern Repeat Cycle (Group 0 G Code) The G73 canned cycle provides the programmer with the capability to program rough contouring repeatedly cutting a fixed pattern (contour). This automatic cycle is usually used in conjunction with the G70 Auto Finishing Cycle. The G73 blocks specify the incremental distance between the first and last roughing pass, the number of roughing passes, and the first and last block in the part program controlling the rough contouring. Refer to Chapter 6 for additional information on the G73 Automatic Pattern Repeat Cycle. G74 Automatic Drilling Cycle (Constant Depth Increments) (Group 0 G Code) The G74 command activates an automatic drilling cycle that uses constant depth increments. In the G74 block, the programmer specifies the hole depth, size of depth increment, and drilling feedrate. The G74 command is non-modal, it is effective only in the block in which it is programmed. Refer to Chapter 6 for additional information on the G74 Constant Depth Increment Automatic Drilling Cycle. G75 Automatic Grooving Cycle (Group 0 G Code) The G75 command activates an automatic grooving cycle that uses constant depth increments. All information for the G75 Auto grooving Cycle is programmed in two data blocks. The G75 command is non-modal; it is effective only in the blocks in which it is programmed. Refer to Chapter 6 for additional information on the G75 Automatic Grooving Cycle. G76 Automatic Threading Cycle (Group 0 G Code) The G76 Automatic Threading Cycle provides the programmer with the capability to program multiple threading passes with two blocks of information instead of programming four blocks per threading pass. The G76 command is non-modal and is canceled when the threading cycle is completed. Straight and tapered threads using plunge or compound infeed can be programmed. The Feedrate Override switch is not effective during the threading pass unless it is set to 0%. Setting the Feedrate Override switch to 0% during a threading pass will stop X and Z axis motion. The Feedrate Override switch is active during the return pass. The Emergency Stop push button and Reset key are active during the threading pass. The Feed Hold push button is not active during the threading pass. Refer to Chapter 7 for additional information on the G76 Automatic Threading Cycle. M-504A 1-21

50 G80 Cancel Machining Cycle (Group 10 G Code) The G80 command is used to cancel the following cycles: G83 Z Axis Drilling Cycle G84 Z Axis Tapping Cycle G85 Z Axis Boring Cycle G87 X Axis Drilling Cycle G88 X Axis Tapping Cycle G89 X Axis Boring Cycle Refer to Chapter 8 for additional information on the G80 command. G83 Z Axis Drilling Cycle (Group 10 G Code) The G83 command is used to activate either a single pass drill cycle or a peck drill cycle that uses constant depth increments to drill parallel with the spindle centerline. When drilling is completed, the tool will retract to the start point of the drilling cycle. The retract move will be performed at rapid traverse rate. The G83 cycle is programmed in one data block. G83 remains effective until canceled by another Group 10 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G83 Z Axis Drilling Cycle. G84 Right-Hand Z Axis Tapping Cycle (Group 10 G Code) The G84 command activates a right-hand tapping cycle to tap parallel with the spindle centerline. When the tapping is completed, the spindle will reverse direction and the tap will feed back to the R point and rapid to the start point of the tapping cycle. The G84 cycle is programmed in one data block. G84 remains effective until canceled by another Group 10 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G84 Right-Hand Z Axis Tapping Cycle. G85 Z Axis Boring Cycle (Group 10 G Code) The G85 command activates a boring cycle to bore parallel with the spindle centerline. After the boring tool reaches the programmed depth, the tool will continue to rotate and retract at the programmed feedrate to the return point specified by the R word. The tool will then rapid to the start point of the boring cycle. The G85 cycle is programmed in one data block. G85 remains effective until canceled by another Group 9 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G85 Z Axis Boring Cycle M-504A

51 G87 X Axis Drilling Cycle (Group 10 G Code) The G87 command is used to activate either a single pass drill cycle or a peck drill cycle that uses constant depth increments to drill perpendicular to the spindle centerline. When drilling is completed, the tool will retract to the start point of the drilling cycle. The retract move will be performed at rapid traverse rate. The G87 cycle is programmed in one data block. G87 remains effective until canceled by another Group 10 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G87 X Axis Drilling Cycle. G88 Right-Hand X Axis Tapping Cycle (Group 10 G Code) The G88 command activates a right-hand tapping cycle to tap perpendicular to the spindle centerline. When the tapping is completed, the spindle will reverse direction and the tap will feed back to the R point and rapid to the start point of the tapping cycle. The G88 cycle is programmed in one data block. G88 remains effective until canceled by another Group 10 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G88 Right-Hand X Axis Tapping Cycle. G89 X Axis Boring Cycle (Group 10 G Code) The G89 command activates a boring cycle to bore perpendicular with the spindle centerline. After the boring tool reaches the programmed depth, the tool will continue to rotate and retract at the programmed feedrate to the return point specified by the R word. The tool will then rapid to the start point of the boring cycle. The G89 cycle is programmed in one data block. G89 remains effective until canceled by another Group 10 G code or a Group 1 G code. Refer to Chapter 8 for additional information on the G89 X Axis Boring Cycle. G90 Canned Turning Cycle (Group 1 G Code) The G90 Canned Turning Cycle provides the programmer with the capability to program multiple turning passes by specifying only the depth of cut in each data block after the G90 block. Straight or tapered turn operations may be performed. The G90 command is modal. A programmed G90 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G90 command. G90 can also be canceled by a control OFF or Reset. The Spindle Increase Override and Decrease Override push buttons, Feedrate Override switch, and Feed Hold push button are active. Refer to Chapter 6 for additional information on the G90 Canned Turning Cycle. M-504A 1-23

52 G92 Canned Threading Cycle (Group 1 G Code) The G92 Canned Threading Cycle provides the programmer with the capability to program multiple threading passes by specifying only the depth of cut in each data block after the G92 block. Straight or tapered threads may be cut in this mode. Compound infeeding is not possible in this mode. The G92 command is modal. A programmed G92 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G92 command. G92 can also be canceled by a control OFF or Reset. The Feed Hold push button is not active during the threading pass, but is active during the return pass. The Feedrate Override switch is not effective during the threading pass unless it is set to 0%. Setting the Feedrate Override switch to 0% during a threading pass will stop X and Z axis motion. The Feedrate Override switch is active during the return pass. The Emergency Stop push button and Reset key are active during the threading pass. Refer to Chapter 7 for additional information on the G92 Canned Threading Cycle. G94 Canned Facing Cycle (Group 1 G Code) The G94 Canned Facing Cycle provides the programmer with the capability to program multiple facing passes by specifying only the depth of cut in each data block after the G94 block. Straight or tapered facing operations may be performed. The G94 command is modal. A programmed G94 command will cancel any currently active Group 1 G code. Any other Group 1 G code will cancel an active G94 command. G94 can also be canceled by a control OFF or Reset. The Feedrate Override switch and Feed Hold push button are active. Refer to Chapter 6 for additional information on the G94 Canned Facing Cycle. G96 Constant Surface Speed (Group 2 G Code) The G96 mode allows programming the speed of the workpiece with respect to the tool point directly in surface feet per minute in inch mode (G20) and surface meters per minute in metric mode (G21). Constant Surface Speed is a function of the spindle speed range and the programmed constant surface speed (S word). The control automatically adjusts the spindle speed within its range to maintain the constant surface speed as the cutting radius varies. Refer to G50 Maximum RPM Limit for limiting spindle rpm while using G96 programming. G96 is canceled by G97. If a new spindle speed is not programmed, the spindle will remain at the speed that was active when Constant Surface Speed was canceled. Refer to Chapter 9 for additional information on Constant Surface Speed M-504A

53 G97 Direct RPM Programming (Constant Surface Speed Cancel) (Group 2 G Code) G97 allows the programmer to program spindle speeds directly in revolutions per minute. When G97 cancels G96, the spindle speed in rpm equals the speed at which the spindle was turning when Constant Surface Speed was canceled. If a different spindle speed is desired, an S word specifying the new spindle speed should be programmed in the same block as the G97 command. The S word format for direct rpm programming is S4.0 G98 Inches / Millimeter per Minute Feedrate (Group 5 G Code) The feedrate (F word) is programmed directly in inches/mm per minute. The feedrate remains unchanged until reprogrammed. Refer to the tables beginning on page 1-2 for data word formats. When entering G98 mode, a new feedrate should be programmed. G98 is modal and cancels G99. The decimal point must be programmed. The following examples are written for inch mode (G20): Example 1: F100 results in a feedrate of 1.00 inches per minute. Example 2: F100. results in a feedrate of inches per minute. G99 Inches / Millimeter per Revolution Feedrate (Group 5 G Code) This is the power-up or reset state. The feedrate (F word) is programmed directly in inches/mm per revolution. The feedrate remains unchanged until reprogrammed. Refer to the tables beginning on page 1-2 for data word formats. The last active spindle (main spindle, sub-spindle, or live tool spindle) will be used for controlling inch [millimeter] per revolution feedrates. The maximum programmable feedrates are inches/revolution and millimeters/revolution. When entering G99 mode, a new feedrate should be programmed. G99 is modal and cancels G98. G107 Cylindrical Interpolation (Group 0 G Code) The G107 command activates cylindrical interpolation for C Axis programming. Refer to Chapter 12 for additional information. G112 Polar Interpolation (Group 21 G Code) The G112 command activates polar interpolation for C Axis programming. Refer to Chapter 12 for additional information. G113 Cancel Polar Interpolation (Group 21 G Code) The G113 command cancels polar interpolation. Refer to Chapter 12 for additional information. M-504A 1-25

54 X WORD NOTICE Programming an X axis move without the correct Tool or Zero Offset active could cause the tool to strike a spindle or workpiece. The X word is a DIAMETER DIMENSION for the machine cross slide. It is measured relative to the spindle centerline and is written with an X followed by a plus or minus sign. The plus sign may be omitted because the control assumes plus (+) if no sign is programmed. The X command establishes the absolute position of a turret top plate reference location in relation to the spindle centerline after movement has been completed. - NOTE - Refer to Appendix One for travel specifications. Only one X command is permitted in a data block. If more than one X command is programmed in a data block, the control will act on the X command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. X is positive when the turret reference point is programmed to move to a position behind the spindle centerline. X is negative when the turret reference point is programmed to move to a position in front of the spindle centerline. X axis programming resolution is discussed under Diameter Programming, page With no tool offset active and no work shift (zero offset) active, all programmed motions will be the final position of the turret reference point in relation to the spindle centerline. The position will be displayed as a diameter whose center is on the spindle centerline. When X axis tool offsets are activated by an offset command (T word), the programmed position will be modified according to the offset. Example: A command of X2.5 will cause the control to position the cross slide with the turret reference point 1.25 inches behind the spindle centerline. A work shift (zero offset) can be used to establish a work coordinate system in which X0 does not coincide with the spindle centerline. If X0 for the work coordinate system used is not on the spindle centerline, all programmed motions will be relative to the X0 established by the work shift. Refer to Chapter 4 for information regarding the work shift. The X word is also used to give a time factor to a Dwell command (G04). Refer to G04 Dwell, page M-504A

55 U WORD NOTICE Programming a U axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike a spindle or workpiece. The U command establishes the incremental move of the cross slide position in relation to the current cross slide location. Only one U command is permitted in a data block. If more than one U command is programmed in a data block, the control will act on the U command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. U is positive when the cross slide is programmed to move toward the back of the machine. U is negative when the cross slide is programmed to move toward the front of the machine. Example: A command of U2.5 will cause the control to position the cross slide 1.25 inches in the +X direction from the previous position on the X axis. The U word is also used to give a time factor to a Dwell command (G04). Refer to G04 Dwell, page M-504A 1-27

56 Z WORD NOTICE Programming a Z axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike a spindle or workpiece. The Z word is a distance command for the machine carriage. It is measured relative to the main spindle face and is written with a Z followed by a plus (+) or minus (-) sign. The plus sign may be omitted because the control assumes plus (+) if no sign is programmed. - NOTE - Refer to Appendix One for travel specifications. Only one Z command is permitted in a data block. If more than one Z command is programmed in a data block, the control will act on the Z command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. Assuming tool offsets are inactive, Z is positive when the turret reference point is programmed to the right of Z0 on the Machine Work Coordinate System. Z is negative when the turret reference point is programmed to the left of Z0 on the Machine Work Coordinate System. With no tool offset active and no work shift (zero offset) active, all programmed Z axis movements will be the final position of the turret reference position in relation to the main spindle face. Since all carriage movement must take place to the right of the headstock, all movements regardless of direction will be plus (+). When a tool offset and/or a zero offset are active, the programmed position will be modified accordingly. Example: A command of Z5. with a feedrate will cause the control to position the carriage with the turret reference position 5 inches from the main spindle face. A command of Z9. with a feedrate will cause the control to position the carriage with the turret reference position 9 inches from the main spindle face. A work shift (zero offset) is used to establish a work coordinate system in which Z0 does not coincide with the main spindle face. If Z0 for the work coordinate system used is not the main spindle face, all programmed Z axis movements will be relative to the Z0 established by the work shift. A positive Z value describes a coordinate point to the right of the Z0 point. A negative Z value describes a coordinate point to the left of the Z0 point M-504A

57 W WORD NOTICE Programming a W axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike a spindle or workpiece. The W command establishes the incremental move of the carriage in relation to the current carriage location. Only one W command is permitted in a data block. If more than one W command is programmed in a data block, the control will act on the W command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. W is positive when the carriage is programmed to move away from the main spindle face. W is negative when the carriage is programmed to move toward the main spindle face. Example: A command of W5. with a feedrate will cause the control to position the carriage 5 inches in the +Z direction from the previous position on the Z axis. A command of W-5. with a feedrate will cause the control to position the carriage 5 inches in the -Z direction from the previous position on the Z axis. M-504A 1-29

58 Y WORD [Option] NOTICE Programming a Y axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike the workpiece. The Y axis option allows off-center machining at the spindle(s). The Y word is an absolute distance command for the turret. The Y coordinate is measured relative to the spindle centerline and is written with a Y followed by a plus (+) or minus (-) sign. The plus sign may be omitted because the control assumes plus (+) if no sign is programmed. - NOTE - Refer to Appendix One for Y axis travel specifications. Only one Y command is permitted in a data block. If more than one Y command is programmed in a data block, the control will act on the Y command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. Y is positive when the reference point is programmed above the spindle centerline. Y is negative when the reference point is programmed below the spindle centerline. Refer to Figure 1.2, page 1-7. With no tool offset active and no work shift (zero offset) active, all programmed Y axis movements will be the final position of the turret reference point in relation to the spindle centerline. Example: A command of Y1. with a feedrate will cause the control to position the turret with the reference point 1 inch above the spindle centerline. A command of Y-1. with a feedrate will cause the control to position the turret with the reference point 1 inch below the spindle centerline M-504A

59 V WORD [Option] NOTICE Programming a V axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike the workpiece. The V command establishes the incremental move of the turret on the Y axis. This incremental move is in relation to the current turret location on the Y axis. Only one V command is permitted in a data block. If more than one V command is programmed in a data block, the control will act on the V command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. V is positive when the turret is programmed to move away from the machine base. V is negative when the turret is programmed to move toward the machine base. Example: A command of V1. with a feedrate will cause the control to position the turret 1 inch in the +Y direction from the previous position on the Y axis. A command of V-1. with a feedrate will cause the control to position the turret 1 inch in the -Y direction from the previous position on the Y axis. E WORD - NOTE - When machining on the sub-spindle, it is recommended that the sub-spindle be located at the E axis reference position. There is no incremental movement command for the E axis. Refer to Appendix One for travel specifications. The E word is a absolute distance command for the tailstock or sub-spindle. It is measured relative to the main spindle face and is written with a E followed by a plus (+) or minus (-) sign. The plus sign may be omitted because the control assumes plus (+) if no sign is programmed. Only one E command is permitted in a data block. If more than one E command is programmed in a data block, the control will act on the E command programmed closest to the End of Block character. Refer to the tables beginning on page 1-2 for data word formats. M-504A 1-31

60 A WORD [Option] The A word is an absolute C axis command for the optional sub-spindle. The C axis feature provides the programmer with the following machining capabilities: - Live Tooling with Spindle Orient - Polar Coordinate Interpolation (face milling) - Cylindrical Interpolation (contoured milling on the O.D.) Refer to Chapters 11 and 12 for additional information. B WORD The B word is a spindle orient command. The spindle is stopped in relation to the spindle 0 (zero) degree mark. Refer to Chapter 11 for additional information. C WORD The C word is an absolute C axis command for the main spindle. The C axis feature provides the programmer with the following machining capabilities: - Live Tooling with Spindle Orient - Polar Coordinate Interpolation (face milling) - Cylindrical Interpolation (contoured milling on the O.D.) Refer to Chapters 11 and 12 for additional information. H WORD The H word is an incremental C axis command. The C axis feature provides the programmer with the following machining capabilities: - Live Tooling with Spindle Orient - Polar Coordinate Interpolation (face milling) - Cylindrical Interpolation (contoured milling on the O.D.) Refer to Chapters 11 and 12 for additional information. I WORD The I word is used during Circular Interpolation (G02/G03). The I word is a signed value defining the distance on the X axis from the start point of an arc to the arc center. The sign is a result of the coordinate direction from the start point to the arc center. Refer to the tables beginning on page 1-2 for data word formats. Refer to Circular Interpolation, in Chapter 3. J WORD The J word is used during Circular Interpolation (G02/G03). The J word is a signed value defining the distance on the Y axis from the start point of an arc to the arc center. The sign is a result of the coordinate direction from the start point to the arc center. Refer to the tables beginning on page 1-2 for data word formats. Refer to Circular Interpolation, in Chapter M-504A

61 K WORD The K word is used during Circular Interpolation and Variable Lead Threadcutting. Circular Interpolation (G02 / G03) The K word is used during Circular Interpolation (G02/G03). The K word is a signed value defining the distance on the Z axis from the start point of an arc to the arc center. The sign is a result of the coordinate direction from the start point to the arc center. Refer to the tables beginning on page 1-2 for data word formats. Refer to Circular Interpolation, in Chapter 3. Variable Lead Threading (G34) The K word specifies the change in thread lead per spindle revolution. The value is positive for an increasing lead and negative for a decreasing lead. Refer to the tables beginning on page 1-2 for data word formats. Refer to Variable Lead Threadcutting, in Chapter 7. R WORD Linear Interpolation (G01) When Linear Interpolation (G01) is active,,r defines the numerical values of a corner radius between any linear (G01) moves. Refer to the tables beginning on page 1-2 for data word formats. Refer to Insert Chamfer or Corner Radius, in Chapter 3. Circular Interpolation (G02 / G03) When Circular Interpolation (G02 or G03) is active, R defines the numerical value of a radius connecting two points. Refer to the tables beginning on page 1-2 for data word formats. Refer to Circular Interpolation, in Chapter 3. Tool Nose Radius Compensation (G41 / G42) When Tool Nose Radius Compensation (G41 or G42) is active, R defines the numerical value of the tool nose radius. Values are stored in the Tool Offset Tables and are activated by a T command. Refer to the tables beginning on page 1-2 for data word formats. Refer to Chapter 2 for additional information. Defining Tapers When used with the following cycles, the R word defines the amount of taper when a tapered turning, threading, or facing cycle is executed: G76 Multiple Repetitive Threading Cycle, Chapter 7 G90 Canned Turning Cycle, Chapter 6 G92 Canned Threading Cycle, Chapter 7 G94 Canned Facing Cycle, Chapter 6 M-504A 1-33

62 P WORD - NOTE - Decimal point programming cannot be used with the P word. Leading zero suppression must be used. Refer to the tables beginning on page 1-2 for the data word format. The P word is used in the following functions: G04 Dwell, page 1-14 G70 Automatic Finishing Cycle, in Chapter 6 G71 Multiple Repetitive Rough Turning Cycle, in Chapter 6 G72 Multiple Repetitive Rough Facing Cycle, in Chapter 6 G73 Rough Pattern Repeat Cycle, in Chapter 6 G80 Series Cycles, Chapter 8 Subprogram Calling, in Chapter 9 Program Entry of Tool Offsets, in Chapter 4 Program Entry of Work Shift, in Chapter 4 Spindle Selection Machining Cycles When used with the G71, G72, and G73 cycles, the P word specifies the sequence number of the first block in the program section that controls the workpiece area being rough contoured. When used with the G70 cycle, the P word specifies the sequence number of the first block in the program section that controls the workpiece area being finish contoured. Subprogram Calling When used with subprogram calling, the P word appears in the M98 calling block of the main part program and specifies the program number of the subprogram to be called. Tool Offsets and Work Shift When used with program entry of tool offsets or work shift offsets, the P word specifies the offset number and has the following numerical ranges: P00 when used with Work shift Offset P01 to P99 when used with tool wear offsets P10001 to P10099 when used with tool geometry offsets Refer to Chapter 4 for information on storing tool offsets and work shift in memory M-504A

63 Spindle Selection When used for spindle selection, the P word is used to specify which spindle will be commanded by a programmed S word (spindle speed). Once the P word has been programmed to select a spindle, it is not necessary to program the P word again unless a different spindle is to be commanded. When used for spindle selection, the data word format is P1. Spindle selection is assigned as follows: P1 = Main Spindle P2 = Sub-Spindle [Option] P3 = Live Tooling (BMT turret top plates only) Programming Format: S P_ ; Q WORD The Q word is used in the following functions: G70 Automatic Finishing Cycle, Chapter 6 G71 Multiple Repetitive Rough Turning Cycle, Chapter 6 G72 Multiple Repetitive Rough Facing Cycle, Chapter 6 G73 Rough Pattern Repeat Cycle, Chapter 6 G83/G87 Drilling Cycles, in Chapter 8 Program Entry of Tool Offsets, Chapter 4 Programming the Tailstock, Chapter 9 When used with the G71, G72, and G73 cycles, the Q word specifies the Sequence Number of the last block in the program section that controls the workpiece area being rough contoured. When used with the G70 cycle, the Q word specifies the sequence number of the last block in the program section that controls the workpiece area being finish contoured. The data word format is Q4. Leading zeros may be omitted. When used with the G83 and G87 cycles, the Q word specifies the depth of each drilling pass during a peck drill operation. Refer to Chapter 8 for additional information. When tool geometry offsets are entered by tape, the Q word specifies the tool tip orientation number. The data word format is Q1, with numerical values ranging from 0 to 9. Refer to Tool Offsets, in Chapter 4. M-504A 1-35

64 F WORD The F word is used to establish a feedrate. When used with the G98 command, it expresses the feedrate in inches or millimeters per minute. When used with the G99 command, it expresses the feedrate in inches or millimeters per revolution. If more than one feedrate is programmed in a data block, the last feedrate programmed will be the active feedrate. Refer to the tables beginning on page 1-2 for data word formats. The decimal point must be programmed. Due to the maximum feedrates on the X, Y, and Z axes, the feedrate in G99 mode is Lead Limited. When G99 mode is active, the maximum feedrate in G01 mode is derived from the following formulas: Maximum Feedrate (in/min) = inches per minute revolutions/minute Maximum Feedrate (mm/min) = millimeters per minute revolutions/minute The maximum programmable feedrate for the E, X, Y, and Z axes is: 150 inches per minute 3810 millimeters per minute The F word, which can be placed anywhere in the data block, remains unchanged until reprogrammed. If G00 is used to obtain the rapid traverse rate, be sure it is canceled by another Group 1 G code after the rapid traverse move is completed. The Feedrate Override switch modifies the programmed feedrate from 0% (Feed Hold) to 150%. When Dry Run mode is active, the control causes all slide motion to take place at a feedrate selected with the Feedrate Override switch M-504A

65 S WORD NOTICE Hardinge recommends that the spindle speed does not exceed 4,200 rpm for machines used with a bar feed. - NOTE - A P word is used to specify which spindle will be commanded by a programmed S word. Refer to page 1-35 for information on using the P word for spindle selection. Do not program a decimal point with the S word. The S word has several functions, depending on the G code it is associated with: CODE FUNCTION: G50 S word selects the spindle rpm limit for Constant Surface Speed G96 S word specifies surface feet/meters per minute in Constant Surface Speed G97 S word selects direct spindle rpm When used with G50, the S word specifies the maximum rpm the spindle can attain during Constant Surface Speed programming (G96). In G96 Constant Surface Speed programming, the format is S4 in both inch and metric modes. The units are surface feet per minute in inch mode (G20) and surface meters per minute in metric mode (G21). Refer to Constant Surface Speed, in Chapter 9. When used in G97 direct rpm mode, the word format is S4. - NOTE - Base speed is the minimum spindle speed for machining. The effective spindle speed range for the main spindle and optional sub-spindle is as follows: Machine Model Main Spindle Base Speed / Maximum Speed Optional Sub-Spindle Base Speed / Maximum Speed T-42 Lathe (16C Main Spindle) T-42 Big-Bore Lathe (20C Main Spindle) T-51 Lathe (20C Main Spindle) T-65 Lathe (25C Main Spindle) 750 / 6, / 6, / 5, / 6, / / 5, / / 5,000 The S word is modal, and once programmed, need not be programmed again until a different spindle speed is required. M-504A 1-37

66 7 16 T WORD - NOTE - On machines equipped with the Y axis option, the turret will not index if the turret is positioned below Y0. Refer to Y Word, page 1-30, for additional information. T-42 machines equipped with BMT 45 turret top plates are capable of half station indexing. Full stations are numbered 1 through 16. Half stations are numbered 17 through 32. Refer to Figure 1.3 for turret station numbers. Refer to Figure 1.4 for turret indexing examples Full Station Numbers Half Station Numbers TI5673 Figure Turret Station Numbers (BMT 45 Top Plate) Machine Spindle Machine Spindle Full Station Index, TurretatStation13 Half Station Index, TurretatStation29 Figure Turret Indexing Examples (BMT 45 Top Plate) TI M-504A

67 T-51 and T-65 machines equipped with BMT 55 turret top plates are capable of half station indexing. Full stations are numbered 1 through 12. Half stations are numbered 13 through 24. Refer to Figure 1.5 for turret station numbers. Refer to Figure 1.6 for turret indexing examples Half Station Numbers Full Station Numbers TI5837 Figure Turret Station Numbers (BMT 55 Top Plate) Machine Spindle Machine Spindle Full Station Index, TurretatStation10 Half Station Index, TurretatStation22 TI5838 Figure Turret Indexing Examples (BMT 55 Top Plate) M-504A 1-39

68 Machines equipped with Hardinge top plates are NOT capable of half station indexing. Turret stations are numbered 1 through 12. The T word selects the turret station that is to be indexed to the cutting position and activates the Tool Offset number. The Tool Offset number selects the following: Tool Geometry Offset File: 1. X and Z axis Tool Dimensions. 2. Tool Nose Radius Value. 3. Tool Orientation Number. Tool Wear Offset File: 1. X and Z axis Tool Wear adjustments. The T word has the word format T4. The first two digits specify the turret station and the last two digits specify the location of the tool offsets. Note that both the geometry and wear offsets are activated by the last two digits. Example: N0120 T0515; Block N0120 calls for turret station 5. Tool geometry offsets on line 15 of the Tool Offset Geometry File will be activated and tool wear offsets on line 15 of the Tool Wear File will also be activated. NOTICE If no tool offsets are to be activated, the last two digits MUST be 00. If no digits are programmed in the last two places, the turret will not index. Instead, the control will use the turret station number as an offset and activate that offset. This could result in a collision as the control will attempt to position the previously active tool using incorrect offsets or no offsets at all. For example, if the turret is to be indexed to station 5 without an offset, T0500 must be programmed. If T05 is programmed, the turret will not be indexed to station 5, but offset 05 will be activated. - NOTE - When the Hardinge Safe Index formats are used, it is not necessary to program T0" before indexing to a new turret station. T0" is included in the Safe Index subprograms. Refer to Chapter 9 for information on Safe Index subprograms. A turret command of T0" should be inserted before indexing to a new turret station and at the end of each operation to cause the active tool offsets to be cleared from the offset registers. Refer to Chapter 4 for additional information on tool offsets M-504A

69 M WORD M codes convey action to the machine. They are known as miscellaneous functions and are designated by a programmed M word having the format M3. Only one M code is allowed in a data block. If more than one M code is programmed in a block from the keyboard or tape, the last M code entered will be the active M code. Refer also to the M code chart in Appendix Two. The M code may be placed anywhere in the data block. M00 Program Stop The M00 command stops the program, stops the spindle, and turns the coolant off. The Collet Open/Close push button is enabled. This function can be used for gauging and end-for-ending the workpiece. Pressing Cycle Start causes the program to continue. It is the programmer s responsibility to program an M03, M04, M08, M13, M14, M51, M52, M53, or M54 to restart the spindle, live tooling, and/or coolant pump when restarting the program after an M00 Program Stop. M01 Optional Stop The M01 command performs the same function as M00, if the Optional Stop push button on the control panel has been activated before the block containing the M01 is read by the control. If the Optional Stop push button has not been activated by the operator, the control will ignore the programmed M01 and will continue to execute the program. This function is useful when it is necessary to gauge the workpiece during setup. Pressing Cycle Start causes the program to continue. It is the programmer s responsibility to program an M03, M04, M08, M13, M14, M51, M52, M53, or M54 to restart the spindle, live tooling, and/or coolant pump(s) when restarting the program after an M01 Optional Stop. M03 Main Spindle Forward M03 commands the main spindle to run in the forward direction at the programmed spindle speed (S word). The spindle is running in the forward direction when rotating clockwise as viewed from the main spindle end of the machine. M03 remains active until canceled by M00, M01, M04, M05, M14, M30, or by pressing the Reset key or Emergency Stop push button. M04 Main Spindle Reverse M04 commands the main spindle to run in the reverse direction at the programmed spindle speed (S word). The spindle is running in the reverse direction when rotating counterclockwise as viewed from the main spindle end of the machine. M04 remains active until canceled by M00, M01, M03, M05, M13, M30, or by pressing the Reset key or Emergency Stop push button. M05 Main Spindle Stop / Coolant OFF M05 commands the main spindle to stop and turns the coolant off, but DOES NOT stop axis motion unless G99 is active. M05 remains active until canceled by M03, M04, M13, or M14. M05 is active at machine start-up and can also be activated by M00, M01, M30, Reset, and Emergency Stop. M07 Sub-Spindle Phase Synchronization with Main Spindle [Option] M07 commands the rotational direction, velocity, and orientation of the sub-spindle to match the main spindle. M07 is canceled by any standard spindle command on the main spindle or sub-spindle. M-504A 1-41

70 M08 Coolant ON M08 activates the turret coolant pump and remains active until canceled by M00, M01, M05, M09, M30, Reset, or Emergency Stop. M09 Coolant OFF M09 deactivates the turret coolant pump and remains effective until canceled by M08, M13, M14, M53, or M54. M09 is active at machine start-up and is activated by M00, M01, M05, M30, Reset, or Emergency Stop. M10 High Pressure Coolant ON [Option] M10 commands all high pressure coolant to be turned ON if this option is activated. The spindle must be rotating and the guard door must be closed to activate the high pressure coolant feature. M10 remains active until canceled by M00, M01, M11, M30, or Emergency Stop. M11 High Pressure Coolant OFF [Option] M11 commands all high pressure coolant to be turned OFF. M11 is active at machine start-up and remains active until canceled by M10. M12 Turret Coolant OFF [Option] M12 turns the turret coolant OFF if thru-spindle coolant is ON. M13 Main Spindle Forward / Coolant ON M13 commands the main spindle to run in the forward direction at the programmed spindle speed (S word) and turns the coolant pump ON. The main spindle is running in the forward direction when rotating clockwise as viewed from the main spindle end of the machine. M13 remains active until canceled by M00, M01, M04, M05, M14, M30, or by pressing the Reset key or Emergency Stop push button. If M04 is programmed after M13, the main spindle will run in the reverse direction and the coolant pump will remain ON. M14 Main Spindle Reverse / Coolant ON M14 commands the main spindle to run in the reverse direction at the programmed spindle speed (S word) and turns the coolant pump ON. The main spindle is running in the reverse direction when rotating counterclockwise as viewed from the main spindle end of the machine. M14 remains active until canceled by M00, M01, M03, M05, M13, M30, or by pressing the Reset key or Emergency Stop push button. If M03 is programmed after M14, the main spindle will run in the forward direction and the coolant pump will remain ON M-504A

71 M15 Thru-Spindle Coolant ON, Main Spindle [Option] The M15 command causes the thru-spindle coolant at the main spindle to turn ON. M15 remains active until canceled by M16, M30, control Reset, or control OFF. Refer to M215 for the equivalent command for the sub-spindle. M16 Thru-Spindle Coolant OFF, Main Spindle [Option] The M16 command causes the thru-spindle coolant at the main spindle to turn OFF. M16 remains active until canceled by M15. Refer to M216 for the equivalent command for the sub-spindle. M20 Speed Arrival Check ON M20 commands the control not to move the machine axes until the spindle reaches the programmed spindle speed. M20 remains active until canceled by M30, M60, control Reset, or control OFF. M21 Main Spindle Collet / Chuck Open M21 commands the main spindle collet closer to release the workpiece. M21 remains active until canceled by M22. M22 Main Spindle Collet / Chuck Close M22 commands the main spindle collet closer to grip the workpiece. M22 remains active until canceled by M21. M23 Main Spindle Contouring Mode ON M23 activates main spindle contouring mode for C Axis programming. Refer to Chapter 12 for additional information. Refer to M223 for the equivalent command for the sub-spindle. M24 Main Spindle Contouring Mode OFF M24 cancels main spindle contouring mode, which is used for C Axis programming. Refer to Chapter 12 for additional information. Refer to M224 for the equivalent command for the sub-spindle. M25 Main Spindle Part Catcher Retract [Option] The M25 command extends the part conveyor into the work envelope; then, retracts the headwall part catcher to deliver the part to the part conveyor. The conveyor retracts from the work envelope and rotates to deliver the part to the unload ramp at the left end of the machine. M-504A 1-43

72 M26 Main Spindle Part Catcher Extend [Option] The M26 command moves the headwall part catcher to the part pickup position at the main spindle. M27 Main Spindle Internal Chucking Mode The M27 command establishes the operation of the main spindle collet closer to support internal gripping work-holding devices. Refer to the operator s manual (M-505) for information on establishing chucking modes. M28 Main Spindle External Chucking Mode The M28 command establishes the operation of the main spindle collet closer to support external gripping work-holding devices. Refer to the operator s manual (M-505) for information on establishing chucking modes. M29 Rigid Tapping Mode The M29 command activates rigid tapping mode. Refer to Chapter 7 for information on rigid tapping mode. M30 End of Program, Auto Door Open M30 indicates the end of a program and is usually found in the last block programmed. It stops the spindle, turns the coolant OFF, rewinds the program to the beginning, and opens the optional auto door. The Collet Open/Close push button is enabled. M32 Spindle Synchronization [Option] M32 commands the optional sub-spindle to match direction and speed with the main spindle. M32 is canceled by any standard spindle command on the main spindle or sub-spindle. M33 Sub-Spindle Forward [Option] M33 commands the sub-spindle to run in the forward direction at the programmed spindle speed (S word). The sub-spindle is running in the forward direction when rotating clockwise as viewed from the main spindle end of the machine. M33 remains active until canceled by M00, M01, M30, M34, M35, or by pressing the Reset key or Emergency Stop push button. M34 Sub-Spindle Reverse [Option] M34 commands the sub-spindle to run in the reverse direction at the programmed spindle speed (S word). The sub-spindle is running in the reverse direction when rotating counterclockwise as viewed from the main spindle end of the machine. M34 remains active until canceled by M00, M01, M30, M33, M35, or by pressing the Reset key or Emergency Stop push button M-504A

73 M35 Sub-Spindle Stop [Option] M35 commands the sub-spindle to stop, but DOES NOT stop axis motion unless G99 is active. M35 remains active until canceled by M33 or M34. M35 is active at machine start-up and can also be activated by M00, M01, M30, Reset, and Emergency Stop. M36 Air Blast ON [Option] M36 activates the main spindle air blast. M37 Air Blast OFF [Option] M37 deactivates the main spindle air blast. M38 Auto Door Open [Option] M38 commands the main coolant guard door to open. M42 No Corner Rounding - Exact Stop M42 is a modal command activating Exact Stop. Exact Stop permits a programmed position exactly. The feedrate is decreased until it is equal to zero and the following error is eliminated. M42 is canceled by M30, M43, or Reset. M43 Corner Rounding M43 is a modal command which is used if no exact position stop is desired from one block to the next. M43 is active at machine power-up, after an M30 command, and after the control has been reset. M43 cancels M42 Exact Stop. M44 Enable Turret Bi-Directional Index M44 enables the bi-directional indexing feature of the control. M44 is active on machine power-up. M44 is modal and cancels M45. M44 can be canceled by programming an M45 command. M45 Disable Turret Bi-Directional Index M45 disables the bi-directional indexing feature of the control. When M45 is active, the turret top plate will rotate only in a clockwise direction, as viewed from the spindle. M45 is modal and cancels M44. M45 can be canceled by programming an M44 command or powering down the control. M46 Sub-Spindle Air Blast ON [Option] M46 activates the sub-spindle air blast. M47 Sub-Spindle Air Blast OFF [Option] M47 deactivates the sub-spindle air blast. M-504A 1-45

74 M48 Enable Feedrate and Spindle Override M48 is the Power-up or Reset state of the control. It enables the use of the feedrate and spindle override features. M48 remains active until canceled by M49. M49 Disable Feedrate and Spindle Override M49 cancels M48 and causes the feedrates and spindle speeds to operate at 100% of the programmed values, ignoring the feedrate and spindle override controls. M49 remains active until canceled by an M30, M48, a control OFF, or a control Reset. M51 Live Tool Rotational Direction Command [Option] M51 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction. M51 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction. M51 cancels M52, M53, M54 and M55. Refer to Chapter 11 for additional information. M52 Live Tool Rotational Direction Command [Option] M52 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction. M52 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction. M52 cancels M51, M53, M54, and M55. Refer to Chapter 11 for additional information. M53 Live Tool Rotational Direction Command / Coolant ON [Option] M53 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction with the coolant turned ON. M53 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction with the coolant turned ON. M53 cancels M51, M52, M54, and M55. Refer to Chapter 11 for additional information. M54 Live Tool Rotational Direction Command / Coolant ON [Option] M54 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction with the coolant turned ON. M54 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction with the coolant turned ON. M54 cancels M51, M52, M53, and M55. Refer to Chapter 11 for additional information M-504A

75 M55 Live Tool Stop / Coolant OFF [Option] M55 causes the live tooling attachment mounted at the active position on the turret to stop rotating and turns the coolant OFF. M55 cancels M51, M52, M53, and M54. Refer to Chapter 11 for additional information. M56 Sub-Spindle Collet / Chuck Open [Option] M56 commands the sub-spindle collet closer to release the workpiece. M56 remains active until canceled by M57. M57 Sub-Spindle Collet / Chuck Close [Option] M57 commands the sub-spindle collet closer to grip the workpiece. M57 remains active until canceled by M56. M58 Feed Bar Stock [Option] M58 commands the optional magazine bar feed unit to feed bar stock to the machine. M59 Cancel Feed Bar Stock [Option] M59 commands the optional magazine bar feed unit to stop feeding bar stock to the machine. M60 Speed Arrival Check OFF M60 commands the control to move the machine axes as programmed and not to wait until the spindle reaches the programmed spindle speed. M60 remains active until canceled by M20. M61 Bar Change [Option] M61 calls the bar change macro program, which commands the magazine bar feed to load another piece of bar stock into the active position. M62 Activate C Axis Spindle Synchronization [Option] The M62 command activates C axis spindle synchronization between the main spindle and the optional sub-spindle. Refer to Spindle Synchronization Sample Programs, in Chapter 14. M63 Cancel C Axis Spindle Synchronization [Option] The M63 command cancels C axis spindle synchronization between the main spindle and the optional sub-spindle. Refer to Spindle Synchronization Sample Programs, in Chapter 14. M-504A 1-47

76 M64 Spindle Feedback from Main Spindle The M64 command selects feedback from the main spindle for controlling inch [millimeter] per revolution feedrates. This command is typically not required. The last active spindle (main spindle, sub-spindle, or live tool spindle) will be used for controlling inch [millimeter] per revolution feedrates unless overridden by an M64, M65, or M66. When required, the M64 command is programmed on a line by itself. M65 Spindle Feedback from Sub-Spindle [Option] The M65 command selects feedback from the sub-spindle for controlling inch [millimeter] per revolution feedrates. This command is typically not required. The last active spindle (main spindle, sub-spindle, or live tool spindle) will be used for controlling inch [millimeter] per revolution feedrates unless overridden by an M64, M65, or M66. When required, the M65 command is programmed on a line by itself. M66 Spindle Feedback from Live Tooling [Option] The M66 command selects feedback from the active live tooling spindle for controlling inch [millimeter] per revolution feedrates. This command is typically not required. The last active spindle (main spindle, sub-spindle, or live tool spindle) will be used for controlling inch [millimeter] per revolution feedrates unless overridden by an M64, M65, or M66. When required, the M66 command is programmed on a line by itself. M68 Sub-Spindle External Chucking Mode [Option] The M68 command establishes the operation of the sub-spindle collet closer to support external gripping work-holding devices. Refer to the operator s manual (M-505) for information on establishing chucking modes. M69 Sub-Spindle Internal Chucking Mode [Option] The M69 command establishes the operation of the sub-spindle collet closer to support internal gripping work-holding devices. Refer to the operator s manual (M-505) for information on establishing chucking modes M-504A

77 M70 Orient Commands to Sub-Spindle [Option] M70 is a modal command which causes all spindle orient commands to be effective on the optional sub-spindle. M70 is canceled by M71. M71 Orient Commands to Main Spindle [Option] M71 is a modal command which causes all spindle orient commands to be effective on the main spindle. M71 is canceled by M70. M72 Chamfer OFF M72 is a modal command which deactivates chamfering at the end of each threading pass during a G76 or G92 threading cycle. The threading tool will pull directly away from the workpiece. M72 is canceled by M73. Refer to Chapter 7 for information on threading cycles. M73 Chamfer ON M73 is a modal command which activates chamfering at the end of each threading pass during a G76 or G92 threading cycle. The chamfer distance is determined by parameter M73 is canceled by M72. Refer to Chapter 7 for information on threading cycles. M76 Sub-Spindle Drive OFF [Option] M76 turns OFF the axis drive for the sub-spindle (E axis). Refer to Chapter 14 for additional information. M77 Sub-Spindle Drive Low Torque [Option] M77 switches the axis drive for the sub-spindle (E axis) to low torque mode. Refer to Chapter 14 for additional information. M78 Sub-Spindle Drive Normal Torque [Option] M78 switches the axis drive for the sub-spindle (E axis) to normal torque mode. Refer to Chapter 14 for additional information. M80 Check Part Missing [Option] M80 commands the sub-spindle part detector to check the sub-spindle for a part. If a part is not detected in the sub-spindle, program execution will stop and an alarm message will be displayed. If a part is detected in the sub-spindle, program execution will continue. M81 Check Part Present [Option] M81 commands the sub-spindle part detector to check the sub-spindle for a part. If a part is not detected in the sub-spindle, program execution will continue. If a part is detected in the sub-spindle, program execution will stop and an alarm message will be displayed. M-504A 1-49

78 M82 E Axis Torque Control Mode ON (Tailstock Programming) The M82 command switches the E axis drive from position control mode to torque control mode. Torque control mode allows the tailstock to be commanded in terms of constant force applied against the workpiece. Refer to Chapter 9 for information on programming the tailstock. M83 E Axis Position Control Mode ON (Tailstock Programming) The M83 command switches the E axis drive from torque control mode to position control mode. Position control mode allows the tailstock to be commanded in terms of coordinate positions on a linear axis. Refer to Chapter 9 for information on the programming the tailstock. M87 Tailstock Brake ON The M87 command turns the tailstock brake ON. This command is used with the tailstock when a live center is used with the tailstock. A typical application would be running small (low inertia) parts. M88 Tailstock Brake OFF The M88 command turns the tailstock brake OFF. This command is used with the tailstock when a dead center is used with the tailstock. M90 Part Probe ON The M90 command is used to turn the optical part probe ON. Program the following lines immediately before the command lines for probe operation: M90 ; (Part Probe ON) G4 X1. ; (Dwell for Probe ON) The optical part probe will automatically turn OFF after a predetermined amount of time. Refer to the Marposs probe documentation for information on macro programs and programming examples for the Marposs part probe. Refer to the Renishaw probe documentation for information on macro programs and programming examples for the Renishaw part probe. M97 Part Counter M97 increments the Fanuc parts counter. Refer to the operator s manual (M-505) for additional information on the parts counter. M98 Subprogram Call This code must be in the main part program block which activates a subprogram. It is programmed with a P word, which specifies the subprogram number. Refer to Subprograms, in Chapter 9. M99 Subprogram End This code is used to return to the main part program after a subprogram has been completed. Refer to Subprograms, in Chapter M-504A

79 M200 Main Spindle Brake ON The M200 command turns the main spindle brake ON. This command is used when programming C axis spindle orient. Refer to Chapter 11 for information on programming C axis spindle orient. M201 Main Spindle Brake OFF The M201 command turns the main spindle brake OFF. This command is used when programming C axis spindle orient. Refer to Chapter 11 for information on programming C axis spindle orient. M202 Sub-Spindle Brake ON [Option] The M202 command turns the sub-spindle brake ON. This command is used with the sub-spindle when programming C axis spindle orient. Refer to Chapter 11 for information on programming C axis spindle orient. M203 Sub-Spindle Brake OFF [Option] The M203 command turns the sub-spindle brake OFF. This command is used with the sub-spindle when programming C axis spindle orient. Refer to Chapter 11 for information on programming C axis spindle orient. M206 Disable Main Spindle Draw Bar Check M206 disables the two proximity switches used to check the position of the main spindle draw tube (open, closed, or overtravel condition). M206 is used to run the main spindle without a part or work-holding device in the spindle. M207 Enable Main Spindle Draw Bar Check M207 enables the two proximity switches used to check the position of the main spindle draw tube (open, closed, or overtravel condition). M207 is the normal operating mode for the main spindle. M207 is active at machine start-up and can also be activated by pressing Reset. M208 Disable Sub-Spindle Draw Bar Check [Option] M208 disables the two proximity switches used to check the position of the sub-spindle draw tube (open, closed, or overtravel condition). M208 is used to run the sub-spindle without a part or work-holding device in the spindle. M209 Enable Sub-Spindle Draw Bar Check [Option] M209 enables the two proximity switches used to check the position of the sub-spindle draw tube (open, closed, or overtravel condition). M209 is the normal operating mode for the sub-spindle. M209 is active at machine start-up and can also be activated by pressing Reset. M-504A 1-51

80 M215 Thru-Spindle Coolant ON, Sub-Spindle [Option] The M215 command causes the thru-spindle coolant at the sub-spindle to turn ON. M215 remains active until canceled by M216, M30, control Reset, or control OFF. Refer to M15 for the equivalent command for the main spindle. M216 Thru-Spindle Coolant OFF, Sub-Spindle [Option] The M216 command causes the thru-spindle coolant at the sub-spindle to turn OFF. M216 remains active until canceled by M215. Refer to M16 for the equivalent command for the main spindle. M221 Part Catcher Slide Extend [Option] M221 commands the part catcher slide to extend to the part pick-up position. Refer to Chapter 9 for additional information. M222 Part Catcher Slide Retract [Option] M222 commands the part catcher slide to retract into the headwall. Refer to Chapter 9 for additional information. M223 Sub-Spindle Contouring Mode ON [Option] The M223 command activates sub-spindle contouring mode for C Axis programming. Refer to Chapter 12 for additional information on C Axis programming. Refer to M23 for the equivalent command for the main spindle. M224 Sub-Spindle Contouring Mode OFF [Option] The M224 command cancels sub-spindle contouring mode, which is used for C Axis programming. Refer to Chapter 12 for additional information on C Axis programming. Refer to M24 for the equivalent command for the main spindle M-504A

81 M225 Sub-Spindle Part Catcher Arm Rotate Out [Option] M226 commands the part catcher arm to swing OUT to the part retrieve position at the spindle centerline. Refer to Chapter 9 for additional information. M226 Sub-Spindle Part Catcher Arm Rotate In [Option] M225 commands the part catcher arm to swing IN to allow the part catcher to be retracted. Refer to Chapter 9 for additional information. M227 Sub-Spindle Part Catcher Gripper Close [Option] M227 commands the part catcher gripper to close, gripping the workpiece. Refer to Chapter 9 for additional information. M228 Sub-Spindle Part Catcher Gripper Open [Option] M228 commands the part catcher gripper to open, releasing the workpiece. Refer to Chapter 9 for additional information. M258 Chip Conveyor ON [Option] M258 turns the chip conveyor ON. M259 Chip Conveyor OFF [Option] M259 turns the chip conveyor OFF. M300 Series M Codes M300 series M codes are spare M codes to be used as needed. Refer to Chapter 9 for additional information on the spare M codes. M-504A 1-53

82 DIAMETER PROGRAMMING Hardinge lathes are configured to allow the programmer to use part diameter dimensions from the workpiece drawing as X word entries. With diameter programming, the workpiece centerline coincides with the spindle centerline unless an X axis Zero Offset is active. Refer to Chapter 4 for information on work shift and tool offsets. NOTICE It is strongly recommended that the X axis register in the Work Shift file be set to zero at all times. PROGRAMMING NOTES 1. X words are programmed as diameters. 2. The format for diameter programming is X±2.5 in inch mode (G20) and X±3.4 in metric mode (G21). Maximum resolution is inches [ mm] on the diameter. 3. Dwell (G04) is not affected by diameter programming and is entered directly in seconds or milliseconds, depending on the data word used. 4. Incremental or continuous jogs are unaffected by diameter programming. The actual moves are incremental, but the final absolute X position will be displayed on the control display screen as an X diameter. 5. Tool geometry offsets in the X axis are entered and displayed as diameters. Tool wear offsets in the X axis are entered and displayed as diameters. Z moves are not affected. 6. X axis Distance to Go is displayed as a diameter value M-504A

83 MAIN SPINDLE OPERATION GENERAL PROGRAM FORMATS - NOTE - Bold text indicates items programmed as required. BEGINNING OF PROGRAM % Stop Code (End of Record) O Letter O and the Program Number #500=- Work Shift Value for Main Spindle Operation #501=- Work Shift Value for Sub-Spindle Operation [Option] #502= X Axis Safe Index Position #503= Z Axis Safe Index Position for Main Spindle Operation #504=- Z Axis Safe Index Position for Sub-Spindle Operation [Option] BEGINNING OF OPERATION N ( ) Sequence Search Number and Message G10 P0 Z#500 Set Main Spindle Work Shift G53 E19.3 Move Tailstock to Reference Position (Tailstock Machine Only) M98 P1 Call Safe Index Subprogram O1 M(13 or 14) S1000 G97 P1 T Spindle Direction, Spindle RPM, Direct RPM, Select Spindle (P1 = Main Spindle) Index to Tool Station and Call Offset X Y Z Move Tool To Activate X, Y, & Z Tool Offsets G50 S G96 S IF USING CONSTANT SURFACE SPEED Maximum RPM Limit Surface Feet (Meters) Per Minute Speed IF USING TOOL NOSE RADIUS COMPENSATION G(41 or 42) X Z Tool Nose Radius Compensation (Non-Cutting Move Required) G1 G99 X Z F X (and/or) Z G53 E19.3 M98 P1 M01 MACHINE PART Machine Part, Inches [mm] Per Revolution Feed CLEAR PART Clear Part by 3 Times the Tool Tip Diameter Move Tailstock to Reference Position (Tailstock Machine Only) Call Safe Index Subprogram O1 Optional Stop PROGRAM END M30 End of Program % Stop Code (End of Record) BAR JOB Use the Repeat Mode push button on the Operator Panel M-504A 1-55

84 SUB-SPINDLE OPERATION [Option] - NOTE - Bold text indicates items programmed as required. BEGINNING OF PROGRAM % Stop Code (End of Record) O Letter O and the Program Number G65 P9150 H_._ ; Call Collet Dwell Macro (Time Delay for Pneumatic Collet Closer) #500=- Work Shift Value for Main Spindle Operation #501=- Work Shift Value for Sub-Spindle Operation #502= X Axis Safe Index Position #503= Z Axis Safe Index Position for Main Spindle Operation #504=- Z Axis Safe Index Position for Sub-Spindle Operation BEGINNING OF OPERATION N ( ) Sequence Search Number and Message G10 P0 Z#501 Set Sub-Spindle Work Shift M98 P2 Call Safe Index Subprogram O2 M(33 or 34) S1000 G97 P2 T Spindle Direction, Spindle RPM, Direct RPM, Select Spindle (P2 = Sub-Spindle) Index to Tool Station and Call Offset X Y Z- Move Tool To Activate X, Y, & Z Tool Offsets G50 S G96 S IF USING CONSTANT SURFACE SPEED Maximum RPM Limit Surface Feet (Meters) Per Minute Speed IF USING TOOL NOSE RADIUS COMPENSATION G(41 or 42) X Z Tool Nose Radius Compensation (Non-Cutting Move Required) G1 G99 X Z F X (and/or) Z- M98 P2 M01 MACHINE PART Machine Part, Inches [mm] Per Revolution Feed CLEAR PART Clear Part by 3 Times the Tool Tip Diameter Call Safe Index Subprogram O2 Optional Stop PROGRAM END M30 End of Program % Stop Code (End of Record) BAR JOB Use the Repeat Mode push button on the Operator Panel 1-56 M-504A

85 - NOTES - M-504A 1-57

86 - NOTES M-504A

87 CHAPTER 2 - TOOL NOSE RADIUS COMPENSATION INTRODUCTION Regardless of the location of the origin of the work coordinate system used, execution of the part program causes a single point (tool nose reference point) to be moved relative to and positioned at coordinates specified by the program. However, the tool nose is not a point; it is a radius. Metal removal does not always take place at the same section of the tool nose. Orientation of the tool nose relative to the work surface determines which portion of the tool is involved in metal removal. (Orientation depends on tool geometry and the type of cut.) Programming the proper tool path for radius and angle contouring requires Tool Nose Radius Compensation. The following example illustrates the need for such compensation. To machine the 30 degree taper shown in Figure 2.3, a contouring tool with a tool nose similar to the one shown in Figure 2.1 is used. The distance this tool nose extends from the X axis turret face is measured from the turret reference point to the X axis touch-off point. The position of the tool nose relative to the Z axis turret face is measured from the turret reference point to the Z axis touch-off point. If a Tool Offset is active while a part program is being executed, the Actual Position register will display the coordinates of the tool nose reference point. This point is formed by the X coordinate of the X axis touch-off point and the Z coordinate of the Z axis touch-off point. In this case, the tool nose reference point is not on the tool nose. Refer to Figure 2.1. However, this is not always the case. Some tools have only one touch-off point. Refer to Figure 2.2. In such a case, the distance the nose extends from the turret centerline and Z axis turret face to this single touch-off point becomes the tool nose reference point. For such tools, the tool nose reference point is located on the tool nose. Some numerical control manuals refer to the tool nose reference point as the imaginary tool tip. This term can be misleading and is avoided in this manual. +X +X +Z ZAxis Touch-Off Point +Z Tool Nose Reference Point XAxis Touch-Off Point TI2373 XAxis Touch-Off Point TI2374 Figure Tool Nose with X and Z Axis Touch-off points. Figure Tool Nose with X Axis Touch-off points. M-504A 2-1

88 C (X.6 Z-.75) r=.01 B (X.6 Z-.1732) 30 A(X.4Z0.) Start Point (X.4 Z.2) N40G01G99; N50 Z0. F.01 ; N60 X.6 Z ; N70 Z-.75 ; +X +Z C L ZZero TI2375 Figure Example of Oversize Cut Caused by Absence of Tool Nose radius Compensation To properly machine the section of the part shown in Figure 2.3, metal removal must take place along the line connecting X.4 Z0. and X6. Z However, if Tool Nose Radius Compensation is ignored and these coordinates are programmed, the resulting cut will be oversize. Block N50 moves the tool nose reference point from X.4 Z.2 to X.4 Z0. and block N60 moves the reference point from X.4 Z0. to X6. Z Stock removal does not take place along the path followed by the tool nose reference point (represented by the dashed line) and the resulting cut (represented by the solid line) is oversize. The amount oversize is a function of the angle of the taper and the size of the tool nose radius. Without automatic Tool Nose Radius Compensation to make the control generate the proper tool path, the programmer must perform the necessary calculations to offset the effect of the tool nose radius. As with tapers, any change in the tool nose radius will require program revisions for all contouring involving arcs. With automatic Tool Nose Radius Compensation, the programmer can write a part program as if a zero radius tool were being used. Programs are written using coordinates taken directly from the workpiece. The operator stores the radius value of each tool in the Tool Offset files and the control makes all necessary calculations and compensations as the program is executed. If a tool is changed, the operator simply modifies the radius in the Tool Offset file and the control recalculates the compensation as the program is executed again. Time consuming manual calculations are eliminated, as is the threat of large scale part program revisions due to tooling changes. 2-2 M-504A

89 TOOL ORIENTATION NUMBER Before Tool Nose Radius Compensation can be activated in a program, the tool nose radius value and the tool orientation number must be stored in the tool geometry offset file. The tool orientation number describes the center of the tool nose radius relative to the X and Z touch-off points. A diagram of the orientation codes appears in Figure 2.4. A diagram showing the proper signs for tool offsets appears in Figure 2.5. Refer to Chapter 4 for information on storing tool nose radius values and tool orientation numbers in the tool offset file from a program X 5 7 +Z 1 Main Spindle 6 2 Turret Figure Tool Orientation Codes TI2376 BMT 45 Turret Top Plate Hardinge Turret Top Plate +X +Z Main Spindle +X +Z +X -Z +X +Z +X -Z TI5663 Figure Tool Offset Dimension Signs M-504A 2-3

90 ACTIVATING TOOL NOSE RADIUS COMPENSATION A tool nose radius value and tool orientation number must be activated before entering Tool Nose Radius Compensation mode. Tool nose radius values and tool orientation codes are activated along with Tool Offsets by a programmed T word with the data word format T4: Txxyy Where: xx = Turret Station yy = Tool Offset Number A programmed T0 command deactivates all active tool offset data. A G41 or G42 Preparatory Command is programmed to activate Tool Nose Radius Compensation. This block is called the entry block. The G41 or G42 entry block must be a non-cutting move on both axes. At least one axis must move a distance equal to or greater than the radius of the tool nose. To determine which G code to use, imagine you are sitting on the tool nose facing the direction of tool motion. If the workpiece is on your right, G41 is the correct code. If the workpiece is on your left, G42 is the correct code. Refer to Figures 2.6 and 2.7. The control has a two block look-ahead capability, which enables the control to complete a compensated move with the tool in position to begin the next compensated move. While the currently active block is being executed, the control searches ahead to read and process the next two data blocks. Refer to Figure 2.8 for a comparison of programmed tool paths with and without Tool Nose Radius Compensation based on similar workpiece contours. 2-4 M-504A

91 +X +X +Z +Z C L C L C L C L G41 G42 TI2378 Figure G41/G42 Diagram: Turret at Main Spindle +X +X +Z +Z C L C L C L C L G41 G42 TI4174 Figure G41/G42 Diagram: Turret at Sub-Spindle M-504A 2-5

92 Tool Compensation Tool Compensation C L C L Tool Compensation Not Active Tool Compensation Active Tool Compensation Tool Compensation C L C L TI2379 Figure Tool Path Comparisons 2-6 M-504A

93 ENTERING AND EXITING THE WORKPIECE WITH TOOL NOSE RADIUS COMPENSATION ACTIVE When entering and exiting the workpiece, axis motion should be perpendicular to the surface of the workpiece. Refer to Figure 2.9 for an illustration of correct axis motion. If axis motion is not perpendicular with the surface of the workpiece, the tool may be boxed in. When a tool is boxed in, it will not reach the programmed end point. Refer to Figure 2.10 for an illustration of incorrect axis motion and boxing the tool in. TI2380 G42 Exit Workpiece C L Entry G42 Figure Correct Axis Motion TI2381 G42 Exit G42 Entry Workpiece C L Figure Incorrect Axis Motion M-504A 2-7

94 SWITCHING G41/G42 CODE WITH TOOL NOSE RADIUS COMPENSATION ACTIVE NOTICE Due to the way in which Tool Nose Radius Compensation is interpolated, G41 or G42 should be programmed in a block with non-cutting linear motion. If Tool Nose Radius Compensation is activated in a block in which cutting is commanded, undesirable axis motion may occur. To switch from G41 to G42 or vice versa while Tool Nose Radius Compensation is active, it is not necessary to program a G40 to cancel the active code. Programming the desired G41 or G42 will cancel the active code and activate the new G code. For example, if G41 is active and G42 is programmed, G41 will be canceled and G42 will be activated. Due to the way Tool Nose Radius Compensation is interpolated, this linear move should usually be a non-cutting move. The notable exception is an axis reversal. Axis reversal is discussed in the next section. 2-8 M-504A

95 AXIS REVERSALS WITH TOOL NOSE RADIUS COMPENSATION ACTIVE Axis reversals are possible with Tool Nose Radius Compensation active. As mentioned in the previous section, an axis reversal represents a case when a G41/G42 switch can occur in a cutting move. In the sample program segment shown below, G41 is activated in the move to Point A (Block N60). Refer to Figure Block N60 establishes the feedrate and moves the tool nose reference position to point A for the facing operation. Block N70 commands the facing move from point A to point C. The position of the center of the tool nose radius at the end of block N70 is on the spindle centerline. Therefore, at the end of block N70, the tool nose reference point is one tool nose radius to the -X side of the spindle centerline. Block N80 switches the code to G42. No Z axis motion takes place as a result of the G41/G42 switch. If Tool Compensation was not changed from G41 to G42 in block N80, the control would assume that the part is still on the right side of the tool and an overcutting alarm would occur. Block N90 moves the tool back up the face of the part to point D. Block N100 commands the turning move from point D in the -Z direction. In summary, axis reversals are possible, but be aware of the tool nose radius overshoot at the end of the move prior to the reversal. SAMPLE PROGRAM SEGMENT N50 G00 G41 X1.2 Z.1 ; N60 G01 G99 Z0. F.01 ; N70 X-.02 ; N80 G42 ; N90 X.8 ; N100 Z-.5 ; C L C L A(X1.2 Z0.) B(X.8 Z0.) B (X.79 Z0.) C(X0. Z0.) C (X-.01 Z0.) D(X.8 Z0.) C(X0. Z0.) C (X-.01 Z0.) Figure Axis Reversal with Tool Compensation Active r=.01 TI2382 M-504A 2-9

96 MODES IN WHICH TOOL NOSE RADIUS COMPENSATION IS NOT PERFORMED Tool Nose Radius Compensation is not performed in the following automatic cycles: G74 Automatic Drilling Cycle G75 Automatic Grooving Cycle G76 Automatic Threading Cycle G92 Canned Threading Cycle If Tool Nose Radius Compensation is active before one of these auto cycles is executed, Tool Nose Radius Compensation is deactivated during the cycle and then reactivated after the cycle is completed. Tool Nose Radius Compensation also is not performed during the G32 Constant Lead Threadcutting mode or the optional G34 Variable Lead Threadcutting mode. MULTIPLE REPETITIVE CYCLES WITH TOOL NOSE RADIUS COMPENSATION ACTIVE Tool Nose Radius Compensation is not active during G71, G72, or G73 roughing cycles, but is active during the G70 finishing cycle. To use Tool Nose Radius Compensation in the multiple repetitive finishing cycle, Tool Nose Radius Compensation must be activated in the move to the start point. If the same tool is used to rough and finish the workpiece, the move to the start point occurs prior to the roughing cycle. Compensation will be suppressed until the finishing cycle is executed. If a different tool is used to finish turn the workpiece, compensation is activated in the move to the start point prior to the G70 cycle M-504A

97 CANNED CYCLES WITH TOOL NOSE RADIUS COMPENSATION ACTIVE Tool Nose Radius Compensation can be used with the G90 Canned Turning Cycle and the G94 Canned Facing Cycle, but it must be activated prior to the block that specifies the G90 or G94 canned cycle. If Tool Nose Radius Compensation is used in either cycle, axis motion is as follows: G90 CANNED TURNING CYCLE Refer to Figure The tool moves from the start point to the compensated position to begin the turn. 2. The tool ends the turn at the compensated position to begin facing the shoulder. Start Point 3. At the end of the facing move, the tool nose reference point is at the X coordinate of the start point. 4. The tool then returns to the start point. At the end of the move, the tool nose reference point is at the coordinates of the start point. C L Rapid Traverse Feed Figure Axis Motion During a G90 Turning Cycle TI2383 G94 CANNED FACING CYCLE Refer to Figure The tool moves from the start point to the compensated position to begin the turn. 2. The tool ends the face at the compensated position to begin the turn. Start Point 3. At the end of the turn, the tool nose reference point is at the Z coordinate of the start point. 4. The tool then returns to the start point. At the end of the move, the tool nose reference point is at the coordinates of the start point. C L Rapid Traverse Feed TI2384 Figure Axis Motion During a G94 Turning Cycle M-504A 2-11

98 TOOL MOVED AWAY FROM THE WORKPIECE WITH TOOL NOSE RADIUS COMPENSATION ACTIVE If a program is stopped during the execution of contouring with Tool Nose Radius Compensation active and the tool is moved away from the workpiece, either by a manual Jog operation or an Manual Data Input command, do not resume the cycle from this new position. Reset the program and perform a Program Restart operation. TOOL NOSE RADIUS COMPENSATION RELATED ALARMS ALARM 033 A point of intersection cannot be determined for Tool Nose Radius Compensation. ALARM 034 Entry or exit move is programmed in G02 or G03 mode. The control must be in G00 or G01 mode to activate or deactivate Tool Nose Radius Compensation. ALARM 035 Skip function (G31) has been programmed with Tool Nose Radius Compensation active. ALARM 038 Arc start point or end point coincides with the arc center. The probable cause of the alarm is a G02/G03 programming error. It is possible that a G01 move was not programmed after cutting the arc. ALARM 039 An Insert Chamfer or Insert Arc was commanded in an entry block, exit block, or in a switch between G41 and G42. The program may cause overcutting to occur. ALARM 040 Overcutting will occur with Tool Nose Radius Compensation active and a G90 or G94 canned cycle programmed. ALARM 041 Overcutting will occur because of one of the following conditions: 1. A programmed groove or inside corner is smaller than the tool nose radius. 2. The direction of the tool nose reference point is between 90 degrees and 270 degrees different than the programmed path M-504A

99 DEACTIVATING TOOL NOSE RADIUS COMPENSATION Program a G40 along with a non-cutting linear move in both axes to deactivate Tool Nose Radius Compensation. An alarm message will appear if: Circular motion is programmed in the exit block. Insert Chamfer or Insert Radius is programmed in the exit block. TOOL NOSE RADIUS COMPENSATION PROGRAMMING RULES 1. Store tool nose radius values and orientation codes along side the appropriate offset numbers in the Tool Offset file. The offset must be activated prior to activation of Tool Nose Radius Compensation. 2. To activate Tool Nose Radius Compensation, program a G41 or G42 along with non-cutting linear motion in both axes. The motion on either axis must be equal to or greater than the radius value of the tool nose. To determine which G code to use, image yourself sitting on the tool tip facing in the direction of the tool motion. If the workpiece is on your right, the correct code is G41. If the workpiece is on your left, the correct code is G Entry to and exit from the workpiece should be perpendicular to the surface of the workpiece. 4. To switch from G41 to G42 and vice versa, program the appropriate G code in a block by itself before motion in the other direction. 5. Tool Nose Radius Compensation is not performed in the following modes: G32, G34, G71, G72, G73, G74, G75, G76, and G When Tool Nose Radius Compensation is active, only one data block which does not contain axis motion may be programmed between blocks which contain axis motion. If two or more non-motion blocks are programmed consecutively, undesirable machine behavior in the form of under-cutting or over-cutting may occur. 7. If Tool Nose Radius Compensation is to be used with G90 or G94 canned cycles, Tool Nose Radius Compensation must be activated prior to the block that specifies the G90 or G94 cycle. 8. If Tool Nose Radius Compensation is to be used with a G70 multiple repetitive finishing cycle, Tool Nose Radius Compensation must be activated in the move to the start point prior to the execution of the G70 cycle. 9. When clearing the workpiece, axis motion should move the tool nose a distance of at least three times the tool nose diameter from the workpiece. M-504A 2-13

100 - NOTES M-504A

101 CHAPTER 3 - LINEAR AND CIRCULAR INTERPOLATION FEEDRATE Feedrate is specified by the value after the word address F. This value can be expressed in inches/millimeters per minute (G98 mode) or as inches/millimeters per revolution (G99 mode). The maximum programmable feedrates are listed below. Programmed feedrates greater than the maximum feedrate allowed will default to the maximum value upon program execution. The maximum programmable feedrate for the E, X, Y, and Z axes is: 150 inches per minute 3810 millimeters per minute To convert in/min [mm/min] to in/rev [mm/rev], divide the in/min [mm/min] feedrate by the programmed spindle speed: English: inches/minute revolutions/minute = inches/revolution Metric: millimeters/minute revolution/minute = millimeters/revolution To convert in/rev [mm/rev] to in/min [mm/min], multiply the in/rev [mm/rev] feedrate by the programmed spindle speed: English: inch/revolution x revolution/minute = inches/minute Metric: millimeter/revolution x revolution/minute = millimeters/minute To override programmed feedrates, use the Feedrate Override switch. The Feedrate Override switch is disabled during threading cycles, except when set to 0%. To override rapid traverse rate, use the Rapid Override switch. NOTICE If the Feedrate Override switch is set to 0% during a threading cycle, X and Z axis motion will STOP. M-504A 3-1

102 ABSOLUTE AND INCREMENTAL PROGRAMMING In absolute programming, the E, X, Y, and Z data words are used to specify the end point of a move as a coordinate on the work coordinate system. For example, the following command calls for a linear move to position the tool nose reference point at X.25 Z5. on the work coordinate system: G01 G98 X.25 Z5. F10. ; In incremental programming, the U, V, and W words are used to specify the end point of a move as an incremental distance from the current position on the work coordinate system. U = Incremental distance on the X axis U- = Toward the operator U+ = Away from the operator V = Incremental distance on the Y axis V- = Toward the machine bed V+ = Away from the machine bed W = Incremental distance on the Z axis W- = Toward the face of the main spindle W+ = Away from the face of the main spindle For example, the following command calls for a linear move in which the cross slide moves.25 inches away from the operator and the carriage moves 2.5 inches toward the spindle face: G01 G98 U.5 W-2.5 F10. ; Absolute and Incremental commands may be used together in a block. For example, the following command causes the cross slide to move.375 inches toward the operator from the current cross slide position and also positions the carriage at Z coordinate point 6.5 on the work coordinate system: G01 G98 U-.75 Z6.5 F10. ; If both X and U, Y and V, or Z and W are programmed in the same block, the one specified last is effective. For example, the following block causes the carriage to move.5 inches away from the spindle face from the current carriage position. (The Z word is ignored). G01 G98 Z.4 W.5 F10. ; 3-2 M-504A

103 INTERPOLATION Interpolation describes the function of the control when it decodes a block of programmed data commanding axis motion. Given the type of motion, the feedrate, and the end point, the control defines the tool path by generating a series of intermediate points between the current slide position and the programmed end point. In the case of tapers and arcs, it also calculates the proper feedrate for each axis to produce the correct tool path. There are two standard types of interpolation performed by the control: Linear Interpolation Circular Interpolation LINEAR INTERPOLATION Linear Interpolation is commanded by the G01 command. G01 is a modal code, which means that it will stay active until a G00 code (positioning) or a G02/G03 code (Circular Interpolation) is programmed. Therefore, it is necessary to program a G01 to return to Linear Interpolation from a currently active G00, G02, or G03 code because these codes are also modal. With G01 active, program blocks command the tool to move in a straight line from its current position to a programmed end point. This end point is specified as either a coordinate position (X, Z) on the work coordinate system or as an incremental movement (U, W) from the current slide position. For example: G01 G99 X.25 Z2. F.008 Slides move from current position to work coordinate X.25 Z2. G01 G99 U.4 W-1. F.008 X axis moves.2 inches in the positive direction as Z axis moves 1 inch in the negative direction. Insert Chamfer or Corner Radius - NOTE - Insert chamfer/insert corner radius cannot be programmed in a threadcutting block. If two linear (G01) moves intersect, it is possible to insert a chamfer or an arc between them without adding a third program block or switching from linear interpolation to circular interpolation and back again. The following rules apply: 1. Both moves must be a G01 move. 2. The end point of the first block is the point where the linear moves would intersect if there was no chamfer or corner radius inserted. It is not the start point of the chamfer or corner radius. M-504A 3-3

104 INSERT CHAMFER To insert a chamfer, program a,c word in the first of the two linear move (G01) blocks. These two linear moves do not have to be perpendicular to each other. The value of,c is unsigned. The (,) comma must precede the C word. INSERT CORNER RADIUS To insert an arc between two linear (G01) moves, program an,r word in the first motion block. The value of the,r word is the radius of the arc to be inserted. The value of,r is unsigned. The (,) comma must precede the R word. SAMPLE PROGRAM - NOTE - The control will try to blend the inserted chamfer into the two linear moves. The inserted radius MUST BLEND into the linear move on each side of it. Figure 3.1 illustrates an Insert Chamfer/Corner Radius programming example and Figure 3.2 illustrates the Insert Chamfer/Corner Radius programming format. ALARM MESSAGES FOR INSERT CHAMFER/INSERT CORNER RADIUS There are a number of alarm messages generated by the control that relate to Insert Chamfer / Insert Corner Radius. Refer to the Fanuc operator s manual for an explanation of these alarm messages. N15 G01 G99 X0. Z0. F.008 ;.01 R N20 X.5,C.01 ; N25Z-.5,C.01;.01 R N30 X1.,R.01 ; N35W-.5,R.01;.01 R N40X1.5,R.01; N45 Z-1.5 ; C L TI2367 Figure Insert Chamfer / Corner Radius Sample Program 3-4 M-504A

105 X(U),C ; Z(W) ; Insert Chamfer +X,C,C +Z,C,C Z(W),C ; X(U) ; +X,C,C +Z,C,C X(U),R ; Z(W) ; Insert Radius +X,R,R +Z,R,R Z(W),R ; X(U) ; +X,R,R +Z,R,R TI2368A Figure Insert Chamfer / Insert Corner Radius M-504A 3-5

106 CIRCULAR INTERPOLATION In Circular Interpolation the control uses the information contained in a single data block to generate an arc. There are two types of Circular Interpolation: Clockwise Arc (G02) Counterclockwise Arc (G03) The Electronics Industries Association (EIA) defines clockwise and counter-clockwise arcs as follows: G02 Clockwise Arc An arc generated by the coordinated motion of two axes in which curvature of the path of the tool with respect to the workpiece is clockwise when viewing the plane of motion in the negative direction of the perpendicular axis. Stated another way, tool motion during a G02 arc will appear clockwise, as viewed by the machine operator. G03 Counter-Clockwise Arc An arc generated by the coordinated motion of two axes in which curvature of the path of the tool with respect to the workpiece is counterclockwise when viewing the plane of motion in the negative direction of the perpendicular axis. Stated another way, tool motion during a G03 arc will appear counterclockwise, as viewed by the machine operator. Besides containing the G code for the rotational direction of tool movement, the data block specifying circular interpolation must contain information indicating the position of the arc end point and the location of the arc center. Data words used to specify these parameters are summarized in Figure 3.3. Note the differences in the definitions depending on whether Tool Nose Radius Compensation is active or inactive. As indicated with Tool Nose Radius Compensation active, the location of the arc end point and arc center is independent of the tool nose radius. These dimensions are taken from the part and the control performs the necessary compensation to generate the proper arc. Refer to Chapter 2 for additional information. 3-6 M-504A

107 Programming Notes for Circular Interpolation 1. In circular interpolation, the feedrate along the arc (feedrate tangent to the arc) is held within ±2% of the programmed feedrate. 2. If I and K are used to indicate the arc center, and either I or K is equal to zero, that word may be omitted. 3. If I and K are used to indicate the arc center and both I and K are programmed as zero with Tool Nose Radius Compensation inactive, the tool will move linearly from the arc start point to the arc end point. However, if I and K are programmed as zero with Tool Nose Radius Compensation active, an alarm message will appear on the control display screen. The alarm indicates that overcutting will occur because the arc start point coincides with the arc center. 4. If I, K, and R are programmed in the same data block, the control will ignore the I and K and generate the arc using R to locate the arc center. 5. If R is used to locate an arc center, a zero degree arc is assumed (no tool motion occurs) if any of the following three conditions occurs: A) If X and Z are the coordinates of the start point. B) If X, U, Z, and W are omitted. C) If U and W are programmed as zero (U0. W0.). 6. If R is used to indicate the arc center, but the R value is less than half the distance from the arc start point to the arc end point, R is ignored and a half circle is produced which connects the arc start point and arc end point. 7. Circular Interpolation may be switched without canceling with G G01 (Linear Interpolation) must be programmed to cancel Circular Interpolation. M-504A 3-7

108 Parameter Command Definition G02 +X Rotational Direction G03 +X +Z +Z Definition (Tool Nose Radius Compensation Not Active) Definition (Tool Nose Radius Compensation Active) Incremental distance from the center of the tool nose radius at the start point to the arc center. IMPORTANT: This value must be signed. (This incremental distance depends on the size of the tool nose radius.) Refer to the example shown in Figure 3.4. Incremental distance from arc start point to the arc center, as measured on the workpiece. IMPORTANT: This value must be signed. (This incremental distance remains the same regardless of the size of the tool nose radius.) Refer to the example shown in Figure 3.5. Location of Arc Center I,K R Radius of the arc. This radius is measured from the center of the tool nose radius to the arc center. This value is unsigned. (This distance depends on the size of the tool nose radius.) NOTE: The R word can only be used when the arc is 180 degrees. Refer to the example shown in Figure 3.4. Radius of the arc. This radius is measured from the arc start point to the arc center, as measured on the workpiece. This value is unsigned. (This distance is independent of the size of the tool nose radius.) NOTE: The R word can only be used when the arc is 180 degrees. Refer to the example shown in Figure 3.5. X,Z Coordinates of the tool nose reference point to the arc end point. (These coordinates depend on the size of the tool nose radius and geometric configuration of the tool nose.) Refer to the example shown in Figure 3.6. Coordinates of the arc end point, as measured on the workpiece. (These coordinates are independent of the size of the tool nose radius and geometric configuration of the tool nose.) Refer to the example shown in Figure 3.7. Location of Arc End Point U,W Incremental distance from the position of the tool nose reference point at the arc start point to the position of the tool nose reference point at the arc end point. (These coordinates depend on the size of the tool nose radius and geometric configuration of the tool nose.) Refer to the example shown in Figure 3.6. Incremental distance from arc start point to the arc end point, as measured on the workpiece. (This incremental distance is independent of the size of the tool nose radius and geometric configuration of the tool nose.) Refer to the example shown in Figure 3.7. Figure Circular Interpolation Parameters 3-8 M-504A

109 R Arc Center K +X +Z K I R I C L C L Arc Center TI2369 Figure Arc Center Parameters (Tool Nose Radius Compensation Not Active) R Arc Center K +X +Z I R I C L K C L Arc Center TI2371 Figure Arc Center Parameters (Tool Nose Radius Compensation Active) M-504A 3-9

110 W +X X,Z Arc Center X,Z +Z U U C L W C L Arc Center TI2370 Figure Arc End Point Parameters (Tool Nose Radius Compensation Not Active) X,Z Arc Center X,Z W +X +Z U U C L W C L Arc Center TI2372 Figure Arc End Point Parameters (Tool Nose Radius Compensation Active) 3-10 M-504A

111 - NOTES - M-504A 3-11

112 - NOTES M-504A

113 CHAPTER 4 - WORK SHIFT AND TOOL OFFSETS WORK SHIFT At the beginning of each separate tool operation in a part program, the program will call the required work shift from the appropriate macro variable register and load the work shift value into the Z axis work shift file. Once the work shift value is copied from the macro variable register to the Z axis work shift file, the work shift offset moves the Z axis origin of the work coordinate system. The value stored in the work shift file is active at all times. NOTICE The Work Shift file contains an E, X, Y and Z offset register. The X and Y axis registers in the Work Shift file should be set to zero at all times. The value entered into the Z axis Work Shift register from the macro variable register must be a negative number. - NOTE - Refer to Chapter 14 for information on Z axis work shift for sub-spindle operation. The E axis work shift will be set by the machine operator. The values stored in the Work Shift file are added to the Absolute Position registers, thus shifting the origin of the work coordinate system by the amount stored in the Work Shift file. For example, if the Z axis is at 14 inches and the operator stores Z-2.5 in the Work Shift file, the Absolute Position registers would then display Z11.5 [14 +(- 2.5)]. Immediately after a Work Shift value is stored, the control adds it to the Absolute Position registers. The registers will remain modified until the Work Shift offset values are set to zero by the operator or from the part program. The part length is stored as the Z Work Shift offset. Typically the X and Y axis Work Shift offsets ARE NOT USED (set to zero). Since the Work Shift value is added to the Absolute Position registers, the part length is stored as a negative Z value. With the part length stored in the Work Shift file, the origin of the Absolute coordinate system is the intersection of the part face and the spindle centerline. MACRO VARIABLE ASSIGNMENTS Macro variable register #500 will contain the work shift value for all main spindle operations. Macro variable register #501 will contain the work shift value for all sub-spindle operations. STORING WORK SHIFT OFFSETS The values for the work shift offsets can be stored in the macro variable registers by either of the following methods: Manually stored by the machine operator at the manual data input keyboard. Refer to the operator s manual (M-505) for information on storing data in the macro variable registers from the manual data input keyboard. Automatically input from the part program. Refer to the section that follows. M-504A 4-1

114 LOADING THE MACRO VARIABLES FROM THE PART PROGRAM The main spindle and sub-spindle Z axis Work Shift offsets can be loaded directly into macro variable registers 500 and 501 from the part program. Main Spindle Programming Format: #500=- ; Programming Example: #500= ; Sub-Spindle [Option] Programming Format: #501=- ; Programming Example: #501= ; LOADING A WORK SHIFT OFFSET FROM THE MACRO VARIABLE REGISTERS The G10 command line will be programmed at the beginning of each tool operation. NOTICE The Work Shift file contains an E, X, Y and Z offset register. The X and Y axis registers in the Work Shift file should be set to zero at all times. - NOTE - This section discusses only the command line structure required to transfer data from the macro variable registers to the work shift files. Programming Format: G10 P0 X0 Y0 Z#500 ; (Main spindle work shift offset) G10 P0 X0 Y0 Z#501 ; (Sub-spindle work shift offset) P0: Selects the Work Shift offset as the offset file to be modified. X: Work Shift offset value on the X axis (absolute) Y: Work Shift offset value on the Y axis (absolute) Z: Work Shift offset value on the Z axis (absolute) In an absolute command, the value in the specified macro variable register is set as the Z axis Work Shift offset. In an incremental command, the value specified in address W is added to the current Z axis Work Shift offset. Use of this command in a program causes the Z axis work shift to advance incrementally. 4-2 M-504A

115 TOOLING AND TOOL OFFSETS TOOLING Top Plate Configurations Hardinge T-42 lathes are available with the following top plate configurations: 16 station BMT station Hardinge English 12 station Hardinge Metric Hardinge T-51 and T-65 lathes are available with the following top plate configurations: 12 station BMT station Hardinge English 12 station Hardinge Metric Left Hand/Right Hand Tooling Hardinge Inc. recommends that all cutting forces be directed into the machine base, which will result in maximum tool life. Making the selection between left-hand or right-hand tooling should be based on: the position of the tool in relation to the spindle the direction of spindle rotation M-504A 4-3

116 TOOL OFFSETS Introduction The Tool Offset file is made up of two types of offsets: Tool Geometry Offsets and Tool Wear Offsets. The control has the capacity to store 99 sets of each offset type (Offsets 01 through 99) in separate files. NOTICE Information stored in the Geometry and Wear Offset files is NOT automatically converted into the correct units when a programmed G20 or G21 command switches programming resolution from inch to metric or vice versa. Offsets in the desired unit of measure should be entered after the control has been set to the proper mode, inch (G20) vs metric (G21). If a G20 or G21 is programmed after the tool offsets are entered, the decimal point will be shifted one place to the left or right. If start-up mode is G20 (inch) and the program switches to G21 (metric), the offset decimal point will shift one place to the right. If start-up mode is G21 (metric) and the program switches to G20 (inch), the offset decimal point will shift one place to the left. The following information is stored in the Tool Geometry Offset file: X Tool Dimension Diameter distance from the X axis tool touch-off point to the turret reference point. Sign is determined by the direction from the tool nose reference point to the turret reference point. Z Tool Dimension Distance from the Z axis tool touch-off point to the turret reference point. Sign is determined by the direction from the tool nose reference point to the turret reference point. - NOTE - Refer to Chapter 2 for a description of the tool nose reference point. Refer to Chapter 5 for a description of coordinate system reference positions. Tool Orientation: The orientation code describes the location of the center of the tool nose in relation to the tool nose reference point. Tool Nose Radius Value: The distance from the cutting edge to the center of the tool nose radius. 4-4 M-504A

117 The Tool Wear Offset file allows the operator to enter minor dimensional changes for each tool to compensate for tool wear. The Tool Wear Offset files coincide with the Geometry Offset files. When a tool offset is activated, the control looks at the corresponding Tool Wear offset and performs the necessary corrections to compensate for tool wear. The Tool Offset files allow the operator to easily make corrections resulting from tool changes, thus large-scale modifications to the part programs are eliminated. Tool Offsets are activated by the last two digits in the T word. The first two digits specify the turret station. The data word format for the T word is T4. Tool Nose Radius Value and Orientation Code If Tool Nose Radius Compensation is to be used, the tool nose radius value (Figure 4.1) and the tool orientation code (Figure 4.2) must be entered for each tool that uses Tool Nose Radius Compensation. Refer to the operator s manual (M-505) for information on inputting tool nose radius values and orientation codes from the control keyboard X 5 7 +Z 1 2 Tool Nose Radius Value Main Spindle 6 Turret TI3638 Figure Tool Nose Radius Illustration Figure Tool Orientation Codes TI2376 M-504A 4-5

118 Storing Tool Offsets from the Part Program Tool Offsets may be input directly from the part program by using the G10 code. Programming Format: G10 P X Y Z R Q ; or G10 P U V W C Q ; P: Selects the Tool Offset file to be modified. For Wear Offset: P = Wear Offset Number For Geometry Offset: P = Geometry Offset Number (2 place Format) Examples of P words used for Geometry Offsets: For Geometry Offset #1: P10001 For Wear Offset #1: P1 For Geometry Offset #15: P10015 For Wear Offset #15: P15 X: Offset value on the X axis (absolute) Y: Offset value on the Y axis (absolute) Z: Offset value on the Z axis (absolute) U: Offset value on the X axis (incremental) V: Offset value on the Y axis (incremental) W: Offset value on the Z axis (incremental) R: Tool nose radius offset value (absolute) C: Tool nose radius offset value (incremental) Q: Tool nose orientation code (Refer to Figure 4.2) Used for X and Z axis only Absolute and incremental values for different axes may be programmed in the same offset data block. Examples: G10 P U Z R Q ; G10 P X W R Q ; 4-6 M-504A

119 Activating Tool Offsets Tool offsets are activated by a T word having the format T4. The first two numbers select the turret station that is to be indexed to the cutting position. The last two numbers specify which tool offsets in the tool geometry and wear offset tables are to be used with the selected turret position. Example: N0120 T0622 ; In data block N0120, turret station 6 will be indexed to the cutting position and the tool offsets stored on line 22 in the tool geometry and wear offset tables will be activated. The leading zero in the T word may be omitted: T0101 = T101 NOTICE If tool offsets are not to be called up with a turret index, the last two numbers in the T word MUST be 00" (Example: T0100). If no numbers are programmed in the last two places, the control will use the numbers programmed in the first two places as the tool offset and the turret will not index (Example: T01 will be interpreted by the control as T0001). When a T word with a tool offset is programmed in a block containing axis motion, the tool offset motion is computed with the programmed axis position, causing the slide(s) to move directly to the corrected axis position at the programmed feedrate. When a T word with a tool offset is programmed in a block without axis motion, the tool offset move will occur in the next block containing axis motion. The tool offset motion is computed with the programmed axis position, causing the turret reference point to move directly to the corrected axis position at the programmed feedrate. Canceling Tool Offsets Tool offsets are deactivated when the machine is first powered up or when the Reset key is pressed. The T0 command is used to cancel tool offsets. Tool offset cancellation (T0) will occur in the next programmed axis movement for the X and Z axes. The next programmed X axis movement will cancel the X axis offset and move the turret reference point to the programmed X axis position. The next programmed Z axis movement will cancel the Z axis offset and move the turret reference point to the programmed Z axis position. M-504A 4-7

120 - NOTES M-504A

121 CHAPTER 5 - WORK COORDINATE SYSTEM HOW THE CONTROL POSITIONS THE SLIDES To understand work coordinate programming, it is helpful to consider how the control positions the slides. We will begin by examining how the slides are positioned on a manual lathe. At the onset this may seem like an in-depth discussion of the obvious, but bear with us, the point of this exercise is to show the similarities between the operation of a manual lathe and a CNC lathe. On a manual lathe, the carriage and cross slide are positioned by manually turning a handle attached to a lead screw. The operator positions each slide by reading the dial attached to each handle. Let s assume that on the manual lathe each slide has 10 pitch lead screw. Therefore, each revolution of the lead screw advances the slide.1 inch. If the dial has 100 graduations, each graduation equals 1/100 of a revolution or.001 inch slide travel. If the operator wants to move a slide.306 inch, he turns the handle in the desired direction and counts three and 6/100 revolutions of the dial. How close to 6/100 of a revolution he gets largely depends on his ability to manually position the dial at the proper graduation. Like the slides on the manual lathe, the CNC lathe carriage and cross slide are positioned by rotating a lead screw. However, there are no handles to rotate the lead screws on the CNC lathe. Instead, each lead screw is rotated by a servo motor. The revolutions of each screw are counted by an encoder. The encoder continuously monitors the radial position of the lead screw. Information from the encoder is fed to the control where it is converted into useful output information to produce the correct feedrate and slide position. As the lead screw rotates so does the encoder shaft, which causes the encoder to generate positioning and velocity data. This data is fed to the control for positioning and velocity control functions. To move a slide.306 inch, we enter a coded instruction into the control specifying type of motion (linear or circular), velocity (feedrate), and distance. (Distance can be indicated as an incremental distance from the current position or as a coordinate which represents the endpoint of the move.) Internally, the control decodes the instruction and converts the command into a voltage which is sent to the servo motor of the slide. As the servo motor turns the lead screw, the lead screw turns the encoder shaft and the encoder produces positioning and velocity data. This data is feed back to the control where it is used to monitor slide motion. The distance from the current slide position to the commanded end point is known as the Distance To Go. Before any slide motion takes place in our example, the distance to go is.306 inch. This value is stored in a register in the control. As the lead screw rotates, the control receives counts from the encoder and subtracts them from the Distance To Go register. When the Distance To Go registers count down to zero, the control knows that the slide has moved.3060 (±.0001) inches. M-504A 5-1

122 This feedback arrangement, in which the actual slide movement is compared with the command originating from the control, is known as a closed loop system. Besides the closed loop system for slide position discussed above, there is also a closed loop system for feedrate, which makes use of the electrical pulses produced by the encoder. By making use of the feedback information it receives from the encoder, the control can accurately move a slide a commanded distance at a commanded feedrate. RECTANGULAR COORDINATES To relate the position of the tool to a position on the workpiece, a system must be set up where the location of a given point can be defined relative to a known reference point. Working with mutually perpendicular axes (X, Y, and Z), rectangular coordinates (also known as Cartesian coordinates) are used to describe the location of any point at which the tool can be positioned. Refer to page 1-6 for axis definitions. To apply the use of rectangular coordinates when programming CNC lathes, it is necessary to define coordinate system reference positions. COORDINATE SYSTEM REFERENCE POSITIONS Figures 5.1 and 5.2 illustrate the axis reference positions. MACHINE ZERO POSITION The intersection of the main spindle face and the spindle centerline. This position never changes. TURRET AXIS REFERENCE POSITION The turret axis reference position is the location to which the specified axes (X, Y, Z) will move when a G28 command is executed. This position never changes. Refer to Chapter 1 for information on programming the G28 command. Refer to Appendix One for the turret axis reference position coordinates. TURRET REFERENCE LOCATION The intersection of the turret face toward the spindle centerline and the centerline of the tool holder mounting location. This location can be modified through the use of tool offsets. SUB-SPINDLE OR TAILSTOCK AXIS REFERENCE POSITION The sub-spindle or tailstock axis reference position is the location to which the E axis will move when a G28 command is executed. This position never changes. Refer to Chapter 1 for information on programming the G28 command. Refer to Appendix One for the sub-spindle or tailstock axis reference position coordinate. SUB-SPINDLE OR TAILSTOCK REFERENCE LOCATION The intersection of the spindle centerline and the face of the sub-spindle or tailstock. 5-2 M-504A

123 NOTE: X, Z, and E axes not shown at reference position. +X Turret Axis Reference Position +Z Turret Reference Location C L Sub-Spindle or Tailstock Reference Location -E +E Machine Zero Position Sub-Spindle or Tailstock Axis Reference Position TI5664A Figure Coordinate System Reference Positions (BMT Turret Top Plate) NOTE: X, Z, and E axes not shown at reference position. +X Turret Axis Reference Position +Z Turret Reference Location C L Sub-Spindle or Tailstock Reference Location Machine Zero Position -E +E Sub-Spindle or Tailstock Axis Reference Position TI5665A Figure Coordinate System Reference Positions (Hardinge Turret Top Plate) M-504A 5-3

124 POSITION REGISTERS Press the Position key; then, press the ALL soft key to view the following position registers on the control display screen: Absolute Distance to Go Machine Relative - NOTE - The Distance To Go registers are only displayed in Automatic or Manual Data Input mode. MACHINE POSITION REGISTERS The Machine Position registers always display the true axis position of the turret reference location relative to the machine zero position. Active tool offsets and work shift values have no affect on the Machine Position display. Refer to Figures 5.3 and 5.4. ABSOLUTE POSITION REGISTERS The Absolute Position registers, which can be modified, are probably of greater interest to the programmer and operator. To simplify programming, the work coordinate system can be modified through the use of a work shift and tool offsets to relate the tool nose position to coordinates on the workpiece. The work shift offset can be used to move the origin of the work coordinate system as needed. The work shift is typically used to set the origin (X0. Z0.) to the intersection of the spindle centerline and the face of the workpiece. The tool offsets can be used to move the turret reference location to the tool nose position. Refer to Figures 5.3 and NOTE - For additional information, refer to Feedrate, Absolute and Incremental Programming, and Linear Interpolation, in Chapter M-504A

125 Z Axis Machine Position Tool Nose Position XAxis Absolute Position XAxis Machine Position C L Z Axis Absolute Position Machine Zero Position TI5666 Figure Position Display Comparison: Main Spindle Operation with Tool Offsets and Work Shift Active Z Axis Machine Position XAxis Machine Position XAxis Absolute Position Tool Nose Position C L Z Axis Absolute Position Machine Zero Position TI5667 Figure Position Display Comparison: Sub-Spindle Operation with Tool Offsets and Work Shift Active M-504A 5-5

126 - NOTES M-504A

127 CHAPTER 6 - MACHINING CYCLES G90 CANNED TURNING CYCLE The G90 Canned Turning Cycle provides the programmer with the capability of defining multiple turning passes by specifying only the depth of cut for each pass. The operation may be either a straight turn or a taper turn. Figure 6.1 and its accompanying program illustrate an elementary part on the main spindle which is to have a 1 inch long,.5 inch diameter turned on a workpiece having a diameter of 1 inch. The part face is set to Z0 by the G10 command in block N20; therefore, all turning passes will be in the minus Z direction. The X and Z axis tool offsets are activated through the Tool Offset selection in block N50. Turret station #1 is selected and Tool Offset #1 is activated. The Tool Offset allows the programmer to program the X axis position of the tool tip as the actual position relative to the spindle centerline and Z axis position of the tool tip as the actual position relative to Z0 on the machine coordinate system. If a Z axis Work Shift is active (G10 command), the Z axis position of the tool tip will be positioned in relation to the shifted Z0, as established by the Work Shift offset. Since all dimensions are in inch mode, G20 is entered in block N10. This assures the correct format in case the previously executed program was in metric data input mode (G21). EXAMPLE 1: G90 STRAIGHT TURNING (Figure 6.1) N10 G20 ; N90 G1 G99 G90 X.875 Z-1. F.02 ; N1 (Operator Message) ; N100 X.75 ; N20 G10 P0 Z#500 ; N110 X.625 ; N30 G97 S1000 M13 P1 ; N120 X.532 ; N40 M98 P1 ; N130 X.5 ; N50 T0101 ; N140 G1 ; N60 X1.5 Z.1 ; N150 M98 P1 ; N70 G50 S3800 ; N160 M1 ; N80 G96 S1000 ; N170 M30 ; Start Point C L Spindle Face Chuck Face Figure G90 Canned Turning Cycle: Straight Turn TI1600 M-504A 6-1

128 The cutting tool path is a box pattern; and, because the Start Point is also the point to which the tool returns on the return path, the Start Point in the X direction was placed at a distance greater than.5 inches from the spindle centerline. This assures that the tool will completely face the workpiece shoulder on each pass. The G90 Preparatory Command is specified in block N90 together with G99 (inch/rev feed), the first pass tool tip position relative to the spindle centerline, the length of cut, and the feedrate. In subsequent turning cycle blocks (N100 through N130) it is only necessary to specify the tool tip position relative to the spindle centerline for each pass. Feedrate and spindle speed changes can also be programmed in these blocks. The Feedrate Override switch is active during the turning passes. To deactivate G90 mode, program another Group 1 G-code. (Refer to the G code chart located in Appendix Two.) The approach and return paths are executed at rapid traverse rate. This rate can be varied with the Rapid Override switch. If Constant Surface Speed or Tool Nose Radius Compensation is to be used, the parameters MUST be entered prior to the G90 block. In cases where U and W commands are used in place of X and Z, make certain each command has the correct sign. EXAMPLE 2: G90 TAPER TURNING (Figure 6.2) N10 G20 ; N110 X ; N1 (Operator Message) ; N120 X ; N20 G10 P0 Z#500 ; N130 X ; N30 G97 S1000 M13 P1 ; N140 X ; N40 M98 P1 ; N150 X ; N50 T0101 ; N160 X ; N60 X2. Z.2 ; N170 G1 ; N70 G50 S3800 ; N180 M98 P1 ; N80 G96 S1000 ; N190 M1 ; N90 G1 G98 G42 X1.76 Z.1 F200. ; N200 M30 ; N100 G99 G90 X Z-1. R F.004 ; Start Point Spindle Face C L Chuck Face TI2670 Figure G90 Canned Turning Cycle: Tapered Turn 6-2 M-504A

129 All rules applying to straight turning in the G90 Canned Turning mode also apply to taper turning in this mode. Figure 6.2 and its accompanying program illustrate an elementary part which is to have a 1 inch long, 15 degree taper turned on a workpiece having a diameter of 1.25 inches. The part face is set to Z0 by the G10 command in block N20; therefore, all turning passes will be in the minus Z direction. The only difference between taper turning and the preceding straight turning is that the amount of taper in the X direction, expressed as an R value, must be programmed in the G90 block. Program the R word as a POSITIVE value if the tool moves in the -X direction as it moves in the -Z direction. Program the R word as a NEGATIVE value if the tool moves in the +X direction as it moves in the -Z direction. For this example, R was determined as follows: R = (Z +.1) x -(Tan 15 degrees) = 1.1 x (Unrounded Value) = (Rounded Value) M-504A 6-3

130 G71/G70 AUTOMATIC MULTIPLE REPETITIVE ROUGH AND FINISH TURNING - NOTE - This section is divided into two parts; standard turning and the optional pocket turning feature. All general information on G71/G70 turning is outlined in the section on standard turning. Specific information relating to the optional G71/G70 pocket turning feature begins on page 6-9. The G71 Multiple Repetitive Turning Cycle provides the programmer with the capability of describing multiple rough turning passes with two blocks of information. The first G71 block specifies the amount of stock to be removed per pass and the distance the tool will retract from the workpiece for the return pass. The second G71 block specifies the data blocks which define the section of the workpiece to be rough turned and the amount of stock to be left for finish machining. Finally, the G70 Preparatory Command specifies the section of the workpiece to be finish machined by specifying the first and last blocks of the required program section. G71/G70 STANDARD TURNING Figure 6.3 and its accompanying program illustrates an elementary part on the main spindle that is to be rough turned and finish contoured to the dimensions shown. The part face is set to Z0 by the G10 command in block N20; therefore, all turning passes will be in the minus Z direction. The X and Z Axis tool offsets are activated through the Tool Offset selection in block N50. Turret station #1 is selected and Tool Offset #1 is activated. The Tool Offset allows the programmer to program the X Axis position of the tool tip as the actual position relative to the spindle centerline and the Z Axis position of the tool tip as the actual position relative to Z0 on the machine coordinate system. If a Z Axis Work Shift (G10 command) is active, the Z Axis position of the tool tip will be positioned in relation to the shifted Z0. Since all dimensions are in the inch mode, G20 is entered in block N10. This assures the correct format in case the previously executed program was in metric mode (G21). The Start Point commanded in block N90 must be located outside the area occupied by the blank stock. 6-4 M-504A

131 Start Point Spindle Face C L Chuck Face W U/ U TI1602 Figure G71/G70 Rough and Finish Turning Cycle: Standard Turning Example 3: G71/G70 Standard Turning Cycle (Figure 6.3) N10 G20 ; N130 G0 X.25 S800 ; N1 (Operator Message) ; N140 G1 G99 Z-.25,R.1 F.004 ; N20 G10 P0 Z#500 ; N150 X.55 ; N30 G97 S1000 M13 P1 ; N160 X.8 Z ; N40 M98 P1 ; N170 Z-.75 ; N50 T0101 ; N180 X.94 ; N60 X1.31 Z.2 ; N190 X1.1 Z-.83 ; N70 G50 S3800 ; N200 Z-1. ; N80 G96 S1000 ; N210 X1.3 ; N90 G1 G98 G42 X1.3 Z.1 F100. ; N220 G70 P130 Q210 ; N100 G99 ; N230 M98 P1 ; N110 G71 U.1 R.025 ; N240 M1 ; N120 G71 P130 Q210 U.03 W.015 F.01 ; N250 M30 ; M-504A 6-5

132 Block N110 will establish the parameters for the rough turning cycle: N110 G71 U.1 R.025 ; Where: G71 = Preparatory command for the repetitive roughing cycle. U: Depth of cut of each pass (as a radius value) during the roughing cycle. In this example the depth of each cutting pass is.100 inches. R: Distance the tool will withdraw from the part for the return pass. Block N120 will execute the roughing cycle: N120 G71 P130 Q210 U.03 W.015 F.01 ; Where: G71 = Preparatory command for the repetitive roughing cycle. P: Sequence number of the first block in the program section that controls the workpiece area to be roughed out. Q: Sequence number of the last block in the program section that controls the workpiece area to be roughed out. U: Amount of stock on the X axis to be left for removal during the finish machining cycle. This is a diameter value. W: Amount of stock on the Z axis to be left for removal during the finish machining cycle. F: Feedrate in inches/revolution for the roughing cycle. The decimal point must be programmed. - NOTE - Decimal point programming cannot be used when programming the P and Q data words. Block N130 establishes the Constant Surface Speed value for the G70 finishing cycle: N130 G0 X.25 S800 ; S: The surface feet per minute for the finishing pass. Block N140 establishes the inch per revolution feedrate for the G70 finishing cycle. N140 G1 G99 Z-.25,R.1 F.004 ; F: The feedrate for the finishing pass. The decimal point must be programmed. 6-6 M-504A

133 Block N220 designates the section of the workpiece to be finish machined by specifying the first (P) and last (Q) blocks of the required program section. N220 G70 P130 Q210 ; P: Sequence number of the first block in the program section that controls the workpiece area to be finish machined. Q: Sequence number of the last block in the program section that controls the workpiece area to be finish machined. - NOTE - Decimal point programming cannot be used when programming the P and Q data words. When the control encounters the G71 preparatory command blocks, the amount of finish stock as specified by the U and W words is treated as a pair of offsets. The slides will move in the direction and distance specified. The U and W words MUST be properly signed (+ or -) to ensure that slide movements occur in the direction to leave stock for finishing. If the sign is omitted, the control automatically assumes plus (+). In this example the cross slide will move.015 inches in the +U direction and the carriage will move.015 inches in the +W direction. The control will then cause the machine to execute multiple roughing passes.1 inches deep and a roughing contour pass (as shown by the dashed lines in Figure 6.3) that follows the contour as designated by blocks N130 through N210. After completion of the roughing contour pass, the finish pass will be executed according to the program section specified in the G70 block. The amount of tool withdrawal after completion of each pass is controlled by the R word in block N110 (R.025). In this example the same tool is used for roughing and finishing; therefore, Tool Nose Radius Compensation must be established in a block preceding the G71 roughing cycle block. Tool Nose Radius Compensation is activated and interpolated in the move to the starting point commanded in block N90. Tool Nose Radius Compensation is deactivated during the G71 cycle and reactivated after the G71 cycle is completed. After the workpiece has been finish machined, Tool Nose Radius Compensation is canceled by the G40 command in sub-program O1", which is called in block N230. Also see Tool Nose Radius Compensation", Chapter 2. Constant Surface Speed must be established in blocks preceding the G71 roughing cycle. The feedrate for the roughing passes may be established prior to the first G71 block or in the second G71 block. The surface speed and feedrate for the finishing pass must be established in the part program after the second G71 block. The surface speed and feedrate for the finishing pass can be changed at will between the starting and ending blocks as designated in the G70 block. The spindle speed command that must precede entry into Constant Surface Speed mode is programmed in block N30. A G99 Preparatory command, programmed in block N100, establishes Inch per Revolution feedrate. Maximum spindle speed is established by the S word and the G50 Preparatory Command in block N70. Constant Surface Speed is established by the G96 command in block N80 and surface speed for the roughing cycle is set by the S word in the same block. Surface speed for the finishing pass is established in block N130. Feedrate for the finishing pass is established in block N140. Constant Surface Speed is canceled by the G97 command in sub-program O1" after the workpiece has been finish machined. Also see Constant Surface Speed, in Chapter 9. M-504A 6-7

134 G71 Standard Turning Programming Rules - NOTE - Refer also to page 6-10 for rules when programming G71/G70 pocket turning. 1. A block specified by a P word cannot contain a Z move. 2. G00 or G01 should be programmed in the block specified by the P word. 3. The contouring path must be a steadily increasing or decreasing pattern on both the X and Z axes. 4. No subprogram can be called in the program between the start of the cycle designated by P and the end of the cycle designated by Q. 5. It is not necessary to program a return to the start point at the end of the program. The control automatically returns the slides to the start point after the block specified by Q is executed. 6. If Tool Nose Radius Compensation is to be used, it must be programmed prior to the first G71 block. Tool Nose Radius Compensation will be deactivated during the G71 cycle and reactivated after the G71 cycle is completed. 7. If Constant Surface Speed is to be used, it must be programmed prior to the first G71 block. 8. Tooling changes for the roughing cycle must be made prior to the first G71 block. Tool offset changes for the finishing cycle may be made within the blocks designated by the P and Q words in the G70 block. 9. The spindle speed and feedrate for the roughing cycle can be specified prior to the first G71 block or in the second G71 block. The spindle speed and feedrate for the finishing cycle can be specified within the blocks designated by the P and Q words in the G70 block. 6-8 M-504A

135 G71/G70 POCKET TURNING [Option] - NOTE - This section contains specific information relating to G71/G70 pocket turning. Refer to G71/G70 Standard Turning, beginning on page 6-4, for additional information on programming the G71/G70 turning cycle. Figure 6.4 and its accompanying program illustrates a pocket contour that is to be rough turned and finish turned on the main spindle to the dimensions shown. Figure 6.5 illustrates the paths followed by the roughing and finishing tools. The part face is set to Z0; therefore, all turning passes will be in the minus Z direction. Example 4: G71/G70 Pocket Turning Cycle (Figure 6.4) N10 G20 ; N130 G0 X.4 W0. S800 ; N1 (Operator Message) ; N140 G1 G99 X.75 Z-.125 F.004 ; N20 G10 P0 Z#500 ; N150 Z-.25 ; N30 G97 S1000 M13 P1 ; N160 X.5 Z-.375 ; N40 M98 P1 ; N170 Z-.625 ; N50 T0101 ; N180 X.75 Z-.75 ; N60 X1.1 Z.1 ; N190 Z-.875 ; N70 G50 S3800 ; N200 X1.1 Z-1.05 ; N80 G96 S1000 ; N210 G70 P130 Q200 ; N90 G1 G98 G42 X1.05 Z.05 F100. ; N220 M98 P1 ; N100 G99 ; N230 M1 ; N110 G71 U.1 R.025 ; N240 M30 ; N120 G71 P130 Q200 U.03 W0 F.01 ; Start Point 45 C L Dia. Dia. Dia. Dia. TI2697 Figure G71/G70 Rough and Finish Turning Cycle: Pocket Turning M-504A 6-9

136 Start Point D U C L Z0 TI2698 Figure G71/G70 Rough and Finish Turning Cycle: Tool Paths - NOTE - When programming G71 pocket turning, the following programming rules supersede the corresponding standard G71 programming rules, as outlined on page 6-8. All other programming rules outlined under standard G71 turning still apply. G71 Pocket Turning Programming Rules 1. The value of the W data word in the second G71 block MUST be zero (W0); otherwise, the tool tip may cut into one of the side walls of the pocket. 2. The block specified by the P word in the second G71 block MUST contain a W0 (zero). 3. The contouring path must be a steadily increasing or decreasing pattern on the Z axis only. 4. A maximum of ten pockets can be programmed in the G71 turning cycle M-504A

137 G94 CANNED FACING CYCLE The G94 Canned Facing Cycle provides the programmer with the capability of defining multiple facing passes by specifying only the depth of cut for each pass. The operation may be either straight or taper facing. Figure 6.6 and its accompanying program illustrate an elementary part on the main spindle having a diameter of 1.5 inches that is to be faced back.5 inches with a.5 inch diameter projection remaining. EXAMPLE 5: G94 STRAIGHT FACING (Figure 6.6) N10 G20 ; N110 Z ; N1 (Operator Message) ; N120 Z-.25 ; N20 G10 P0 Z#500 ; N130 Z ; N30 G97 S1000 M13 P1 ; N140 Z-.375 ; N40 M98 P1 ; N150 Z ; N50 T0101 ; N160 Z-.484 ; N60 X1.6 Z.1 ; N170 Z-.5 ; N70 G50 S3800 ; N180 G1 ; N80 G96 S1000 ; N190 M98 P1 ; N90 G1 G99 G94 X.5 Z F.002 ; N200 M1 ; N100 Z-.125 ; N210 M30 ; Start Point C L.500 Spindle Face Chuck Face TI1603 Figure G94 Canned Facing Cycle: Straight Facing M-504A 6-11

138 The X and Z axis tool offsets are activated through the Tool Offset selection in block N50. Turret station #1 is selected and Tool Offset #1 is activated. The Tool Offset allows the programmer to program the X axis position of the tool tip as the actual position relative to the spindle centerline and Z axis position of the tool tip as the actual position relative to Z0 on the machine coordinate system. If a Z axis Work Shift is active (G10 command), the Z axis position of the tool tip will be positioned in relation to the shifted Z0. Since all dimensions are in the inch mode, G20 is entered in block N10. This assures the correct format in case the previously executed program was in metric mode (G21). The cutting tool path is a box pattern. Since the Start Point is also the point to which the tool returns on the return path, the starting point in the X direction was placed at a distance greater than.75 inches from the spindle centerline. This assures that the cutting tool will completely face the workpiece shoulder on each pass. In the Z direction, the start point was placed in front of the workpiece face to ensure that the.5 inch diameter is completely turned on each pass. The G94 Preparatory Command is specified in block N90 along with the depth of cut for the first pass (Z) on relation to Z0 (zero) and the diameter to which the facing operation is to extend (X). The feedrate is also specified. In subsequent blocks (N100 through N170) it is only necessary to specify the depth of cut for each pass in relation to Z0 (zero). Feedrate and spindle speed changes can also be programmed in these blocks. The Feedrate Override switch is active during the facing passes. To deactivate the G94 mode, program another group 1 G code. Refer to the G Code chart in Appendix Two. NOTICE All facing passes MUST be toward the spindle centerline. If the facing operation is programmed to face away from the spindle centerline, the cutting tool will advance into the workpiece at the rapid traverse rate. The approach and return paths are executed at the rapid traverse rate. This rate may be varied with the Rapid Override switch. If Constant Surface Speed or Tool Nose Radius Compensation is used, the parameters MUST be entered prior to the G94 block. In cases where U and W commands are used in place of X and Z make certain each command has the correct sign M-504A

139 EXAMPLE 6: G94 TAPER FACING (Figure 6.7) N10 G20 ; N130 Z ; N1 (Operator Message) ; N140 Z-.15 ; N20 G10 P0 Z#500 ; N150 Z ; N30 G97 S1000 M13 P1 ; N160 Z-.275 ; N40 M98 P1 ; N170 Z ; N50 T0101 ; N180 Z-.4 ; N60 X1.75 Z.2 ; N190 Z ; N70 G50 S3800 ; N200 Z-.49 ; N80 G96 S1000 ; N210 Z-.5 ; N90 G1 G98 G41 X1.6 Z.1 F200. ; N220 G1 ; N100 G99 G94 X.5 Z.1 R F.002 ; N230 M98 P1 ; N110 Z.0375 ; N240 M1 ; N120 Z-.025; N250 M30 ; All rules applying to straight facing in the G94 Canned Facing cycle also apply to taper facing. Figure 6.7 illustrates an elementary part on the main spindle with a 1.5 inch diameter. This part is faced back.5 inches and leaves a shoulder that tapers back 15 degrees. A.5 inch diameter projection remains. The only difference between taper facing and the preceding straight facing example is that the amount of taper in the Z direction, expressed as an R value, must be programmed in the G94 block. Program the R word as a POSITIVE value if the tool moves in the +X direction as it moves in the +Z direction. Program the R word as a NEGATIVE value if the tool moves in the -X direction as it moves in the +Z direction. For this example, R was determined as follows: R = ( x) x (-Tan 15 ) = ( ) x (Unrounded Value) = (Rounded Value) Start Point Spindle Face C L Chuck Face Figure G94 Canned Facing Cycle: Tapered Facing.500 TI1604A M-504A 6-13

140 G72/G70 AUTOMATIC MULTIPLE REPETITIVE ROUGH AND FINISH FACING The G72 Multiple Repetitive Facing Cycle provides the programmer with the capability of describing multiple rough facing passes with two blocks of information. The first G72 block specifies the amount of stock to be removed per pass and the distance the tool will retract from the workpiece for the return pass. The second G72 block specifies the data blocks which define the section of the workpiece to be rough faced, the amount of stock to be left for finish machining, and the feedrate for the G72 roughing cycle. Finally, the G70 Preparatory Command specifies the section of the workpiece to be finish machined by specifying the first and last blocks of the required program section. Figure 6.8 and its accompanying program illustrate an elementary part on the main spindle that is to be rough and finish contoured to the dimensions shown. EXAMPLE 7: G72/G70 FACING CYCLE (Figure 6.8) N10 G20 ; N120 G72 P130 Q180 U.03 W.015 F.01 ; N2 (Operator Message) ; N130 G0 Z-1.25 S800 ; N20 G10 P0 Z#500 ; N140 G1 G99 X3. F.004 ; N30 G97 S1000 M13 P1 ; N150 Z ; N40 M98 P1 ; N160 X1. Z-.375 ; N50 T0202 ; N170 X.75 ; N60 X4.11 Z0.2 ; N180 Z.1 ; N70 G50 S3800 ; N190 G70 P130 Q180 ; N80 G96 S1000 ; N200 M98 P1 ; N90 G1 G98 G41 X4.1 Z.1 F100. ; N210 M1 ; N100 G99 ; N220 M30 ; N110 G72 W.1 R.03 ; W (N120).375 Start Point W (N110) U Spindle Face C L Chuck Face.750 Figure G72/G70 Rough and Finish Facing Cycle TI M-504A

141 The face of the part extends from the face of the spindle. Since block N20 sets the part face to Z0, all facing passes will be in the minus Z direction. The X and Z axis tool offsets are compensated for through the Tool Offset selection in block N50. Turret Station #2 is selected and Tool Offset #2 is activated. The Tool Offset allows the programmer to program the X axis position of the tool tip as the actual position relative to the spindle centerline and Z axis position of the tool tip as the actual position relative to Z0 on the machine coordinate system. If a Z axis Work Shift is active (G10 command), the Z axis position of the tool tip will be positioned in relation to the shifted Z0, as established by the Work Shift offset. Since all dimensions are in the inch mode, G20 is entered in block N10. This assures the correct format in case the previously executed program was in metric (G21) mode. The start point commanded in block N90 must be located outside the area occupied by the blank stock. Block N110 will establish the parameters for the rough facing cycle: N110 G72 W.1 R.03 ; Where: G72 = Preparatory command for the repetitive rough facing cycle. W: Specifies the depth of cut of each pass during the roughing cycle. R: Specifies the distance the tool will retract from the workpiece for the return pass. Block N120 will execute the rough facing cycle: N120 G72 P130 Q180 U.03 W.015 F.01 ; Where: G72 = Preparatory command for the repetitive rough facing cycle. P: Sequence number of the first block in the program section that controls the workpiece area being roughed out. Q: Sequence number of the last block in the program section that controls the workpiece area being roughed out. U: Amount of stock on the X axis to be left for removal during the finish machining cycle. This is a diameter value W: Amount of stock on the Z axis to be left for removal during the finish machining cycle. F: Feedrate for the roughing passes. The decimal point must be programmed. Block N130 establishes the Constant Surface Speed value for the G70 finishing cycle: N130 G0 Z-1.25 S800 ; S: The surface feet per minute for the finishing pass. M-504A 6-15

142 Block N140 establishes the inch per revolution feedrate for the G70 finishing cycle. N140 G1 G99 X3. F.004 ; F: The feedrate for the finishing pass. The decimal point must be programmed. Block N190 designates the section of the workpiece to be finish machined by specifying the first (P) and the last (Q) blocks of the required program section: N190 G70 P130 Q180 ; Where: G70 = Preparatory command for the finishing cycle. P: Sequence number of the first block in the program section that controls the workpiece area being finish machined. Q: Sequence number of the last block in the program section that controls the workpiece area being finish machined. When the control encounters the G72 preparatory command blocks, the amount of finish stock as specified by the U and W words is treated as a pair of offsets. The slides will move in the direction and distance specified. The U and W words MUST be properly signed (+ or -) to ensure that slide movements occur in the direction to leave stock for finishing. If the sign is omitted, the control automatically assumes plus (+). In this example, the cross slide will move.015 in the +U direction and the carriage will move.015 in the +W direction. The control will then cause the machine to execute multiple roughing passes.1 inches deep and a roughing contour pass (as shown by the dashed lines in Figure 6.6) that follows the contour as designated by blocks N130 through N180. After completion of the roughing contour pass, the finish pass will be executed according to the program section specified by the G70 block. The amount of tool withdrawal after completion of each pass is controlled by the R word in block N110 (R0.03). The spindle speed for the roughing passes is specified in block N80. It is recommended that the spindle speed be established before the G72 blocks to ensure the spindle reaches full commanded speed before the roughing passes begin. Spindle speed and feedrate changes for the finish cycle can be made at will between the starting and ending blocks as designated by P and Q in the G70 block. Tool changes (T function) for the roughing cycle MUST be made prior to the first G72 block. Tool offset changes for the finishing cycle can be made within the blocks designated by the P and Q words in the G70 block. In this example the same tool is used for roughing and finishing; therefore, Tool Nose Radius Compensation must be established in a block preceding the first G72 block. Tool Nose Radius Compensation is activated and interpolated in the move to the starting point commanded in block N90. Tool Nose Radius Compensation is deactivated during the G71 cycle and reactivated after the G72 cycle is completed. Compensation is canceled by a G40 command in subroutine O1", which is called by line N200. Also see Tool Nose Radius Compensation" Chapter 2. If Constant Surface Speed is to be used, it must be established in blocks preceding the first G72 block. Feedrate for the roughing passes may be established prior to the G72 blocks or in the second G72 block. If a different surface speed and feedrate is required for the finishing pass, it must be established in the part program after the second G72 block. Surface speed and feedrate can be changed at will between the starting and ending block as designated by the P and Q words in the G70 block M-504A

143 The spindle speed command that must precede entry into Constant Surface Speed mode is programmed in block N30. Maximum spindle speed is established by the S word and the G50 Preparatory command in block N70. Constant Surface Speed is established by the G96 command in block N80 and surface speed for the roughing cycle by the S word in the same block. Surface speed for the finishing pass is established in block N130. Constant Surface Speed is canceled by the G97 command in sub-program O1" after the workpiece has been finish machined. Also see Constant Surface Speed, in Chapter 9. The feedrate for the finishing pass is established in block N140. G72 PROGRAMMING NOTES 1. A block specified by a P word cannot contain an X move. 2. G00 or G01 should be programmed in the block specified by the P word. 3. The contouring path must be a steadily increasing or decreasing pattern. 4. No subprogram can be called in the program between the start of the cycle designated by P and the end of the cycle designated by Q. 5. It is not necessary to program a return to the start point at the end of the program. The control automatically returns the slides to the start point after the block specified by Q is executed. 6. If Tool Nose Radius Compensation is to be used, it must be programmed prior to the first G72 block. Tool Nose Radius Compensation will be deactivated during the G72 cycle and reactivated after the G72 cycle is completed. 7. If Constant Surface Speed is to be used, it must be programmed prior to the first G72 block. 8. Tooling changes for the roughing cycle must be made prior to the first G72 block. Tool offset changes for the finishing cycle may be made within the blocks designated by the P and Q words. 9. The spindle speed and feedrate for the roughing cycle can be specified prior to the first G72 block or in the second G72 block. The spindle speed and feedrate for the finishing cycle can be specified within the blocks designated by the P and Q words. M-504A 6-17

144 G73/G70 AUTOMATIC ROUGH AND FINISH PATTERN REPEAT The G73 Canned Pattern Repeat Cycle provides the programmer with the capability of repeatedly cutting a fixed pattern (contour) with two blocks of information. The first block specifies the incremental distance between the first and last roughing pass and the number of roughing passes to be executed. The second block specifies the section of the workpiece to be roughed out, the amount of stock to be left for finish machining, and the roughing feedrate. Finally, the G70 Preparatory Command specifies the section of the workpiece to be finish machined by specifying the first and last block of the required program section. This automatic cycle is especially useful for rough and finish contouring a workpiece whose rough shape has already been created by casting, forging or rough machining. If this cycle is to be used to contour a workpiece from bar stock, make certain the first pass starts at a point that will not cause excessive hogging on the first pass. Figure 6.9 illustrates an elementary part on the main spindle that is to be finished to the dimensions shown with three roughing passes and a finishing pass. It is assumed the configuration of the blank workpiece approximates that of the finish piece. EXAMPLE 8: G73/G70 PATTERN REPEAT CYCLE (Figure 6.9) Sample Program N10 G20 ; N130 G0 X.5 ; N7 (Operator Message) ; N140 G1 G99 Z-.25 F.002 ; N20 G10 P0 Z#500 ; N150 X.75 ; N30 G97 S1000 M13 P1 ; N160 X1. Z ; N40 M98 P1 ; N170 Z-.72 ; N50 T0707 ; N180 X1.5 Z-.97 ; N60 X2.15 Z.2 ; N190 Z-1.25 ; N70 G50 S3000 ; N200 X2.05 ; N80 G96 S500 ; N210 G70 P130 Q200 ; N90 G1 G98 G42 X2.05 Z.1 F100. ; N220 M98 P1 ; N100 G99 ; N230 M1 ; N110 G73 U.135 W.05 R3 ; N240 M30 ; N120 G73 P130 Q200 U.03 W.015 F.01 ; - NOTE - The legends in lower half of Figure 6.9 are explained as follows: U1 = U (N110) U2 = U (N120) W1 = W (N110) W2 = W (N120) Since all dimensions are in the inch mode, G20 is entered in block N10. This assures the correct format in case the previously executed program was in metric (G21) mode. The start point commanded in block N90 must be located outside the maximum diameter occupied by the blank stock to be machined M-504A

145 Start Point C L Spindle Face Chuck Face W 1 +W 2 U 1 U 2 Start Point U 1 +U 2 W 2 W 1 TI1606 Figure G73/G70 Rough and Finish Pattern Repeat M-504A 6-19

146 Block N110 will establish the parameters for the G73 rough facing cycle: N110 G73 U.135 W.05 R3 ; U: Distance and direction of relief in the X axis direction. (radius value) This value tells the control the amount of material to be removed from the workpiece in the X direction. This value will allow the control to calculate the correct distance and direction to pull away from the workpiece before beginning the automatic cycle. This programmed value is equal to the amount of stock to be removed from each side during the roughing cycle minus the depth of the first cut and finish allowance on each side. Example: Total amount of stock to remove =.200 (radius value) Depth of first cut = X axis finish amount left = Programmed U word (Block N110) =.135 W: Distance and direction of relief in the Z axis direction. This value tells the control the amount of material to be removed from the workpiece in the Z direction. This value will allow the control to calculate the correct distance and direction to pull away from the workpiece before beginning the automatic cycle. This programmed value is equal to the amount of stock to be removed during the roughing cycle minus the depth of the first cut and finish allowance. R: The number of rough passes desired. - NOTE - The above entries are modal and are not changed until another value is programmed. Block N120 will execute the G73 rough facing cycle: N120 G73 P130 Q200 U.03 W.015 F.01 ; P: Sequence number of the first block for the program section that controls the workpiece area being roughed out. Q: Sequence number of the last block for the program section that controls the workpiece area being roughed out. U: Distance and direction of finishing allowance in X direction (diameter value). W: Distance and direction of finishing allowance in Z direction. F: Feedrate to be active during the automatic roughing cycle. The decimal point must be programmed. Block N140 establishes the inch per revolution feedrate for the G70 finishing cycle. N140 G1 G99 Z-.25 F.002 ; F: The feedrate for the finishing pass. The decimal point must be programmed M-504A

147 G73 PROGRAMMING NOTES 1. G00 or G01 should be programmed in the block specified by the P word. 2. No subprogram can be called in the program between the start of the cycle designated by P and the end of the cycle designated by Q. 3. It is not necessary to program a return to the start point at the end of the program. The control automatically returns the slides to the start point after the block specified by Q is executed. 4. If Tool Nose Radius Compensation is to be used, it must be programmed prior to the first G73 block. Tool Nose Radius Compensation will be deactivated during the G73 cycle and reactivated after the G73 cycle is completed. 5. If Constant Surface Speed is to be used, it must be programmed prior to the first G73 block. 6. Tooling changes for the roughing cycle must be made prior to the first G73 block. Tool offset changes for the finishing cycle may be made within the blocks designated by the P and Q words in the G70 block. 7. The spindle speed and feedrate for the roughing cycle can be specified prior to the first G73 block or in the second G73 block. The spindle speed and feedrate for the finishing cycle can be specified within the blocks designated by the P and Q words in the G70 block. M-504A 6-21

148 G70 AUTOMATIC FINISHING CYCLE After rough cutting by G71, G72, or G73, the following command permits finishing. G70 P(starting block) Q(finishing block) ; Refer to the sections on the G71, G72, and G73 automatic cycles for G70 programming examples. P: Sequence number of the first block in the program section that controls the workpiece area to be finish machined. Q: Sequence number of the last block in the program section that controls the workpiece area to be finish machined. G70 PROGRAMMING NOTES NOTICE Never position the Start Point below the Q Line diameter. When the G70 finish turn is completed, the tool rapids back to the Start Point. 1. F, S and T words programmed between sequence numbers P and Q, as defined by the G70 program block will be recognized by the G70 cycle. 2. When the G70 Automatic Finishing Cycle is completed, the tool is returned to the start point and the next block is read. 3. In blocks between the starting block and finishing block programmed in G70 through G73, subprograms cannot be called M-504A

149 AUTOMATIC DRILLING CYCLES In any auto deep hole drilling cycle, the Z axis is reversed at prescribed intervals to provide for proper chip removal. An automatic drilling cycle must be flexible enough to accommodate a wide variety of materials and a full range of hole depths. It is the programmer s responsibility to make certain that the programmed parameters result in a cycle that satisfactorily removes chips during the drilling operation. If the chip load builds up: The drill bit could break. The spindle could stall. The Z axis servo motor could overload. G74 CONSTANT DEPTH INCREMENT AUTOMATIC DRILLING CYCLE A G74 command activates an automatic drilling cycle that uses constant depth increments. All information for the cycle is programmed in two data blocks. The data word formats are defined in the section below and illustrated in Figure NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. Block Format Inch Programming G74 R(e) ; G74 Z(W)±2.5 Q7 F3.2 (in/min) or F1.6 (in/rev) ; Metric Programming G74 R(e) ; G74 Z(W)±3.4 Q7 F5.0 (mm/min) or F3.4 (mm/rev) ; M-504A 6-23

150 Start Point W Z C L +Z R Q TI2159A Figure G74 Automatic Drilling Cycle Parameters Where: G74 = G code for Automatic Drilling Cycle (Constant Depth Increments) R = Amount of retract between cutting moves. Z = Z coordinate of Final Hole Depth (signed) W = Z Increment from Start Point to Final Depth (signed) Q = Size of Depth Increment (unsigned) F = Feedrate. Before the G74 block is encountered, the drill must be positioned at the start point. During execution of the cycle, the series of Z axis moves (see Figure 6.10) is as follows: a) From the start point, the drill feeds in Q amount. b) The drill retracts at rapid traverse R amount. c) The drill feeds in Q+R amount. d) The drill continues to rapid retract R amount, then feed in Q+R amount until the last pass. On the last pass, the drill feeds in to the final hole depth, then rapid retracts to the start point M-504A

151 Q Word Programming The control assumes decimal point placement as Q2.5 for English units (inches) and Q3.4 for Metric units (millimeters). Decimal point programming is NOT allowed with the Q data word. Leading zeros may be omitted, however trailing zeros MUST be programmed. Refer to the following examples: Inch: Q25000 =.25 inches Metric: Q25000 = 2.5 millimeters Q = 2.50 inches Q = 25.0 millimeters G74 Automatic Drilling Sample Program In this sample program, Z0 (zero) is the face of the part and the final depth of the hole is 1.5 inches. Refer to Figure Sample Program N7 (Operator Message) ; N260 X0. Z.1 ; N220 G10 P0 Z#500 ; N270 G74 R.05 ; N230 G97 S1000 M13 P1 ; N280 G74 G99 Z-1.5 Q25000 F.005 ; N240 M98 P1 ; N290 M98 P1 ; N250 T0707 ; N300 M1; C L Start Point (X0. Z.1) TI2160B Figure G74 Automatic Drilling Cycle: Sample Workpiece M-504A 6-25

152 R WORD (N270) Specifies the amount of retract between each cutting move of the drill bit. Refer to R, in Figure In this example, the amount of retract is.05 inches. F WORD (N280) Specifies the feedrate for the G74 Automatic Drilling Cycle. In this example, the feedrate is.005 inches per revolution. Q WORD (N280) Specifies the depth of cut in the Z direction. In this example, the depth of cut is.25 inches. Decimal point programming is NOT allowed with the Q word. The Q word in this sample program is structured for Super-Precision lathes. Z WORD (N280) Specifies the final depth of the drilled hole, in reference to Z0 (zero). In this example, the final depth of the drilled hole is 1.5 inches. Instead of programming Z-1.5 in block N280, we could have programmed W-1.6 (the incremental distance from the start point to the final hole depth) and the cycle would have behaved exactly the same way M-504A

153 VARIABLE DEPTH INCREMENT AUTOMATIC DRILLING CYCLE The G74 Automatic Drilling Cycle has limited applications because of its constant infeed, constant retract increments, and absence of a dwell. To create a more versatile automatic drilling cycle, Hardinge Inc. has developed an auto drilling cycle with variable depth increments, a retract point clear of the part, and a programmable dwell at the retract point. All information required for this drilling cycle is programmed in one data block. - NOTE - The values shown in the following data blocks are data word format designations, NOT actual dimensions. Decimal point programming MUST be used in data blocks containing macro calls. Block Format Inch Format: G65 P9136 K±2.5 B2.5 F1.6 W2.5 C2.5 A5.1 Z±2.5 ; Metric Format: G65 P9136 K±3.4 B3.4 F3.4 W3.4 C3.4 A5.1 Z±3.4 ; Data Word Definitions G65 = G Code for Macro Call P9136 = Macro Program 9136 (Deep Drill) K = Z Axis End Position (SIGNED absolute value) B = Start Feed Increment Value (Incremental value, always positive) F = Drill Feedrate per Revolution W = Depth of First Drill In-Feed C = Minimum Increment A = Amount of Dwell (in seconds) at Retract Point Z = First Rapid-to-Feed Point Inside Workpiece (SIGNED absolute value) Optional Command, refer to page 6-32 Refer to Figures 6.12 and 6.13 to see how these data words relate to the workpiece. M-504A 6-27

154 C L ZStartPoint B C C 3rd Pass 2nd Pass 1st Pass (W) K ZEndPoint Rapid Traverse Feed TI2163 Figure Macro 9136: Deep Drill Cycle Parameters (Main Spindle) ZStartPoint C L B 1st Pass (W) 2nd Pass 3rd Pass C C K Rapid Traverse Feed ZEndPoint TI4226 Figure Macro 9136: Deep Drill Cycle Parameters (Sub-Spindle) 6-28 M-504A

155 Positioning the Drill The data block preceding the block calling Deep Drill Macro Program 9136 will position the drill tip at the start point for the drilling cycle. All retract motion during the drilling cycle will be to this start point. MAIN SPINDLE OPERATION The face of the workpiece will be set to Z0 by the work shift; therefore, the Z axis start point will be located at a positive Z coordinate. Based on the positive sign of the Z axis start point, the macro program will verify the sign of the K data word is negative. Program Block Structure: X0. Z.1 ; G65 P9136 K- B W F C A Z- ; SUB-SPINDLE OPERATION The face of the workpiece will be set to Z0 by the work shift; therefore, the Z axis start point will be located at a negative Z coordinate. Based on the negative sign of the Z axis start point, the macro program will verify the sign of the K data word is positive. Program Block Structure: X0. Z-.1 ; G65 P9136 K B W F C A Z ; Calculating the Drill Pass Increments 1. 1st Pass Increment = Specified by the W word. 2. 2nd pass increment =.5 times the 1st pass increment. 3. 3rd pass increment =.5 times the 2nd pass increment. 4. 4th pass increment =.5 times the 3rd pass increment. The control will not allow the pass increment to drop below the minimum pass increment, as established by the C word. - NOTE - If desired, the value of W can be increased or decreased to lengthen or shorten the first pass depth. This will have a direct affect on the rest of the passes. M-504A 6-29

156 Macro 9136 without Optional Z Word SAMPLE PART DESCRIPTION A.25 inch diameter hole, 1.5 inches deep, is to be drilled in a piece of 1-3/16 inch diameter stock. The part has already been center drilled and the face of the workpiece is set to Z0 (zero) in block N160. The depth of the first pass is to be.75 inches. A one-half second dwell is programmed at the retract position. The start feed increment will be set to.02 inches and the minimum increment will be set to.0625 inches. EXAMPLE 1: MAIN SPINDLE (Refer to Figure 6.14) Sample Program Segment:.. N140 M98 P1 ; N150 M1 ; N2 (Operator Message) ; N160 G10 P0 Z#500 ; N170 G97 S1400 M13 P1 ; N180 M98 P1 ; N190 T0202 ; N200 X0. Z.1 ; N210 G65 P9136 K-1.5 B.02 F.008 W.75 C.0625 A.5 ; N220 M98 P1 ; N230 M1 ; C L Second Rapid-to-Feed Point (X0. Z-.73) Start Point (X0. Z.1) First Rapid-to-Feed Point (X0. Z.02) Z0 TI2166 Figure Macro Program 9136: Main Spindle Operation without the Optional Z Word 6-30 M-504A

157 EXAMPLE 2: SUB-SPINDLE (Refer to Figure 6.15) Sample Program Segment:.. N140 M98 P2 ; N150 M1 ; N2 (Operator Message) ; N160 G10 P0 Z#501 ; N170 G97 S1400 M13 P1 ; N180 M98 P2 ; N190 T0202 ; N200 X0. Z.-1 ; N210 G65 P9136 K1.5 B.02 F.008 W.75 C.0625 A.5 ; N220 M98 P2 ; N230 M1 ; Start Point (X0. Z-.1) C L First Rapid-to-Feed Point (X0. Z-.02) Second Rapid-to-Feed Point (X0. Z.73) Z0 TI4227 Figure Macro Program 9136: Sub-Spindle Operation without the Optional Z Word M-504A 6-31

158 Macro 9136 with Optional Z Word NOTICE The Z word is an optional command and is NOT TO BE PROGRAMMED UNLESS REQUIRED. MAIN SPINDLE OPERATION Assuming the part face has been set to Z0, a Z word with a negative value may be programmed if the drill is to start inside the workpiece; for example, inside a counterbore. The depth of the counterbore will be programmed in the macro data block as a negative value, assuming the face of the workpiece is set to Z0. The drill will rapid into the counterbore a distance equal to the value of the Z word plus the value of the B word. The drill will feed in from this position at the programmed feedrate. Refer to Example 3, on page SUB-SPINDLE OPERATION Assuming the part face has been set to Z0, a Z word with a positive value may be programmed if the drill is to start inside the workpiece; for example, inside a counterbore. The depth of the counterbore will be programmed in the macro data block as a positive value, assuming the face of the workpiece is set to Z0. The drill will rapid into the counterbore a distance equal to the value of the Z word minus the value of the B word. The drill will feed in from this position at the programmed feedrate. Refer to Example 4, on page SAMPLE PART DESCRIPTION A.25 inch diameter hole, 1.5 inches deep from the face of the workpiece, is to be drilled in a piece of 1-3/16 inch diameter stock. The bottom of the counterbore has already been center drilled and the face of the workpiece is set to Z0 (zero) in block N160. The hole will begin at the base of a.25 inch counterbore. The depth of the first pass is to be.75 inches. A one-half second dwell is programmed at the retract position. The start feed increment will be set to.02 inches and the minimum increment will be set to.0625 inches M-504A

159 EXAMPLE 3: MAIN SPINDLE (Refer to Figure 6.16) The only difference between this sample program segment and the sample program segment in Example 1 is that in this sample the drill bit will rapid from the start point (X0. Z.1) to X0. Z-.23 before going to the programmed feedrate. The coordinate location X0. Z-.23 was determined by adding the Feed Increment Value (B word) to the value of the programmed Z word. Sample Program Segment.. N140 M98 P1 ; N150 M1 ; N2 (Operator Message) ; N160 G10 P0 Z#500 ; N170 G97 S1400 M13 P1 ; N180 M98 P1 ; N190 T0202 ; N200 X0. Z0.1 ; N210 G65 P9136 K-1.5 B.02 F.008 W.75 C.0625 A.5 Z-.25 ; N220 M98 P1 ; N230 M1 ; C L Start Point (X0. Z.1) Second Rapid-to-Feed Point (X0. Z-.98) First Rapid-to-Feed Point (X0. Z-.23) Z0 TI2174 Figure Macro Program 9136: Main Spindle Operation with the Optional Z Word M-504A 6-33

160 EXAMPLE 4: SUB-SPINDLE (Refer to Figure 6.17) The only difference between this sample program segment and the sample program segment in Example 2 is that in this sample the drill bit will rapid from the start point (X0. Z-.1) to X0. Z.23 before going to the programmed feedrate. The coordinate location X0. Z.23 was determined by subtracting the Feed Increment Value (B word) from the value of the programmed Z word. The following sample program segment is written for lower turret operation. Sample Program Segment.. N140 M98 P2 ; N150 M1 ; N2 (Operator Message) ; N160 G10 P0 Z#501 ; N170 G97 S1400 M13 P1 ; N180 M98 P2 ; N190 T0202 ; N200 X0. Z-0.1 ; N210 G65 P9136 K1.5 B.02 F.008 W.75 C.0625 A.5 Z.25 ; N220 M98 P2 ; N230 M1 ; Start Point (X0. Z.-1) C L First Rapid-to-Feed Point (X0. Z.23) Second Rapid-to-Feed Point(X0.Z.98) Z0 TI4228 Figure Macro Program 9136: Sub-Spindle Operation with the Optional Z Word 6-34 M-504A

161 G75 AUTOMATIC GROOVING CYCLE BLOCK FORMAT All information for the G75 Automatic Grooving Cycle is programmed in two data blocks, as follows: Inch Format G75 R2.4 ; G75 X(U)±2.4 Z(W)±2.4 P6 Q6 F3.2 (ipm) or F1.6 (ipr); Metric Format G75 R3.3 ; G75 X(U)±3.3 Z(W)±3.3 P6 Q6 F5.0 (mmpm) or F3.4 (mmpr); - NOTE - The values shown in the preceding data blocks are data word format designations, NOT actual dimensions. Where: G75 = G code for Automatic Grooving Cycle (Constant Depth Increments) R = Amount of retract between cutting moves. X = X coordinate at full depth of pass (signed) U = Incremental distance from X axis start point to X axis final position (signed) Z = Z axis position for final pass (signed) W = Incremental distance from first pass Z axis position to last pass Z axis position (signed) P = Size of depth increment (unsigned) Q = Incremental amount of Z axis move between full cutting passes (unsigned) F = Feedrate. Refer to Figure 6.18 to see how these data words relate to the workpiece. M-504A 6-35

162 P AND Q WORD PROGRAMMING On High Performance lathes, the control assumes decimal point placement as P2.4 and Q2.4 for English units (inches) and P3.3 and Q3.3 for Metric units (millimeters). On Super-Precision lathes, the control assumes decimal point placement as P2.5 and Q2.5 for English units (inches) and P3.4 and Q3.4 for Metric units (millimeters). Decimal Point programming is NOT allowed with the P or Q data words. Leading zeros may be omitted; however trailing zeros MUST be programmed. Refer to the following examples: HIGH PERFORMANCE LATHES Inch: P2500 =.25 inches Metric: P2500 = 2.5 millimeters P25000 = 2.50 inches P25000 = 25.0 millimeters Inch: Q2500 =.25 inches Metric: Q2500 = 2.5 millimeters Q25000 = 2.50 inches Q25000 = 25.0 millimeters SUPER-PRECISION LATHES Inch: P25000 =.25 inches Metric: P25000 = 2.5 millimeters P = 2.50 inches P = 25.0 millimeters Inch: Q25000 =.25 inches Metric: Q25000 = 2.5 millimeters Q = 2.50 inches Q = 25.0 millimeters TOOL MOVEMENT SEQUENCE Before the G75 blocks are encountered, the grooving tool must be positioned at the X and Z axis start point. During execution of the cycle, the series of X and Z axis moves (Refer to Figure 6.18) is as follows: a) From the start point, the tool feeds in P amount. b) The tool retracts at rapid traverse R amount. c) The tool feeds in P+R amount. d) The tool continues to rapid retract R amount, then feed in P+R amount until the last pass. On the last pass, the tool feeds in a distance equal to or less than P until the final depth is reached. e) The tool rapid retracts to the X axis start position. f) The tool moves toward the Z axis end point a distance specified by the Q word to arrive at the start point for the next full cut. g) Steps a through f are repeated until the entire groove is completed. h) When the final cut is completed, the tool rapid retracts to the X axis start position; then rapids to the X and Z axis start point specified by the program blocks immediately preceding the G75 blocks M-504A

163 1 4 W Start Point Z0 U U X,Z C L C L 2 5 P U C L C L 3 6 Q ZAxis Movement R C L C L TI2164A Figure G75 Automatic Grooving Cycle Parameters M-504A 6-37

164 G75 AUTOMATIC GROOVING SAMPLE PROGRAM In this sample program segment, X0 (zero) is the spindle centerline, Z0 (zero) is the face of the workpiece and the final depth of the groove is.25 inches. The width of the grooving tool is.125 inches. Refer to Figure NOTE - The P word in block N300 is an incremental value. Each cutting pass will be an actual.075 inch cut. Sample Program Segment N7 (Operator Message) ; N270 G50 S5200 P1 ; N220 G10 P0 Z#500 ; N280 G96 S280 ; N230 G97 M13 ; N290 G75 R.02 ; N240 M98 P1 ; N300 G75 G99 X.5 Z-.8 P750 Q1000 F.005 ; N250 T0707 ; N310 M98 P1 ; N260 X1.1 Z-.625 ; N320 M1 ; R WORD (N290) Specifies the incremental amount of retract between each cutting move of the grooving tool. Refer to R, in Figure In this example, the amount of retract is.02 inches. F WORD (N300) Specifies the feedrate for the G75 Automatic Grooving Cycle. In this example, the feedrate is.005 inches per revolution. +X.800 +Z.500 Start Point (X1.1 Z-.625) C L Dia Dia..500 Dia. TI2165 Figure G75 Automatic Grooving Cycle: Sample Workpiece 6-38 M-504A

165 P WORD (N300) Specifies the incremental depth of each cutting move in the X direction. In this example, the depth of each cutting move is.075 inches. Decimal point programming is NOT allowed with the P word. Q WORD (N300) Specifies the incremental move in the Z direction between each full cutting pass. In this example, the incremental move is.100 inches. Decimal point programming is NOT allowed with the Q word. X WORD (N300) Specifies the X axis position of the tool at the end of each complete cutting pass, in reference to X0 (zero). In this example, the X axis position is X.5 inches. Z WORD (N300) Specifies the Z axis position for the final full cutting pass, in reference to Z0 (zero). In this example, the final Z axis position is Z-.8 inches. - NOTE - If the Z values in blocks N260 and N300 are swapped, the tool will begin at Z-.8 and finish at Z M-504A 6-39

166 POLYGON TURNING INTRODUCTION The purpose of polygon turning is to provide the capability of turning a symmetrical polygon on the outside diameter of a workpiece. Polygon turning can be performed on the main spindle or the optional sub-spindle. Refer to Spindle Selection, below. The type of polygon produced is determined by the following factors: the ratio between the spindle speed and the rotational speed of the polygon turning live tooling cutter the number of cutting edges on the tool (2 or 3) The size of the polygon is determined by the following factors: diameter and cutting depth of the polygon turning live tooling cutter diameter of the workpiece The spindle speed is programmed through the use of the S word. The cutter speed is programmed in the G51.2 program block as a ratio of the spindle speed. The location of the tool tip on the polygon turning live tooling cutter is defined in terms of X,Y coordinates. SPINDLE SELECTION - NOTE - It is not possible to enable polygon turning on both spindles at the same time. Setting parameter 7640 to 1 will enable polygon turning on the main spindle. Setting parameter 7640 to 2 will enable polygon turning on the sub-spindle. Parameter 7640 can be set from a program or through the manual data input keyboard. Program Entry Program Format: G10 L50 ; Activate Parameter Entry Mode N7640 R1 (or R2) ; Sets parameter 7640 to 1 (or 2) G11 ; Cancel Parameter Entry Mode Manual Data Input Keyboard Entry Refer to the operator s manual (M-505) for information on changing machine parameters through the manual data input panel M-504A

167 G CODES Two G codes are used to control polygon turning. G51.2 Activates polygon turning. Refer to Block Format, below. G50.2 Cancels polygon turning. BLOCK FORMAT G51.2 P_ Q_ ; G51.2 = Activate polygon turning P_ = Spindle speed factor (Range: 1 to 9) Q_ = Live tooling speed factor (Range: 1 to 9) (Positive value = Live tool forward rotation) (Negative value = Live tool reverse rotation) The ratio between the spindle speed factor (P word) and the live tooling speed factor (Q word) determines the rotational speed of the polygon turning live tool. Example 1: Spindle speed is 1000 rpm G51.2 P1 Q2 ; Live tool forward rotation, 2000 rpm Example 2: Spindle speed is 1000 rpm G51.2 P1 Q3 ; Live tool forward rotation, 3000 rpm Example 3: Spindle speed is 1000 rpm G51.2 P1 Q-2 ; Live tool reverse rotation, 2000 rpm M-504A 6-41

168 RT RW RW RT RT CROWNING Crowning is a result of the relative elliptical path of each tool tip in relation to the workpiece. The amount of crowning is dependent upon the radius of the workpiece and the radius of the polygon turning live tooling cutter. The amount of crowning will decrease as the radius of the polygon turning live tooling cutter increases in relation to the radius of the workpiece. Refer to Figure Rw+f Direction of Rotation Direction of Rotation Corner to corner distance (Actual, due to crowning) f Corner to corner distance (Theoretical) = Radius of polygon turning live tooling cutter = Radius of workpiece f = Crown (radius value) TI4749 Figure Example of Crowning During Polygon Turning 6-42 M-504A

169 SELECTING THE CUTTER AND SPEED RATIO NOTICE The actual speed of the polygon turning live tooling cutter must be 1000 rpm or greater. Select a spindle speed and speed factor values that will result in cutter speed of 1000 rpm or greater. For clearance purposes: the polygon turning live tooling cutter should always be running at a higher rpm than the machine spindle. use a one tooth cutter and program a speed ratio of 1:2 when cutting two flats on a workpiece. Refer to the chart shown below. The number of sides on the polygon to be produced will indicate the number of teeth on the polygon turning live tooling cutter that must engage the workpiece per revolution of the spindle. Equation: Number of Sides Teeth per Cutter Speed Ratio Refer to the examples listed in the following chart: Polygon Type Number of Sides Teeth per Cutter Spindle Speed Factor Live Tool Speed Factor (2 Flats) Square Pentagon Hexagon Hexagon Octagon M-504A 6-43

170 SAMPLE PROGRAM SEGMENTS These sample program segments involve a single plunge cut on the outer diameter of the workpiece. When machining on the end of the workpiece, the width of the cutter must be equal to or greater than the width of the polygon to be machined. Typically, a single plunge cut requires the width of the cutter to be equal to the width of the polygon to be machined. When machining on the end of the workpiece, the width of the cutter can be equal to or greater than the width of the polygon to be machined. Main Spindle Program Segment.. N2 (Operator Message) ; N160 G10 P0 Z#500 ; Set Main Spindle Work Shift N170 G97 S1000 M14 P1 ; Main Spindle Reverse 1000 RPM, Coolant ON N180 M98 P1 ; Call Safe Index Subprogram O1 N190 T0202 ; Select Tool and Tool Offset N200 G0 X4. Z.875 ; Move to Start Point N210 M52 S2000 P3 ; Activate Live Tooling at 2000 RPM N220 G51.2 P1 Q2 ; Activate Polygon Turning, Speed Ratio 1:2 N230 G1 X.75 F.4 ; Cut to Depth N240 G4 X2. ; Dwell 2 seconds N250 G0 X4. Rapid Away from Workpiece N260 G50.2 ; Cancel Polygon Turning N270 M5 ; Main Spindle Stop, Coolant OFF N280 M98 P1 ; Call Safe Index Subprogram O1 N290 M1 ; Option Stop M-504A

171 Sub-Spindle Program Segment.. N2 (Operator Message) ; N160 G10 P0 Z#501 ; Set Sub-Spindle Z Axis Work Shift N170 G97 S1000 M33 P2 ; Sub-Spindle Forward 1000 RPM N180 M98 P2 ; Call Safe Index Subprogram O2 N190 T0202 ; Select Tool and Tool Offset N200 G0 X4. Z-.875 M08 ; Move to Start Point, Coolant ON N210 M52 S2000 P3 ; Activate Live Tooling at 2000 RPM N220 G51.2 P1 Q2 ; Activate Polygon Turning, Speed Ratio 1:2 N230 G1 X.75 F.4 ; Cut to Depth N240 G4 X2. ; Dwell 2 seconds N250 G0 X4. Rapid Away from Workpiece N260 G50.2 ; Cancel Polygon Turning N270 M35 ; Sub-Spindle Stop N280 M98 P2 ; Call Safe Index Subprogram O2 N290 M1 ; Option Stop.. CANCELING POLYGON TURNING Polygon turning is canceled by any of the following: Programmed G50.1 Control OFF Emergency Stop Servo alarm Control Reset P/S alarm 217, 218, 219, 220, or 221. Refer to the Fanuc operator s manual for information on these alarms. M-504A 6-45

172 - NOTES M-504A

173 CHAPTER 7 - THREADING CYCLES INTRODUCTION The feedrate for precision threading should be lead limited to 120 inches [3048 mm] per minute. Above this value, to the maximum machine feedrate, the lead error should be checked to make certain it does not exceed specifications for the individual thread being produced. It is the programmer s responsibility to ensure that the combination of lead and spindle speed does not exceed a feedrate which produces threads that are not within specifications. The maximum spindle speed for a given thread lead is calculated through the use of the following formulas: English Threads: Maximum rpm = 120 inches/minute Thread Lead Metric Threads: Maximum rpm = 3048 millimeters/minute Thread Lead SINGLE BLOCK THREADCUTTING The spindle encoder monitors RPM during a threading pass and when feeding in Inches/Millimeters per Revolution (G99). The encoder sends data relating axis position and velocity to the servo drives. With the Single Block Threadcutting feature, the programmer can cut a thread in any desired number of passes using either the G32 or G92 preparatory command. The principle differences between the two commands are: 1. The G92 command causes the X axis movements of the threading tool to be controlled automatically by the machine during the threading cycle. The G32 command is used to program each threading pass individually. 2. The G92 command requires fewer blocks of information for a complete threading operation. The feedrate of the carriage and/or cross slide is determined by programming the thread Lead using the F word address. The format for F is: Inch Programming: F1.6 Metric Programming: F3.4 M-504A 7-1

174 - NOTE - Thread pitch is the axial distance from the center of one thread to the center of the next. Lead is the distance the screw will advance when turned one revolution. On a single thread screw, the pitch and lead are equal since a screw will advance an amount equal to the pitch when turned one revolution. On a double thread the screw will advance two threads or twice the pitch in one revolution. Therefore, the programmed lead is twice the pitch. Program the spindle speed for a threading operation in a block of data preceding the threadcutting calling block (G32 or G92). This will allow time for the spindle speed to stabilize before entering the threadcutting mode. The Feedrate Override switch is not active during a G32 or G92 threadcutting pass unless it is set to 0%. When the Feedrate Override switch is set to 0%, axis motion WILL STOP. The spindle Increase Override and Decrease Override push buttons are active. The Feed Hold push button allows the operator to immediately retract the tool from the workpiece during a threading pass. Refer to the operator s manual (M-505) for information on the Thread Cutting Cycle Retract feature. ESTABLISHING A START POINT FOR THREADING For accurate thread leads it is essential that the per revolution feedrate of the tool is held constant during the threading pass. The location of the start point for each threading pass is important in that sufficient distance must be provided to accelerate the tool from its Z axis velocity at the end of the infeed to the proper threading velocity. Due to the nature of the servo-controlled axis drive system, provide a minimum of four leads or.250 inch, whichever distance is greater, between the first thread to be cut and the start point for the threading pass. The X axis start point should be equal to the diameter of the workpiece plus two times the single depth of thread. - NOTE - This minimum clearance must be provided for all threading passes. If a compound infeed is used, (see Compound Infeed Threading, page 7-8) work backwards to calculate the start point for the cycle. Beginning with the last threading pass, calculate the Z axis motion during infeed for the first pass. Add this distance to the Z axis clearance (four leads or.250 inch, whichever is greater). This gives the Z axis position of the start point for the cycle relative to the first thread to be cut. 7-2 M-504A

175 G32 PROGRAMMING The G32 Threadcutting command, which must be programmed in each threadcutting data block, automatically synchronizes the threadcutting mode so that the same thread is cut in each pass. The G32 command is modal and remains active until canceled by another Group 1 G code. Only one axis need be programmed for a straight thread; both axes must be programmed for a tapered thread. The thread length and lead must be programmed in each G32 block. EXAMPLE 1: G32 STRAIGHT THREADS For this example it is assumed that the part has been turned to the required diameter and is ready to have a.0625 lead, single start, 1.00 inch long thread cut on its O.D. Refer to Figure 7.1. The face of the part is set to Z0. All threading passes will, therefore, be in the minus Z direction. The spindle centerline is X0. G98 is activated by Safe Index Subprogram O1 in block N360. Sample Program Segment N7 (T0707 7/8-16 THREAD) ; N450 X.951 ; N340 G10 P0 Z#500 ; N460 G0 Z.25 ; N350 G97 S500 M13 P1 ; N470 G1 X.8176 F50. ; N360 M98 P1 ; N480 G32 Z-1. F.0625 ; N370 T0707 ; N490 X.951 ; N380 X.951 Z.25 S1920 ; N500 G0 Z.25 ; N390 G1 G98 X.8559 F50. ; N510 G1 X.7984 F50. ; N400 G32 Z-1. F.0625 ; N520 G32 Z-1. F.0625 ; N410 X.951 ; N530 G1 X.951 ; N420 G0 Z.25 ; N540 M98 P1 ; N430 G1 X.8367 F50. ; N550 M1 ; N440 G32 Z-1. F.0625 ; Single Depth of Thread = x Lead = C L.0383 Lead Z0 TI1607 Figure G32 Threading Cycle: Straight Thread M-504A 7-3

176 EXAMPLE 2: G32 TAPERED THREADS When programming tapered threads, movements must be programmed in both the X and Z axes. The lead is specified by the F word, whose lead orientation (X or Z axis) is determined by the angle of the taper with the part centerline. If the angle of taper B, Figure 7.2, is less than or equal to 45 degrees, the value of F is measured parallel to the Z axis. If angle of the taper is greater than 45 degrees, F is measured parallel to the X axis. For the example shown, it is assumed that the part has been turned to the required 1 degree 47 minute taper and is ready to have a lead, single start thread 1.25 inches long turned on its O.D. The value of the lead F is measured parallel to the Z axis because the angle of taper is less than 45 degrees. The face of the part is set to Z0. All threading passes will, therefore, be in the minus Z direction. The spindle centerline is X0. Sample Program Segment N7 (T TAPER THREAD) ; N450 X1.614 ; N340 G10 P0 Z#500 ; N460 G0 Z.2857 ; N350 G97 S1000 M13 P1 ; N470 G1 X F50. ; N360 M98 P1 ; N480 G32 X Z-1.25 F ; N370 T0707 ; N490 X1.614 ; N380 X1.614 Z.2857 S1680 ; N500 G0 Z.2857 ; N390 G1 G98 X F50. ; N510 G1 X F50. ; N400 G32 X Z-1.25 F ; N520 G32 X Z-1.25 F ; N410 X1.614 ; N530 X1.614 ; N420 G0 Z.2857 ; N540 M98 P1 ; N430 G1 X F50. ; N550 M1 ; N440 G32 X Z-1.25 F ; Single Depth of Thread =.8 x Lead =.0571 Angle B = 1 47 Taper (R) =.0478 Start Point Lead B C L Z0 TI2583 Figure G32 Threading Cycle: Tapered Thread 7-4 M-504A

177 G92 CANNED THREADING CYCLE The G92 Threadcutting command provides the programmer with the capability to define multiple threading passes by specifying only the depth of cut for each pass. The G92 lead and thread length commands are programmed in the first threadcutting data block only. Only positions in the X (U) axis (thread pass coordinate) need be programmed in subsequent blocks. The G92 command is modal and remains active until canceled by another Group 1 G code. When cutting a tapered thread, an R word must be programmed in the G92 block. EXAMPLE 3: G92 STRAIGHT THREADS For this example, it is assumed that the part has been turned to the required diameter and is ready to have a.0625 lead, single start, 1.00 inch long thread cut on its O.D. The face of the part extends 3.00 inches from the face of the spindle. This value is stored in the Work Shift offset. This causes the face of the part to be set to Z0. All threading passes will be in the minus Z direction. Refer to Figure 7.3. The tool nose reference point is 1.25 inches from the turret face in the -X direction and.25 inches in the -Z direction. These dimensions are stored in the Tool Offset (Geometry) file under offset 07 as positive values. The offset is activated by the T0707 command in block N370. Sample Program Segment N7 (T0707 7/8-16 THREAD) ; N400 X.8367 ; N340 G10 P0 Z#500 ; N410 X.8176 ; N350 G97 S500 M13 P1 ; N420 X.7984 ; N360 M98 P1 ; N430 G0 ; N370 T0707 ; N440 M98 P1 ; N380 X.951 Z0.25 S1920 ; N450 M1 ; N390 G92 X.8559 Z-1. F.0625 ; Single Depth of Thread = x Lead =.0383 Start Point Return Path Lead C L Z0 TI2582 Figure G92 Threading Cycle: Straight Thread M-504A 7-5

178 Note that the start point, block N380, must be outside the thread O.D. as this point establishes the return path after the completion of each threading pass. Block N390 establishes the threading mode, the X coordinate for the first pass (X.8559), thread length (Z-.75) and lead (F.0625). In subsequent blocks, N400 through N420, it is only necessary to program the X coordinate for each pass until the final depth is reached in block N420. A G00 code MUST be on the line after the last threading pass. If the G00 code is not present, the tool will make two extra passes on the workpiece at the last programmed thread depth. EXAMPLE 4: G92 TAPERED THREADS O.D. tapered threads are programmed as a Negative R word in the G92 block to define the amount of taper. I.D. tapered threads are programmed with Positive R words in the G92 block. For the example shown, it is assumed that the part has been turned to the required 1 degree 47 minute taper and is ready to have a lead, single start, 1.25 inch long thread turned on its O.D. The value of the lead F is measured parallel to the Z axis and R is measured parallel to the X axis because the angle of the taper is less than 45 degrees. Refer to Figure 7.4. The face of the part extends 2.25 inches from the face of the spindle. This value is stored in Work Shift offset as Z Storing the part length as a Work Shift offset causes the face of the part to be set to Z0. All threadcutting passes will be in the minus Z direction. Sample Program Segment N7 (T TAPER THREAD) ; N400 X ; N340 G10 P0 Z#500 ; N410 X ; N350 G97 S1000 M13 P1 ; N420 X ; N360 M98 P1 ; N430 X ; N370 T0707 ; N440 G0 ; N380 X1.614 Z.2857 S1680 ; N450 M98 P1 ; N390 G92 X Z-1.25 F R ; N460 M1 Single Depth of Thread =.8 x Lead =.0571 Angle B = 1 47 Taper (R) =.0478 Start Point Lead B C L Z0 Figure G92 Threading Cycle: Tapered Thread TI M-504A

179 The tool tip is located on the turret centerline and extends 1.25 inches from the turret face. The tool dimensions are stored in the Tool Offset (Geometry) file under offset number 07. Note that the start point, block N380, must be outside the thread O.D. as this point establishes the return path after completion of each threading pass. Block N390 establishes the threading mode, the X coordinate for the first pass (X1.4771), thread length (Z-1.25), lead (F ), and amount of taper (R-.0478). In subsequent blocks, N400 through N440, it is only necessary to program the X coordinate for each pass until the final thread depth is reached in block N440. Notice that the sign of R must be minus to cause the threading tool to move in the plus X direction. See R Word in G76 Automatic Multiple Repetitive Threading Cycle, page If the angle of taper B is less than or equal to 45 degrees, the value of F is measured parallel to the Z axis. If the angle of taper is greater than 45 degrees, F is measured parallel to the X axis. PLUNGE INFEED THREADING A plunge infeed is used in the threading example shown in Figure 7.1. During a plunge infeed, Figure 7.5, the tool moves along the X axis from the start point for the threading cycle to the start point for the current threading pass. Infeed is at 90 degrees relative to the spindle centerline. The next block contains the threading G Code (G32) which synchronizes axis motion with spindle rotation. When the spindle is properly oriented, axis motion begins at the commanded per revolution feedrate. As illustrated in Figure 7.5, an equal amount of material is removed by each edge of the tool. Return Path Start Point First Pass Second Pass Third Pass Fourth Pass TI1611 Figure Plunge Infeed M-504A 7-7

180 COMPOUND INFEED THREADING When machining a material that presents threading difficulties due to its toughness or when cutting a coarse thread of extreme depth, it is often desirable to infeed the tool so that the leading edge of the tool cuts the major portion of the material. This reduces deformation of the tool nose due to pressure and heat, thus adding to the tool life. To accomplish this, the X and Z axis position of the tool at the start point of each pass is altered to produce the desired infeed angle, as shown in Figure 7.6. This is known as Compound Infeed. When using compound infeed, the Z axis start point is shifted by an amount determined by the X axis shift ( X) and the desired angle of the compound infeed. In Figure 7.7, the infeed angle, designated, is at 25 degrees relative to the face of the part. The incremental shift in the Z axis start point for each pass ( Z) is calculated with the following equation (Refer to Figure 7.7): Z = X x Tan During a compound infeed thread, Figure 7.6, the tool moves on the X axis from threading cycle start point to the start point for the current threading pass. After the threading pass, the tool moves along the return path to the next Z axis start position, which is equal to the previous Z axis start point minus Z. When the spindle is properly oriented, axis motion begins. With a compound infeed, the Z axis position of the tool, at the start of each cut, is closer to the part face than it was on the previous pass. The result of this is that the majority of all metal removal takes place along the leading edge of the tool with the trailing edge making a slight clean-up cut. Return Path Start Point First Pass Second Pass Third Pass Fourth Pass TI1612A Figure Compound Infeed 7-8 M-504A

181 Figure 7.7 illustrates how the incremental shift in the Z start position for the compound infeed is calculated for each threading pass. Where: X 1 = X Axis Position for the 1st Pass. X 2 = X Axis Position for the 2nd Pass. X 3 = X Axis Position for the 3rd Pass. X 4 = X Axis Position for the 4th Pass. = Infeed Angle Z 1 = Initial Z Axis Start Point Z 2 =Z 1 - Z Z 3 =X 2 - Z Z 4 =Z 3 - Z Z 1 Z 2 Z 4 Z 3 X X 1 X 2 X 3 X 4 Z C L TI1613A Figure Z Start Point for Compound Infeed M-504A 7-9

182 The following program segment has been taken from Example 1 and modified to incorporate compound infeed (Refer to Figure 7.1): N7 (T0707 7/8-16 THREAD) ; N450 X.951 ; N340 G10 P0 Z#500 ; N460 G0 Z.2411 ; N350 G97 S1920 M13 P1 ; N470 G1 X.8176 F50. ; N360 M98 P1 ; N480 G32 Z-1. F.0625 ; N370 T0707 ; N490 X.951 ; N380 X.951 Z.25 ; N500 G0 Z.2366 ; N390 G1 G98 X.8559 F50. ; N510 G1 X.7984 F50. ; N400 G32 Z-1. F.0625 ; N520 G32 Z-1. F.0625 ; N410 X.951 ; N530 G1 X.951 ; N420 G0 Z.2455 ; N540 M98 P1 ; N430 G1 X.8367 F50. ; N550 M1 ; N440 G32 Z-1. F.0625 ; CALCULATIONS Single Depth of Thread= x Lead =.0383 (Radius Value) Number of Threading Passes = 4 (Infeed Angle)= 25 Incremental Change in Depth per Pass ( X) = (Radius Value) (Diameter Value) Incremental Change in Z ( Z) = X (Radius Value) x Tan 25 = x = Coordinate Values for each Threading Pass X 1 = = X 2 = = X 3 = = X 4 = = Z 1 = Z 2 =Z = Z 3 =X = Z 4 =Z = M-504A

183 G76 AUTOMATIC MULTIPLE REPETITIVE THREADING CYCLE The G76 Multiple Repetitive Threading Cycle provides the programmer with the capability of defining a complete threading operation with two blocks of information. The control interprets the data in these two blocks and generates the multiple passes required to cut an entire thread. This automatic threading cycle can be used for cutting straight or tapered threads of constant lead in either Absolute or Incremental mode. The thread may be either external or internal. Plunge (X axis) or compound (X and Z axis) infeed can be performed. BLOCK FORMAT Specification of the threading cycle parameters is achieved by using the G76 preparatory command and its associated parameters as follows: Inch Programming: G76 P6 Q5 R0.5 ; G76 X(U)±2.5 Z(W)±2.5 R±1.5 P5 Q5 F1.6 ; Metric Programming: G76 P6 Q4 R1.4 ; G76 X(U)±3.4 Z(W)±3.4 R±2.4 P4 Q4 F3.4 ; - NOTE - Decimal point programming cannot be used when programming the P or Q words in a G76 Multiple Repetitive Threading Cycle. With leading zero suppression, the decimal point is not programmed. Leading zeros can be omitted, but all trailing zeros must be programmed. Example: The format for the P word in the execution line is P5 for Inch mode and P4 for metric mode. The format for the Q word in the execution line is Q5 for Inch mode and Q4 for metric mode. The numbers indicate the number of places to the right of the assumed decimal point. The control counts from right to left, inserts the decimal point the number of places from the right as set by the format. Leading zeros will be automatically inserted when required. M-504A 7-11

184 EXAMPLE 5: G76 STRAIGHT THREADS (Constant lead on a part having a uniform diameter.) For this example, it is assumed that the part has been turned to the required diameter and is ready to have a.125 lead, single start thread, 1.75 inches long cut on its O.D. The thread is to be cut in ten passes on a High Performance lathe. Refer to Figure 7.8. Sample Program Segment N4 (T THREAD) ; N190 G10 P0 Z#500 ; N200 G97 S500 M13 P1 ; N210 M98 P1 ; N220 T0404 ; N230 X Z.5 S960 ; N240 G76 P Q0015 R.0004 ; N250 G76 X Z-1.75 P0767 Q0242 F.125 ; N260 M98 P1 ; N270 M1 ; Single Depth of Thread = x Lead =.0383 FWord.125 Return Path Start Point X Z.500 PWord.0767 Z QWord.0242 X C L Z0 TI2580 Figure G76 Threading Cycle: Straight Thread 7-12 M-504A

185 EXAMPLE 6: G76 TAPERED THREADS (Constant lead on a tapered part) For this example, it is assumed that the part has been turned to the required 1 47 taper and is ready to have a lead, single start thread, 1.25 inch long thread cut on its O.D. Refer to Figure 7.9. N9 (T Taper Thread) ; N90 G10 P0 Z#500 ; N100 G97 S1000 M13 P1 ; N110 M98 P1 ; N120 T0909 ; N130 X1.614 Z.2857 S1100 ; N140 G76 P Q0015 R.0004 ; N150 G76 X Z-1.25 P0571 Q0120 R F ; N160 M98 P1 ; N170 M1 ; Return Path Start Point R F Tool Tip Angle Q P Angle B X C L Angle B = 1 47 Thread Lead F = Single Depth of Thread =.8 x Lead =.0571 First Pass Depth =.012 Note: All Dimensions are in inches. Z Z0 ZStart Part Diameter = Length of Thread = Start Point Coordinates: X1.614 Z.2857 TI2581 Figure G76 Threading Cycle: Tapered Thread M-504A 7-13

186 G76 PARAMETER LINE (Figures 7.8 and 7.9) P Word (First G76 Block) The number of finishing passes is specified by parameter 723 and has a valid range from 1 to 99. This parameter is set by the first two digits in the P word located in the first line of the G76 programming blocks. The thread chamfer (anticipated pullout) amount is specified by parameter 109 and has a valid range from 00 to 99. This range allows the programmer to specify a chamfer amount from 0.0 times the thread lead to 9.9 times the thread lead. This parameter is set by the second two digits in the P word located in the first line of the G76 programming blocks. A setting of 00 will pull straight out of the part. A setting of 10 will have an anticipated pullout of one lead. The tool nose angle is specified by parameter 724 and can be set to 0, 29, 30, 55, 60, or 80 degrees. This parameter is set by the last two digits in the P word located in the first line of the G76 programming blocks. A 0 setting will give a plunge feed. Decimal point programming is NOT allowed with the P word. Refer to Block Format, page 7-11, for the data word format. Q Word (First G76 Block) Parameter 725 specifies the minimum depth of cut for a threading pass and is set by this data word. Decimal point programming is NOT allowed with the Q word. Refer to Block Format, page 7-11, for the data word format. R Word (First G76 Block) Parameter 726 specifies the finish pass allowance per side and is set by this data word. For the examples shown in Figures 7.8 and 7.9, R.0004 will leave.0004 inches per side for the clean-up pass. Refer to Block Format, page 7-11, for the data word format M-504A

187 G76 EXECUTION LINE P Word (Second G76 Block) Specifies the single depth of the thread and is always positive. It is measured parallel to the X axis. The P Word value for an American National Thread is calculated as follows: Straight Thread: Single Depth of Thread = Number of Threads per Inch Tapered Thread: Single Depth of Thread =.8 Number of Threads per Inch See Figure 7.8 for the P word definition when cutting a straight thread and Figure 7.9 when cutting a tapered thread. Decimal point programming is NOT allowed with the P data word. Refer to Block Format, page 7-11, for the data word format. Q Word (Second G76 Block) Specifies the cutting depth of the first pass and is always positive. It is measured parallel to the X axis. See Figure 7.8 for the Q word definition when cutting a straight thread and Figure 7.9, when cutting a tapered thread. This value is calculated by dividing the Single Depth of Thread by the square root of the number of threading passes to be taken. Decimal point programming is NOT allowed with the Q data word. Refer to Block Format, page 7-11, for the data word format. F Word (Second G76 Block) Specifies the thread lead and is always positive. It is measured parallel to the Z axis for straight threads. It is measured parallel to the Z axis for tapered threads when the angle of the workpiece centerline is equal to or less than, 45 degrees. If the angle of taper with the workpiece centerline is greater than 45 degrees, it is measured parallel to the X axis. Refer to Block Format, page 7-11, for the data word format. X Word (Second G76 Block) For a straight external thread the X word specifies the root (Minor) diameter of the thread. For a straight internal thread the X word specifies the O.D. (Major Diameter) of the thread. When cutting tapered threads, the X word specifies the root (Minor) diameter at the large end of the external thread or O.D. (Major) diameter at the small end for an internal thread. The sign will be positive for cutting on the back side of the spindle centerline (+X). Refer to Block Format, page 7-11, for the data word format. M-504A 7-15

188 Z Word (Second G76 Block) In Absolute programming mode the Z word specifies the Absolute Z coordinate at the end of the thread. Unless the face of the part has been set to Z Zero by a Work Shift offset, Z will be relative to the spindle face. When a Work Shift is used, Z will be relative to the face of the part. The sign of Z will be positive when measured from the spindle face and negative when measured from the face of the part. Refer to Block Format, page 7-11, for the data word format. R Word (Second G76 Block) The R word is only programmed when tapered threads are to be produced. When it is programmed, the R word must be in the second G76 block. The R word specifies the amount of taper in a tapered thread and is measured parallel to the X axis. It is calculated as follows: R = W * TAN B (* = Multiplication) (B = Angle of taper with workpiece centerline) The R word may be programmed as R0 (zero) or omitted when cutting a straight thread. When cutting a tapered thread, length W must include the additional travel required for the start point on the Z axis. When cutting a tapered thread in the +X direction, as shown in the example, R must have a NEGATIVE (-) value. If the minus sign is not used, R is assumed to be positive and the taper will be cut in the -X direction or opposite the direction shown. The same rule applies to internal threads cut on the +X side of the spindle centerline. A conventional pipe thread would require a NEGATIVE R for O.D. threading and a POSITIVE R value for I.D. Threading. Refer to Block Format, page 7-11, for the data word format. G76 PROGRAMMING NOTES 1. After the initial pass, the control automatically calculates the depth of cut based on a constant volume removal of material. The minimum cutting depth is controlled by parameter 725. This parameter is controlled by the Q word in the first G76 block. 2. During the return path the control defaults to rapid traverse. If a slower rate is desired use the Rapid Override switch. 3. For precision threadcutting, the feedrate should be lead limited to 120 inches per minute. 4. The number of clean-up passes is set by parameter 723. This parameter is controlled by the first two digits in the P word in the first G76 block. As shipped from Hardinge Inc., this parameter is set at 1. It may be set from 1 to 99 passes. 5. The Reset button is active during the threading pass. The Feedrate Override switch is disabled during a G76 Automatic Threading Cycle unless it is set to 0%. When the Feedrate Override switch is set to 0%, axis motion will stop M-504A

189 G34 VARIABLE LEAD THREADCUTTING The Variable Lead Threadcutting feature enables the programmer to cut straight or tapered threads having linear increasing or decreasing leads. The G34 code is used to prepare the control for cutting leads of either type. The length of thread is determined by the distance command for X and/or Z. Only one axis need be programmed for a linear thread; both axes must be programmed for a tapered thread. The initial thread lead is determined by programming an F word. For tapered threads, F is measured parallel to the Z axis when the angle of taper with the workpiece centerline is equal to or less than 45 degrees. When the angle is greater than 45 degrees, F is measured parallel to the X axis. The rate at which the thread lead increases or decreases is programmed as a K word. This is the linear increase or decrease per revolution - not the change in lead per inch. It is calculated from the formula: K = [Final Lead 2 - Initial Lead 2 ] [2 x Thread Length] - NOTE - When solving the preceding formula for threads with decreasing lead, the value of K will be negative. The minus sign must be programmed for a thread with decreasing lead or the control will assume plus and cut a thread with increasing lead. The maximum spindle speed that can be programmed when cutting variable lead threads is determined by the maximum lead from the formula: Maximum rpm = 120 ipm Maximum Lead When cutting a thread with decreasing lead, if the K word is large enough to decrease the thread lead to zero before the end of the thread is reached, the control will go into a Cycle Stop and an alarm message will be displayed on the control display screen. The Feedrate Override switch is not active during a threadcutting pass. The G34 command is modal and remains active until canceled by another Group 1 G code. The data words have the following format: Inch Programming: X(U)±2.4, Z(W)±2.4, F1.6, K±1.6 Metric Programming: X(U)±3.3, Z(W)±3.3, F3.4, K±3.4 - NOTE - The Threadcutting Cycle Retract feature is NOT active during G34 Variable Lead Threadcutting. M-504A 7-17

190 LEFT-HAND THREADS If left-hand threads are to be cut from right to left (-Z direction, tool path toward the spindle face), the spindle must be run in the reverse (M04) direction. This will require the tool to be mounted cut side up on the turret top plate. If left-hand threads are to be cut from left to right (+Z direction, tool path toward the part face), the spindle must be running in the forward (M03) direction. This will require the threading tool tip to be mounted upside down on the turret top plate. When this method is used, a relief of.25 inches [6.35 mm] or four times the thread lead, whichever is greater, is required to ensure that lead error does not occur. This clearance is necessary to allow the CNC control to synchronize spindle and axis motion and also to prevent ringing of the first thread M-504A

191 TAPPING Use a self-releasing style tap holder with sufficient longitudinal float to allow the spindle to reverse direction. The Hardinge Model TT-5/8 and TT-3/4 tap holders have a pullout to release increment of 3/32 inch, which is sufficient. 1. Program a dwell to allow the spindle to reach the programmed speed before the tool engages the workpiece. Minimum Dwell (Previous Spindle Speed Tapping Spindle Speed) Use the G32 Preparatory Command. 3. Program the lead command F.001 inch (.0254 mm) per revolution less than the thread lead where practical. 4. Minimum dwell for holder release is determined as follows: Tap Pullout x Minimum Dwell ( ) ( 60 ) ( Lead) x ( RPM) 5. Reverse spindle and feed out at lead (F), a distance Z that is sufficient to clear the workpiece. EXAMPLE Tap a ¼-20 thread, ½ inch deep using a Hardinge TT-5/8 tap holder. Previous spindle speed was 1500 rpm. Spindle speed is 250 RPM. Minimum dwell (step 1) for spindle speed change is determined as follows: Dwell ( ) seconds Minimum dwell (step 4) for Hardinge TT-5/8 tap holder is determined as follows: (. 094) x ( 60) Dwell. 45 seconds (. 05) x ( 250) (Rounded to nearest tenth of a second equals.5). M-504A 7-19

192 SAMPLE PROGRAM SEGMENT NOTICE During set up, the operator must activate AUTO mode before line 190 is read by the control. SINGLE mode (block-by-block) execution should not be used for spindle reversal (M04). Tap breakage or thread damage will occur. It is suggested that the operator activate AUTO mode after completion of line 150. Assume that the part length has been stored as a Work Zero Offset and that tool offset dimensions have been stored in Tool Offset (Geometry) file. - NOTE - Hole was drilled to a depth greater than the depth of the tapped thread. N5 (T0505 ¼-20 Tap) ; N110 G10 P0 Z#500 ; N120 G97 S250 M13 P1 ; N130 M98 P1 ; N140 T0505 ; N150 X0. Z0.5 ; N160 G4 X1.25 ; N170 G32 Z-0.5 F0.049 ; N180 G4 X0.5 ; N190 M14 ; N200 G32 Z0.5 F0.05; N210 M98 P1 ; N220 M1 ; Operator Message Set Main Spindle Work Shift Spindle Forward 250 RPM, Coolant ON, Spindle Select Call Safe Index Subprogram O1 Select Tool and Tool Offset Approach Dwell for 1.25 Sec. for Spindle Speed Change Tap Dwell.5 Seconds Spindle Reverse, Coolant ON Clear Workpiece by.50 Inch Call Safe Index Subprogram O1 Optional Stop 7-20 M-504A

193 RIGID TAPPING Rigid tapping is performed through interpolation between the X or Z axis and the spindle. When rigid tapping is active, the spindle rotates one revolution as the X or Z axis is fed a distance equal to the lead of the tap. This eliminates the need for a floating tap holder. This capability allows high speed, high precision tapping. Rigid tapping can be performed on the main or sub-spindle. Rigid tapping is activated by the M29 command. RIGID TAPPING WITH STANDARD TOOLING (Non-Live Tooling) NOTICE The basic programming formats shown in this section must be used when performing rigid tapping with standard tooling. - NOTE - A spindle speed (S word) must be programmed in the M29 data block after the M29 command. These programming formats are written for 20 threads per inch. Modify the tool assignment and data values as needed for the thread to be produced. M-504A 7-21

194 Program Formats for Standard Tooling TURRET AT THE MAIN SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S500 M13 P1 ; Spindle Forward 500 RPM, Coolant ON, Spindle Select M98 P1 ; Call Safe Index Subprogram O1 T0505 ; Select Tool and Tool Offset G0 X0. Z.1 ; Approach M29 S500 ; Activate Rigid Tapping Mode G84 G99 Z-1. F.05 ; Tapping Cycle Data G80 ; Cancel Tapping Cycle M98 P1 ; Call Safe Index Subprogram O1 M01 ; Option Stop TURRET AT THE SUB-SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift G97 S500 M33 P2 ; Sub-Spindle Forward 500 RPM, Spindle Select M98 P2 ; Call Safe Index Subprogram O2 T0505 ; Select Tool and Tool Offset G0 X0. Z.-1 M8 ; Approach, Coolant ON M29 S500 ; Activate Rigid Tapping Mode G84 G99 Z1. F.05 ; Tapping Cycle Data G80 ; Cancel Tapping Cycle M98 P2 ; Call Safe Index Subprogram O2 M01 ; Option Stop 7-22 M-504A

195 RIGID TAPPING WITH LIVE TOOLING NOTICE The basic programming formats shown in this section must be used when performing rigid tapping with live tooling. - NOTE - These programming formats are written for 20 threads per inch. Modify the tool assignment and data values as needed for the thread to be produced. Program Formats for Live Tooling END-WORKING ATTACHMENT AT THE MAIN SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift M98 P1 ; Call Safe Index Subprogram O1 T0505 ; Select Tool and Tool Offset M54 S500 P3 ; Live Tool Forward, 500 RPM, Coolant ON, Spindle Select G0 X1.5 Z.1 C0. ; Approach, Orient Main Spindle M29 S500 ; Activate Rigid Tapping Mode G84 G99 Z-1. F.05 ; Tapping Cycle Data, Tap Hole #1 Z-1. C90. ; Orient Main Spindle and Tap Hole #2 Z-1. C180. ; Orient Main Spindle and Tap Hole #3 Z-1. C270. ; Orient Main Spindle and Tap Hole #4 G80 ; Cancel Tapping Cycle M55 ; Live Tool Stop M98 P1 ; Call Safe Index Subprogram O1 M01 ; Option Stop M-504A 7-23

196 CROSS-WORKING ATTACHMENT AT THE MAIN SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift M98 P1 ; Call Safe Index Subprogram O1 T0505 ; Select Tool and Tool Offset M53 S500 P3 ; Live Tool Forward, 500 RPM, Coolant ON, Spindle Select G0 X2.5 Z-.75 C0. ; Approach, Orient Main Spindle M29 S500 ; Activate Rigid Tapping Mode G88 G99 X1.75 F.05 ; Tapping Cycle Data, Tap Hole #1 X1.75 C90. ; Orient Main Spindle and Tap Hole #2 X1.75 C180. ; Orient Main Spindle and Tap Hole #3 X1.75 C270. ; Orient Main Spindle and Tap Hole #4 G80 ; Cancel Tapping Cycle M55 ; Live Tool Stop M98 P1 ; Call Safe Index Subprogram O1 M01 ; Option Stop 7-24 M-504A

197 END-WORKING ATTACHMENT AT THE SUB-SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift M98 P2 ; Call Safe Index Subprogram O2 T0505 ; Select Tool and Tool Offset M54 S500 P3 ; Live Tool Forward, 500 RPM, Coolant ON, Spindle Select G0 X1.5 Z-.1 A0. ; Approach, Orient Sub-Spindle M29 S500 ; Activate Rigid Tapping Mode G84 G99 Z1. F.05 ; Tapping Cycle Data, Tap Hole #1 Z1. A90. ; Orient Sub-Spindle and Tap Hole #2 Z1. A180. ; Orient Sub-Spindle and Tap Hole #3 Z1. A270. ; Orient Sub-Spindle and Tap Hole #4 G80 ; Cancel Tapping Cycle M55 ; Live Tool Stop M98 P2 ; Call Safe Index Subprogram O2 M01 ; Option Stop M-504A 7-25

198 CROSS-WORKING ATTACHMENT AT THE SUB-SPINDLE N10 (Rigid Tap) ; Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift M98 P2 ; Call Safe Index Subprogram O2 T0505 ; Select Tool and Tool Offset M53 S500 P3 ; Live Tool Forward, 500 RPM, Coolant ON, Spindle Select G0 X2.5 Z.75 A0. ; Approach, Orient Sub-Spindle M29 S500 ; Activate Rigid Tapping Mode G88 G99 X1.75 F.05 ; Tapping Cycle Data, Tap Hole #1 X1.75 A90. ; Orient Sub-Spindle and Tap Hole #2 X1.75 A180. ; Orient Sub-Spindle and Tap Hole #3 X1.75 A270. ; Orient Sub-Spindle and Tap Hole #4 G80 ; Cancel Tapping Cycle M55 ; Live Tool Stop M98 P2 ; Call Safe Index Subprogram O2 M01 ; Option Stop 7-26 M-504A

199 THREAD MILLING - NOTE - Thread milling requires the optional Y axis. INTRODUCTION Thread milling is capable of producing threads of superior quality than those produced by conventional tapping. Thread milling involves coordinating the rotation and linear motion of the live tooling used for the thread milling operation. Helical Interpolation is used to rotate the live tooling one revolution (360 ) while moving on the X axis a distance equal to the thread lead. CONVENTIONAL MILLING AND CLIMB MILLING It is recommended that climb milling be used whenever possible. Climb milling offers the following advantages over conventional milling: Lower cutting forces Better thread quality Longer insert life Better chip development GENERAL GUIDELINES 1. The preferred method of entry and exit is to arc into and out of the workpiece. 2. The radius of the tool is stored in the R column of the tool geometry offset. 3. A tool quadrant of 0 or 9 is stored in the T column of the tool geometry offset. 4. To simplify programming, program all moves as incremental moves. WORK PLANE SELECTION - NOTE - When performing thread milling on the side of the work piece, G19 specifies the Z,Y plane selection. G19 must be active for Circular Interpolation and Tool Nose Radius Compensation to function properly during thread milling. M-504A 7-27

200 INTERNAL THREAD MILLING Variable Definitions and Formulas D O D P D CL R E R I = Major Diameter = Minor Diameter = Pitch Diameter = Starting Clearance = Entry Radius =D 2 R O =D O 2 Entry Radius Formula: R E ( RI CL) 2 2 RO 2R O Programming Example Thread Description: 1-1/8 x 20 Major Diameter: Minor Diameter: Pitch Diameter: Entry Radius Calculation: R E ( RI CL) RO ( ) R O BASIC TOOL MOTION 1. Position the tool at the center of the hole to be milled. 2. Move the X axis to thread depth plus ¼ of the thread lead. 3. Move the Y axis in the positive direction to clear the minor diameter by.02 inches. 4. Arc into the workpiece, moving upward ¼ lead on the X axis. 5. Helical Interpolation on the Z and Y axes for the radial move (360 ) while making a linear move upward 1 lead on the X axis. 6. Arc out of the workpiece, moving upward ¼ lead on the X axis M-504A

201 SAMPLE PROGRAM SEGMENT - NOTE - Tool motion indicated in this program segment is illustrated in Figure The flat on the sample workpiece, shown in Figure 7.11, was machined in a previous operation. This example uses climb milling to produce a right-hand thread, starting at the bottom of the hole and milling out. Incremental programming is used to simplify programming. Refer to Figure N6 ; M98 P1 ; Call Safe Index Subprogram O1 T0606 ; Select Tool and Tool Offset G97 S4000 M53 P3 ; Live Tool Forward, 4000 RPM, Coolant ON, Spindle Select G0 X1.7 Z-.9 ; Cutter to Hole Center G1 G98 X.55 F20. ; Feed X Axis to Thread Depth + ¼ Lead (Motion 1) G19 ; Select Work Plane G1 G98 G41 V.5155 W0. F8. ; Move to Y Axis Clearance Position (Motion 2) G3 W.5625 V U.025 R.5175 ; Entry Arc (Motion 3) G3 K U.1 ; Mill Thread (Motion 4) G3 W V U.025 R.5175 ; Exit Arc (Motion 5) G1 G40 Y0. W0. ; Move to Center of Hole and Cancel Tool Compensation (Motion 6) G18 ; Select Work Plane X2. F20. ; Move to Clear Workpiece M98 P1 ; Call Safe Index Subprogram O1 M55 ; Live Tool Stop M01 ; Optional Stop TI4534 Figure Tool Motion for Sample Program Segment (Viewed on the X Axis) M-504A 7-29

202 TI4533 Figure Workpiece for Sample Program Segment 7-30 M-504A

203 EXTERNAL THREAD MILLING Variable Definitions and Formulas D O D P D CL R E R I = Major Diameter = Minor Diameter = Pitch Diameter = Starting Clearance = Entry Radius =D 2 R O =D O 2 Entry Radius Formula: R E ( RO CL) 2 2 RI 2R I Basic Tool Motion 1. Position the tool as follows: Y Axis: Z Axis: Clear of the Workpiece at the center of the post to be milled 2. Move the X axis to the Start Point. 3. Move the Y axis in the negative direction to position the tool clear the major diameter by.02 inches. 4. Arc into the workpiece, moving ¼ lead on the X axis. 5. Helical Interpolation on the Z and Y axes for the radial move (360 ) while making a linear move upward 1 lead on the X axis. 6. Arc out of the workpiece, moving ¼ lead on the X axis. M-504A 7-31

204 - NOTES M-504A

205 CHAPTER 8 - G80 SERIES CYCLES NOTICE Live tooling attachments are available with or without through-tool coolant capability. Live tooling attachments without through-tool coolant capability can be run with or without coolant, as the machining process requires. Live tooling attachments with through-tool coolant capability MUST be run with coolant turned ON. INTRODUCTION The control offers six G80 series cycles. The G80 series includes a cycle for each of the following operations: Face and Side Drilling Face and Side Tapping Face and Side Boring CANCELING CYCLES Cycles MUST be canceled immediately after completion. If a cycle is not canceled and axis motion is commanded, the axes will move to the new coordinate position and execute the active cycle. Program a G80 command in a data block by itself immediately after the last data block to be acted on by the cycle. SPINDLE ORIENT B axis and C axis spindle orient are included with the live tooling feature. B axis and C axis spindle orient are separate purchased options on machines not equipped with the live tooling feature. Refer to Chapter 11 for information on programming spindle orient. M-504A 8-1

206 GENERAL DESCRIPTIONS G83 FACE DRILLING CYCLE The G83 cycle performs drilling operations on the face of the workpiece. The G83 cycle is extremely versatile, in that it can perform the single-pass, peck, or high speed peck drilling. Refer to page 8-3 for a description of the G83 Face Drilling Cycle. G84 FACE TAPPING CYCLE The G84 cycle performs tapping operations on the face of the workpiece. The G84 cycle taps to depth, reverses tool direction, and feeds out at the programmed feedrate. Refer to page 8-15 for a description of the G84 Face Tapping Cycle. G85 FACE BORING CYCLE The G85 cycle performs boring operations on the face of the workpiece. The G85 cycle bores to depth and feeds out at the programmed feedrate. Spindle motion is continuous. Refer to page 8-23 for a description of the G85 Face Boring Cycle. G87 SIDE DRILLING CYCLE The G87 cycle performs drilling operations on the side of the workpiece. The G87 cycle is extremely versatile, in that it can perform the single-pass, peck, or high-speed peck drilling. Refer to page 8-9 for a description of the G87 Side Drilling Cycle. G88 SIDE TAPPING CYCLE The G88 cycle performs tapping operations on the side of the workpiece. The G88 cycle taps to depth, reverses tool direction, and feeds out at the programmed feedrate. Refer to page 8-19 for a description of the G88 Side Tapping Cycle. G89 SIDE BORING CYCLE The G89 cycle performs boring operations on the side of the workpiece. The G89 cycle bores to depth and feeds out at the programmed feedrate. Spindle motion is continuous. Refer to page 8-27 for a description of the G89 Side Boring Cycle. 8-2 M-504A

207 DRILLING CYCLES G83 FACE DRILLING CYCLE Data Words FORMATS - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G83 Z±2.4 Q6 P8 R±2.4 (C3.2 or B3) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G83 Z±3.3 Q6 P8 R±3.3 (C3.2 or B3) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS G83 COMMAND Z WORD Q WORD * - NOTE - * denotes optional command G code for the Face Drilling Cycle. Specifies the final depth of the drilled hole, in reference to Z0 (zero). In the sample program segment, the final depth of the drilled hole is inches. Specifies the depth of each cutting pass when peck drilling. If the Q word is not programmed, a single-pass drilling operation will be performed. In the sample program segment, each cutting pass is.775 inches. Decimal point programming is NOT allowed. The control assumes decimal point placement as Q2.4 for English units (inches) and Q3.3 for metric units (millimeters). Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: Inch: Q2500 = 0.25 Inches Metric: Q2500 = 2.5 Millimeters M-504A 8-3

208 P WORD * R WORD * C WORD B WORD (Optional) K WORD * F WORD Specifies the dwell at the bottom of the drilled hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the Z axis from the start point to the return point. If the R word is not programmed, the return point will be equal to the start point. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G83 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the drilling cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the drilling cycle. In the sample program segment, the feedrate is 8 inches per minute. 8-4 M-504A

209 Tool Movement in the G83 Cycle SINGLE PASS DRILLING Refer to Figure 8.1. If the Q word is NOT programmed, a single pass drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the Z axis to the return point. 2. The drill feeds to depth (Z word). 3. If the P word is programmed, the drill dwells at the bottom of the hole. 4. The drill rapids to the start point. +X +Z ZWord Z0 Start Point RWord C L Return Point TI4187 Figure G83 Single Pass Drilling Cycle M-504A 8-5

210 PECK DRILLING Refer to Figure 8.2. If the Q word is programmed and parameter 5101, bit 2 is set to 1", a peck drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the Z axis to the return point. 2. From the return point, the drill feeds in Q amount. 3. The drill rapids to the return point. 4. The drill rapids down to the Rapid-to-Feed point. 5. The drill feeds in Q + Rapid-to-Feed. 6. Steps 3, 4, and 5 are repeated until full depth of cut is achieved. 7. If the P word is programmed, the drill dwells at the bottom of the hole. 8. The drill rapids to the start point. +X * The Rapid-to-Feed distance is determined by parameter Z ZWord Z0 Start Point RWord C L Rapid-to-Feed Distance* Q Word (In-Feed) Return Point TI4186 Figure G83 Peck Drilling Cycle 8-6 M-504A

211 HIGH SPEED PECK DRILLING Refer to Figure 8.3. If the Q word is programmed and parameter 5101, bit 2 is set to 0", a high speed peck drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the Z axis to the return point. 2. From the return point, the drill feeds in Q amount. 3. The drill rapids up a distance equal to the retract increment. 4. The drill feeds in Q + Retract Increment. 5. Steps 3 and 4 are repeated until full depth of cut is achieved. 6. If the P word is programmed, the drill dwells at the bottom of the hole. 7. The drill rapids to the start point. +X * The Retract increment is determined by parameter Z ZWord Z0 Start Point RWord C L Retract Increment* Q Word (In-Feed) Return Point TI4186 Figure G83 High Speed Peck Drilling Cycle M-504A 8-7

212 G83 Sample Program Segment Refer to Figure 8.4. Z0 (zero) is the face of the workpiece. Three.625 inch diameter holes will be drilled in the face of the workpiece to a depth of inches.. M23 ; Activate Contouring Mode X1. Z.1 C0. ; Position Tool at Start Point, Orient Spindle M54 S1000 P3 ; Live Tooling Forward, Coolant ON, 1000 RPM, Spindle Select G98 G83 Z-3. Q7750 C0. F8. M200 ; Per Minute Feedrate, Define G83 Cycle, Drill First Hole, Spindle Brake ON C120. Z-3. Q7750 ; Drill Second Hole C240. Z-3. Q7750 ; Drill Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X +Z Z0.625 Dia. (3 Places) Dia. 120 Typical C L NOTE: All dimensions shown in Inches [Millimeters]. TI4188 Figure G83 Face Drilling Cycle: Sample Workpiece 8-8 M-504A

213 G87 SIDE DRILLING CYCLE Data Words FORMATS - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G87 X±2.4 Q6 P8 R±2.4 (C3.2 or B3.2) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G87 X±3.3 Q6 P8 R±3.3 (C3.2 or B3.2) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS - NOTE - All X dimensions are shown as diameter values. * denotes optional command G87 COMMAND X WORD Q WORD * G code for the Side Drilling Cycle. Specifies the final depth of the drilled hole, in reference to X0 (zero). X is programmed as a diameter value. In the sample program segment, the final depth of the drilled hole is.500 inches, as measured on the diameter. Specifies the depth of each cutting pass when peck drilling. If the Q word is not programmed, a single-pass drilling operation will be performed. In the sample program segment, each cutting pass is.75 inches, as measured on the diameter. Decimal point programming is NOT allowed. The control assumes decimal point placement as Q2.4 for English units (inches) and Q3.3 for metric units (millimeters). Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: Inch: Q2500 = 0.25 Inches Metric: Q2500 = 2.5 Millimeters M-504A 8-9

214 P WORD * R WORD * C WORD B WORD (Optional) K WORD * F WORD Specifies the dwell at the bottom of the drilled hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the X axis from the start point to the return point. The R word is always programmed as a RADIUS value. In the sample program segment, the distance is.40 inches, as measured on the radius. If the R word is not programmed, the return point will be equal to the start point. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G87 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the drilling cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the drilling cycle. In the sample program segment, the feedrate is.005 inches per revolution M-504A

215 Tool Movement in the G87 Cycle SINGLE PASS DRILLING Refer to Figure 8.5. If the Q word is NOT programmed, a single pass drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the X axis to the return point. 2. The drill feeds to depth (X word). 3. If the P word is programmed, the drill dwells at the bottom of the hole. 4. The drill rapids to the start point. +X +Z RWord Return Point Start Point C L X0 ZWord (Diameter Value) TI4189 Figure G87 Single Pass Drilling Cycle M-504A 8-11

216 PECK DRILLING Refer to Figure 8.6. If the Q word is programmed and parameter 5101, bit 2 is set to 1", a peck drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the X axis to the return point. 2. From the return point, the drill feeds in Q amount. 3. The drill rapids to the return point. 4. The drill rapids down to the Rapid-to-Feed point. 5. The drill feeds in Q + Rapid-to-Feed. 6. Steps 3, 4, and 5 are repeated until full depth of cut is achieved. 7. If the P word is programmed, the drill dwells at the bottom of the hole. 8. The drill rapids to the start point. +X * The Rapid-to-Feed distance is determined by parameter Z QWord (In-Feed) RWord Return Point Start Point Rapid-to-Feed Distance* C L X0 XWord (Diameter Value) TI4190 Figure G87 Peck Drilling Cycle 8-12 M-504A

217 HIGH SPEED PECK DRILLING Refer to Figure 8.7. If the Q word is programmed and parameter 5101, bit 2 is set to 0", a high speed peck drilling operation is performed. The series of axis movements is as follows: 1. From the start point, the drill rapids on the X axis to the return point. 2. From the return point, the drill feeds in Q amount. 3. The drill rapids up a distance equal to the retract increment. 4. The drill feeds in Q + Retract Increment. 5. Steps 3 and 4 are repeated until full depth of cut is achieved. 6. If the P word is programmed, the drill dwells at the bottom of the hole. 7. The drill rapids to the start point. +X * The Retract increment is determined by parameter Z QWord (In-Feed) RWord Return Point Start Point C L Retract Increment* X0 XWord (Diameter Value) TI4190 Figure G87 High Speed Peck Drilling Cycle M-504A 8-13

218 G87 Sample Program Segment Refer to Figure NOTE - This sample program segment illustrates the use of G99 (per revolution feedrate). X0 (zero) is the centerline of the workpiece. Three.375 inch diameter holes will be drilled in the diameter of the workpiece to a depth of inches.. M23 ; Activate Contouring Mode X2.7 Z-1.5 C0. ; Position Tool at Start Point, Orient Spindle M53 S1000 P3 ; Live Tooling Forward, Coolant ON, 1000 RPM, Spindle Select G99 G87 X0.5 Q7500 C0. F.005 M200 ; Per Revolution Feedrate, Define G87 Cycle, Drill First Hole, Spindle Brake ON C120. X0.5 Q7500 ; Drill Second Hole C240. X0.5 Q7500 ; Drill Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X +Z (3 Places) Z [38.1] Dia. [38.1] 120 Typical C L X0.500 [12.7] [63.5] NOTE: All dimensions are shown in Inches [Millimeters]. All measurements for X are diameter values from the spindle centerline. TI4191 Figure G87 Side Drilling Cycle: Sample Workpiece 8-14 M-504A

219 G84 RIGHT-HAND FACE TAPPING CYCLE Data Words FORMATS TAPPING CYCLES - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G84 Z±2.4 P8 R±2.4 (C3.2 or B3.2) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G84 Z±3.3 P8 R±3.3 (C3.2 or B3.2) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS G84 COMMAND Z WORD P WORD * R WORD * - NOTE - * denotes optional command G code for the Right-Hand Face Tapping Cycle. Specifies the final depth of the tapped hole, in reference to Z0 (zero). In the sample program segment, the final depth of the tapped hole is inches. Specifies the dwell at the bottom of the tapped hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the Z axis from the start point to the return point. If the R word is not programmed, the return point will be equal to the start point. M-504A 8-15

220 C WORD B WORD (Optional) K WORD * F WORD Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G84 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the tapping cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the tapping cycle. In the sample program segment, the feedrate is inches per revolution M-504A

221 Tool Movement in the G84 Cycle Refer to Figure 8.9. The series of axis movements is as follows: 1. From the start point, the tap rapids on the Z axis to the return point. 2. The tap feeds to depth (Z word). 3. If the P word is programmed, the live tooling stops and the tap dwells at the bottom of the hole. 4. The live tooling reverses direction and the tap feeds to the return point. 5. The tap rapids to the start point. +X +Z ZWord Z0 Start Point RWord C L Return Point TI4192 Figure G84 Face Tapping Cycle M-504A 8-17

222 G84 Sample Program Segment Refer to Figure Z0 (zero) is the face of the workpiece. Tapped hole size is ½-13. Three holes drilled in the face of the workpiece will be tapped to a depth of inches.. M23 ; Activate Contouring Mode X1. Z.1 C0. ; Position Tool at Start Point, Orient Spindle M54 S260 P3 ; Live Tooling Forward, Coolant ON, 250 RPM, Spindle Select M29 S260 ; Activate Rigid Tapping Mode G99 G84 Z C0. F.0769 M200 ; Per Revolution Feedrate, Define G84 Cycle, Tap First Hole, Spindle Brake ON C120. Z ; Tap Second Hole C240. Z ; Tap Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X NOTE: All dimensions are shown in Inches [Millimeters]. +Z Z [66.68] ½-13Tap (3 Places) [25.40] Dia. 120 Typical C L TI4193 Figure G84 Face Tapping Cycle: Sample Workpiece 8-18 M-504A

223 G88 RIGHT-HAND SIDE TAPPING CYCLE Data Words FORMATS - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G88 X±2.4 P8 R±2.4 (C3.2 or B3.2) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G88 X±3.3 P8 R±3.3 (C3.2 or B3.2) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS G88 COMMAND X WORD P WORD * R WORD * - NOTE - * denotes optional command G code for the Right-Hand Side Tapping Cycle. Specifies the final depth of the tapped hole, in reference to X0 (zero). In the sample program segment, the final depth of the tapped hole is.768 inches. Specifies the dwell at the bottom of the tapped hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the X axis from the start point to the return point. The R word is always programmed as a RADIUS value. In the sample program segment, the distance is.40 inches, as measured on the radius. If the R word is not programmed, the return point will be equal to the start point. M-504A 8-19

224 C WORD B WORD (Optional) K WORD * F WORD Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G88 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the tapping cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the tapping cycle. In the sample program segment, the feedrate is.05 inches per revolution M-504A

225 Tool Movement in the G88 Cycle Refer to Figure The series of axis movements is as follows: 1. From the start point, the tap rapids on the X axis to the return point. 2. The tap feeds to depth (X word). 3. If the P word is programmed, the live tooling stops and the tap dwells at the bottom of the hole. 4. The live tooling reverses direction and the tap feeds to the return point. 5. The tap rapids to the start point. +X +Z RWord Return Point Start Point C L X0 XWord (Diameter Value) TI4195 Figure G88 Side Tapping Cycle M-504A 8-21

226 G88 Sample Program Segment Refer to Figure X0 (zero) is the centerline of the workpiece. Tapped hole size is ¼-20. Three holes drilled in the diameter of the workpiece will be tapped to a depth of.768 inches.. M23 ; Activate Contouring Mode X2.7 Z-1.5 C0. ; Position Tool at Start Point, Orient Spindle M53 S250 P3 ; Live Tooling Forward, Coolant ON, 250 RPM, Spindle Select G98 G88 X.964 C0. F12.5 M200 ; Per Minute Feedrate, Define G88 Cycle, Tap First Hole, Spindle Brake ON C120. X.964 ; Tap Second Hole C240. X.964 ; Tap Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X NOTE: All dimensions are shown in Inches [Millimeters]. All measurements for X are diameter values from the spindle centerline. +Z ¼-20 Tap (3 Places) [38.10] Z0 C L X [63.50] 120 Typical.964 [24.49] TI4196 Figure G88 Side Tapping Cycle: Sample Workpiece 8-22 M-504A

227 BORING CYCLES G85 FACE BORING CYCLE Data Words FORMATS - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G85 Z±2.4 P8 R±2.4 (C3.2 or B3.2) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G85 Z±3.3 P8 R±3.3 (C3.2 or B3.2) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS G85 COMMAND Z WORD P WORD * R WORD * - NOTE - * denotes optional command G code for the Face Boring Cycle. Specifies the final depth of the bored hole, in reference to Z0 (zero). In the sample program segment, the final depth of the bored hole is inches. Specifies the dwell at the bottom of the bored hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the Z axis from the start point to the return point. If the R word is not programmed, the return point will be equal to the start point. M-504A 8-23

228 C WORD B WORD (Optional) K WORD * F WORD Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G85 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the boring cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the boring cycle. In the sample program segment, the feedrate is 1.5 inches per minute M-504A

229 Tool Movement in the G85 Cycle Refer to Figure The series of axis movements is as follows: 1. From the start point, the boring bar rapids on the Z axis to the return point. 2. The boring bar feeds to depth (Z word). 3. If the P word is programmed, the boring bar dwells at the bottom of the hole. Tool motion continues. 4. The boring bar feeds to the return point. 5. The boring bar rapids to the start point. +X +Z ZWord Z0 Start Point RWord C L Return Point TI4197 Figure G85 Face Boring Cycle M-504A 8-25

230 G85 Sample Program Segment Refer to Figure Z0 (zero) is the face of the workpiece. Three holes drilled in the face of the workpiece will be bored to a depth of inches.. M23 ; Activate Contouring Mode X1. Z.1 C0. ; Position Tool at Start Point, Orient Spindle M54 S150 P3 ; Live Tooling Forward, Coolant ON, 150 RPM, Spindle Select G98 G85 Z C0. F1.5 M200 ; Per Minute Feedrate, Define G85 Cycle, Bore First Hole, Spindle Brake ON C120. Z ; Bore Second Hole C240. Z ; Bore Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X +Z [58.75] Z0.500 Dia. (3 Places) Dia. 120 Typical C L NOTE: All dimensions are shown in Inches [Millimeters]. TI4198 Figure G85 Face Boring Cycle: Sample Workpiece 8-26 M-504A

231 G89 SIDE BORING CYCLE Data Words FORMATS - NOTE - The values shown in the following data blocks are data word formats, NOT actual dimensions. The M200 (or M202) command is not required if programming spindle orient with the B axis command. Inch Programming: G89 X±2.4 P8 R±2.4 (C3.2 or B3.2) K1.0 F3.2 (in/min) or F1.6 (in/rev) M200 (or M202) ; Metric Programming: G89 X±3.3 P8 R±3.3 (C3.2 or B3.2) K1.0 F5.0 (mm/min) or F3.4 (mm/rev) M200 (or M202) ; DEFINITIONS G89 COMMAND X WORD P WORD * R WORD * C WORD - NOTE - * denotes optional command G code for the Side Boring Cycle. Specifies the final depth of the bored hole, in reference to X0 (zero). In the sample program segment, the final depth of the bored hole is.80 inches. Specifies the dwell at the bottom of the bored hole. The dwell is specified in milliseconds. P0" is assumed if the P word is not programmed. Decimal point programming is NOT allowed. The control assumes decimal point placement as 5.3. Leading zeros may be omitted; however, trailing zeros MUST be programmed. Refer to the following examples: P300 = 0.3 Second Dwell P6500= 6.5 Second Dwell Specifies the incremental distance from the start point to the return point of the cycle. The sign is determined by the direction of motion on the Z axis from the start point to the return point. If the R word is not programmed, the return point will be equal to the start point. Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the C word, M23 (or M223) must be programmed in a block by itself before the G89 command block and M24 (or M224) must be programmed in a block by itself immediately after the G80 command block. The appropriate spindle brake must be engaged to lock the spindle in position. When peck drilling is desired, the C word must be programmed with a Q word. The spindle orientation can also be specified with the optional B word. M-504A 8-27

232 B WORD (Optional) K WORD * F WORD Specifies the spindle orientation for the drilled hole. When specifying spindle orientation with the B word, the spindle brake will automatically engage to lock the spindle in position. The X word must be programmed for each hole to be drilled. When peck drilling is desired, the B word must be programmed with a Q word. The spindle orientation can also be specified with the C word. Specifies the number of times the boring cycle will be performed at each location. K is assumed to be 1" if it is not programmed. Specifies the feedrate for the boring cycle. In the sample program segment, the feedrate is 1.5 inches per minute. Tool Movement in the G89 Cycle Refer to Figure The series of axis movements is as follows: 1. From the start point, the boring bar rapids on the X axis to the return point. 2. The boring bar feeds to depth (X word). 3. If the P word is programmed, the boring bar dwells at the bottom of the hole. Tool motion continues. 4. The boring bar feeds to the return point. 5. The boring bar rapids to the start point. +X +Z RWord Return Point Start Point C L X0 XWord Diameter Value TI4199 Figure G89 Side Boring Cycle 8-28 M-504A

233 G89 Sample Program Segment Refer to Figure X0 (zero) is the centerline of the workpiece. Three holes drilled in the diameter of the workpiece will be bored to a depth of.80 inches.. M23 ; Activate Contouring Mode X2.7 Z-1.5 C0. ; Position Tool at Start Point, Orient Spindle M53 S150 P3 ; Live Tooling Forward, Coolant ON, 150 RPM, Spindle Select G98 G89 X.9 C0. F1.5 M200 ; Per Minute Feedrate, Define G89 Cycle, Bore First Hole Spindle Brake ON C120. X.9 ; Bore Second Hole C240. X.9 ; Bore Third Hole G80 ; Cancel Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF M55 ; Live Tooling Stop, Coolant OFF. +X NOTE: All dimensions are shown in Inches [Millimeters]. All measurements for X are diameter values from the spindle centerline. +Z (3 Places).500 [12.70] Dia [38.10] Z [63.50] 120 Typical C L X0.900 [22.86] TI4200 Figure G89 Side Boring Cycle: Sample Workpiece M-504A 8-29

234 - NOTES M-504A

235 CHAPTER 9 - MISCELLANEOUS CONSTANT SURFACE SPEED Constant Surface Speed programming provides the capability of programming the speed of the workpiece with respect to the tool tip directly in surface feet per minute in inch mode or surface meters per minute in metric mode. Constant Surface Speed programming is a function of the spindle speed range and the programmed constant surface speed (S word). Constant Surface Speed mode is selected by the G96 command and is canceled by G97. The G97 command is the start-up mode and selects the direct RPM mode, which allows direct RPM programming of the spindle speed. Before programming a G96 command, a block containing a G50 command and an S word to establish the maximum RPM limit for the following Constant Surface Speed operation MUST be programmed. The format for the S word is S4. As the distance between the tool tip and the spindle centerline varies during a Constant Surface Speed operation, the variable spindle speed is compared to this maximum RPM limit. If the limit is reached, the control will continue execution of the part program at the spindle speed limit. NOTICE When establishing the Constant Surface Speed spindle RPM limit, do not program any other data words in the same block with the G50 command and the S word. In Constant Surface Speed mode, the constant surface speed command to the spindle is also programmed as an S word. The format is S4 in inch mode and S3 in metric mode. The units are surface feet per minute in inch mode and surface meters per minute in metric mode. A feedrate must also be programmed. The control will then automatically adjust the spindle speed within its range to maintain a constant surface speed as the cutting radius of the workpiece varies. Since the feedrate is held constant while the spindle speed varies, it is recommended that the feedrate be programmed in Inches per Revolution (G99). This will prevent overloading the tool in case a fast feedrate is active when the spindle speed is decreasing (as when facing from the center outward). Figure 9.1 illustrates an elementary part that uses Constant Surface Speed programming. For this example, it is assumed that the part has already been roughed out and is ready to be finish contoured. The part face is set to Z Zero by the G10 command in block N10. All turning passes will, therefore, be in the NEGATIVE Z direction. X Zero is at the spindle centerline. The tool tip extends 1.25 inches from the turret reference point in the X direction and 2.25 inches from the turret reference point in the Z direction. These dimensions will be compensated for by the tool offsets selected in block N30. M-504A 9-1

236 A maximum spindle speed of 4000 RPM for the operation is established in block N60. Block N70 establishes Constant Surface Speed mode and a surface speed of 500 surface feet per minute. The Inch per Revolution feedrate (G99) is established in block N80 along with a feedrate of.007 inches per revolution. Sample Program: N7 (Operator Message) ; 2.90 N10 G10 P0 Z#500 ; N20 M98 P1 ; 1.50 N30 T0707 ; N40 G97 S1000 M13 P1 ; N50 X1.14 Z.1 ; N60 G50 S4000 ;.75 N70 G96 S500 ;.50 N80 G1 G99 Z0. F.007 ;.030 (Face Off) N90 X0. ; N100 X1. ; N110 X2. Z-.5 ; N120 Z-.7 ; 4.00 N130 X3. Z-1.2 ; N140 Z-1.5 ; 3.00 N150 X4.1 ; N160M98P1; 2.00 N170 M1 ; N180 M30 ; 1.00 C L Spindle Face Chuck Face TI2444 Figure Constant Surface Speed Example A spindle speed MUST be active when entering Constant Surface Speed mode or a Cycle Stop condition will be created when the first block following the Constant Surface Speed command is encountered. The Spindle Increase and Decrease push buttons, Feedrate Override switch, and Rapid Override switch are active in Constant Surface Speed mode. 9-2 M-504A

237 SUBPROGRAMS The subprogram feature provides the main part program with the capability of calling frequently repeated patterns from memory, and executing them a specified number of times. The subprogram is called from a special block in the main part program. The subprogram must be in memory, when called. Subprogram Format: O ; Subprogram Name N ; Program Block N ;. N ;. N ;. M99; Return to calling program Subprograms stored in memory must be identified by the letter O followed by program number in the first data block. See Program Number, page The last data block of the subprogram MUST contain an M99 command. This command should be in a block by itself. Subprograms may be stored from the Manual Data Input keyboard, through the RS-232 serial port, or through the ATA flash card port. Refer to the operator s manual (M-505) for information on inputting programs from the Manual Data Input keyboard, through the RS-232 serial port, or through the ATA flash card port. M-504A 9-3

238 SUBPROGRAM CALL Subprograms are activated by a special call block in the main part program which must have the following format: M98 Paaabbbb ; Where: M98 is the miscellaneous command to activate the subprogram call function. P is the letter address used to specify the number of times the subprogram is to be performed and the subprogram number. aaa specifies the number of times the subprogram is to be performed. The subprogram may be performed up to 999 times. IF NO VALUE IS ENTERED, THE SUBPROGRAM IS PERFORMED ONCE. bbbb specifies number of the subprogram to be executed. Sample Program Line #1: M98 P50100 ; (Subprogram O0100 will be executed five times.) Sample Program Line #2: M98 P100 ; (Subprogram O0100 will be executed one time.) Sample Program Line #3: M98 P ; (Subprogram O0100 will be executed 999 times.) - NOTE - When the subprogram is to be executed just once, use the format shown in sample program line #2. As shown, leading zeros may be omitted from the subprogram number when this format is used. 9-4 M-504A

239 SAFE INDEX SUBPROGRAMS INTRODUCTION CAUTION NEVER use subprogram O1 when machining on the optional sub-spindle. Personal injury and/or damage to the tooling and the machine tool may result. NEVER use subprogram O2 when machining on the main spindle. Personal injury and/or damage to the tooling and the machine tool may result. NOTICE The cutting tool must be moved clear of the workpiece before calling a Safe Index subprogram. Refer to the programming formats beginning on page NOTE - Use of the Hardinge Safe Index subprograms is strongly recommended. They are designed for machine safety and to help simplify programming. The Safe Index subprograms are used to reactivate start-up modes, for example; positioning mode, deactivate Tool Nose Radius Compensation, establish in/min [mm/min] feed, and move the turret to the safe index position. MAIN SPINDLE OPERATION During main spindle operation the tool typically engages the workpiece with negative (-) Z moves and clears the workpiece with positive (+) Z moves. This is just the opposite of machining a workpiece in the optional sub-spindle. Safe Index subprogram O1 has been developed specifically for use when machining on the main spindle. This main spindle Safe Index subprogram is NOT to be used when machining on the sub-spindle. SUB-SPINDLE OPERATION [Option] During sub-spindle operation the tool typically engages the workpiece with positive (+) Z moves and clears the workpiece with negative (-) Z moves. This is just the opposite of machining a workpiece in the main spindle. Safe Index subprogram O2 has been developed specifically for use when machining on the sub-spindle. This sub-spindle Safe Index subprogram is NOT to be used when machining on the main spindle. M-504A 9-5

240 SUBPROGRAM DESCRIPTIONS Main Spindle Safe Index Subprogram O1 Safe Index subprogram O1 is to be loaded permanently into the control memory for all machines. The X safe index value should be equal to the X axis Reference position. Refer to Appendix One for information on the X axis Reference position. The main spindle Z axis safe index value is set by the machine operator. It should be equal to the Z axis distance from the turret top plate reference point to the tip of the longest tool PLUS 1 inch. Refer to Figure 9.2. The main spindle safe index positions will be assigned to the following macro variables at the beginning of the part program: X axis safe index position: Macro variable 502 Z axis safe index position: Macro variable 503 BMT 45 Turret Top Plate Hardinge Turret Top Plate +X +Z Z Safe Index = Z + 1 [25mm] Figure Z Axis Safe Index Value for Main Spindle Operations Z TI M-504A

241 Sub-Spindle Safe Index Subprogram O2 Safe Index subprogram O2 is to be loaded permanently into the control memory for machines equipped with the optional sub-spindle. The X safe index value should be equal to the X axis Reference position. Refer to Appendix One for information on the X axis Reference position. The sub-spindle Z axis safe index value is set by the machine operator. It should be equal to the Z axis distance from the turret top plate reference point to the tip of the longest tool PLUS 1 inch. Refer to Figure 9.3. The sub-spindle safe index positions will be assigned to the following macro variables at the beginning of the part program: X axis safe index position: Macro variable 502 Z axis safe index position: Macro variable 504 BMT 45 Turret Top Plate Hardinge Turret Top Plate +X +Z Z Safe Index = Z + 1 [25mm] Figure Z Axis Safe Index Value for Sub-Spindle Operations Z TI5668A M-504A 9-7

242 SUBPROGRAM STRUCTURE NOTICE If the machine is to be run in metric mode, the X and Z coordinates in macro variable registers 502, 503, and 504 MUST be converted to metric values. The sub-spindle reference position in the following subprograms is shown in inches. Main Spindle Safe Index Subprogram O1 The command M98 P1" is used at the start and end of every main spindle operation to call the safe index subprogram. This ensures that the proper G codes are active and that the turret is in a safe position before indexing. O1 ; N1 G53 E16.5 ; N2 G0 Y0 ; N3 G00 G18 G40 G97 G98 T0 ; N4 X#502 Z#503 ; N5 M99 ; % SAFE INDEX PROGRAM MAIN SPINDLE Sub-Spindle to Reference Position (Sub-Spindle Machine Only) Y Axis to Reference Position (Y Axis Machine Only) Positioning Mode, X/Z Axis Plane Selection Cancel Tool Nose Radius Compensation, Direct RPM, Inch [mm] Per Minute Feed Cancel tool Offsets Move to Safe Index Position Return to Calling Program Sub-Spindle Safe Index Subprogram O2 The command M98 P2" is used at the start and end of every sub-spindle operation to call the safe index subprogram. This ensures that the proper G codes are active and that the turret is in a safe position before indexing. O2 ; N1 G53 E16.5 ; N2 G0 Y0 ; N3 G00 G18 G40 G97 G98 T0 ; N4 X#502 Z#504 ; N5 M99 ; % SAFE INDEX PROGRAM SUBSPINDLE Sub-Spindle to Reference Position (Sub-Spindle Machine Only) Y Axis to Reference Position (Y Axis Machine Only) Positioning Mode, X/Z Axis Plane Selection Cancel Tool Nose Radius Compensation, Direct RPM, Inch [mm] Per Minute Feed Cancel tool Offsets Move to Safe Index Position Return to Calling Program 9-8 M-504A

243 HARDINGE PERMANENT MACRO PROGRAMS Hardinge permanent macro programs are assigned 9000 series program numbers. These permanent macro programs cannot be edited. Macro programs are called as follows: G65 Pxxxx y ; Where: G65 = Macro call command P = Required format letter xxxx = Macro program number y = Macro variable(s), if required ; = End of Block character MACRO 9112: SAFE TOOL OFFSET NOTICE This macro program resets ALL tool offset registers. Any tool offsets already entered will be lost. - NOTE - Macro 9112 is designed to work on machines set for DIAMETER operation ONLY. This macro must be executed from a program. Otherwise, an indefinite loop is produced and the control will hang itself up executing the cycle indefinitely. It is recommended that the following program be loaded into the control memory, to be executed as needed: Sample Program: O8999 ; G65 P9112 ; M30 ; G65 P9112 is interpreted as follows: G65 = Macro call command P = Required format letter 9112 = Macro program number ; = End of Block character M-504A 9-9

244 To ensure safe machine operation, macro program 9112 has been developed to reset the machine coordinate system offsets in the following manner: 1. All Tool Wear Offset registers are set to zero. 2. All R (Radius) and T (Quadrant) Tool Geometry Offset registers are set to zero. 3. All X Tool Geometry Offset registers are set to (English mode) or (Metric mode). 4. All Z Tool Geometry Offset registers are set to (English mode) or (Metric mode). MACRO 9136: VARIABLE DEPTH INCREMENT AUTOMATIC DRILLING CYCLE An explanation of Macro 9136 is presented in Chapter 6, Machining Cycles. MACRO 9150: COLLET DWELL - NOTE - Collet Dwell macro 9150 is not required for hydraulic collet closers and will be ignored. Collet Dwell macro 9150 sets a time delay to allow the pneumatic collet closer sufficient time to fully close on the workpiece. Collet Dwell macro 9150 MUST be programmed near the beginning of the part program, before any machining blocks are programmed. If this command is not programmed, the following conditions will occur: 1. The time delay for operation of the pneumatic collet closer will default to 30 seconds and will remain the same unless changed with the Collet Dwell macro. 2. When changing jobs or programs, unless the control is turned OFF or a new delay time is programmed, the time setting established by the previously active program will be active. This may cause one of the following conditions to occur: A) Cycle Start will be activated before the work-holding device is fully closed. B) Delay time will be excessive for the type of work-holding device and collet closer pressure being used. WARNING Failing to program an appropriate collet dwell could create unsafe operating conditions. Timer Range: 1.0 to 30.0 seconds Minimum Increment:.1 seconds Default Value: 30 seconds 9-10 M-504A

245 Recommended Settings To ensure maximum safety during machining cycles, the collet closer delay time MUST be programmed for each job. The collet closer pressure setting must be known to determine the correct dwell time. Refer to the chart and instructions which follow when programming the collet closer dwell macro. Collet Closer Pressure Setting English [Metric] Recommended Time Delay psi [ bar] 4.9 seconds psi [ bar] 3.0 seconds psi [ bar] 2.0 seconds psi [ bar] 1.5 seconds The timer can be set from 1.0 to 30.0 seconds; however, the settings listed above are recommended. Setting the Delay The collet closer timer delay is set by calling Macro Program 9150 near the beginning of the part program, as follows: BLOCK FORMAT: G65 P9150 Hx. ; Data Word Definitions: G65 = Macro call command P = Required format letter 9150 = Macro program number H = Required data letter x = Time delay value (Decimal point must be programmed) ; = End of Block character Program Collet Dwell macro 9150 near the beginning of the part program. The data word format is H1.1 with a valid range from 1.0 to 30.0, in increments of.1 seconds. Example: O3333 ; (Program Number) G20 ; (Select Inch Mode) G65 P9150 H2. ; (Collet closer dwell is set to 2.0 seconds)... - NOTE - The H word in the G65 block can be replaced with a D word. The D word will be programmed and interpreted exactly like the H word. M-504A 9-11

246 TAILSTOCK INTRODUCTION The tailstock has two programming modes: M82 TORQUE CONTROL MODE The M82 command switches the E axis drive from position control mode to torque control mode. Torque control mode allows the tailstock to be commanded in terms of constant force applied against the workpiece. Once the E axis is switched to torque control mode, any attempt to move the tailstock under position control mode (commanding an E axis move) will result in an alarm. M83 POSITION CONTROL MODE The M83 command switches the E axis drive from torque control mode to position control mode. Position control mode allows the tailstock to be commanded in terms of coordinate positions on a linear axis. The M83 also resets the E axis position register and resets the spindle acceleration/deceleration to standard values. Refer to the S word on the next page. Position control mode is active at machine power-up. Position control mode is also activated by M30, Reset, or Emergency Stop. DATA WORD DEFINITIONS - NOTE - Refer to the tailstock programming examples beginning on page Refer to the tailstock programming notes on page The tailstock (E axis) is programmed to a position near the face workpiece in position control mode. Torque control mode is then used to move the center into contact with the workpiece and apply a constant force on the workpiece. M82 Command Line Format: M82 F A S B_ ; M82 COMMAND A WORD Switch the E axis to torque control mode. The A word establishes an E axis position as an overtravel limit. An alarm message will be issued by the control if the E axis reaches or passes this position. The A word must be programmed. The decimal point must be programmed with the A word M-504A

247 B WORD F WORD S WORD (Optional) The use of the brake is determined by the type of center. A live center requires that the brake is ON. A dead center requires that the brake is OFF. When the tailstock brake is OFF, the spindle arrival signal is monitored. When a tool axis (X Z) changes from rapid (G00) to cutting (G01, G02, G03) the axis will not start into the move until the spindle has reached the program speed. The B word must be programmed. The decimal point must be programmed with the B word. B1. = Brake ON (live center) B2. = Brake OFF (dead center) Specifies the force to be applied to the workpiece in constant torque mode. The F word must be programmed. The desired force is entered in pound-force or dekanewtons depending on the inch/metric mode of the CNC. The functional range is 350 to 1500 pound-force [156 to 669 dekanewtons]. Any value above or below this range will result in an alarm message. The force value is not automatically changed when the inch/metric mode of the control is changed. It will be necessary to change the programmed value if the mode is changed. When using a dead center (tailstock brake OFF), the spindle acceleration/deceleration needs to be adjusted to prevent slipping between the center and the part. Acceleration/deceleration will be adjusted based on the programmed force as follows: Below 500 lbs (223 DaN) 800 rpm/second 500 lbs to 600 (267 DaN) 1200 rpm/second 600 lbs to 700 (312 DaN) 1600 rpm/second 700 lbs to 800 (357 DaN) 1900 rpm/second 800 lbs to 1500 (669 DaN) 2200 rpm/second Due to the unknown variables, such as center size and depth, the user has the option to set the acceleration/deceleration with the S word. This sets acceleration/deceleration in rpm per second. The change in the acceleration/deceleration is effective with any spindle stop command (M00, M01, M05, M30). The change is also effective on Emergency Stop and Reset. If the tailstock brake is set to ON, the spindle acceleration is not altered and any programmed S word in the M82 command line is ignored. M-504A 9-13

248 TAILSTOCK PROGRAMMING EXAMPLES Example 1: Workpiece Held in Collet/Chuck, Live Center in Tailstock O4455 ; Program Name N1 (TURN) ; Sequence Search Number and Message M98 P1 ; Call Safe Index Subprogram O1 T0101 ; Index to Tool Station and Call Offset G0 E.5 Z.5 ; Position Z and E Axes (Position Control Mode Active on E Axis) M82 F500. A-.3 B1. ; Activate Torque Control Mode and Advance Tailstock to Workpiece, Set Tailstock Force, Set Tailstock Overtravel Limit, Tailstock Brake ON G97 S P1 M4 ; Direct RPM, Spindle RPM, Select Spindle (P1 = Main Spindle), Spindle Direction X1.6 ; Position X Axis G50 S ; Maximum RPM Limit G96 S ; Surface Feet (Meters) Per Minute Speed G1 G99 ; Linear Interpolation, Inches [Millimeters] per Revolution Feed (MACHINE PART) G0 X ; Move to Clear Workpiece M98 P1 ; Call Safe Index Subprogram O1 M01 ; Optional Stop N2 (F TURN) ; Sequence Search Number and Message M98 P1 ; Call Safe Index Subprogram O1 T0202 ; Index to Tool Station and Call Offset G0 Z.1 ; Position Z Axis M82 F500. A-.3 B1. ; (Repeated in case Reset is pressed between operations) G97 S P1 M4 ; Direct RPM, Spindle RPM, Select Spindle (P1 = Main Spindle), Spindle Direction X1.6 ; Position X Axis G50 S ; Maximum RPM Limit G96 S ; Surface Feet (Meters) Per Minute Speed G1 G99 ; Linear Interpolation, Inches [Millimeters] per Revolution Feed (MACHINE PART) G0 X ; Move to Clear Workpiece M98 P1 ; Call Safe Index Subprogram O1 M05 ; Stop Spindle M83 ; Cancel Torque Control Mode G0 E.75 ; Move Tailstock Away from Workpiece M30 ; End of Program 9-14 M-504A

249 Example 2: Machining Between Centers O4455 ; N1 (TURN) ; M98 P1 ; M82 F500. A-.3 B2. ; G97 S M4 P1 ; T0101 ; G0 X1.6 Z.1 ; G50 S ; G96 S ; G1 G99 ; (MACHINE PART) G0 X ; M98 P1 ; M01 ; N2 (F TURN) ; M98 P1 ; M82 F500. A-.3 B2. ; G97 S M4 P1 ; T0202 ; G0 X1.6 Z.1 ; G50 S ; G96 S ; G1 G99 ; (MACHINE PART) G0 X ; M98 P1 ; M05 ; M30 ; Program Name Sequence Search Number and Message Call Safe Index Subprogram O1 Activate Torque Control Mode and Advance Tailstock to Workpiece, Set Tailstock Force, Set Tailstock Overtravel Limit, Tailstock Brake OFF Direct RPM, Spindle RPM, Select Spindle (P1 = Main Spindle), Spindle Direction Index to Tool Station and Call Offset Position X and Z Axes Maximum RPM Limit Surface Feet (Meters) Per Minute Speed Linear Interpolation, Inches [Millimeters] per Revolution Feed Move to Clear Workpiece Call Safe Index Subprogram O1 Optional Stop Sequence Search Number and Message Call Safe Index Subprogram O1 (Repeated in case Reset is pressed between operations) Direct RPM, Spindle RPM, Select Spindle (P1 = Main Spindle), Spindle Direction Index to Tool Station and Call Offset Position X and Z Axes Maximum RPM Limit Surface Feet (Meters) Per Minute Speed Linear Interpolation, Inches [Millimeters] per Revolution Feed Move to Clear Workpiece Call Safe Index Subprogram O1 Stop Spindle End of Program M-504A 9-15

250 TAILSTOCK PROGRAMMING NOTES 1. Torque control mode (M82) is not canceled between operations. 2. The tailstock is left engaged with the workpiece after each tool until the workpiece is complete. 3. The tailstock programming mode is switched from torque control mode to position control mode by M30, M83, Reset, or Emergency Stop. 4. When using a dead center, it is recommended that the spindle is stationary when the tailstock advances into the work piece. Also have the spindle stopped before programming the M83 to switch from torque control mode to position control mode. This is needed to prevent skidding between the part and the center. 5. When performing between-center machining, it is recommended that the force programmed on the M82 command line be set 30% higher than the setting on the Tailstock setting screen. Refer to the operator's manual (M-505) for information on entering the force value on the Tailstock setting screen M-504A

251 SUB-SPINDLE PART CATCHER [Option] INTRODUCTION The sub-spindle part catcher is a multiple axis part removal system designed to remove a workpiece from the sub-spindle and deposit the workpiece on a conveyor, which will carry the workpiece to an unload ramp located at the left end of the machine. M CODES The sub-spindle part catcher is controlled through the use of the following six M codes: M221 PART CATCHER SLIDE EXTEND M221 commands the part catcher to slide OUT to the fixed part pick-up position. Refer to Figure 9.4. M222 PART CATCHER SLIDE RETRACT M222 commands the part catcher to slide IN to the headwall. M225 PART CATCHER ARM ROTATE OUT M225 commands the part catcher arm to swing OUT to the part retrieve position at the spindle centerline. Refer to Figure 9.5. M226 PART CATCHER ARM ROTATE IN M226 commands the part catcher arm to swing IN to allow the part catcher to be retracted. M227 PART CATCHER GRIPPER CLOSE M227 commands the part catcher gripper to close and grip the workpiece. M228 PART CATCHER GRIPPER OPEN M228 commands the part catcher gripper to open and release the workpiece. Figure Part Catcher Extended, Arm Rotated to Down Position TP7933 Figure Part Catcher Extended, Arm Rotated to Up Position TP7934 M-504A 9-17

252 INTERLOCKS 1. M221 must be active (Part Catcher Slide Extend) before M225 (Part Catcher Arm Rotate Up) can be commanded. 2. The sub-spindle must be at the reference position before M226 (Part Catcher Arm Rotate Down) can be commanded. 3. M226 (Part Catcher Arm Rotate Down) must be active before M222 (Part Catcher Slide Retract) can be commanded. CAPACITY The part catcher has the following workpiece capacities: Machine Model Maximum Length Maximum Diameter Maximum Weight T-42 Lathe (16C Main Spindle) 6 inches [152.4 millimeters] 1.62 inches [42 millimeters] 5.34 lb [2.42 Kg] T-42 Big-Bore Lathe (20C Main Spindle) 6 inches [152.4 millimeters] 1.62 inches [42 millimeters] 5.34 lb [2.42 Kg] T-51 Lathe (20C Main Spindle) 8.00 inches [203.2 millimeters] 2 inches [50.8 millimeters] 5.34 lb [2.42 Kg] T-65 Lathe (25C Main Spindle) 8.00 inches [203.2 millimeters] 2.5 inches [63.5 millimeters] 5.34 lb [2.42 Kg] PROGRAMMING SEQUENCE FOR UNLOADING A WORKPIECE 1. Move the sub-spindle to the reference position. 2. M221 (Part Catcher Slide Extend). 3. M225 (Part Catcher Arm Rotate Up). 4. Move the sub-spindle to position the workpiece inside the part catcher gripper. 5. M227 (Part Catcher Gripper Closed). 6. Open the sub-spindle work-holding device. 7. Move the sub-spindle to the reference position. 8. M226 (Part Catcher Arm Rotate Down). 9. M222 (Part Catcher Slide Retract). 10. M228 (Part Catcher Gripper Open). 11. The part conveyor carries the workpiece out of the machine M-504A

253 ENGLISH / METRIC MODE One of the Setting pages is used to establish whether the control is to power-up and operate in English mode or Metric mode. This section outlines the procedure for selecting the desired operating mode. Through the use of the G20 (Inch Mode) and G21 (Metric Mode) commands, it is possible to operate in either mode regardless of which mode has been selected on the Setting page. However, the use of these two G codes will not automatically adjust the position registers to display the position values in the proper units (inches vs millimeters). NOTICE Part programs should usually be written in the same format as selected on the Setting page. Programs not written in the same format as established on the Setting page MUST contain the appropriate English/Metric G code, G20/G21 respectively. When required, this G code must be programmed by itself in the first data block. When the operating mode is changed through the Setting page, the work shift is NOT automatically changed to the appropriate units. The work shift must be changed manually. - NOTE - When the operating mode is changed through the Setting page, the tool offsets are automatically changed to the appropriate units. Refer to the operator s manual (M-505) for information on establishing English/Metric mode. M-504A 9-19

254 SPARE M CODES - NOTE - Refer to the schematic supplied with the machine for complete wiring information. M codes relating to inputs are not functional on software versions below 1.0 O2. OUTPUTS M301 turns ON AUXO08 (output Y30.7) M302 turns ON AUXO07 (output Y30.6) M303 turns ON AUXO06 (output Y30.5) M304 turns ON AUXO05 (output Y30.4) M305 turns ON AUXO04 (output Y30.3) M306 turns OFF AUXO08 (output Y30.7) M307 turns OFF AUXO07 (output Y30.6) M308 turns OFF AUXO06 (output Y30.5) M309 turns OFF AUXO05 (output Y30.4) M310 turns OFF AUXO04 (output Y30.3) M321 turns ON AUXO03 (output Y30.2) M322 turns ON AUXO02 (output Y30.1) M323 turns ON AUXO01 (output Y30.0) M326 turns OFF AUXO03 (output Y30.2) M327 turns OFF AUXO02 (output Y30.1) M328 turns OFF AUXO01 (output Y30.0) INPUTS M311 waits for a high signal on AUXI08 (input X42.7) M312 waits for a high signal on AUXI07 (input X42.6) M313 waits for a high signal on AUXI06 (input X42.5) M314 waits for a high signal on AUXI05 (input X42.4) M315 waits for a high signal on AUXI04 (input X42.3) M316 waits for a high signal on AUXI03 (input X42.2) M317 waits for a high signal on AUXI02 (input X42.1) M318 waits for a high signal on AUXI01 (input X42.0) 9-20 M-504A

255 - NOTES - M-504A 9-21

256 - NOTES M-504A

257 CHAPTER 10 - TOOL LIFE MANAGEMENT INTRODUCTION The basic concept of Tool Life Management is that after a specific number of parts or a specific amount of machining time, the control will automatically begin using another tool in place of the current tool being used for a particular operation. Tools are assigned to specific groups, as designated by the programmer. The control will monitor the measurement value assigned to each tool group and automatically switch to the next tool in the group when the counter for that tool group reaches the measurement value specified by the programmer. TOOL LIFE MEASUREMENT UNITS Tool life can be measured using one of the two following methods: Number of parts (machined by the tool) Amount of machining time (on the tool) Only one of these methods may be used at a time. Number of parts will be the active measurement unit when the machine is shipped from the factory. Refer to the operator s manual (M-505) for information on verifying or switching the active measurement unit. An alarm message will be displayed when any tool group has reached its programmed tool life and an M30" (End of Program) is read by the control. At that point, the machine operator will replace the tooling and reset the counter relating to the affected tool group. Refer to the operator s manual (M-505) for information on resetting a tool group counter. NUMBER OF PARTS When this type of measurement is used, the control will increment the tool group counter for the active tool each time the tool group is called by the part program. AMOUNT OF MACHINING TIME When this type of measurement is used, the control will run the tool group counter for the current tool whenever G01, G02, or G03 is active. M-504A 10-1

258 TOOL LIFE MANAGEMENT PROGRAM DESCRIPTION When using Tool Life Management, tools and offsets are assigned to specific groups. These groups are established by the programmer through the use of a Tool Life Management program, which is independent of the part program. The Tool Life Management program will define the parameters required for Tool Life Management. The Tool Life Management program defines the following parameters: Group numbers. Tool life value for each group. Tool stations and offsets for each group. NOTICE When the Tool Life Management program is executed, all Tool Life Management counters will be reset to 0 (zero). When using Tool Life Management, the machine operator MUST load and execute the Tool Life Management program BEFORE executing the part program for the first time. Refer to Programming, beginning on page 10-3, for information on the structure of the Tool Life Management program and how to incorporate Tool Life Management information in the part program. BAR FEED OPERATION There are no special considerations for running bar jobs. When running a bar job and using Tool Life Management, the programmer will program an M30 at the end of the part program and the machine operator will activate Repeat mode to cause the part program to loop. Refer to the operator s manual (M-505) for information on Repeat mode M-504A

259 TOOL LIFE MANAGEMENT PROGRAM PROGRAMMING Program Format Define Tool Group 1 Define Tool Group 2 Define Tool Group 3 O ; N G10 L3 ; N P1 L ; N T ; N T ; N T ; N P2 L ; N T ; N T ; N T ; N P3 L ;.. N G11 ; N M30 ; Data Word Definitions O = Program Number N = Block Number G10 = Begin Tool Data Input L3 = Memory Location for Tool Life Management Data (DO NOT ALTER) P = Tool Group Number L = Tool Life Value Data Word T = Turret Station and Offset Number G11 = End Tool Data Input M30 = End of Program M-504A 10-3

260 P WORD - TOOL GROUP NUMBER The P word is used to specify the group number to be assigned to each group of tooling. The numerical value for the data word must be a whole number. Decimal point programming is not allowed. Examples: P1 (Tool Group 1) P12 (Tool Group 12) Refer to the operator s manual (M-505) for information on verifying or switching the maximum number of tool groups allowed. L WORD - TOOL LIFE VALUE DATA WORD The L word is used to specify tool life for each tool group in the Tool Life Management program. The numerical value for the data word must be a whole number. Decimal point programming is not allowed. Examples: L25 (Tool life equals 25) L200 (Tool Life equals 200) The following chart shows the minimum and maximum values that may be used with the L word when programming Tool Life Management. Measurement Unit Minimum Value Maximum Value Number of Parts Machining Time (minutes) Refer to the operator s manual (M-505) for information on verifying or setting the measurement unit to be used. T WORD - TURRET STATION AND OFFSET NUMBER The standard T word format is used when defining turret stations and tool offsets in the Tool Life Management program. Refer to Chapter 4 for information on defining turret stations and tool offsets M-504A

261 Sample Tool Life Management Program In this sample program we will assume that the measurement unit is set to Number of Parts. Refer to the operator s manual (M-505) for information on verifying or setting the measurement unit to be used. O7500 ; N1 (Operator Message) ; N10 G10 L3 ; Define Tool Group 1 N20 P1 L10 ; N30 T0101 ; N40 T0212 ; N50 T0313 ; Define Tool Group 2 N60 P2 L3 ; N70 T0404 ; N80 T0515 ; Define Tool Group 3 N90 P3 L30 ; N100 T0919 ; N110 G11 ; N120 M30 ; DATA BLOCK DEFINITIONS Block N1 contains an operator message. Block N10 contains the Begin Tool Data Input command (G10) and the memory location (L3) where the data will be stored. Block N20 contains the number of the first tool group (Group 1) and the measurement value for each group 1 tool (value = 10). Blocks N30 through N50 contain the turret station and tool offset data for the tools assigned to group 1. Block N60 contains the number of the second tool group (Group 2) and the measurement value for each group 2 tool (value = 3). Blocks N70 and N80 contain the turret station and tool offset data for the tools assigned to group 2. Block N90 contains the number of the third tool group (Group 3) and the measurement value for each group 3 tool (value = 30). Block N100 contains the turret station and tool offset data for the tool assigned to group 3. Block N110 contains the End Tool Data Input command (G11). Block N120 contains the End of Program command (M30). M-504A 10-5

262 PART PROGRAM Tool Commands Tool stations and offsets were assigned to tool groups in the Tool Life Management program. Refer to Tool Life Management Program, beginning on page The tool groups are called from the part program using the T word. The data word format for the T word is T4. Decimal point programming is not allowed. ACTIVATE A TOOL GROUP T 99 T Word Format (99 activates the specified tool group) T0199 Activate Tool Group 1 T1299 Activate Tool Group 12 DEACTIVATE A TOOL GROUP T 88 T Word Format (88 deactivates the specified tool group) T0188 Deactivate Tool Group 1 T1288 Deactivate Tool Group 12 Sample Part Program Structure using Tool Life Management O1278 ; N ( ) ; Sequence Search Number and Operator Message N G10 P0 Z ; Set Work Shift N G97 M(13, 14, 33, or 34) S1000 P_ ; 1000 RPM and Direction, Coolant ON, Spindle Select N M98 P(1 or 2) ; Call Safe Index Subprogram N T0199 ; Activate Tool Group 1 N X _ Z _ ; Move to Activate Tool Offsets - MACHINE PART - N T0188 ; Deactivate Tool Group 1 N M98 P(1 or 2) ; Call Safe Index Subprogram N M01 ; Option Stop N ( ) ; Sequence Search Number and Operator Message N G97 M(13, 14, 33, or 34) S1000 P_ ; 1000 RPM and Direction, Coolant ON, Spindle Select N M98 P(1 or 2) ; Call Safe Index Subprogram N T0299 ; Activate Tool Group 2 N X _ Z _ ; Move to Activate Tool Offsets - MACHINE PART - N T0288 ; Deactivate Tool Group 2 N M98 P(1 or 2) ; Call Safe Index Subprogram N M01 ; Option Stop.. N M30 ; End of Program 10-6 M-504A

263 Combining Tool Commands Some tools may be expected to last the full life of a particular job. In this case it would be desirable to program the individual tool in the part program, rather than go to the trouble of assigning the tool to a tool group and defining the tool group life high enough to run for the full life of the job. It is possible to combine standard tool commands and Tool Life Management commands in the same part program. Standard tool commands may be programmed in operations that precede or follow operations using Tool Life Management commands. The only restriction is that the active tool or tool group must be canceled before another tool or tool group can be called. Sample Part Program Structure using Combined Tool Commands O1278 ; N ( ) ; Sequence Search Number and Operator Message N G10 P0 Z ; Set Work Shift N G97 M(13, 14, 33, or 34) S1000 P_ ; 1000 RPM and Direction, Coolant ON, Spindle Select N M98 P(1 or 2) ; Call Safe Index Subprogram N T0101 ; Index to Turret Station 1 and Call Offset 1 N X _ Z _ ; Move to Activate Tool Offsets - MACHINE PART - N M98 P(1 or 2) ; Call Safe Index Subprogram N M01 ; Option Stop N ( ) ; Sequence Search Number and Operator Message N G97 M(13, 14, 33, or 34) S1000 P_ ; 1000 RPM and Direction, Coolant ON, Spindle Select N M98 P(1 or 2) ; Call Safe Index Subprogram N T0199 ; Activate Tool Group 1 N X _ Z _ ; Move to Activate Tool Offsets - MACHINE PART - N T0188 ; Deactivate Tool Group 1 N M98 P(1 or 2) ; Call Safe Index Subprogram N M01 ; Option Stop.. N M30 ; End of Program PROGRAMMING NOTES 1. Decimal point programming is NOT allowed with the P or L data words. 2. The same turret station and/or tool offset may be assigned to more than one tool group. 3. Turret stations may NOT be assigned to the same tool group more than once, regardless of the tool offset to be used. M-504A 10-7

264 - NOTES M-504A

265 CHAPTER 11 - LIVE TOOLING AND SPINDLE ORIENT INTRODUCTION NOTICE Live tooling attachments are available with or without through-tool coolant capability. Live tooling attachments without through-tool coolant capability can be run with or without coolant, as the machining process requires. Live tooling attachments with through-tool coolant capability MUST be run with coolant turned ON. - NOTE - This chapter is intended for programming live tooling operations with a stationary spindle. Refer to Chapter 12 for information on programming live tooling with spindle motion. Refer to Chapter 8 for information on machining cycles that can be used with live tooling. B axis and C axis spindle orient are included with the live tooling feature. B axis and C axis spindle orient are separate purchased options on machines not equipped with the live tooling feature. Live tooling is a standard feature on T-42, T-51, and T-65 lathes equipped with a BMT top plate. The live tooling attachments are not included with the machine tool and must be purchased separately. Programming the live tooling is accomplished by means of five special M codes and a C, A, or B word in addition to the M codes used for standard machining. Live tooling is designed to perform machining such as milling, drilling, and tapping on workpiece locations not parallel or not in line with the spindle centerline. Live tooling attachments can be mounted at any turret station. The live tooling attachments have a maximum spindle speed of 8000 rpm, as measured at the tool tip, and can be operated at 30 percent of the total duty cycle at 8000 rpm. M-504A 11-1

266 LIVE TOOLING M CODES NOTICE Refer to "Determining Rotational Direction", on the next page, for specific information regarding tool rotation. The live tooling M codes command rotational direction and control whether coolant is ON or OFF. An S word must be programmed with the M word to indicate the live tooling spindle speed. This S word has a data word format of S4, with a maximum spindle speed of 8000 rpm. Axis motion may also be programmed in this data block. M51 ROTATIONAL DIRECTION COMMAND M51 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction. M51 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction. M51 cancels M52, M53, M54 and M55. M52 ROTATIONAL DIRECTION COMMAND M52 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction. M52 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction. M52 cancels M51, M53, M54, and M55. M53 ROTATIONAL DIRECTION COMMAND/COOLANT ON M53 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction with the coolant turned ON. M53 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction with the coolant turned ON. M53 cancels M51, M52, M54, and M55. M54 ROTATIONAL DIRECTION COMMAND/COOLANT ON M54 causes a cross-working live tooling attachment mounted at the active position on the turret to rotate in the reverse direction with the coolant turned ON. M54 causes a standard end-working live tooling attachment mounted at the active position on the turret to rotate in the forward direction with the coolant turned ON. M54 cancels M51, M52, M53, and M55. M55 STOP RPM / COOLANT OFF M55 causes the live tooling to stop rotating and turns the coolant OFF. M55 cancels M51, M52, M53, and M M-504A

267 DETERMINING ROTATIONAL DIRECTION NOTICE Directional commands for sub-spindle operations when using a double end-working live tool attachment are the opposite of the descriptions on the previous page. Refer to Figure Live tooling spindle direction can be best described in terms of a drill bit or tap. Right-hand drill bits and taps require a spindle forward command to machine the workpiece. Left-hand drill bits and taps require a spindle reverse command to machine the workpiece. When using a standard end-working live tool attachment, main spindle and sub-spindle operations are programmed as described on the previous page. When using a double end-working live tool attachment: Main spindle operations are programmed as described on the previous page. Sub-spindle operations require the opposite directional commands. Main Spindle Sub-Spindle M51 Spindle Reverse M52 Spindle Forward M53 Spindle Reverse, Coolant M54 Spindle Forward, Coolant M51 Spindle Forward M52 Spindle Reverse M53 Spindle Forward, Coolant M54 Spindle Reverse, Coolant TI5753 Figure Double End-Working Live Tool Attachment M-504A 11-3

268 C AXIS SPINDLE ORIENT The main spindle or optional sub-spindle can be oriented from 0 degrees to degrees. The spindle brake must be activated to hold the spindle in position after the spindle orient has been completed. NOTICE Be sure no tooling is touching the workpiece when spindle orient (A, C, or H word), M51, M52, M53, or M54 is executed. - NOTE - G00 mode is used for C axis orientation to ensure the orient is done at a rapid rate. If G1 mode is active, spindle feed rate is interpreted as degrees. The A, C, or H spindle orient command should be programmed immediately before the live tooling commands. When needed, the orient command can be programmed without a live tooling command following it. Contouring mode must be activated on the appropriate spindle before commanding C axis spindle orient. M23 activates contouring mode on the main spindle. M223 activates contouring mode on the sub-spindle. PROGRAMMING C AXIS SPINDLE ORIENT Absolute Orientation The C word is used to program absolute spindle orientation on the main spindle. The control will orient the main spindle in relation to the spindle zero degree position. The C word must be programmed with a decimal point. The data word format is C±5.3 with a valid range of 0 to The A word is used to program absolute spindle orientation on the sub-spindle. The control will orient the sub-spindle in relation to the spindle zero degree position. The A word must be programmed with a decimal point. The data word format is A±5.3 with a valid range of 0 to Refer to page 11-6 for information on the spindle zero degree position. Incremental Orientation - NOTE - The H word is used to command incremental spindle orientation on the main spindle. Incremental spindle orientation is not available on the sub-spindle. The H word is used to program incremental spindle orientation. The control will orient the spindle in relation to the current spindle position. The H word must be programmed with a decimal point. The data word format is H±5.3 with a valid range of 0 to Refer to the sample program starting on page M-504A

269 B AXIS SPINDLE ORIENT Each spindle equipped with B axis spindle orient (main spindle or optional sub-spindle) can be oriented in one degree increments from 0 degrees to 359 degrees. The spindle brake will automatically hold the spindle in position after the spindle orient has been completed. NOTICE Be sure no tooling is touching the workpiece when spindle orient (B word), M51, M52, M53, or M54 is executed. The B word commands the control to orient the spindle in relation to the spindle 0 degree mark and should be programmed immediately before the live tooling commands. When needed, the B word may be programmed without a live tooling command following it. The data word format is B3 with a valid range of 0 to 359 in increments of one degree. - NOTE - The control interprets 0 degrees and 360 degrees to be the same location. SPINDLE ORIENT M CODES M70 selects the sub-spindle for all B axis spindle orient commands. M71 selects the main spindle for all B axis spindle orient commands. PROGRAMMING B AXIS SPINDLE ORIENT The B word can be programmed with or without a decimal point. The decimal point is not required. The control always indexes the spindle to the absolute angle programmed. It is not possible to incrementally orient the spindle from any angle other than 0 degrees. M-504A 11-5

270 DIRECTION OF ORIENTATION When spindle orient is commanded when the spindle is NOT in motion, the control rotates the spindle to the programmed angle. When spindle orient is commanded while the spindle is in motion, the spindle will decelerate and orient to the programmed angle. Unless spindle motion (M03, M04, M13, or M14) is commanded or the Reset key is pressed, subsequent orient commands will cause the spindle to go shortest path to arrive at the commanded angle. When main spindle motion (M03, M04, M13, or M14) is commanded, the shortest path feature for the main spindle will be canceled. When sub-spindle motion (M33 or M34) is commanded, the shortest path feature for the sub-spindle will be canceled. When the control Reset key is pressed, the shortest path feature for both spindles will be canceled. DETERMINING SPINDLE ORIENTATION The spindle is oriented to 0 degrees when the spindle drive button is located 45 degrees from the machine bed and the spindle key is located 90 degrees from the machine bed, as shown in Figures 11.2 and Turret Top Plate Turret Top Plate Spindle Drive Button Spindle Drive Button Spindle Key Spindle Key Main Spindle Sub-Spindle Rotation M03 90 Machine Bed Machine Bed 90 Rotation M TI1777 TI4648 Floor Floor Figure Zero Reference Position (Main Spindle Viewed from Sub-Spindle) Figure Zero Reference Position (Sub-Spindle Viewed from Main Spindle) 11-6 M-504A

271 LIVE TOOLING PROGRAMMING FORMATS USING C AXIS SPINDLE ORIENT Beginning of Operation: N (Operator Message) ; Sequence Number and Operator Message M98 P(1 or 2) ; Call Safe Index Subprogram T M(23 or 223) ; Index to Station, Select Tool Offset, Activate Contouring Mode X Z (C or A) ; Move to Activate Tool Offset, Orient Spindle M(200 or 202) ; Spindle Brake ON G97 M(51, 52, 53, or 54) S P3 ; Cutter RPM, Rotational Direction, Coolant ON, Spindle Select G1 X (or) Z F ; Position Tool at Start Point Machining the Part: Machine the Part (Inches per Minute Feedrate) Reorient Spindle, if Required: X (or) Z F ; Move the Tool to a Clear Area M(201 or 203) ; Spindle Brake OFF C ; Orient the Spindle End of Operation: X (or) Z F ; Move the Tool to a Clear Area M(24 or 224) ; Cancel Contouring Mode M(201 or 203) ; Spindle Brake OFF (Optional Command) M55 ; Live Tooling Stop, Coolant OFF M98 P(1 or 2) ; Call Safe Index Subprogram M01 ; Optional Stop M-504A 11-7

272 USING B AXIS SPINDLE ORIENT Beginning of Operation: N (Operator Message) ; M98 P(1 or 2) ; T M(70 or 71) ; X Z B ; G97 M(51, 52, 53, or 54) S P3 ; G1 X (or) Z F ; Sequence Number and Operator Message Call Safe Index Subprogram Index to Station, Select Tool Offset, Select Spindle Move to Activate Tool Offset, Orient Spindle Cutter RPM, Rotational Direction, Coolant ON, Spindle Select Position Tool at Start Point Machining the Part: Machine the Part (Inches per Minute Feedrate) Reorient Spindle, if Required: X (or) Z F ; B ; Move the Tool to a Clear Area Orient the Spindle End of Operation: X (or) Z F ; M98 P(1 or 2) ; M01 ; Move the Tool to a Clear Area Call Safe Index Subprogram Optional Stop 11-8 M-504A

273 DEACTIVATING LIVE TOOLING NOTICE Be sure the live tooling is not touching the workpiece when the spindle is reactivated. There are two methods for deactivating the live tooling: 1. Programming an M55 will deactivate live tooling and coolant. If coolant is required, be sure to reactivate coolant with an M08, M13, or M14 when standard machining is resumed. 2. Programming a spindle command with a spindle speed will reactivate the spindle and automatically deactivate live tooling if M51, M52, M53, or M54 is not programmed in the same data block. In this case it is not necessary to program an M55 command. LIVE TOOLING PROGRAMMING NOTES 1. Move to enter the tool offset in G00 (rapid) mode. A G01 MUST be programmed on the next move for inch per minute feedrate. 2. Spindle orient is programmed in absolute degrees from the spindle 0 degree mark. 3. Activating live tooling with an M51, M52, M53, or M54 command will NOT automatically stop spindle rotation. 4. Programming an M55 will cancel live tooling commands. 5. Programming a turret index will cancel live tooling commands. 6. Refer to Chapter 9 for information on the Hardinge Safe Index subprograms. M-504A 11-9

274 SAMPLE LIVE TOOLING PROGRAM The sample workpiece is shown in Figure TOOL DEFINITIONS Turret Tooling Station 1, 7/8 End Mill Station 3, #4 Center Drill Station 5, #7 Drill Station 7, ¼ - 20 Tap Operation Sequence 3 Flats (1/8 Depth) 3 Holes (¼ Depth) 3 Holes (9/16 Depth) 3 Holes (7/16 Depth) 2.50 NOTE: All dimensions shown in inches Typ..80 Typ Typ. 7/16 Radius Typ Dia. #4 Center Drill,.25 Deep #7 Drill, 9/16 Deep ¼-20 UNC Tap, 7/16 Deep 3 Places, 120 Apart 3 Places, 120 Apart TI2026 Figure Sample Live Tooling Workpiece M-504A

275 SAMPLE PROGRAM USING C AXIS SPINDLE ORIENT % Stop Code O1135 ; Letter O and Program No. N1 (T0101 7/8 End Mill) ; N Sequence No. and Message (Programmed to Tool Center Line) ; Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift M98 P1 ; Call Safe Index Program O1 T0101 M23 ; Index to Turret Station #1, Offset #1, Activate Contouring Mode X1.25 Z1. C0. ; Move to Enter Offset, Orient Spindle to 0 Degrees M200 ; Main Spindle Brake ON G97 S2500 M53 P3 ; 2500 RPM, Forward/Coolant ON, Select Spindle G1 Z.5 F50. ; Tool Center to.5 from Part Face Z F3. ; Mill IN at 3 ipm X1.6 F50. ; X Axis Clear Move Z.5 ; Z Axis to Start Point M201 ; Spindle Brake OFF X1.25 C120. ; X Axis to Start Point, Orient Spindle to 120 Degrees M200 ; Spindle Brake ON Z F3. ; Mill IN at 3 ipm X1.6 F50. ; X Axis Clear Move Z.5 ; Z Axis to Start Point M201 ; Spindle Brake OFF X1.25 C240. ; X Axis to Start Point, Orient Spindle to 240 Degrees M200 ; Spindle Brake ON Z F3. ; Mill IN at 3 ipm X1.6 F50. ; X Axis Clear Move Z.5 ; Z Axis Clear Move M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF (Optional Command) M55 ; Live Tooling Stop, Coolant OFF M98 P1 ; Call Safe Index Program O1 M01 ; Optional Stop (Continued on next page) M-504A 11-11

276 N3 (T0303 #4 Center Drill) ; N Sequence No. and Message M98 P1 ; Call Safe Index Program O1 T0303 M23 ; Index to Turret Station #3, Offset #3, Activate Contouring Mode X1.6 Z.25 C240. ; Move to Enter Offset, Orient Spindle to 240 Degrees G97 S2000 M53 P3 ; 2000 RPM, Forward/Coolant ON, Spindle Select G1 Z-.8 F50. ; Tool to Z Start Point G87 G99 X.75 F.002 M200 ; Define G87 Side Drilling Cycle, Spindle Brake ON X.75 C0. ; Orient Spindle to 0 Degrees, Drill to Depth X.75 C120. ; Orient Spindle to 120 Degrees, Drill to Depth G80 ; Cancel G87 Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF (Optional Command) M55 ; Live Tooling Stop, Coolant OFF M98 P1 ; Call Safe Index Program O1 M01 ; Optional Stop N5 (T0505 #7 Drill) ; N Sequence No. and Message M98 P1 ; Call Safe Index Program O1 T0505 M23 ; Index to Turret Station #5, Offset #5, Activate Contouring Mode X1.6 Z.25 C120. ; Move to Enter Offset, Orient Spindle to 120 Degrees G97 S1500 M53 P3 ; 1500 RPM, Forward/Coolant ON, Spindle Select G1 Z-.8 F50. ; Tool to Z Start Point G87 G99 X.125 F.003 M200 ; Define G87 Side Drilling Cycle, Spindle Brake ON X.125 C240. ; Orient Spindle to 240 Degrees, Drill to Depth X.125 C0. ; Orient Spindle to 0 Degrees, Drill to Depth G80 ; Cancel G87 Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF (Optional Command) M55 ; Live Tooling Stop, Coolant OFF M98 P1 ; Call Safe Index Program O1 M01 ; Optional Stop M-504A

277 N7 (T0707 ¼-20 Tap) ; N Sequence No. and Message M98 P1 ; Call Safe Index Program O1 T0707 M23 ; Index to Turret Station #7, Offset #7, Activate Contouring Mode X1.7 Z.25 C0. ; Move to Enter Offset, Orient Spindle to 0 Degrees G97 S500 M53 P3 ; 500 RPM, Forward/Coolant ON, Spindle Select G1 Z-.8 F50. ; Tool to Z Start Point M29 S500 ; Activate Rigid Tapping Mode G88 G99 X.375 F.05 M200 ; Define G88 Side Tapping Cycle, Spindle Brake ON X.375 C120. ; Orient Spindle to 120 Degrees, Tap to Depth X.375 C240. ; Orient Spindle to 240 Degrees, Tap to Depth G80 ; Cancel G88 Cycle M24 ; Cancel Contouring Mode M201 ; Spindle Brake OFF (Optional Command) M55 ; Live Tooling Stop, Coolant OFF M98 P1 ; Call Safe Index Program O1 M01 ; Optional Stop M30 ; End Program M-504A 11-13

278 - NOTES M-504A

279 CHAPTER 12 - POLAR AND CYLINDRICAL INTERPOLATION NOTICE Live tooling attachments are available with or without through-tool coolant capability. Live tooling attachments without through-tool coolant capability can be run with or without coolant, as the machining process requires. Live tooling attachments with through-tool coolant capability MUST be run with coolant turned ON. - NOTE - This chapter is intended for programming live tooling operations with spindle motion. Refer to Chapter 11 for information on programming live tooling with a stationary spindle. DATA WORD DESCRIPTIONS The following data words, G codes, and M code are used when programming Polar and Cylindrical Interpolation: A Word - Absolute position command for C axis on the sub-spindle. With Polar Coordinate Interpolation, A values are linear (inch or millimeter) units. With Spindle Orient or Cylindrical Interpolation, A values are in degrees. A decimal point is required with the A word. C Word - Absolute position command for C axis on the main spindle. With Polar Coordinate Interpolation, C values are linear (inch or millimeter) units. With Spindle Orient or Cylindrical Interpolation, C values are in degrees. A decimal point is required with the C word. H Word - Incremental position command for C axis on the main spindle. With Polar Coordinate Interpolation, H values are linear (inch or millimeter) units. When using Spindle Orient or Cylindrical Interpolation, H values are in degrees. G17 - Used to specify the X,C plane. G18 - Used to specify the X,Z plane. G19 - Used to specify the Z,C plane. M-504A 12-1

280 G107 - G112 - G113 - M23 - M24 - M223 - M224 - Specifies Cylindrical Interpolation. Once cylindrical interpolation has been activated, it is only necessary for the programmer to specify the end point of a move by a linear Z value in inches or millimeters, an angular C value in degrees and a feedrate. Moves requiring circular interpolation must be programmed with the appropriate G02 or G03 command and an R value for the arc radius. Specifies Polar Coordinate Interpolation. Cancel Polar Coordinate Interpolation. Activate Contouring mode on the main spindle. This command must be programmed in a block preceding the block calling for C axis. Cancel Contouring mode on the main spindle. Activate Contouring mode on the optional sub-spindle. This command must be programmed in a block preceding the block calling for C axis. Cancel Contouring mode on the optional sub-spindle M-504A

281 POLAR COORDINATE INTERPOLATION Polar Coordinate Interpolation is used when it is desired to perform milling operations on the face of the workpiece that require synchronous movement of the spindle and the live tooling mounted on the turret. When Polar Coordinate Interpolation is commanded by the G112 command, the control interprets several pieces of data to determine the direction and speed that the axes must be moved to reach the commanded end point. The sample programs in this section illustrate of how Polar Coordinate Interpolation is used. Refer also to the guidelines on page 12-5 and to the program format on page COORDINATE SYSTEMS Figure 12.1 shows the coordinate systems used with Polar Coordinate Interpolation. The program examples in this section illustrate the use of these coordinate systems. Main Spindle Rotation A negative C command will cause the main spindle to turn in the forward (M03) direction and a positive C command will cause the main spindle to rotate in the reverse (M04) direction. Sub-Spindle Rotation A negative A command will cause the main spindle to turn in the forward (M33) direction and a positive A command will cause the main spindle to rotate in the reverse (M34) direction. Main Spindle Viewed from Front of Machine Sub-Spindle Viewed from Front of Machine C - - X +Z -Z - - A C and X Axis Moves A and X Axis Moves TI4778A Figure Coordinate System for Polar Coordinate Interpolation M-504A 12-3

282 Defining X, C, and A Axis Motion The programmed end points are defined as coordinates on the appropriate plane. Note the signs for X, C, and A shown in Figure Main Spindle Viewed from Tailstock/Sub-Spindle Sub-Spindle Viewed from Main Spindle +C +X +X +A X0 C0 A0 X0 +C +X +X +A -X -C -A -X -X -C Machine Bed Machine Bed -A -X TI4781 Figure Direction of X, C, and A Axis Motion during Polar Coordinate Interpolation 12-4 M-504A

283 POLAR COORDINATE INTERPOLATION GUIDELINES 1. The following G codes may be used when G112 is active: G01, G02, G03, G40, G41, G42, G65, and G98. Refer to Chapter 1 for descriptions of these G codes. 2. G00 positioning is not allowed when G112 is active. 3. When using circular interpolation, G02 or G03, the arc radius is specified using the R word. 4. M23 contouring mode must be activated before commanding C axis on the main spindle. M223 contouring mode must be activated before commanding C axis on the sub-spindle. Refer to the Polar Coordinate Interpolation programming format, on page The spindle should be oriented to 0 (zero degrees) before commanding Polar Coordinate Interpolation. Refer to the Polar Coordinate Interpolation programming format, on page If machining in the X axis only (Normal Live Tooling Command), do not program G112 to activate Polar Coordinate Interpolation. 7. With G112 active, the tool cannot be programmed to pass over the center of the workpiece. 8. The H word is used to program incremental C axis moves on the main spindle. There is no incremental C axis command for the sub-spindle. 9. Z axis moves are made independently of Polar Coordinate Interpolation. 10. The unit of command for the C axis, when Polar Coordinate Interpolation is used, is inches or millimeters, not degrees. 11. When using cutter compensation during Polar Coordinate Interpolation, the same basic Tool Nose Radius Compensation rules apply as with normal lathe programming. However, the following rules must also be observed: A) The tool radius and the quadrant must be loaded into the tool geometry offset file. For Polar Coordinate Interpolation, the X tool offset represents the center of the cutter and the tool tip location (Quadrant) will be 9. B) The Tool Nose Radius Compensation start up block (G41 or G42 line) must be programmed after the polar interpolation command (G112 line) has been activated. This Tool Nose Radius Compensation block should contain an X and Z axis air move. For Polar Coordinate Interpolation, the X axis move must be equal to at least two times the tool radius entered in the offset file. C) Program the G40 (Tool Nose Radius Compensation Cancel) command before the block containing the G113 (Cancel Polar Coordinate interpolation). 12. Program restart and block restart are not allowed when Polar Coordinate Interpolation is active. 13. Specify the feedrate in inches or millimeters per minute. 14. X values are diameters. 15. A and C values are radii. M-504A 12-5

284 PROGRAM FORMAT FOR POLAR COORDINATE INTERPOLATION - NOTE - This format should be used in conjunction with the general program format provided in Chapter 1. The C or H word is used to command C axis motion on the main spindle. The A word is used to command C axis motion on the sub-spindle. BEGINNING OF OPERATION N ( ) ; Sequence Number and Message M98 P(1 or 2) ; Call Safe Index Subprogram T ; Index and Call Offset X Z M(23 or 223) ; Enter Offset and Activate Contour Mode G97 S M53 (M54) P3 ; Cutter RPM and Direction, Select Spindle C0. (or A0.) ; Orient Spindle to 0 Degrees G1 G112 ; Activate Polar Coordinate Interpolation C_ (or A_) F50. ; Reorient Before Tool Nose Radius Compensation (if desired) ACTIVATE TOOL NOSE RADIUS COMPENSATION G41 (G42) X C(or A) F50. ; Enter Tool Nose Radius Compensation Non-Cutting Air Move Z ; Move to Depth of Cut G1 X and/or C(or A) F ; MACHINE PART Move to Machine Part, IPM Feed CLEAR PART X or Z F ; Move to Clear Part G40 U1. ; Cancel Tool Nose Radius Compensation G113 ; Cancel Polar Coordinate Interpolation M(24 or 224) ; Cancel Contour Mode M55 ; Live Tool Stop M98 P(1 or 2) ; M01 ; END OF OPERATION Call Safe Index Subprogram Optional Stop 12-6 M-504A

285 TOOL NOSE RADIUS COMPENSATION AND CIRCULAR INTERPOLATION USED WITH G112 POLAR COORDINATE INTERPOLATION Main Spindle Figure 12.3 shows the combinations of tool nose radius and circular interpolation codes used with Polar Coordinate Interpolation on the main spindle. Tool motion is shown as viewed from the tailstock/sub-spindle end of the machine. The shaded area of each drawing represents the finished part contour. C0 C0 X0 Active Codes Tool Compensation: G41 Circular Interpolation: G02 Spindle Motion: M03 Active Codes Tool Compensation: G42 Circular Interpolation: G03 Spindle Motion: M04 C0 C0 X0 Active Codes Tool Compensation: G42 Circular Interpolation: G02 Spindle Motion: M03 Active Codes Tool Compensation: G41 Circular Interpolation: G03 Spindle Motion: M04 TI2086 Figure Tool Nose Radius Compensation and Circular Interpolation used with G112 Polar Coordinate Interpolation on the Main Spindle M-504A 12-7

286 Sub-Spindle Figure 12.4 shows the combinations of tool nose radius and circular interpolation codes used with Polar Coordinate Interpolation on the sub-spindle. Tool motion is shown as viewed from the main spindle. The shaded area of each drawing represents the finished part contour. C0 C0 X0 Active Codes Tool Compensation: G42 Circular Interpolation: G03 Spindle Motion: M34 Active Codes Tool Compensation: G41 Circular Interpolation: G02 Spindle Motion: M33 C0 C0 X0 Active Codes Tool Compensation: G41 Circular Interpolation: G03 Spindle Motion: M34 Active Codes Tool Compensation: G42 Circular Interpolation: G02 Spindle Motion: M33 TI2086 Figure Tool Nose Radius Compensation and Circular Interpolation used with G112 Polar Coordinate Interpolation on the Sub-Spindle 12-8 M-504A

287 PROGRAM EXAMPLES - NOTE - Refer to page 12-3 for information on the coordinate systems used with Polar Coordinate Interpolation. The end points must be defined on the coordinate system before the programs can be written. Figure 12.5 shows the end point positions required to write the program for Example 1, on the next page. As illustrated in this figure: X and C are used to define the cutter end points when machining on the main spindle X and A are used to define the cutter end points when machining on the sub-spindle Although the tool cannot actually move around the part, for programming purposes, it is easier to imagine that this is what is taking place. Tool Nose Radius Compensation is used in all of the polar coordinate examples shown in this chapter. When entering the tool orientation code for milling tools, use 0 or 9. Main Spindle Viewed from Tailstock/Sub-Spindle Sub-Spindle Viewed from Main Spindle X0 X.750 C.375 C0 A0 X.750 A.375 X0 X.750 C0. X.750 A0. X-.750 C.375 X.750 C-.375 X.750 A-.375 X-.750 A.375 X-.750 C-.375 X-.750 A-.375 TI4782 Figure End Point Cutter Positions (Tool Nose Radius Compensation Active) M-504A 12-9

288 Start Point Start Point NOTE: All dimensions shown in inches. TI2018 Figure Polar Coordinate Interpolation, Programming Example 1: Square Example 1: Square Figure 12.6 shows a inch diameter piece of stock on which a.750 inch by.200 inch deep square is to be milled. In this example, the diameter of the milling tool is.50 inches MAIN SPINDLE PROGRAMS (START POINT 1) (START POINT 2) (START CUT AT C0) (START CUT AT C-.375) N2 (MILL ¾ SQ R.25 Q9) ; N2 (MILL ¾ SQ R.25 Q9) ; M98P1; M98P1; T0202 ; T0202 ; X1.4Z.2M23; X1.4Z.2M23; G97S900M54P3; G97S900M54P3; C0. ; C0. ; G1 G112 ; G1 G112 ; G41 X.75 Z.1 F50. ; C-.375 F100. ; Z-.2 F3. ; G41 X.75 Z.1 F50. ; C-.375 ; Z-.2 F3. ; X-.75 ; X-.75 ; C.375 ; C.375 ; X.75 ; X.75 ; C0. ; C-.375 ; Z.2 F20. ; Z.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M24 ; M24 ; M98P1; M98P1; M01 ; M01 ; M-504A

289 SUB-SPINDLE PROGRAMS (START POINT 1) (START POINT 2) (START CUT AT A0) (START CUT AT A.375) N2 (MILL ¾ SQ R.25 Q9) ; N2 (MILL ¾ SQ R.25 Q9) ; M98P2; M98P2; T0202 ; T0202 ; X1.4 Z-.2 M223 ; X1.4 Z-.2 M223 ; G97S900M54P3; G97S900M54P3; A0.; A0.; G1 G112 ; G1 G112 ; G41 X.75 Z-.1 F50. ; A.375 F100. ; Z.2 F3. ; G41 X.75 Z-.1 F50. ; A-.375 ; Z.2 F3. ; X-.75 ; X-.75 ; A.375 ; A-.375 ; X.75 ; X.75 ; A0. ; A.375 ; Z-.2 F20. ; Z-.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M224 ; M224 ; M98P2; M98P2; M01 ; M01 ; M-504A 12-11

290 NOTE: All dimensions shown in inches. TI2020 Figure Polar Coordinate Interpolation, Programming Example 2: Hexagon Example 2: Hexagon Figure 12.7 shows a inch diameter piece of stock on which a hexagon is to be machined. The hexagon measures inches across the flats and the width of the flats is.6875 inches. The diameter of the cutter is.25 inches. MAIN SPINDLE PROGRAMS (REVERSE SPINDLE DIRECTION) (FORWARD SPINDLE DIRECTION) N4 (MILL HEX R.125 Q9) ; N4 (MILL HEX R.125 Q9) ; M98P1; M98P1; T0404 ; T0404 ; X1.5Z.2M23; X1.5Z.2M23; G97S750M54P3; G97S750M54P3; C0. ; C0. ; G1 G112 ; G1 G112 ; G42 X Z.1 F50. ; G41 X Z.1 F50. ; Z-.25F3.5; Z-.25F3.5; C.3437 ; C ; X0 C.6875 ; X0 C ; X C.3437 ; X C ; C ; C.3437 ; X0 C ; X0 C.6875 ; X C ; X C.3437 ; C0. ; C0. ; Z.2 F20. ; Z.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M24 ; M24 ; M98P1; M98P1; M01 ; M01 ; M-504A

291 SUB-SPINDLE PROGRAMS N4 (MILL HEX R.125 Q9) ; N4 (MILL HEX R.125 Q9) ; M98P2; M98P2; T0404 ; T0404 ; X1.5 Z-.2 M223 ; X1.5 Z-.2 M223 ; G97S750M54P3; G97S750M54P3; A0.; A0.; G1 G112 ; G1 G112 ; G42 X Z-.1 F50. ; G41 X Z-.1 F50. ; Z.25 F3.5 ; Z.25 F3.5 ; A.3437 ; A ; X0 A.6875 ; X0 A ; X A.3437 ; X A ; A ; A.3437 ; X0 A ; X0 A.6875 ; X A ; X A.3437 ; A0.; A0.; Z-.2 F20. ; Z-.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M224 ; M224 ; M98P2; M98P2; M01 ; M01 ; M-504A 12-13

292 NOTE: All dimensions shown in inches. TI2019 Figure Polar Coordinate Interpolation, Programming Example 3: Triangle Example 3: Triangle Figure 12.8 shows a inch piece of stock that is to have an equilateral triangle with.8438 inch sides machined on it. The diameter of the cutter is.50 inches. MAIN SPINDLE PROGRAMS (FEED INTO PART FACE) (FEED ONTO PART O.D.) N6 (MILL TRIANGLE R.25 Q9) ; N6 (MILL TRIANGLE R.25 Q9) ; M98P1; M98P1; T0606 ; T0606 ; X1.5 Z.2 M23 ; X1.75 Z0 M23 ; G97S650M54P3; G97S650M54P3; C0. ; C0. ; G1 G112 ; G1 G112 ; G41 X.9742 Z.1 F50. ; G41 X1.2 Z-.125 F50. ; Z-.125 F2.5 ; X.9742 F2.5 ; X-.487 C ; X-.487 C ; C.4219 ; C.4219 ; X.9742 C0. ; X.9742 C0. ; Z.2 F20. ; Z.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M24 ; M24 ; M98P1; M98P1; M01 ; M01 ; M-504A

293 SUB-SPINDLE PROGRAMS (FEED INTO PART FACE) (FEED ONTO PART O.D.) N6 (MILL TRIANGLE R.25 Q9) ; N6 (MILL TRIANGLE R.25 Q9) ; M98P2; M98P2; T0606 ; T0606 ; X1.5 Z-.2 M223 ; X1.75 Z0 M223 ; G97S650M54P3; G97S650M54P3; A0.; A0.; G1 G112 ; G1 G112 ; G41 X.9742 Z-.1 F50. ; G41 X1.2 Z.125 F50. ; Z.125 F2.5 ; X.9742 F2.5 ; X-.487 A ; X-.487 A ; A.4219 ; A.4219 ; X.9742 A0. ; X.9742 A0. ; Z-.2 F20. ; Z-.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M224 ; M224 ; M98P2; M98P2; M01 ; M01 ; M-504A 12-15

294 Start Point Start Point NOTE: All dimensions shown in inches. TI2017 Figure Polar Coordinate Interpolation, Programming Example 4: Tongue Example 4: Tongue Figure 12.9 shows a inch piece of stock on which a tongue.625 inch is to be machined. The cutter diameter is.75 inches. MAIN SPINDLE PROGRAMS (START POINT 1) (START POINT 2) (Start CUT AT C0) (START CUT AT C-.5825) N2 (5/8 TONGUE R.375 Q9) ; N2 (5/8 TONGUE R.375 Q9) ; M98P1; M98P1; T0202 ; T0202 ; X2. Z.2 M23 ; X2. Z.2 M23 ; G97S700M54P3; G97S700M54P3; C0. ; C0. ; G1 G112 ; G1 G112 ; G41 X.625 Z.1 F50. ; C F100. ; Z-.156 F3. ; G41 X-.625 Z-.156 F50. ; C ; Z-.156 F.3 ; X-.625 F20. (AIR MOVE) ; C.5825 ; C.5825 F3. ; X.625 F20. ; X.625 F20., (AIR MOVE) ; C ; C0. F3. ; Z.1 F20. ; Z.1 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M24 ; M24; M98P1; M98P1; M01; M01 ; M-504A

295 SUB-SPINDLE PROGRAMS (START POINT 1) (START POINT 2) (Start CUT AT C0) (START CUT AT A.5825) N2 (5/8 TONGUE R.375 Q9) ; N2 (5/8 TONGUE R.375 Q9) ; M98P2; M98P2; T0202 ; T0202 ; X2. Z-.2 M223 ; X2. Z-.2 M223 ; G97S700M54P3; G97S700M54P3; A0.; A0.; G1 G112 ; G1 G112 ; G41 X.625 Z-.1 F50. ; A.5825 F100. ; Z.156 F3. ; G41 X.625 Z-.1 F50. ; A ; Z.156 F.3 ; X-.625 F20. (AIR MOVE) ; A ; A.5825 F3. ; X-.625 F20. (AIR MOVE) ; X.625 F20., (AIR MOVE) ; C.5825 ; A0. F3. ; Z-.1 F20. ; Z-.1 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M224 ; M224 ; M98 P2 ; M98P2; M01; M01 ; M-504A 12-17

296 Radius NOTE: All dimensions shown in inches. TI2021 Figure Polar Coordinate Interpolation, Programming Example 5: Radius Diamond Example 5: Radius Diamond Figure shows a inch diameter piece of stock on which four 1.00 inch radii are to be cut to form a diamond shaped pattern. Cutter diameter is.50 inches. MAIN SPINDLE PROGRAMS (FORWARD SPINDLE) (REVERSE SPINDLE) N6 (MILL DIAMOND R.25 Q9) ; N6 (MILL DIAMOND R.25 Q9) ; M98P1; M98P1; T0606 ; T0606 ; X2. Z.2 M23 ; X2. Z.2 M23 ; G97S800M54P3; G97S800M54P3; C0. ; C0. ; G1 G112 ; G1 G112 ; G41 X1.375 Z.1 F50. ; G42 X1.375 Z.1 F50. ; Z-.2 F3.5 ; Z-.2 F3.5 ; G3 X0 C R1. ; G2 X0 C.6875 R1. ; G3 X C0. R1. ; G2 X C0. R1. ; G3 X0 C.6875 R1. ; G2 X0 C R1. ; G3 X1.375 C0. R1. ; G2 X1.375 C0. R1. ; G1 Z.2 F20. ; G1 Z.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M24 ; M24 ; M98P1; M98P1; M01 ; M01 ; M-504A

297 SUB-SPINDLE PROGRAMS (FORWARD SPINDLE) (REVERSE SPINDLE) N6 (MILL DIAMOND R.25 Q9) ; N6 (MILL DIAMOND R.25 Q9) ; M98P2; M98P2; T0606 ; T0606 ; X2. Z-.2 M223 ; X2. Z.2 M223 ; G97S800M54P3; G97S800M54P3; A0.; A0.; G1 G112 ; G1 G112 ; G41 X1.375 Z-.1 F50. ; G42 X1.375 Z-.1 F50. ; Z.2F3.5; Z.2F3.5; G3 X0 A R1. ; G2 X0 A.6875 R1. ; G3 X A0. R1. ; G2 X A0. R1. ; G3 X0 A.6875 R1. ; G2 X0 A R1. ; G3 X1.375 A0. R1. ; G2 X1.375 A0. R1. ; G1 Z-.2 F20. ; G1 Z-.2 F20. ; G40 U1. ; G40 U1. ; G113 ; G113 ; M224 ; M224 ; M98P2; M98P2; M01 ; M01 ; M-504A 12-19

298 CYLINDRICAL INTERPOLATION NOTICE G19 is programmed to active the Z,C plane for machining during Cylindrical Interpolation. G19 remains active after Cylindrical Interpolation is canceled. G18 must be programmed to specify the X,Z plane for machining after Cylindrical Interpolation is canceled. Refer to page for information on adding the G18 command to the safe index subprograms. Cylindrical Interpolation (G107) is used to perform contoured milling operations on the outside diameter of the workpiece. The Z and C words are used to specify the end points of the moves when using Cylindrical Interpolation on the main spindle. The Z and A words are used to specify the end points of the moves when using Cylindrical Interpolation on the sub-spindle. When using cylindrical interpolation, the C or A word is programmed in degrees. The C or A word is also used to specify the radius of the part in the G107 block which activates cylindrical interpolation. The X word is used to program the depth of cut. Figure shows the coordinate systems used with Cylindrical Interpolation. Main Spindle Viewed from Back of Machine Sub-Spindle Viewed from Back of Machine X + + Z - C + A + + Z - + X - C, X, and Z Axis Moves A, X, and Z Axis Moves TI4779A Figure Coordinate System for Cylindrical Interpolation M-504A

299 PROGRAM FORMAT FOR CYLINDRICAL INTERPOLATION - NOTE - This format should be used in conjunction with the general program format provided in Chapter 1. The C or H word is used to command C axis motion on the main spindle. The A word is used to command C axis motion on the sub-spindle. N ( ) ; M98 P(1 or 2) ; T ; X Z M(23 or 223) ; G97 S M53 (M54) P3 ; G19 C0. (or A0.) ; G1 G107 C(A) (Part Radius) ; C(A) F50. ; BEGINNING OF OPERATION Sequence Number and Message Call Safe Index Subprogram Index and Call Offset Enter Offset and Activate Contour Mode Cutter RPM and Direction, Select Spindle Work Plane Selection, Orient Spindle to 0 Degrees Activate Cylindrical Interpolation and Part Radius Reorient Before Tool Nose Radius Compensation (if desired) G41 (G42) X Z F50. ; ACTIVATE TOOL NOSE RADIUS COMPENSATION Enter Tool Nose Radius Compensation, Non-Cutting Air Move G1 Z and/or C(A) F ; MACHINE PART Move to Machine Part, IPM Feed CLEAR PART X and/or Z and/or C(A) F50. ; Move to Clear Part G40 U1. ; Cancel Tool Nose Radius Compensation G107 C0. (or A0.) ; Cancel Cylindrical Mode G18 ; Work Plane Selection M(24 or 224) ; Cancel Contour Mode M55 ; Live Tool Stop M98 P(1 or 2) ; M01 ; END OPERATION Call Safe Index Subprogram Optional Stop M-504A 12-21

300 CYLINDRICAL INTERPOLATION GUIDELINES 1. The following G codes may be used when G107 is active: G01, G02, G03, G40, G41, G42, G65, and G98. Refer to Chapter 1 for descriptions of these G codes. 2. G00 positioning is not allowed when G107 is active. 3. When using Circular Interpolation, G02 or G03, the arc radius is specified using the R word. 4. M23(223) contouring mode must be activated before commanding the C axis. Refer to Program Format for Cylindrical Interpolation, on page The spindle should be oriented to 0 (zero degrees) before commanding Cylindrical Interpolation. Refer to Program Format for Cylindrical Interpolation, on page The formula for calculating the value of the C or A word is shown in Figures through If machining in the Z axis only (Normal Live Tooling Command), do not program G107 to activate Cylindrical Interpolation. 7. Cylindrical interpolation is activated on the main spindle by commanding G107 and the C word. The value programmed with the C word specifies the radius of the workpiece. Cylindrical interpolation is activated on the sub-spindle by commanding G107 and the A word. The value programmed with the A word specifies the radius of the workpiece. 8. The H word is used to program incremental C axis moves on the main spindle. There is no incremental C axis command for the sub-spindle. 9. The unit of command for the C axis, when Cylindrical Interpolation is used, is degrees, not inches or millimeters. 10. When using cutter compensation with Cylindrical Interpolation, the same basic Tool Nose Radius Compensation rules apply as with normal lathe programming. However, the following rules must also be observed: A) The tool radius and the quadrant must be loaded into the tool geometry offset file. For cylindrical interpolation, the Z tool offset represents the center of the cutter and the tool tip location (Quadrant) will be 9. B) The Tool Nose Radius Compensation start up block (G41 or G42 line) must be programmed after the Cylindrical Interpolation command (G107 line) has been activated. Refer to Program Format for Cylindrical Interpolation, on page This Tool Nose Radius Compensation block should contain an X and Z axis air move. For Cylindrical Interpolation, the Z axis move must be equal to at least the tool radius amount entered in the offset file. C) Program the G40 (Tool Nose Radius Compensation Cancel) command before the block containing the G107 C0 command (Cancel Cylindrical Interpolation). Refer to Program Format for Cylindrical Interpolation on page Program restart and block restart are not allowed when Cylindrical Interpolation is active. 12. Specify the feedrate in inches or millimeters per minute M-504A

301 TOOL NOSE RADIUS COMPENSATION AND CIRCULAR INTERPOLATION USED WITH G107 CYLINDRICAL INTERPOLATION Main Spindle Figure shows the combinations of tool nose radius and circular interpolation codes used with cylindrical interpolation at the main spindle. The part circumference is viewed laying flat with the part face (Z0) at the base. Z0 Z0 CAxis CAxis Z0 (Part Face) Z0 (Part Face) Tool Compensation: G41 Circular Interpolation: G02 Tool Compensation: G42 Circular Interpolation: G03 Z0 Z0 CAxis CAxis Z0 (Part Face) Tool Compensation: G42 Circular Interpolation: G02 Z0 (Part Face) Tool Compensation: G41 Circular Interpolation: G03 TI2087 Figure Tool Nose Radius Compensation and Circular Interpolation used with G107 Cylindrical Interpolation on the Main Spindle M-504A 12-23

302 Sub-Spindle Figure shows the combinations of tool nose radius and circular interpolation codes used with cylindrical interpolation at the sub-spindle. The part circumference is viewed laying flat with the part face (Z0) at the base. Z0 Z0 CAxis CAxis Z0 (Part Face) Tool Compensation: G42 Circular Interpolation: G03 Z0 (Part Face) Tool Compensation: G41 Circular Interpolation: G02 Z0 Z0 CAxis CAxis Z0 (Part Face) Tool Compensation: G41 Circular Interpolation: G03 Z0 (Part Face) Tool Compensation: G42 Circular Interpolation: G02 TI4783 Figure Tool Nose Radius Compensation and Circular Interpolation used with G107 Cylindrical Interpolation on the Sub-Spindle M-504A

303 NOTE: All dimensions shown in inches. Circumference inches Inch x x 360 Degree Circumference Z Z Z R.194 Z C0 C (-.1875) C (-.375) TI1985A Figure Cylindrical Interpolation: Lettering on the Part Diameter (Main Spindle Viewed from Back of Machine) PROGRAMMING EXAMPLES Example 6: Lettering on Part Diameter MAIN SPINDLE PROGRAM (Refer to Figure 12.14) N2 (Sharp Tool.025 Depth) ; M98P1; T0202 ; X1.6 Z-.5 M23 ; G97S850M53P3; G19 C0. ; G1 G107 C.7 ; X1.35F4.5; C F3. ; Z-.7 ; C ; X1.5 F20. ; C0. ; X1.35F4.5; C F3. ; Z-.5 ; C ; X1.5 F20. ; Z-.750 ; X1.35F4.5; C0. F3. ; Z-.85 ; G2 Z-.85 C R.094 ; G1 Z-.750 ; Z-.85 F5. ; G2 Z-.85 C R.094 F3. ; G1 Z-.75 ; X1.5 F20. ; Z-.994 ; X1.35F4.5; Z F3. ; X1.5 F20. ; C0. ; X1.35F4.5; Z-.994 F3. ; Z F5. ; C F3. ; X1.5 F20. ; G107 C0. ; G18 ; M24 ; M98P1; M01 ; M-504A 12-25

304 NOTE: All dimensions shown in inches. Circumference inches Inch x x 360 Degree Circumference Z Z Z R.194 Z A0 A15.34 (.1875) A30.69 (.375) TI4784 Figure Cylindrical Interpolation: Lettering on the Part Diameter (Sub-Spindle Viewed from Back of Machine) SUB-SPINDLE PROGRAM (Refer to Figure 12.15) N2 (Sharp Tool.025 Depth) ; G2 Z.85 A15.34 R.094 ; M98P2; G1Z.750; T0202 ; Z.85 F5. ; X1.6 Z.5 M223 ; G2 Z.85 A30.69 R.094 F3. ; G97S850M53P3; G1Z.75; G19 A0. ; X1.5 F20. ; G1 G107 A.7 ; Z.994 ; X1.35F4.5; X1.35F4.5; A15.34 F3. ; Z1.094 F3. ; Z.7 ; X1.5 F20. ; A30.69 ; A0. ; X1.5 F20. ; X1.35 F4.5 ; A0. ; Z.994 F3. ; X1.35 F4.5 ; Z1.044 F5. ; A15.34 F3. ; A30.69 F3. ; Z.5 ; X1.5 F20. ; A30.69 ; G107 A0. ; X1.5 F20. ; G18 ; Z.750 ; M224 ; X1.35F4.5; M98P2; A0. F3. ; M01 ; Z.85 ; M-504A

305 NOTE: All dimensions shown in inches. Z C0 C (-.375) Z Circumference inches Inch x x 360 Degree Circumference ( = ) Z-.700 TI1988A Figure Cylindrical Interpolation: Rectangle Etched on the Part Diameter (Main Spindle Viewed from Back of Machine) Example 7: Rectangle Etched on Part Diameter MAIN SPINDLE (Refer to Figure 12.16) N4 (Sharp Tool.020 Depth) ; M98P1; T0404 ; X1.7 Z-.7 M23 ; G97 S1500 M53 P3 ; G19 C0. ; G1 G107 C.750 ; X1.46F3.5; Z-1.3 ; C ; Z-.7 ; C0. ; X1.6 F20. ; G107 C0. ; G18 ; M24 ; M98P1; M01 ; M-504A 12-27

306 NOTE: All dimensions shown in inches Z A0 A28.64 (.375) Z1.300 Z Circumference inches Inch x x 360 Degree Circumference ( = ) TI4785 Figure Cylindrical Interpolation: Rectangle Etched on the Part Diameter (Sub-Spindle Viewed from Back of Machine) SUB-SPINDLE (Refer to Figure 12.17) N4 (Sharp Tool.020 Depth) ; M98P2; T0404 ; X1.7 Z.7 M223 ; G97 S1500 M53 P3 ; G19 A0. ; G1 G107 A.750 ; X1.46F3.5; Z1.3 ; A28.64 ; Z.7 ; A0. ; X1.6 F20. ; G107 A0. ; G18 ; M224 ; M98P2; M01 ; M-504A

307 NOTE: All dimensions shown in inches. Z /8 Radius (4) C0 C-.5 Z Circumference inches Inch x x 360 Degree Circumference ( = ) Start Point Z-.750 Tool Path Typical Corner TI1989A Figure Cylindrical Interpolation: Rectangle with Corner Radius (Main Spindle Viewed from Back of Machine) Example 8: Rectangle with Corner Radius MAIN SPINDLE (Refer to Figure 12.18) N6 (Sharp Tool.02 Depth) ; G2 Z-1.5 C R.125 ; M98P1; G1Z-.875; T0606 ; G2 Z-.750 C R.125 ; X1.6 Z-.875 M23 ; G1 C-9.96 ; G97 S1200 M53 P3 ; G2 Z-.875 C0. R.125 ; G19 C0. ; G1 X1.5 F20. ; G1 G107 C.7185 ; G107 C0. ; X1.397 F4. ; G18 ; Z-1.5 F3. ; M24 ; G2 Z C-9.96 R.125 ; M98 P1 ; G1 C ; M01 ; M-504A 12-29

308 NOTE: All dimensions shown in inches Z /8 Radius (4) A0 A.5 Z Start Point Z.750 Tool Path Typical Corner Circumference inches Inch x x 360 Degree Circumference ( = ) TI4786 Figure Cylindrical Interpolation: Rectangle with Corner Radius (Sub-Spindle Viewed from Back of Machine) SUB-SPINDLE (Refer to Figure 12.19) N6 (Sharp Tool.02 Depth) ; G3 Z1.5 A R.125 ; M98P2; G1Z.875; T0606 ; G3 Z.750 A R.125 ; X1.6 Z.875 M223 ; G1 A-9.96 ; G97 S1200 M53 P3 ; G3 Z.875 A0. R.125 ; G19 A0. ; G1 X1.5 F20. ; G1 G107 A.7185 ; G107 A0. ; X1.397 F4. ; G18 ; Z1.5 F3. ; M224 ; G3 Z1.625 A-9.96 R.125 ; M98 P2 ; G1 A ; M01 ; M-504A

309 NOTE: All dimensions shown in inches Pitch.125 TI2124 Figure Cylindrical Interpolation: Worm Gear (Main Spindle) Example 9: Worm Gear MAIN SPINDLE (Refer to Figure 12.20) To calculate the total amount of C in degrees: (Z travel pitch) x 360 N2 (1/8" END MILL, 5/16" PITCH) ; M98P1; T0202 ; X.95 Z-.3 M23 ; G97 S1200 M53 P3 ; G19 C0. ; G1 G107 C.375 ; X.5 F4. ; Z-2.05 C F2. ; X.85 F20. ; G107 C0. ; G18 ; M24 ; M98P1; M01 ; NOTES: 1. C- command (forward spindle) for right-hand thread. 2. X, Z, and C data words may be programmed together in the same block if the root diameter is to increase or decrease (tapered thread). M-504A 12-31

310 NOTE: All dimensions shown in inches Pitch TI4787 Figure Cylindrical Interpolation: Worm Gear (Sub-Spindle) SUB-SPINDLE (Refer to Figure 12.21) To calculate the total amount of C in degrees: (Z travel pitch) x 360 N2 (1/8" END MILL, 5/16" PITCH) ; M98P2; T0202 ; X.95 Z.3 M223 ; G97 S1200 M53 P3 ; G19 A0. ; G1 G107 A.375 ; X.5 F4. ; Z2.05 A2016. F2. ; X.85 F20. ; G107 A0. ; G18 ; M224 ; M98P2; M01 ; NOTES: 1. A+ command (reverse spindle) for right-hand thread. 2. X, Z, and A data words may be programmed together in the same block if the root diameter is to increase or decrease (tapered thread) M-504A

311 C AXIS ALARMS - NOTE - For a complete listing of control error codes, refer to the Fanuc Operation Manual. Alarm Description 021 An axis not included in selection plane was commanded in Circular Interpolation. Cylindrical Interpolation requires G In the plane selected, two or more axes in the same direction are commanded. 041 Overcutting will occur in Tool Nose Radius Compensation. 145 Polar Coordinate Interpolation commands G112 and G113 require that Tool Nose Radius Compensation be inactive (G40 condition). 146 Illegal G code commanded while in Polar Coordinate Interpolation (G00 is not allowed). 175 Cylindrical Interpolation G107 must have C(part radius) or A(part radius) at start and C0. or A0. at end. Tool Nose Radius Compensation must be inactive when above commands are read (G40 condition). 176 Illegal G code has been commanded while in Cylindrical Interpolation (G00, G28, G50, G52 - G59, G76, G81 - G89 are not allowed). 197 M23(223) contour mode must be active for C axis commands. 212 Insert Chamfer and Insert Corner Radius commands are allowed only while X,Z plane is active. Illegal command while Polar Coordinate Interpolation or Cylindrical Interpolation is active. M-504A 12-33

312 - NOTES M-504A

313 CHAPTER 13 - BLUEPRINT PROGRAMMING INTRODUCTION The Blueprint Programming feature allows the programmer to define the part contour by specifying the end point values along with the desired angle. The intersection points of the straight lines are input as coordinate values or a coordinate value and an angle. Straight lines can be directly connected to form sharp, chamfered, or rounded corners. It is only necessary to specify the size of the chamfer or corner radius and the CNC control performs the required calculations. The respective end point coordinates can be programmed using absolute or incremental positioning data. Linear Interpolation (G01) must be active while blueprint programming blocks are executed. ANGLE DEFINITIONS Angles are defined by referencing the part contour to a zero reference angle. Refer to Figures 13.1 and The determining factor for selecting the appropriate angle definition is the turret to perform the machining. The data word format for angle definition (A Words) is 3.4. A comma MUST precede an A (angle) command and a decimal point MUST be programmed with the numerical value. Minimum Input Value:.0001 degrees Maximum Input Value: degrees +90 Angle Command: A30. Positive 0 30 Workpiece 180 ZAxis Negative 0 Workpiece Angle Command: A-30. Figure Angle Definitions for Main Spindle Operation TI4559 M-504A 13-1

314 Angle Command: A30. Positive 0 Workpiece 180 ZAxis Negative 0 Workpiece Angle Command: A-30. Figure Angle Definitions for Sub-Spindle Operation TI4560 BLUEPRINT PROGRAMMING EXAMPLES Eight basic examples of blueprint programming are illustrated in Figures 13.3 through 13.34, beginning on page The lines of programming which accompany each of these examples illustrate the programming format used for blueprint programming. These basic examples can be combined to form a wide range of programming variations. - NOTE - The numerical values shown in the following examples are not coordinate values. They serve only as part of the coordinate designation to help distinguish between the various X, Z,,A,,C, and,r values M-504A

315 EXAMPLE 1: TWO POINTS (Refer to Figures 13.3 through 13.6) N X 2,A ; or N Z 2,A ; This basic two point definition allows the programmer to specify a linear move by either programming an X and an A word or programming a Z and an A word. The CNC control moves the tool nose reference point from the start point at the prescribed angle until the appropriate position register is equal to the programmed coordinate value. OPERATION AT THE MAIN SPINDLE +X (End Point) X 2,Z 2 +X X2. Z? X.4 Z0. ; Z-.687 ; X2.,A28. ; A X 1,Z 1 (Start Point) +Z 28 Z-.687 X.4 Z0. +Z TI1836 TI1836 Figure Linear Move Between Two Points Figure Sample Program Segment OPERATION AT THE SUB-SPINDLE +X +X X.4 Z0. ; Z.687 ; X2.,A152. ; (End Point) X 2,Z 2 X2. Z? A X 1,Z 1 (Start Point) +Z X.4 Z Z.687 +Z TI4538 TI4538 Figure Linear Move Between Two Points Figure Sample Program Segment M-504A 13-3

316 EXAMPLE 2: THREE POINTS (Refer to Figures 13.7 through 13.10) N,A 1 ; N X 3 Z 3,A 2 ; This basic three point definition allows the programmer to specify two consecutive linear moves. The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The second linear move is programmed with an X, Z, and an A word (,A 2 ). The X and Z values specify the end point of the second linear move. The A word specifies the angle of the second linear move in relation to the zero reference angle. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection point of the two linear moves. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the calculated intersection point. The control then moves the tool nose reference point from the calculated intersection point to the programmed endpoint, as defined by the X 3 and Z 3 coordinates. OPERATION AT THE MAIN SPINDLE +X (End Point) X 3,Z 3 +X X2. Z-1.8 X.4 Z0. ; Z-.6 ;,A20. ; X2. Z-1.8,A43. ; A 2 43 X 2,Z 2 A 1 X 1,Z 1 (Start Point) +Z X? Z? 20 Z-.6 X.4 Z0. +Z TI1837 TI1837 Figure Linear Moves Between Three Points Figure Sample Program Segment 13-4 M-504A

317 OPERATION AT THE SUB-SPINDLE +X (End Point) X 3,Z 3 +X X.4 Z0. ; Z.6 ;,A160. ; X2. Z1.8,A137. ; X2. Z1.8 A A 1 X 1,Z 1 (Start Point) X 2,Z 2 +Z X.4 Z X? Z? Z.6 +Z TI4540 TI4540 Figure Linear Moves Between Three Points Figure Sample Program Segment M-504A 13-5

318 EXAMPLE 3: THREE POINTS WITH A RADIUS (Refer to Figures through 13.14) This three point definition allows the programmer to specify two linear moves with a radius automatically inserted at the intersection of the two moves. Two methods of programming are illustrated in this example. The first method uses programmed end points for both linear moves. The second method uses an angle definition for the first linear move and programmed end points for the second linear move. Method #1: N X 2 Z 2,R 1 ; N X 3 Z 3 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed radius. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the programmed radius and performs a linear move to arrive at the programmed endpoint, as defined by the X 3 and Z 3 coordinates. Method #2: N,A 1,R 1 ; N X 3 Z 3,A 2 ; The first straight line move is programmed with an A word (,A 1 ). This A word specifies the angle of the first straight line move in relation to the zero reference angle. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3,Z 3, and A 2 data words. The X and Z coordinate values specify the end point of the second linear move. The A word specifies the angle. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection point of the two linear moves as well as the insertion of the programmed radius. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the programmed radius and performs a linear move to arrive at the programmed endpoint, as defined by the X 3,Z 3, and A M-504A

319 OPERATION AT THE MAIN SPINDLE +X (End Point) X 3,Z 3 +X X2.4 Z-1.8 X.4 Z0. ; Z-.5 ;,A25.,R.1 ; X2.4 Z-1.8,A60. ; A 2 R 60.1R X 2,Z 2 A 1 X 1,Z 1 (Start Point) +Z X? Z? 25 Z-.5 X.4 Z0. +Z TI1838 TI1838 Figure Radius Inserted Between Two Linear Moves Figure Sample Program Segment (Using Method #2) OPERATION AT THE SUB-SPINDLE +X (End Point) X 3,Z 3 +X X.4 Z0. ; Z.5 ;,A155.,R.1 ; X2.4 Z1.8,A120. ; X2.4 Z1.8 R A 2.1R 120 A 1 X 1,Z 1 (Start Point) X 2,Z 2 +Z X.4 Z Z.5 X? Z? +Z TI4542 TI4542 Figure Radius Inserted Between Two Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-7

320 EXAMPLE 4: THREE POINTS WITH A CHAMFER (Refer to Figure through 13.18) This three point definition allows the programmer to specify two linear moves with a chamfer automatically inserted at the intersection of the two moves. Two methods of programming are illustrated in this example. The first method uses programmed end points for both linear moves. The second method uses an angle definition for the first linear move and programmed end points along with an angle definition for the second linear move. Method #1: N X 2 Z 2,C 1 ; N X 3 Z 3 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed chamfer. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the programmed chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the X 3 and Z 3 coordinates. Method #2: N,A 1,C 1 ; N X 3 Z 3,A 2 ; The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3,Z 3, and A 2 data words. The X and Z coordinate values specify the end point of the second linear move. The A word specifies the angle. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection point of the two linear moves as well as the insertion of the programmed chamfer. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the programmed chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the X 3,Z 3, and A M-504A

321 OPERATION AT THE MAIN SPINDLE +X (End Point) X 3,Z 3 +X X2.3 Z-1.9 X.4 Z0. ; Z-.5 ;,A18.,C.125 ; X2.3 Z-1.9,A65. ; A 2 65 X 2,Z 2 X? Z? C A 1 X 1,Z 1 (Start Point) +Z Z-.5 X.4 Z0. +Z TI1839 TI1839 Figure Chamfer Inserted Between Two Linear Moves Figure Sample Program Segment (Using Method #2) OPERATION AT THE SUB-SPINDLE +X (End Point) X 3,Z 3 +X X.4 Z0. ; Z.5 ;,A162.,C.125 ; X2.3 Z1.9,A115. ; X2.3 Z1.9 A A 1 X 1,Z 1 (Start Point) X 2,Z 2 C +Z X.4 Z Z.5 X? Z?.125 +Z TI4544 TI4544 Figure Chamfer Inserted Between Two Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-9

322 EXAMPLE 5: FOUR POINTS WITH TWO RADII (Refer to Figures through 13.22) This four point definition allows the programmer to specify three linear moves with a radius automatically inserted at each of the two intersection points. Two methods of programming are illustrated in this example. The first method uses programmed end points for all three linear moves. The second method uses an angle definition for the first linear move, angle and end point data for the second linear move, and programmed end points for the third linear move. Method #1: N X 2 Z 2,R 1 ; N X 3 Z 3,R 2 ; N Z 4 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The radius (,R 2 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed radii. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the first radius is to begin. The control moves the tool nose reference point through the proper arc to create the first programmed radius and then performs a linear move to arrive at the point where the second radius is to begin. The control moves the tool nose reference point through the proper arc to create the second programmed radius and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate M-504A

323 Method #2: N,A 1,R 1 ; N X 3 Z 3,A 2,R 2 ; N Z 4 ; The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The angle definition for the second linear move (,A 2 ) supplies the CNC control with the information required to calculate the intersection point of the first and second linear moves. The radius (,R 2 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection points of the three linear moves as well as the insertion of the programmed radii. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the first programmed radius and then performs a linear move to arrive at the point where the second radius is to begin. The control moves the tool nose reference point through the proper arc to create the second programmed radius and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate. OPERATION AT THE MAIN SPINDLE +X Z 4 (End Point) X 3,Z 3 +X Z-2.3 X2.25 Z-1.8 X.4 Z0. ; Z-.5 ;,A20.,R.2 ; X2.25 Z-1.8,A60.,R.4 ; Z-2.3 ; R 2 A 2.4R 60 R 1.2R X 2,Z 2 A 1 X 1,Z 1 (Start Point) +Z X? Z? 20 Z-.5 X.4 Z0. +Z TI1840 TI1840 Figure Two Radii Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-11

324 OPERATION AT THE SUB-SPINDLE +X A 2 X 3,Z 3 R 2 Z 4 (End Point) +X X.4 Z0. ; Z.5 ;,A160.,R.2 ; X2.25 Z1.8,A120.,R.4 ; Z2.3 ; 120 X2.25 Z1.8.4R Z2.3 R 1.2R A 1 X 1,Z 1 (Start Point) X 2,Z 2 +Z X.4 Z Z.5 X? Z? +Z TI4546 TI4546 Figure Two Radii Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A

325 EXAMPLE 6: FOUR POINTS WITH TWO CHAMFERS (Refer to Figures through 13.26) This four point definition allows the programmer to specify three linear moves with a chamfer automatically inserted at each of the two intersection points. Two methods of programming are illustrated in this example. The first method uses programmed end points for all three linear moves. The second method uses an angle definition for the first linear move, angle and end point data for the second linear move, and programmed end points for the third linear move. Method #1: N X 2 Z 2,C 1 ; N X 3 Z 3,C 2 ; N X 4 Z 4 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The chamfer (,C 2 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the X 4 and Z 4 data words. The X and Z coordinate values specify the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed chamfers. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the first chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the first chamfer and then performs a linear move to arrive at the point where the second chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the second chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the X 4 and Z 4 coordinates. M-504A 13-13

326 Method #2: N,A 1,C 1 ; N X 3 Z 3,A 2,C 2 ; N X 4 Z 4 ; The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The angle definition for the second linear move (,A 2 ) supplies the CNC control with the information required to calculate the intersection point of the first and second linear moves. The chamfer (,C 2 ) is programmed in the same data block as the second linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection points of the three linear moves as well as the insertion of the programmed chamfers. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the first chamfer and then performs a linear move to arrive at the point where the second chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the second chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the X 4 and Z 4 coordinates. OPERATION AT THE MAIN SPINDLE +X C 2 +X.156 X.4 Z0. ; Z-.5 ;,A20.,C.07 ; X2.3 Z-1.75,A63.,C.156 ; X2.4 Z-2.2 ; X 4 Z 4 (End Point) X 3,Z 3 X2.4 Z-2.2 X2.3 Z-1.75 A 2 63 X 2,Z 2 X? Z? C 1 A 1 X 1,Z 1 (Start Point) +Z Z-.5 X.4 Z0. +Z Figure Two Chamfers Inserted Between Three Linear Moves TI1841 TI1841 Figure Sample Program Segment (Using Method #2) M-504A

327 OPERATION AT THE SUB-SPINDLE +X C 2 +X X.4 Z0. ; Z.5 ;,A160.,C.07 ; X2.3 Z1.75,A117.,C.156 ; X2.4 Z2.2 ;.156 X 3,Z 3 X 4 Z 4 (End Point) X2.3 Z1.75 X2.4 Z2.2 A X 2,Z 2 X? Z? A 1 X 1,Z 1 (Start Point) C 1 +Z X.4 Z Z Z TI4548 TI4548 Figure Two Chamfers Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-15

328 EXAMPLE 7: FOUR POINTS WITH ONE RADIUS AND CHAMFER (Refer to Figures through 13.30) This four point definition allows the programmer to specify three linear moves with a radius automatically inserted at the first intersection point and a chamfer automatically inserted at the second intersection point. Two methods of programming are illustrated in this example. The first method uses programmed end points for all three linear moves. The second method uses an angle definition for the first linear move, angle and end point data for the second linear move, and a programmed end point for the third linear move. Method #1: N X 2 Z 2,R 1 ; N X 3 Z 3,C 1 ; N Z 4 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The chamfer (,C 1 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed radius and chamfer. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the radius and then performs a linear move to arrive at the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate M-504A

329 Method #2: N,A 1,R 1 ; N X 3 Z 3,A 2,C 1 ; N Z 4 ; The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The radius (,R 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The angle definition for the second linear move (,A 2 ) supplies the CNC control with the information required to calculate the intersection point of the first and second linear moves. The chamfer (,C 1 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection points of the three linear moves as well as the insertion of the programmed radius and chamfer. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the radius and then performs a linear move to arrive at the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the chamfer and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate. OPERATION AT THE MAIN SPINDLE +X +X X.4 Z0. ; Z-.5 ;,A22.,R.25 ; X2.5 Z-2.03,A60.,C.2 ; Z-2.5 ; Z 4 (End Point) X 3,Z 3 C A 2 Z X2.5 Z R.25R X 2,Z 2 A 1 X 1,Z 1 (Start Point) +Z X? Z? 22 Z-.5 X.4 Z0. +Z TI1842 TI1842 Figure Radius and Chamfer Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-17

330 OPERATION AT THE SUB-SPINDLE +X A 2 C X 3,Z 3 Z 4 (End Point) +X X.4 Z0. ; Z.5 ;,A158.,R.25 ; X2.5 Z2.03,A120.,C.2 ; Z2.5 ; X2.5 Z Z2.5 R.25R A 1 X 1,Z 1 (Start Point) X 2,Z 2 +Z X.4 Z Z.5 X? Z? +Z TI4550 TI4550 Figure Radius and Chamfer Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A

331 EXAMPLE 8: FOUR POINTS WITH ONE CHAMFER AND RADIUS (Refer to Figures through 13.34) This four point definition allows the programmer to specify three linear moves with a chamfer automatically inserted at the first intersection point and a radius automatically inserted at the second intersection point. Two methods of programming are illustrated in this example. The first method uses programmed end points for all three linear moves. The second method uses an angle definition for the first linear move, angle and end point data for the second linear move, and a programmed end point for the third linear move. Method #1: N X 2 Z 2,C 1 ; N X 3 Z 3,R 1 ; N Z 4 ; The first straight line move is programmed with the X 2 and Z 2 data words. These data words specify the intersection point of the first and second linear moves. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The radius (,R 1 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the insertion of the programmed chamfer and radius. The tool nose reference point is moved from the start point, designated X 1 Z 1, toward the programmed end point, designated X 2 Z 2, until the tool nose reference point reaches the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the chamfer and then performs a linear move to arrive at the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the radius and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate. M-504A 13-19

332 Method #2: N,A 1,C 1 ; N X 3 Z 3,A 2,R 1 ; N Z 4 ; The first linear move is programmed with an A word (,A 1 ). This A word specifies the angle of the first linear move in relation to the zero reference angle. The chamfer (,C 1 ) is programmed in the same data block as the first linear move. The second linear move is programmed with the X 3 and Z 3 data words. The X and Z coordinate values specify the end point of the second linear move. The angle definition for the second linear move (,A 2 ) supplies the CNC control with the information required to calculate the intersection point of the first and second linear moves. The radius (,R 1 ) is programmed in the same data block as the second linear move. The third linear move is programmed with the Z 4 data word. The Z coordinate value specifies the end point of the third linear move. Based on the data programmed in the blueprint programming blocks, the CNC control calculates the intersection points of the three linear moves as well as the insertion of the programmed chamfer and radius. The tool nose reference point is moved from the start point at the prescribed angle until the tool nose reference point reaches the point where the chamfer is to begin. The control moves the tool nose reference point in the proper direction to create the chamfer and then performs a linear move to arrive at the point where the radius is to begin. The control moves the tool nose reference point through the proper arc to create the radius and then performs a linear move to arrive at the programmed endpoint, as defined by the Z 4 coordinate. OPERATION AT THE MAIN SPINDLE +X +X X.4 Z0. ; Z-.5 ;,A17.,C.09 ; X2. Z-1.5,A56.,R.25 ; Z-2.1 ; X 3,Z 3 X2. Z-1.5 Z 4 (End Point) R A 2 Z R 56 X 2,Z 2 X? Z? C A 1 X 1,Z 1 (Start Point) +Z Z-.5 X.4 Z0. +Z TI1843 Figure Chamfer and Radius Inserted Between Three Linear Moves TI1843 Figure Sample Program Segment (Using Method #2) M-504A

333 OPERATION AT THE SUB-SPINDLE +X +X X.4 Z0. ; Z.5 ;,A163.,C.09 ; X2. Z1.5,A124.,R.25 ; Z2.1 ; X 3,Z 3 X2. Z1.5 A 2 R Z 4 (End Point) R Z2.1 A 1 X 1,Z 1 (Start Point) X 2,Z 2 C +Z X.4 Z Z.5 X? Z?.09 +Z TI4552 TI4552 Figure Chamfer and Radius Inserted Between Three Linear Moves Figure Sample Program Segment (Using Method #2) M-504A 13-21

334 .0625 Chamfer.125 Radius.125 Radius.0625 Chamfer.06 Radius TI1774 Figure Finished Workpiece for Sample Program BLUEPRINT PROGRAMMING SAMPLE PROGRAM This sample program is written for operation at the main spindle. Refer to Figure N1 (Finish Face and Turn R.015 Q3) ; Sequence Number and Operator Message G97 S1000 M13 P1 ; Main Spindle Forward 1000 RPM/Coolant ON M98 P1 ; Call Safe Index Subprogram O1 T0101 ; Index to Station 1 and Select Tool Offset 1 X Z0.2 ; Move Tool to Activate Tool Offset G50 S4000 ; Constant Surface Speed 4000 RPM Limit G96 S370 ; Establish Constant Surface Speed, 370 Surface Feet per Minute G1 G42 X-0.03 Z.1 F100. ; Move to Activate Tool Nose Radius Compensation G99 Z0. F.004 ; Feed to Face of Workpiece X1.,R0.06; Cuttoa1inchDiameter,Inserta.06Radius Z-0.25,C ; Cut to Z-.25, Insert a.0625 Chamfer X0.5,A230.,R0.125 ; Cut to a.5 inch diameter at an angle of 230 degrees, Insert a.125 Radius,A180.,R.125 ; Cut at 180 degree angle, Insert a.125 radius X1. Z-1.375,A130.,C ; Cut to a1inchdiameter,cuttoz-1.375, Cut at an angle of 130 degrees, Insert a.0625 Chamfer Z ; Cut to Z X1.09 ; Clear workpiece by three times the tool nose diameter. M98 P1 ; Call Safe Index Subprogram O1 M01 ; Optional Stop M-504A

335 BLUEPRINT PROGRAMMING NOTES 1. A comma must precede an A (angle), C (chamfer), or R (radius) command. 2. When a chamfer in inserted, the chamfer will be equal on both sides of the lines intersected. 3. When a radius in inserted, the radius must be tangentially blended between the two moves. If a non-tangential radius is required, program the radius using a G02/G03 code. 4. When programming either an insert chamfer or radius, the intersection point must be programmed. 5. The value of the chamfer or radius is always positive and it is to be programmed at the end of the first linear move. 6. When defining angles, the decimal point MUST be programmed. 7. G01 (Linear Interpolation) must be active while blueprint programming blocks are executed. M-504A 13-23

336 - NOTES M-504A

337 CHAPTER 14 - SUB-SPINDLE [Option] INTRODUCTION The sub-spindle allows the workpiece to be machined at both ends without stopping the machine to end-for-end the workpiece. This reduces cycle time by reducing or eliminating handling of the workpiece by the machine operator. Drilling, boring, turning, and facing operations can be performed on a workpiece that is chucked in the sub-spindle. Depending on the machining sequence that is selected, the first end of the workpiece is machined in either the main spindle or sub-spindle. The workpiece is then transferred to the other spindle to complete machining of the second end. The maximum sub-spindle speed is shown in the following table. Machine Model Maximum RPM T-42 Lathe (16C Main Spindle) 6,000 T-42 Big Bore Lathe (20C Main Spindle) 6,000 T-51 Lathe (20C Main Spindle) 5,000 T-65 Lathe (25C Main Spindle) 5,000 TRAVEL SPECIFICATIONS The sub-spindle travel is established at the factory. Refer to page A1-8 for the sub-spindle travel specifications. M-504A 14-1

338 PROGRAMMING AXIS MOTION FEEDRATE Sub-spindle feedrate is commanded by the F data word, with a maximum programmable feedrate of 150 in/min [3,810 mm/min]. Refer to Chapter 1 for additional information on the F data word. E AXIS MOTION - NOTE - When E axis motion is programmed by itself, the sub-spindle moves at the programmed feedrate. When E axis motion is programmed with X and/or Z axis motion, the sub-spindle moves at a compensated feedrate to cause the sub-spindle to complete the move at the same time as the other axes. The E data word is used to command direction and distance when moving the sub-spindle. The face of the sub-spindle is the sub-spindle reference point. The E data word commands an absolute move referenced against the Z0 (zero) position of the machine coordinate position. Positive E coordinates are to the right of Z0 and negative E coordinates are to the left of Z0. The Z0 position will be equal to the face of the main spindle unless modified through the Z axis work shift offset. Refer to Chapter 4 for information on the Z axis work shift offset. The E axis work shift will be used to set the distance from the sub-spindle collet face to Z0. Setting an E axis work shift will allow the programmer to program the sub-spindle position in relation to Z0. The E axis work shift is typically used for workpiece transfer between the main spindle and sub-spindle. Refer to the operator's manual (M-505) for information on setting the E axis work shift. E Axis Position Verification NOTICE G53 E#5025 MUST be commanded before E axis motion is commanded whenever the E axis drive has been turned OFF through the use of the M76 command and turned back ON through the use of the M77 or M78 command. The G53 E#5025 data block commands the control to verify the position of the E axis. Refer to the programming examples used in this chapter. X/U AXIS MOTION Programming incremental and absolute axis motion on the X axis during sub-spindle operation is the same as programming incremental and absolute axis motion on the X axis during main spindle operation M-504A

339 Z/W AXIS MOTION NOTICE Z Axis motion required to clear the workpiece during sub-spindle operation is in the opposite direction of that required to clear the workpiece during main spindle operation. The control assumes all numerical data to be positive (+) unless a minus (-) sign is programmed. When required, be sure the minus (-) sign is programmed. Main Spindle When the workpiece is in the main spindle, all Z axis tool motion away from the face of the workpiece is to the right of the workpiece. All incremental moves in this direction are positive (+) W moves. Assuming a work shift offset has set the face of the workpiece to Z0, all absolute coordinates on the Z axis to the right of the workpiece are positive (+). Therefore, to clear the workpiece on the Z axis, program either a positive (+) W or positive (+) Z move along with whatever X axis move that may be required. Refer to Figure Sub-Spindle NOTICE Refer to the sub-spindle / tool holder clearance requirement outlined on the next page before programming machining operations on the sub-spindle. When the workpiece is in the sub-spindle, all Z axis tool motion away from the face of the workpiece is to the left of the workpiece. All incremental moves in this direction are negative (-) W moves. Assuming a work shift offset has set the face of the workpiece to Z0, all absolute coordinates on the Z axis to the left of the workpiece are negative (-). Therefore, to clear the workpiece on the Z axis, program either a negative (-) W or negative (-) Z move along with whatever X axis move that may be required. Refer to Figure M-504A 14-3

340 SUB-SPINDLE / TOOL HOLDER CLEARANCE REQUIREMENT - NOTE - This clearance requirement exists on machines equipped with a Hardinge turret top plate and an optional sub-spindle. When drilling, boring, or tapping at the sub-spindle, the minimum clearance required between the round shank tool holder and the face of the sub-spindle is 1.25 inches [ 32 millimeters]. Refer to Figure Inches [Millimeters] Turret Top Plate Optional Sub-Spindle 1.25 [32.0] TI5755B Figure Minimum Tool Holder Clearance for Round Shank Tool Holders 14-4 M-504A

341 SUB-SPINDLE G CODES Most of the G codes are programmed in the same manner, regardless of whether the workpiece is in the main spindle or the sub-spindle. However, there are G codes that deserve extra attention to be sure the proper G code is used. The following G codes are discussed simply to eliminate possible questions. G02 / G03 CIRCULAR INTERPOLATION Circular Interpolation for sub-spindle programming is interpreted in the same manner as Circular Interpolation for main spindle programming. Refer to Figure G02 is a clockwise arc as viewed from above the tool and looking down toward the bed of the machine. G03 is a counterclockwise arc as viewed from above the tool and looking down toward the bed of the machine. Refer to Chapter 3 for information on Circular Interpolation. G41 / G42 TOOL NOSE RADIUS COMPENSATION Tool Nose Radius Compensation for sub-spindle programming is interpreted in the same manner as Tool Nose Radius Compensation for main spindle programming. Refer to Figure G41 activates Tool Nose Radius Compensation with the workpiece to the right of the tool. G42 activates Tool Nose Radius Compensation with the workpiece to the left of the tool. Refer to Chapter 2 for information on Tool Nose Radius Compensation. Tool Quadrant Q3 Tool Quadrant Q4 G42 G41 G03 G02 Main Spindle Z0 Sub-Spindle Z0 -Z Inside Part +Z Move to -Z Move to +Z Inside Part Clear Part Clear Part TI5770 Figure Programming Circular Interpolation and Tool Nose Radius Compensation M-504A 14-5

342 SUB-SPINDLE M CODES The following M codes are used only in conjunction with sub-spindle operation. M07 SUB-SPINDLE PHASE SYNCHRONIZATION WITH MAIN SPINDLE NOTICE Be sure the machine tool is equipped with matched collets when the use of the M07 command is required. - NOTE - M32 MUST be programmed in the block immediately preceding the M07 block. M07 commands the rotational direction, velocity, and orientation of the work-holding device of the sub-spindle to match the main spindle. This allows the transfer of non-symmetrical parts between the main spindle and the sub-spindle. M07 is programmed in a block by itself. Refer to Figures 14.3 and M07 is canceled by any standard spindle command on the main spindle or sub-spindle. M32 SUB-SPINDLE SYNCHRONIZATION WITH MAIN SPINDLE M32 commands the rotational direction and velocity of the sub-spindle to match the main spindle. This mode is only used for part transfer between the main spindle and the sub-spindle. M32 is canceled by any standard spindle command on the main spindle or sub-spindle. Spindle Command: M33 Sub-Spindle Forward TI5761 Spindle Command: M34 Sub-Spindle Reverse TI5762 Figure Sub-Spindle Forward Rotation Figure Sub-Spindle Reverse Rotation 14-6 M-504A

343 M33 SUB-SPINDLE FORWARD M33 commands the sub-spindle to rotate in the forward direction at the programmed spindle speed (S word). Inch per Minute or Inch per Revolution programming is allowed. The sub-spindle is rotating in the forward direction when rotating clockwise, as viewed from the sub-spindle end of the machine. M33 remains active until canceled by M00, M01, M30, M34, M35, or by pressing the Reset or Emergency Stop push button. Refer to Figure Refer to M03, in Chapter 1, for the main spindle forward command. M34 SUB-SPINDLE REVERSE M34 commands the sub-spindle to rotate in the reverse direction at the programmed spindle speed (S word). Inch per Minute or Inch per Revolution programming is allowed. The sub-spindle is rotating in the reverse direction when rotating counterclockwise, as viewed from the sub-spindle end of the machine. M34 remains active until canceled by M00, M01, M30, M33, M35, or by pressing the Reset or Emergency Stop push button. Refer to Figure Refer to M04, in Chapter 1, for the main spindle reverse command. M35 SUB-SPINDLE STOP M35 commands the sub-spindle to stop. M35 remains active until canceled by M07, M32, M33, or M34. M35 is active at machine start-up and can also be activated by M00, M01, M30, Reset, and Emergency Stop. Refer to M05, in Chapter 1, for the main spindle stop command. M46 SUB-SPINDLE AIR BLAST ON [Option] M46 activates the sub-spindle air blast. M47 SUB-SPINDLE AIR BLAST OFF [Option] M47 deactivates the sub-spindle air blast. M56 SUB-SPINDLE COLLET / CHUCK OPEN M56 commands the sub-spindle collet closer to open, releasing the workpiece. M56 remains active until canceled by M57. Refer to M21 for the corresponding command for the main spindle. M57 SUB-SPINDLE COLLET / CHUCK CLOSE M57 commands the sub-spindle collet closer to close, gripping the workpiece. M57 remains active until canceled by M56. Refer to M22 for the corresponding command for the main spindle. M62 ACTIVATE C AXIS SPINDLE SYNCHRONIZATION The M62 command activates C axis spindle synchronization between the main spindle and the sub-spindle. Refer to the sample programs beginning on page M63 CANCEL C AXIS SPINDLE SYNCHRONIZATION The M63 command cancels C axis spindle synchronization between the main spindle and the sub-spindle. Refer to the sample programs beginning on page M-504A 14-7

344 M68 EXTERNAL CHUCKING MODE M68 commands the control to use the sub-spindle collet closer with external gripping style work-holding devices. External chucking is activated through Manual Data Input mode. Refer to the operator s manual (M-505) for information on switching chucking modes. M69 INTERNAL CHUCKING MODE M69 commands the control to use the sub-spindle collet closer with internal gripping style work-holding devices. Internal chucking is activated through Manual Data Input mode. Refer to the operator s manual (M-505) for information on switching chucking modes. M76 SUB-SPINDLE DRIVE OFF The M76 command turns OFF the axis drive for the sub-spindle. M77 SUB-SPINDLE DRIVE LOW TORQUE The M77 command switches the axis drive for the sub-spindle to low torque mode. M78 SUB-SPINDLE DRIVE NORMAL TORQUE The M78 command switches the axis drive for the sub-spindle to normal torque mode. M215 THRU-SPINDLE COOLANT ON The M215 command causes the thru-spindle coolant at the sub-spindle to turn ON. M215 remains active until canceled by M216, M30, control Reset, or control OFF. M216 THRU-SPINDLE COOLANT OFF The M216 command causes the thru-spindle coolant at the sub-spindle to turn OFF. M216 remains active until canceled by M M-504A

345 SUB-SPINDLE WORK SHIFT NOTICE The work shift file contains an E, X, Y, and Z axis register. The X and Y axis registers should be set to zero at all times. The value entered into the Z axis work shift register MUST be a NEGATIVE number. The Z axis work shift MUST be modified whenever the workpiece is transferred between the main spindle and the sub-spindle. The Z axis work shift sets the face of the workpiece to Z0 (zero) and is programmed as a NEGATIVE number regardless of whether the workpiece is in the main spindle or sub-spindle. Refer to Figure 14.5 for a comparison of main spindle and sub-spindle work shifts. Program a G10 line at the beginning of each tool operation to be sure the proper work shift is active for that particular operation. Refer to Chapter 4 for additional information on work shift. Main Spindle Z Main Spindle Z Axis Work Shift Entry: G10 P0 Z ; Sub-Spindle Z Axis Work Shift Entry: G10 P0 Z ; Sub-Spindle Z TI5771 Figure Main Spindle and Sub-Spindle Work Shift Offset Comparison M-504A 14-9

346 TOOL OFFSETS Tool offsets are established and activated for sub-spindle operations in the same manner as they are for main spindle operations. Refer to Chapter 4 for additional information on tool offsets. TOOL GEOMETRY OFFSETS A point of concern when programming for sub-spindle operations is the tool nose orientation number. (Refer to Figure 14.2) Be sure the proper orientation codes are entered in the tool offset registers. Refer to Chapter 4 for information on entering tool geometry offsets into the control. TOOL WEAR OFFSETS Refer to Chapter 4 for information on entering tool wear offsets into the control. X Axis Tool Wear Offsets When the X axis tool wear offset is increased in value, the tool tip will be positioned further from the spindle centerline for a given X axis coordinate. As a result, the workpiece diameter will increase. When the X axis tool wear offset is decreased in value, the tool tip will be positioned closer to the spindle centerline for a given X axis coordinate. As a result, the workpiece diameter will decrease. Z Axis Tool Wear Offsets When the Z axis tool wear offset is increased in value, the tool tip will be positioned further from the face of the main spindle (closer to the face of the sub-spindle) for a given Z axis coordinate. As a result, the workpiece length will increase for main spindle operations and decrease for sub-spindle operations. When the Z axis tool wear offset is decreased in value, the tool tip will be positioned closer to the face of the main spindle (further from the face of the sub-spindle) for a given Z axis coordinate. As a result, the workpiece length will decrease for main spindle operations and increase for sub-spindle operations M-504A

347 SPINDLE SYNCHRONIZATION SAMPLE PROGRAMS SAMPLE PROGRAM USING STANDARD COLLETS OR PULL BACK SYSTEMS N10 (T1010-DRILL CROSS HOLE) G10 P0 Z#500 M66 M56 M98 P1 T1010 M23 M51 S3000 G97 P3 Sequence Number and Operator Message Set Main Spindle Work Shift, Spindle Feedback from Live Tool Spindle Sub-Spindle Collet/Chuck Open Call Safe Index Subprogram O1 Index to Tool Station, Select Offset, Activate Main Spindle Contouring Mode Live Tool Rotation Command, 3000RPM, Direct RPM, Select Spindle (P3 = Live Tool) X1.2 Z-3.5 Y0 C0 E-.5 Position Tool, Orient Main Spindle to 0 Degrees, Position Sub-Spindle over Workpiece M223 Activate Sub-Spindle Contouring Mode G0A0 Orient Sub-Spindle to 0 Degrees M77 Sub-Spindle Axis Drive to Low Torque Mode M57 Sub-Spindle Collet/Chuck Close M62 Activate C Axis Spindle Synchronization G87 X.5 F3.5 Execute G87 Side Drilling Cycle X.5 C90. Orient Spindles to 90 Degrees, Execute G87 Side Drilling Cycle X.5 C180. Orient Spindles to 180 Degrees, Execute G87 Side Drilling Cycle X.5 C270. Orient Spindles to 270 Degrees, Execute G87 Side Drilling Cycle G80 Cancel G87 Side Drilling Cycle M63 Cancel C Axis Spindle Synchronization M24 Cancel Main Spindle Contouring Mode M224 Cancel Sub-Spindle Contouring Mode M55 Live Tool Stop Command M56 Sub-Spindle Collet/Chuck Open M76 Sub-Spindle Axis Drive OFF M78 Sub-Spindle Axis Drive to Normal Torque Mode G53 E#5025 E Axis Position Verification G0 G53 E16.5 Rapid Sub-Spindle to Reference Position M98 P1 Call Safe Index Subprogram O1 M1 Optional Stop NOTICE Refer to page 14-2 for information regarding E Axis position verification. Verify subprogram O1 to be sure there are no E axis commands if the part will remain engaged for subsequent operations while gripped with both spindles. M-504A 14-11

348 SAMPLE PROGRAM USING DEAD LENGTH COLLETS OR CHUCKS N10 (T1010-DRILL CROSS HOLE) G10 P0 Z#500 M66 M56 M98 P1 T1010 M23 M51 S3000 G97 P3 Sequence Number and Operator Message Set Main Spindle Work Shift, Spindle Feedback from Live Tool Spindle Sub-Spindle Collet/Chuck Open Call Safe Index Subprogram O1 Index to Tool Station, Select Offset, Activate Main Spindle Contouring Mode Live Tool Rotation Command, 3000RPM, Direct RPM, Select Spindle (P3 = Live Tool) X1.2 Z-3.5 Y0 C0 E-.5 Position Tool, Orient Main Spindle to 0 Degrees, Position Sub-Spindle over Workpiece M223 Activate Sub-Spindle Contouring Mode G0 A0 Orient Sub-Spindle to 0 Degrees M57 Sub-Spindle Collet/Chuck Close M62 Activate C Axis Spindle Synchronization G87 X.5 F3.5 Execute G87 Side Drilling Cycle X.5 C90. Orient Spindles to 90 Degrees, Execute G87 Side Drilling Cycle X.5 C180. Orient Spindles to 180 Degrees, Execute G87 Side Drilling Cycle X.5 C270. Orient Spindles to 270 Degrees, Execute G87 Side Drilling Cycle G80 Cancel G87 Side Drilling Cycle M63 Cancel C Axis Spindle Synchronization M24 Cancel Main Spindle Contouring Mode M224 Cancel Sub-Spindle Contouring Mode M55 Live Tool Stop Command M56 Sub-Spindle Collet/Chuck Open G4 U0.5 ; Dwell.5 Seconds G0 G53 E16.5 Rapid Sub-Spindle to Reference Position M98 P1 Call Safe Index Subprogram O1 M1 Optional Stop NOTICE Verify subprogram O1 to be sure there are no E axis commands if the part will remain engaged for subsequent operations while gripped with both spindles M-504A

349 WORKPIECE TRANSFER The sample program segments in this section illustrate the recommended formats and sequence for programming workpiece transfer between the main spindle and the sub-spindle. There are three basic types of workpiece transfers: 1. Bar Job Transfer from Main Spindle to Sub-Spindle (Figures 14.8 through 14.10) 2. Slug Job Transfer from Main Spindle to Sub-Spindle (Figures through 14.13) 3. Slug Job Transfer from Sub-Spindle to Main Spindle (Figures through 14.16) Examples of each type of part transfer will be shown in the following sections. M-504A 14-13

350 TRANSFERRING FROM MAIN SPINDLE TO SUB-SPINDLE Bar Job Transfer from Main Spindle to Sub-Spindle NOTICE Refer to the spindle clearance requirements outlined below before programming a bar job transfer. SPINDLE CLEARANCE REQUIREMENTS Refer to Figures 14.6 and T-42 lathe: The tip of the cut-off tool MUST extend 3.94 inches [100 millimeters] from the edge of the turret top plate. T-51 and T-65 lathes: The tip of the cut-off tool MUST extend 4.33 inches [110 millimeters] from the edge of the turret top plate. 2. The face of the sub-spindle must be at least 1.80 inches [45.7 millimeters] from the face of the main spindle. Square Shank Cut-Off Tool Holder Required Turret Top Plate Turret Top Plate Square Shank Cut-Off Tool Holder Required 3.94 [100] 4.33 [110] Main Spindle Sub-Spindle Main Spindle Sub-Spindle 1.80 [45.7] 1.80 [45.7] Inches [Millimeters] Figure T-42 Lathe: Spindle Clearance Requirements TI5799 Inches [Millimeters] Figure T-51 and T-65 Lathes: Spindle Clearance Requirements TI M-504A

351 The following sample program segments illustrate the recommended format and sequence for programming bar job transfers from the main spindle to the sub-spindle. Refer to Figures 14.8 through DEAD LENGTH COLLET NOT INSTALLED IN SUB-SPINDLE COLLET N12 (CUT OFF & TRANSFER) ; Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S2000 M14 P1 ; Main Spindle 1000 RPM Reverse, Coolant ON, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 T1212 ; Index to Station 12 and Select Tool Offset 12 X1. Z-2.5 M32 ; Rapid to Start, Sub-Spindle Synchronization with Main Spindle (Figure 14.8) M7 ; Sub-Spindle Phase Synchronization with Main Spindle [Optional] G50 S4500 ; Establish Maximum RPM Limit G96 S700 ; Constant Surface Speed, 700 Surface Feet per Minute M56 ; Sub-Spindle Collet Open G0 E-1. ; Rapid Sub-Spindle to 1" over Part (Figure 14.9) M76 ; Sub-Spindle Drive OFF G4 U.2 ; Dwell.2 Seconds M57 ; Sub-Spindle Collet Close G4 U.2 ; Dwell.2 Seconds M78 ; Sub-Spindle Drive Normal Torque G1 G99 X-.02 F ; Feed Tool to X-.02 Diameter (Cut-off) G53 E#5025 ; E Axis Position Verification G4 U0.2 ; Dwell.2 Seconds G0 G53 E16.5 ; Rapid Sub-Spindle to Reference Position X1.1 ; Tool Rapid to Clear Workpiece (Figure 14.10) M98 P1 ; Call Safe Index Subprogram O1 M1 : Optional Stop M-504A 14-15

352 TI5763 Figure Tool Positioned for Cut-Off Operation TI5764 Figure Cut-Off Operation TI5765 Figure Sub-Spindle Moved to Reference Position M-504A

353 DEAD LENGTH COLLET INSTALLED IN SUB-SPINDLE COLLET N12 (CUT OFF & TRANSFER) ; Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S1000 M14 P1 ; Main Spindle 1000 RPM Reverse, Coolant ON, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 T1212 ; Index to Station 12 and Select Tool Offset 12 X1. Z2.5 M32 ; Position X and Z Axes, Sub-Spindle Synchronization with Main Spindle (Figure 14.8) M7 ; Sub-Spindle Phase Synchronization with Main Spindle [Optional] G50 S4500 ; Establish Maximum RPM Limit G96 S300 ; Constant Surface Speed, 300 Surface Feet per Minute M56 ; Sub-Spindle Collet Open G0 E-1. ; Rapid Sub-Spindle to 1" over Part (Figure 14.9) M77 ; Sub-Spindle Drive to Low Torque Mode G1 G98 E-1.05 F10. ; Feed Stock Stop against Workpiece G4 U.2 ; Dwell.2 seconds M57 ; Sub-Spindle Collet Close G4 U.2 ; Dwell.2 seconds M76 ; Sub-Spindle Drive OFF M78 ; Sub-Spindle Drive Normal Torque G1 G99 X-.02 F ; Feed Tool to X-.02 Diameter (Cut-off) G53 E#5025 ; E Axis Position Verification G4 U.2 ; Dwell.2 Seconds G0 G53 E16.5. ; Rapid Sub-Spindle to Reference Position X1.1 ; Tool Rapid to Clear Workpiece (Figure 14.10) M98 P1 ; Call Safe Index Subprogram O1 M1 : Optional Stop This format activates Sub-Spindle Drive Low Torque mode before the sub-spindle collet is closed. After the part has been transferred, program M76 and M78 to return the sub-spindle to Normal Torque mode BEFORE the rapid move to the E axis reference position. M-504A 14-17

354 Slug Job Transfer from Main Spindle to Sub-Spindle The following sample program segment illustrates the recommended format and sequence for programming slug job transfers from the main spindle to the sub-spindle. Refer to Figures through N84 (TRANSFER TO SUB) ; Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S2500 M14 P1 ; Main Spindle 2500 RPM Reverse, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 M32 ; Sub-Spindle Synchronization with Main Spindle M7 ; Sub-Spindle Phase Synchronization with Main Spindle [Optional] M56 ; Sub-Spindle Collet Open G0 E-1. ; Rapid Sub-Spindle to 1" over Part (Figure 14.12) M76 ; Sub-Spindle Drive OFF G4 U.2 ; Dwell.2 Seconds M57 ; Sub-Spindle Collet Close G4 U.2 ; Dwell.2 Seconds M21 ; Main Spindle Collet Open G4 U0.5 ; Dwell.5 Seconds M78 ; Sub-Spindle Drive Normal Torque G53 E#5025 ; E Axis Position Verification G0 G53 E16.5. ; Rapid Sub-Spindle to Reference Position (Figure 14.13) M1 ; Optional Stop M-504A

355 TI5766 Figure Workpiece Held in Main Spindle TI5767 Figure Workpiece Held in Both Spindles TI5768 Figure Workpiece Held in Sub-Spindle (Sub-Spindle Moved to Reference Position) M-504A 14-19

356 TRANSFERRING FROM SUB-SPINDLE TO MAIN SPINDLE The following sample program segments illustrate the proper format and sequence for programming transfers from the sub-spindle to the main spindle. Unlike main spindle to sub-spindle transfers, the only type of transfer which is used when transferring from the sub-spindle to the main spindle is slug job transfer. Refer to Figures through N84 (TRANSFER TO MAIN) ; Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G10 P0 E#501 ; Set Sub-Spindle Work Shift for Part Transfer G97 S2500 M14 P1 ; Main Spindle 2500 RPM Reverse, Select Spindle M98 P1 ; Call Safe Start Subprogram O1 M32 ; Sub-Spindle Synchronization with Main Spindle M7 ; Sub-Spindle Phase Synchronization with Main Spindle [Optional] M21 ; Main Spindle Collet Open M36 ; Main Spindle Air Blast ON G0 E-1. ; Rapid Part 1" into Main Spindle (Figure 14.15) M76 ; Sub-Spindle Drive OFF G4 U.2 ; Dwell.2 Seconds M22 ; Main Spindle Collet Close G4 U.2 ; Dwell.2 Seconds M37 ; Main Spindle Air Blast OFF M56 ; Sub-Spindle Collet Open M78 ; Sub-Spindle Drive Normal Torque G4 U0.5 ; Dwell.5 Seconds G53 E#5025 ; E Axis Position Verification G0 G53 E16.5. ; Rapid Sub-Spindle to Reference Position (Figure 14.16) M1 ; Optional Stop M-504A

357 TI5768 Figure Workpiece Held in Sub-Spindle (Sub-Spindle at Reference Position) TI5767 Figure Workpiece Held in Both Spindles TI5766 Figure Workpiece Held in Main Spindle (Sub-Spindle Moved to Reference Position) M-504A 14-21

358 SUB-SPINDLE SAMPLE PROGRAM The following sample program is written for a T-42 lathe. The workpiece will be machined from bar stock which is 1-7/16 inches in diameter. The workpiece will be machined on the main spindle first; then transferred to the sub-spindle to complete the machining operation. Refer to Figure BASIC SEQUENCE OF OPERATIONS Tool Station and Offset Main Spindle Work Shift Z Feed Bar Stock Rough Facing and Turning Operation Finish Facing and Turning Operation Workpiece Cut-off and Transfer T1010 T0101 T0202 T0404 Sub-Spindle Work Shift Z Finish Facing and Turning Operation Center Drill T0808 T0909 Drop Part Main Spindle Work Shift Sub-Spindle Work Shift Main Spindle Face Sub-Spindle Reference Position Sub-Spindle Face TI5769 Figure Sample Program Work Shift Values M-504A

359 SAMPLE PROGRAM % Stop Code O1112 ; Program Number N10 (Feed Stock) ; Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S100 M14 P1 ; Main Spindle Reverse 100 RPM, Coolant ON, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 T1010 ; Index to Station 10 and Select Tool Offset 10 X0. Z0.1 ; Rapid Tool to Start Point G1 Z-2. F100. ; Position Stock Stop M21 ; Main Spindle Open G4 U0.2 ; Dwell.2 Seconds Z0.02 F20. ; Move to Z.02 G4 U0.2 ; Dwell.2 Seconds M22 ; Main Spindle Close G4 U0.2 ; Dwell.2 Seconds M98 P2 ; Call Safe Index Subprogram O2 M1 ; Optional Stop N1 (Rough Face and Turn O.D.) Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S1000 M14 P1 ; Main Spindle Reverse 1000 RPM, Coolant ON, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 T0101 ; Index to Station 1 and Select Tool Offset 1 X1.5 Z0.005 ; Rapid Tool to Start Point G50 S5000 ; Constant Surface Speed 5000 RPM Limit G96 S750 ; Constant Surface Speed, 750 Surface Feet per Minute G1 G99 X-0.06 F0.005 ; Rough Face the Workpiece G98 X1.45 Z0.05 F100. ; Move to Clear the Workpiece G90 G99 X1.3 Z-1.19 F0.008 ; G90 Turning Cycle - Single Pass G1 G98 X1.025 F75. ; Position for Rough Turn G99 Z0.005 F0.007 ; Feed to Face of Workpiece X1.135 Z-0.05 ; Rough Turn the 45 Degree Angle,A0. ; Rough Turn the O.D. X1.26 Z-1.195,A20. ; Rough Turn the 20 Degree Angle X1.45 ; Feed to Clear the Workpiece M98 P1 ; Call Safe Index Subprogram O1 M1 ; Optional Stop M-504A 14-23

360 N2 (Finish R.015 Q3) Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S1000 M14 P1 ; Main Spindle Reverse 1000 RPM, Coolant ON, Select Spindle M98 P1 ; Call Safe Index Subprogram O1 T0202 ; Index to Station 2 and Select Tool Offset 2 X0. Z0.2 ; Rapid Tool to Start Point G50 S5000 ; Constant Surface Speed 5000 RPM Limit G96 S800 ; Constant Surface Speed, 800 Surface Feet per Minute G1 G42 X-0.03 Z0.1 F100. ; Move to Activate Tool Nose Radius Compensation G99 Z0. F0.003 ; Feed to Face of Workpiece X1.125,C0.05 ; Face and Chamfer Workpiece,A0 ; Finish Turn the O.D. X1.25 Z-1.2,A20. ; Finish Turn the 20 Degree Angle X1.49 ; Feed to Clear the Workpiece M98 P1 ; Call Safe Index Subprogram O1 M1 ; Optional Stop N4 (.125 Cut-off and Transfer) Sequence Number and Operator Message G10 P0 Z#500 ; Set Main Spindle Work Shift G97 S1000 M14 P1 ; Main Spindle Reverse 1000 RPM, Coolant ON M98 P1 ; Call Safe Index Subprogram O1 T0404 ; Index to Station 4 and Select Tool Offset 4 X1.5 Z M32 ; Rapid Tool to Start Point, Sub-Spindle Synchronization with Main Spindle M7 ; Sub-Spindle Phase Synchronization with Main Spindle [Optional] G50 S3000 ; Constant Surface Speed 3000 RPM Limit G96 S220 ; Constant Surface Speed, 220 Surface Feet per Minute M56 ; Sub-Spindle Collet Open G0 E-.5 ; Position Sub-Spindle to Grip Workpiece M76 ; Sub-Spindle Drive OFF G4 U.2 ; Dwell.2 Seconds M57 ; Sub-Spindle Collet Closed G4 U.2 ; Dwell.2 Seconds M78 ; Sub-Spindle Drive Normal Torque G1 G99 X-.02 F.002 ; Cut off Workpiece G4 U.2 ; Dwell.2 Seconds G53 E#5025 ; E Axis Position Verification G0 G53 E16.5. ; Sub-Spindle Rapid Traverse to Reference Position G0 X1.5 ; Rapid Tool Clear of Bar Stock M98 P1 ; Call Safe Index Subprogram O1 M1 ; Optional Stop M-504A

361 N08 (Finish R.015 Q4) Sequence Number and Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift G97 S1000 M33 P2 ; Sub-Spindle Forward 1000 RPM, Coolant ON M98 P2 ; Call Safe Index Subprogram O2 T0808 ; Index to Station 8 and Select Tool Offset 8 X1.51 Z-0.1 M8 ; Rapid Tool to Start Point, Coolant ON G50 S3000 ; Constant Surface Speed 3000 RPM Limit G96 S800 ; Constant Surface Speed, 800 Surface Feet per Minute G1 G42 X1.5 Z0. F100. ; Move to Activate Tool Nose Radius Compensation G99 X-0.03 F0.004 ; Finish Face the Workpiece G41 ; Tool Nose Radius Compensation Axis Reversal X1.2 ; Feed to Arc Start G2 X1.4 Z0.1 R0.1 F0.002 ; Cut Radius G1 Z0.85 F0.004 ; Finish Turn the O.D. X1.49 ; Feed to Clear the Workpiece M98 P2 ; Call Safe Index Subprogram O2 M1 ; Optional Stop N09 (#4 Center Drill) Sequence Number and Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift G97 S1000 M33 P2 ; Sub-Spindle Forward 1000 RPM M98 P2 ; Call Safe Index Subprogram O2 T0909 ; Index to Station 9 and Select Tool Offset 9 X0. Z-0.1 S1600 M8 ; Rapid Tool to Start Point, Spindle and Coolant ON G1 G99 Z0.28 F.009 ; Drill to Depth Z-.25 ; Feed to Clear the Workpiece M98 P2 ; Call Safe Index Subprogram O2 M1 ; Optional Stop N026 (Drop Workpiece) Sequence Number and Operator Message G10 P0 Z#501 ; Set Sub-Spindle Work Shift M35 ; Sub-Spindle Stop M98 P2 ; Call Safe Index Subprogram O2 M26 ; Extend Part Catcher M56 ; Sub-Spindle Open G4 U0.5 ; Dwell.5 Seconds M25 ; Retract Part Catcher M1 ; Optional Stop M30 ; End of Program % Stop Code M-504A 14-25

362 SUB-SPINDLE PROGRAMMING NOTES 1. Cycle Start is inhibited when the main spindle and sub-spindle work-holding devices are both open. 2. When operating the spindles in sync mode, DO NOT reverse spindle directions. 3. When it is necessary to program M07 (Sub-Spindle Phase Synchronization with Main Spindle), M32 MUST be programmed in the block immediately preceding the M07 block. 4. For safety, the Work Shift Offset is programmed after each Operation Sequence number. 5. Be sure to call the correct Safe Index subprogram for the spindle being used. Refer to Safe Index Subprograms, page Enter a 0 (zero) at the beginning of each sub-spindle operation sequence number to distinguish sub-spindle operation sequence numbers from main spindle sequence numbers. 7. When the operator is running a bar job, the Repeat Mode push button will be activated. When an M30 command is read by the control, the program rewinds back to the beginning. If Repeat Mode is active when the program rewinds, the program will begin executing again. 8. When using a bar feed and a new piece of bar stock is loaded in the bar feed, the face of the bar stock should be flush with the face of the collet in the main spindle since the part program begins with a feed stock operation M-504A

363 - NOTES - M-504A 14-27

364 - NOTES M-504A

365 CHAPTER 15 - BASIC Y AXIS PROGRAMMING INTRODUCTION The purpose of this chapter is to illustrate basic Y axis machining concepts. Y axis machining requires the use of live tooling attachments. Live tooling is a standard feature on T-42, T-51, and T-65 lathes equipped with a BMT top plate. The live tooling attachments are not included with the machine tool and must be purchased separately. The Y axis option allows programming of the live tools in a plane that is perpendicular to the bed of the machine. Refer to Appendix One for Y axis travel specifications. Y0 (zero) is designated as part centerline. This feature will allow machining of flats, pockets, and drilling of holes off the spindle centerline. The spindle may be oriented with the C axis as outlined in Chapter 11. In addition, all canned cycles for drilling and rigid tapping are available. NOTICE Live tooling attachments are available with or without through-tool coolant capability. Live tooling attachments without through-tool coolant capability can be run with or without coolant, as the machining process requires. Live tooling attachments with through-tool coolant capability MUST be run with coolant turned ON. M-504A 15-1

366 MAIN SPINDLE OPERATION Y AXIS PROGRAMMING FORMATS - NOTE - Bold text indicates items programmed as required. N ( ) Sequence Search Number and Message G10 P0 Z#500 Set Main Spindle Work Shift M98 P1 Call Safe Index Subprogram #1 T M23 Index to Tool Station and Call Offset C Axis Commands to Main Spindle (G17 or G19) X Z Y C Set Plane, Position Axis, Orient Main Spindle M(51, 52, 53, or 54) S G97 P3 Live Tool Direction, Spindle RPM, Direct RPM, Select Spindle (P3 = Live Tool Spindle) G1 G99 X Z Y F Machine Part G0 X Z Y Clear Part by 3 Times the Tool Tip Diameter C Orient Main Spindle as Required G1 G99 X Z Y F Machine Part G0 G18 X Z Y Set X-Z Plane, Clear Part by 3 Times the Tool Tip Diameter M55 Stop Live Tool Spindle M24 Cancel C Axis M98 P1 Call Safe Index Subprogram #1 M01 Optional Stop 15-2 M-504A

367 SUB-SPINDLE OPERATION - NOTE - Bold text indicates items programmed as required. N ( ) Sequence Search Number and Message G10 P0 Z#501 Set Sub-Spindle Work Shift M98 P2 Call Safe Index Subprogram #2 T M223 Index to Tool Station and Call Offset C Axis Commands to Sub-Spindle (G17 or G19) X Z Y A Set Plane, Position Axis, Orient Sub-Spindle M(51, 52, 53, or 54) S G97 P3 Live Tool Direction, Spindle RPM, Direct RPM, Select Spindle (P3 = Live Tool Spindle) G1 G99 X Z Y F Machine Part G0 X Z Y Clear Part by 3 Times the Tool Tip Diameter A Orient Sub-Spindle as Required G1 G99 X Z Y F Machine Part G0 G18 X Z Y Set X-Z Plane, Clear Part by 3 Times the Tool Tip Diameter M55 Stop Live Tool Spindle M224 Cancel C Axis M98 P2 Call Safe Index Subprogram #2 M01 Optional Stop M-504A 15-3

368 MACHINING ON THE DIAMETER OF THE WORKPIECE SAMPLE PROGRAM 1 - DRILLING OFFSET HOLES Figure 15.1 and its accompanying program illustrate an elementary part in the main spindle that is to be cross drilled parallel with the X axis. The drilled holes will be offset from the spindle centerline by.375 inches. Sample Program O1234 ; N2 (Operator Message) ; G10 P0 Z#500 M98 P1 ; T0202 ; G0 X1.825 Z-.875 Y.375 B0. ; G97 S2500 M53 P3 ; G87 G98 X.941 F7.5 ; Z ; Y-.375 ; Z-.875 ; G80 ; M55 ; M98 P1 ; M01 ; M30 ; Program Number Sequence Number and Operator Message Set Main Spindle Work Shift Safe Index Subprogram O1 Index and Call Tool Offset Rapid Move to Start Point, Orient Spindle to 0 Degrees Live Tool 2500 RPM Forward, Coolant ON, Select Spindle Initiate X Axis Drilling Cycle, Drill First Hole Drill Second Hole Drill Third Hole Drill Fourth Hole Cancel Drilling Cycle Live Tool Stop Safe Index Subprogram O1 Optional Stop End of Program 15-4 M-504A

369 NOTE: All dimensions shown in inches Z Y +X Viewed from the Back of the Machine TI4834 Figure Drilling Offset Holes on the Workpiece Diameter M-504A 15-5

370 SAMPLE PROGRAM 2 - MILLING A SLOT Figure 15.2 and its accompanying program illustrates an elementary part in the main spindle that is to be cross milled as shown. G Codes G00 - Positioning Mode G01 - Linear Interpolation G02 - Circular Interpolation, Clockwise Arc G03 - Circular Interpolation, Counterclockwise Arc G18 - X,Z Work Plane G19 - Z,C Work Plane G40 - Cancel Tool Nose Radius Compensation G41 - Tool Nose Radius Compensation, Workpiece Right of Tool G42 - Tool Nose Radius Compensation, Workpiece Left of Tool Sample Program O2420 ; N4 (Operator Message) ; G10 P0 Z#500 M98 P1 ; T0404 ; G0 G19 X2.1 Z-.65 Y0. B0. ; G97 S1500 M53 P3 ; G42 Z-.4 ; G1 G98 X1.8 F10. ; G2 Y Z R ; G1 Z ; G2 Y R ; G1 Z ; G2 Y0. Z-.4 R ; G1 G40 Z-.625 ; G0 G18 X2.1 ; M55 ; M98 P1 ; M01 ; M30 ; Program Number Sequence Number and Operator Message Set Main Spindle Work Shift Safe Index Subprogram O1 Index and Call Tool Offset Rapid Move to Start Point, ZC Work Plane Selection, Orient Spindle to 0 Degrees Live Tool 1500 RPM Forward, Coolant ON, Select Spindle Activate Tool Nose Radius Compensation Feed Tool to Depth Cutting Move Cutting Move Cutting Move Cutting Move Cutting Move Cancel Tool Nose Radius Compensation Rapid Move to Clear Workpiece, XZ Work Plane Selection Live Tool Stop Safe Index Subprogram O1 Optional Stop End of Program 15-6 M-504A

371 NOTE: All dimensions shown in inches. Viewed from the Back of the Machine +Y +X Z0 2 Coordinate Locations: Tool Path 1: Y0. Z-.4 2: Y Z : Z Y : Y : Z Y TI4835 Figure Milling a Slot on the Workpiece Diameter M-504A 15-7

372 MACHINING THE END OF THE WORKPIECE Y axis machining on the end of the workpiece requires the use of end-working live tooling attachments. SAMPLE PROGRAM 3 - DRILLING OFFSET HOLES Figure 15.3 and its accompanying program illustrates an elementary part in the main spindle that is to be face drilled as shown. Sample Program O3110 ; Program Number N5 (Operator Message) ; Sequence Number and Operator Message G10 P0 Z#500 Set Main Spindle Work Shift M98 P1 ; Safe Index Subprogram O1 T0505 ; Index and Call Tool Offset G0 X1. Y.5 Z.1 B0. ; Rapid Move to Start Point, Orient Spindle to 0 Degrees G97 S2500 M54 P3 ; Live Tool 2500 RPM Forward, Coolant ON G83 G99 Z-.25 F.003 ; Initiate Z Axis Drilling Cycle, Drill First Hole X2. ; Drill Second Hole Y1. ; Drill Third Hole X1. ; Drill Fourth Hole G80 ; Cancel Drilling Cycle M55 ; Live Tool Stop M98 P1 ; Safe Index Subprogram O1 M01 ; Optional Stop M30 ; End of Program 15-8 M-504A

373 NOTE: All dimensions shown in inches X0.500 Viewed from the Tailstock or Sub-Spindle End of the Machine +Y +X Y0.500 TI4836 Figure Drilling Offset Holes on the Face of the Workpiece M-504A 15-9

374 SAMPLE PROGRAM 4 - MILLING A POCKET Figure 15.4 and its accompanying program illustrates an elementary part in the main spindle that is to be face milled as shown. G Codes G00 - Positioning Mode G01 - Linear Interpolation G02 - Circular Interpolation, Clockwise Arc G03 - Circular Interpolation, Counterclockwise Arc G17 - X,C Work Plane G18 - X,Z Work Plane G40 - Cancel Tool Nose Radius Compensation G41 - Tool Nose Radius Compensation, Workpiece Right of Tool G42 - Tool Nose Radius Compensation, Workpiece Left of Tool Sample Program O1440 ; N3 (Operator Message) ; G10 P0 Z#500 M98 P1 ; T0303 ; G0 G17 X1.5 Y-1. Z.1 B0. ; G97 S1500 M54 P3 ; G1 G99 Z-.15 F.005 ; G41 Y ; Program Number Sequence Number and Operator Message Set Main Spindle Work Shift Safe Index Subprogram O1 Index and Call Tool Offset Rapid Move to Start Point, XC Work Plane Selection, Orient Spindle to 0 Degrees Live Tool 1500 RPM Forward, Coolant ON, Select Spindle Feed Tool to Depth Activate Tool Nose Radius Compensation G3 J ; Move Tool 360 G1 G40 Y-1. ; Cancel Tool Nose Radius Compensation G0 G18 Z.1 ; Rapid Move to Clear Workpiece, XZ Work Plane Selection M55 ; Live Tool Stop M98 P1 ; Safe Index Subprogram O1 M01 ; Optional Stop M30 ; End of Program M-504A

375 X0 +Y +X Y Start and End Point Tool Path TI4837 Figure Milling a Pocket on the Face of the Workpiece M-504A 15-11

376 - NOTES M-504A

377 APPENDIX ONE Z0 +Z Software Limit [ ] 16C Spindle [ ] 20C Spindle [ ] Z Axis Reference Position +X [12.700] -Z Software Limit +Z 5.00 [127.0] Turret Top Plate Main Spindle Headwall X and Z Axis Reference Position Main Spindle [96.418] -X Software Limit [ ] XAxis Reference Position [ ] +X Software Limit C L NOTES: 1. Turret shown without tool station covers. 2. All dimensions are shown in inches [millimeters]. 3. All X axis travel specifications are diameter values measured from the spindle centerline. 4. All Z axis travel specifications are measured from the face of the main spindle. 5. Full programmable travel on the X axis is [323.60], measured on the diameter. 6. Full programmable travel on the Z axis is: [406.53] 16C Spindle [382.40] 20C Spindle TI5670A Figure A1.1 - Turret Travel Specifications: X and Z Axes (T-42 Lathe Equipped with BMT 45 Turret Top Plate) M-504A A1-1

378 Z0 +Z Software Limit [ ] 16C Spindle [ ] 16C Spindle [ ] Z Axis Reference Position [12.700] -Z Software Limit +X 5.00 [127.0] Turret Top Plate +Z Main Spindle Headwall Main Spindle [54.762] -X Software Limit [ ] XAxis Reference Position [ ] +X Software Limit C L NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All X axis travel specifications are diameter values measured from the spindle centerline. 3. All Z axis travel specifications are measured from the face of the main spindle. 4. Full programmable travel on the X axis is [323.60], measured on the diameter. 5. Full programmable travel on the Z axis is: [364.87] 16C Spindle [340.74] 20C Spindle TI5718A Figure A1.2 - Turret Travel Specifications: X and Z Axes (T-42 Lathe Equipped with Hardinge Turret Top Plate) A1-2 M-504A

379 Z [ ] +Z Software Limit [ ] Z Axis Reference Position +X [12.700] -Z Software Limit 5.00 [127.0] Turret Top Plate +Z Main Spindle Headwall X and Z Axis Reference Position Main Spindle [114.3] -X Software Limit [ ] XAxis Reference Position [ ] +X Software Limit C L NOTES: 1. Turret shown without tool station covers. 2. All dimensions are shown in inches [millimeters]. 3. All X axis travel specifications are diameter values measured from the spindle centerline. 4. All Z axis travel specifications are measured from the face of the main spindle. 5. Full programmable travel on the X axis is [394.21], measured on the diameter. 6. Full programmable travel on the Z axis is [635.00]. TI5802 Figure A1.3 - Turret Travel Specifications: X and Z Axes (T-51 and T-65 Lathes Equipped with BMT 55 Turret Top Plate) M-504A A1-3

380 Z [ ] +Z Software Limit [ ] Z Axis Reference Position +X [12.700] -Z Software Limit +Z Main Spindle Headwall 5.00 [127.0] Turret Top Plate Main Spindle [57.150] -X Software Limit [ ] XAxis Reference Position [ ] +X Software Limit C L NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All X axis travel specifications are diameter values measured from the spindle centerline. 3. All Z axis travel specifications are measured from the face of the main spindle. 4. Full programmable travel on the X axis is [ ], measured on the diameter. 5. Full programmable travel on the Z axis is [ ]. TI5832 Figure A1.4 - Turret Travel Specifications: X and Z Axes (T-51 and T-65 Lathes Equipped with Hardinge Turret Top Plate) A1-4 M-504A

381 NOTE: All dimensions are shown in inches [millimeters] [57.18] +Y +X -X [390.00] -Y [161.80] [25.43] [48.21] Spindle Centerline Waycover [122.48] [342.90] TI5721 Figure A1.5 - Turret Travel Specifications: Y Axis Option (T-42 Lathe Equipped with a BMT 45 Turret Top Plate, Viewed from the Tailstock/Sub-Spindle End of the Machine) M-504A A1-5

382 NOTE: All dimensions are shown in inches [millimeters] [63.50] +Y +X [400.00] -Y -X 7.76 [197.10] [25.40] [57.15] Spindle Centerline [376.22] Waycover [150.83] TI5830 Figure A1.6 - Turret Travel Specifications: Y Axis Option (T-51 and T-65 Lathes Equipped with a BMT 55 Turret Top Plate, Viewed from the Tailstock/Sub-Spindle End of the Machine) A1-6 M-504A

383 +X Z [ ] 16C Spindle [ ] 20C Spindle +E Software Limit [ ] 16C Spindle [ ] 20C Spindle E Axis Reference Position +Z Main Spindle [83.82] -E Software Limit Dependent on Tailstock Center Used Tailstock C L NOTE: All dimensions are shown in inches [millimeters]. TI5722A Figure A1.7 - Tailstock Travel Specifications (T-42 Lathe) +X [ ] +E Software Limit +Z Main Spindle [ ] E Axis Reference Position [ ] -E Software Limit Dependent on Tailstock Center Used Tailstock C L NOTE: All dimensions are shown in inches [millimeters]. TI5853A Figure A1.8 - Tailstock Travel Specifications (T-51 and T-65 Lathes) M-504A A1-7

384 +X +Z Z0 +E Software Limit [ ] 16C Spindle [ ] 20C Spindle E Axis Reference Position [ ] 16C Spindle [ ] 20C Spindle [12.700] -E Software Limit Main Spindle Sub-Spindle C L NOTE: All dimensions are shown in inches [millimeters]. TI5723A Figure A1.9 - Sub-Spindle Travel Specifications (T-42 Lathe) +X Z [ ] +E Software Limit +Z Main Spindle [ ] E Axis Reference Position [15.875] -E Software Limit Sub-Spindle C L NOTE: All dimensions are shown in inches [millimeters]. TI5831 Figure A Sub-Spindle Travel Specifications (T-51 and T-65 Lathes) A1-8 M-504A

385 [406.53] 16C Spindle [382.40] 20C Spindle (Z Axis Travel) [12.70] [161.80] (X Axis Travel) Dependent on Tailstock Center Used [83.82] C L [48.21] Main Spindle NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The tailstock is shown at the Reference position [490.22] 16C Spindle [466.09] 20C Spindle (Reference) Tailstock TI5737 Figure A Work Envelope: T-42 Lathe Equipped with Tailstock and BMT 45 Turret Top Plate M-504A A1-9

386 [364.87] 16C Spindle [340.74] 20C Spindle (Z Axis Travel) [12.70] [161.80] (X Axis Travel) Dependent on Tailstock Center Used [125.48] C L [27.38] Main Spindle NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The tailstock is shown at the Reference position [490.22] 16C Spindle [466.09] 20C Spindle (Reference) Tailstock TI5748 Figure A Work Envelope: T-42 Lathe Equipped with Tailstock and Hardinge Turret Top Plate A1-10 M-504A

387 [406.53] 16C Spindle [382.40] 20C Spindle (Z Axis Travel) [12.70] [161.80] (X Axis Travel) Potential Interference C L [48.21] Main Spindle [419.10] 16C Spindle [394.97] 20C Spindle (Reference) NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The sub-spindle is shown at the Reference position. Sub-Spindle TI5736A Figure A Work Envelope: T-42 Lathe Equipped with Sub-Spindle and BMT 45 Turret Top Plate M-504A A1-11

388 [364.87] 16C Spindle [340.74] 20C Spindle (Z Axis Travel) [12.70] [161.80] (X Axis Travel) [41.53] 16C [65.66] 20C C L [27.38] Potential Interference Main Spindle [419.10] 16C Spindle [394.97] 20C Spindle (Reference) Sub-Spindle NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The sub-spindle is shown at the Reference position. TI5749B Figure A Work Envelope: T-42 Lathe Equipped with Sub-Spindle and Hardinge Turret Top Plate A1-12 M-504A

389 [635.00] (Z Axis Travel) [12.70] [ ] (X Axis Travel) Dependent on Tailstock Center Used [98.30] C L [57.15] [746.00] (Reference) NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The tailstock is shown at the Reference position. TI5854A Figure A Work Envelope: T-51 and T-65 Lathes Equipped with Tailstock and BMT 55 Turret Top Plate M-504A A1-13

390 [593.34] (Z Axis Travel) [12.70] [ ] (X Axis Travel) Dependent on Tailstock Center Used [139.95] C L [28.58] [746.00] (Reference) NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The tailstock is shown at the Reference position. TI5855A Figure A Work Envelope: T-51 and T-65 Lathes Equipped with Tailstock and Hardinge Turret Top Plate A1-14 M-504A

391 [635.00] (Z Axis Travel) [12.70] [ ] (X Axis Travel) [8.78] Potential Interference C L [57.15] Main Spindle [650.88] (Reference) Sub-Spindle NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The sub-spindle is shown at the Reference position. TI5833 Figure A Work Envelope: T-51 and T-65 Lathes Equipped with Sub-Spindle and BMT 55 Turret Top Plate M-504A A1-15

392 [593.34] (Z Axis Travel) [12.70] [ ] (X Axis Travel) [44.83] C L [28.58] Potential Interference Main Spindle [650.88] (Reference) Sub-Spindle NOTES: 1. All dimensions are shown in inches [millimeters]. 2. All measurements for X are radius values. 3. The turret is shown at the +X and +Z software limits. 4. The sub-spindle is shown at the Reference position. TI5834 Figure A Work Envelope: T-51 and T-65 Lathes Equipped with Sub-Spindle and Hardinge Turret Top Plate A1-16 M-504A

393 25.00 [635.0] Diameter (Turret at Maximum -Y Travel) [685.8] Diameter (Turret at Y0 or above) [147.8] Radial Distance to Waycover 4.82 [122.4] Radial Distance to Waycover NOTE: All dimensions are shown in inches [millimeters]. TI5703 Figure A Turret Top Plate Distance to Waycover: T-42 Lathe Equipped with a BMT 45 Turret Top Plate M-504A A1-17

394 [685.8] Diameter [127.0] Radial Distance to Waycover NOTE: All dimensions are shown in inches [millimeters]. TI5704 Figure A Turret Top Plate Distance to Waycover: T-42 Lathe Equipped with a Hardinge Turret Top Plate A1-18 M-504A

395 27.62 [701.5] Diameter (Turret at Maximum -Y Travel) [752.3] Diameter (Turret at Y0 or above) 6.94 [176.2] Radial Distance to Waycover 5.94 [150.8] Radial Distance to Waycover NOTE: All dimensions are shown in inches [millimeters]. TI5835 Figure A Turret Top Plate Distance to Waycover: T-51 and T-65 Lathes Equipped with a BMT 55 Turret Top Plate M-504A A1-19

396 29.62 [752.3] Diameter 5.81 [147.6] Radial Distance to Waycover NOTE: All dimensions are shown in inches [millimeters]. TI5836 Figure A Turret Top Plate Distance to Waycover: T-51 and T-65 Lathes Equipped with a Hardinge Turret Top Plate A1-20 M-504A

397 2.45 [62.2] 1.22 [31.0] Ø8.02 [203.7] Ø7.05 [179.0] Ø6.74 [171.2] Ø25.00 [635.0] Ø7.52 [191.0] Ø7.20 [182.9] Ø7.48 [190.0] Ø8.27 [210.0] Ø6.74 [171.2] Ø7.05 [179.0] NOTE: All dimensions are shown in inches [millimeters]. TI5725 Figure A Sample Tooling Layout: T-42 Lathe Equipped with a BMT 45 Turret Top Plate with Static and Live Tooling M-504A A1-21

398 Ø9.276 [Ø235.61] Ø8.788 [Ø223.21] Centerline at [31.75] [22.19] Ø8.576 [Ø217.84] Ø9.276 [Ø235.61] Ø9.276 [Ø235.61] Ø9.199 [Ø233.65] Centerline at [50.8] [31.75] Ø9.128 [Ø231.86] [31.75] Ø8.920 [Ø226.56] Ø9.276 [Ø235.61] Ø9.276 [Ø235.61] NOTE: All dimensions are shown in inches [millimeters]. TI5750 Figure A Sample Tooling Layout: T-42 Lathe Equipped with a Hardinge Turret Top Plate A1-22 M-504A

399 Ø [Ø258.33] Ø [Ø295.74] Ø [Ø258.33] Ø [Ø701.55] Ø [Ø752.35] Ø [Ø272.20] Ø [Ø265.83] [38.10] Ø9.410 [Ø239.00] Ø [Ø260.95] Ø [Ø271.92] Ø9.734 [Ø247.26] NOTE: All dimensions are shown in inches [millimeters]. TI5846 Figure A Sample Tooling Layout: T-51 and T-65 Lathes Equipped with a BMT 55 Turret Top Plate with Static and Live Tooling M-504A A1-23

400 Ø9.314 [Ø236.59] Ø [Ø260.87] Ø [Ø260.90] Ø9.314 [Ø236.59] Centerline at [71.44] Centerline at [38.10] Ø [Ø260.79] [28.57] Ø [Ø260.87] Ø9.344 [Ø237.33] Ø [Ø261.14] Ø [Ø261.12] Ø [Ø260.83] Ø9.312 [Ø236.53] Ø [Ø260.83] [38.10] Ø [Ø260.79] Ø [Ø260.87] NOTE: All dimensions are shown in inches [millimeters]. TI5845 Figure A Sample Tooling Layout: T-51 and T-65 Lathes Equipped with a Hardinge Turret Top Plate A1-24 M-504A

401 20 [14.9] Maximum Torque 108 [146.4] 120 [162.7] 15 [11.2] Maximum Power 15.5 [11.6] 90 [122.0] Power hp [Kw] 10 [7.5] 60 [81.3] Torque lb-ft [Nm] 5 [3.7] Base Speed [40.7] Motor Speed (RPM) TI5744B Figure A Main Spindle Power and Torque Curves (T-42 and T-42 Big-Bore Lathes) M-504A A1-25

402 25 [18.7] 300 [406.7] Maximum Torque 256 [347.1] 20 [14.9] Maximum Power 20.5 [15.3] 240 [325.4] 15 [11.2] 180 [244.0] Power hp [Kw] Torque lb-ft [Nm] 10 [7.5] 120 [162.7] 5 [3.7] Base Speed [81.3] Motor Speed (RPM) TI5824A Figure A Main Spindle Power and Torque Curves (T-51 Lathe) A1-26 M-504A

403 40 [29.8] 400 [542.3] 35 [26.1] 30 [22.4] Maximum Power 35 [26.1] Maximum Torque 311 [421.7] 350 [474.5] 300 [406.7] 25 [18.7] 250 [339.0] Power hp [Kw] 20 [14.9] 200 [271.1] Torque lb-ft [Nm] 15 [11.2] 150 [203.4] 10 [7.5] 5 [3.7] 0 0 Base Speed [135.6] 50 [67.8] 0 Motor Speed (RPM) TI5826A Figure A Main Spindle Power and Torque Curves (T-65 Lathe) M-504A A1-27

404 20 [14.9] Maximum Torque 108 [146.4] 120 [162.7] 15 [11.2] Maximum Power 15.5 [11.6] 90 [122.0] Power hp [Kw] 10 [7.5] 60 [81.3] Torque lb-ft [Nm] 5 [3.7] Base Speed [40.7] Motor Speed (RPM) NOTE: Maximum 5000 RPM on T-51 and T-65 lathes. TI5744B Figure A Sub-Spindle Power and Torque Curves (All Models) A1-28 M-504A

405 kW 30 Minute, S3 60% Operating Zone Output (kw) 4 3.7kW 3.7kW Continuous Operating Zone 2.5kW Motor Speed (RPM) TI5746A Figure A Live Tooling Power Curves (T-42 Lathe, BMT 45 Turret Top Plate) Torque (N m) Minute, S3 60% Operating Zone Continuous Operating Zone Motor Speed (RPM) TI5747A Figure A Live Tooling Torque Curves (T-42 Lathe, BMT 45 Turret Top Plate) M-504A A1-29

406 kW Output (kw) kW 30 Minute, S3 60% Operating Zone Continuous Operating Zone Motor Speed (RPM) Figure A Live Tooling Power Curves (T-51 and T-65 Lathes, BMT 55 Turret Top Plate) TI Torque (N m) Minute, S3 60% Operating Zone Continuous Operating Zone Motor Speed (RPM) Figure A Live Tooling Torque Curves (T-51 and T-65 Lathes, BMT 55 Turret Top Plate) TI5829 A1-30 M-504A

407 - NOTES - M-504A A1-31

408 - NOTES - A1-32 M-504A

409 APPENDIX TWO G CODES G Code Group Definition G00 1 Rapid Traverse Positioning Mode G01 1 Linear Interpolation G02 1 Clockwise Circular Interpolation G03 1 Counterclockwise Circular Interpolation G04 0 Dwell G10 0 Offset Value Setting G17 16 X,C Work Plane Selection G18 16 X,Z Work Plane Selection G19 16 Z,C Work Plane Selection G20 6 Inch Data Input G21 6 Metric Data Input G22 9 Stored Stroke Limits ON G23 9 Stored Stroke Limits OFF G28 0 Return to Reference Position G31 0 Skip Function G32 1 Threadcutting Routine (Constant Lead) G34 1 Threadcutting Routine (Variable Lead) G40 7 Cancel Tool Nose Radius Compensation G41 7 Tool Nose Radius Compensation (Part Right) G42 7 Tool Nose Radius Compensation (Part Left) G50 0 Maximum RPM Limit for Constant Surface Speed G65 0 User Macro Call G70 0 Automatic Finishing Cycle G71 0 Automatic Rough Turning Cycle G72 0 Automatic Rough Facing Cycle M-504A A2-1

410 G Code Group Definition G73 0 Automatic Rough Pattern Repeat Cycle G74 0 Automatic Drilling Cycle G76 0 Automatic Threading Cycle G80 10 Cancel G80 Series Cycle G83 10 Z Axis Drilling Cycle G84 10 Z Axis Tapping Cycle G85 10 Z Axis Boring Cycle G87 10 X Axis Drilling Cycle G88 10 X Axis Tapping Cycle G89 10 X Axis Boring Cycle G90 1 Canned Turning Cycle G92 1 Canned Threading Cycle G94 1 Canned Facing Cycle G96 2 Constant Surface Speed G97 2 Direct RPM Programming G98 5 Inches/mm per Minute Feedrate G99 5 Inches/mm per Revolution Feedrate G107 0 Activate Cylindrical Interpolation G Activate Polar Interpolation G Cancel Polar Interpolation A2-2 M-504A

411 M CODES M Code Definition Standard / Option M00 Program Stop Standard M01 Option Stop Standard M03 Main Spindle Forward Rotation Standard M04 Main Spindle Reverse Rotation Standard M05 Main Spindle Stop / Coolant OFF Standard M07 Spindle Phase Synchronization Option M08 Coolant ON Standard M09 Coolant OFF Standard M10 High Pressure Coolant ON Option M11 High Pressure Coolant OFF Option M12 Turret Coolant OFF Option M13 Main Spindle Forward Rotation / Coolant ON Standard M14 Main Spindle Reverse Rotation / Coolant ON Standard M15 Thru-Spindle Coolant ON, Main Spindle Option M16 Thru-Spindle Coolant OFF, Main Spindle Option M20 Speed Arrival Check ON Standard M21 Main Spindle Collet / Chuck Open Standard M22 Main Spindle Collet / Chuck Close Standard M23 Main Spindle Contouring Mode ON Standard M24 Main Spindle Contouring Mode OFF Standard M25 Main Spindle Part Catcher Retract Option M26 Main Spindle Part Catcher Extend Option M27 Main Spindle Internal Chucking Mode Standard M28 Main Spindle External Chucking Mode Standard M29 Rigid Tapping Mode Standard M30 Program End, Optional Auto Door Open Standard M32 Spindle Synchronization Option M-504A A2-3

412 M Code Definition Standard / Option M33 Sub-Spindle Forward Rotation Option M34 Sub-Spindle Reverse Rotation Option M35 Sub-Spindle Stop Option M36 Main Spindle Air Blast ON Option M37 Main Spindle Air Blast OFF Option M38 Auto Door Open Option M42 No Corner Rounding - Exact Stop Standard M43 Corner Rounding Standard M44 Enable Turret Bi-Directional Index Standard M45 Disable Turret Bi-Directional Index Standard M46 Sub-Spindle Air Blast ON Option M47 Sub-Spindle Air Blast OFF Option M48 Enable Feedrate and Spindle Override Standard M49 Disable Feedrate and Spindle Override Standard M51 Live Tooling Rotation Option M52 Live Tooling Rotation Option M53 Live Tooling Rotation / Coolant ON Option M54 Live Tooling Rotation / Coolant ON Option M55 Live Tooling Stop / Coolant OFF Option M56 Sub-Spindle Collet / Chuck Open Option M57 Sub-Spindle Collet / Chuck Close Option M58 Feed Bar Stock Option M59 Cancel Feed Bar Stock Option M60 Speed Arrival Check OFF Standard M61 Bar Change Option M62 Activate C Axis Spindle Synchronization Option M63 Cancel C Axis Spindle Synchronization Option M64 Spindle Feedback from Main Spindle Standard A2-4 M-504A

413 M Code Definition Standard / Option M65 Spindle Feedback from Sub-Spindle Option M66 Spindle Feedback from Live Tool Spindle Option M68 Sub-Spindle External Chucking Mode Option M69 Sub-Spindle Internal Chucking Mode Option M70 Spindle Orient Commands to Sub-Spindle Option M71 Spindle Orient Commands to Main Spindle Option M72 Chamfering OFF Standard M73 Chamfering ON Standard M76 Sub-Spindle Axis Drive OFF (E Axis) Option M77 Sub-Spindle Axis Drive Low Torque (E Axis) Option M78 Sub-Spindle Axis Drive Normal Torque (E Axis) Option M80 Check Part Missing Option M81 Check Part Present Option M82 E Axis Torque Control Mode ON (Tailstock) Standard M83 E Axis Position Control Mode ON (Tailstock) Standard M87 Tailstock Brake ON Standard M88 Tailstock Brake OFF Standard M90 Part Probe ON Option M97 Increment Part Counter Standard M98 Sub-Program Call Standard M99 Return from Sub-Program Standard M200 Main Spindle Brake ON Standard M201 Main Spindle Brake OFF Standard M202 Sub-Spindle Brake ON Option M203 Sub-Spindle Brake OFF Option M206 Disable Main Spindle Draw Bar Check Standard M207 Enable Main Spindle Draw Bar Check Standard M208 Disable Sub-Spindle Draw Bar Check Option M-504A A2-5

414 M Code Definition Standard / Option M209 Enable Sub-Spindle Draw Bar Check Option M215 Thru-Spindle Coolant ON, Sub-Spindle Option M216 Thru-Spindle Coolant OFF, Sub-Spindle Option M221 Part Catcher Slide Extend Option M222 Part Catcher Slide Retract Option M223 Sub-Spindle Contouring Mode ON Option M224 Sub-Spindle Contouring Mode OFF Option M225 Sub-Spindle Part Catcher Arm Rotate Out Option M226 Sub-Spindle Part Catcher Arm Rotate In Option M227 Sub-Spindle Part Catcher Gripper Close Option M228 Sub-Spindle Part Catcher Gripper Open Option M258 Chip Conveyor ON Option M259 Chip Conveyor OFF Option M301 Turns ON AUXO08 (output Y30.7) Standard M302 Turns ON AUXO07 (output Y30.6) Standard M303 Turns ON AUXO06 (output Y30.5) Standard M304 Turns ON AUXO05 (output Y30.4) Standard M305 Turns ON AUXO04 (output Y30.3) Standard M306 Turns OFF AUXO08 (output Y30.7) Standard M307 Turns OFF AUXO07 (output Y30.6) Standard M308 Turns OFF AUXO06 (output Y30.5) Standard M309 Turns OFF AUXO05 (output Y30.4) Standard M310 Turns OFF AUXO04 (output Y30.3) Standard M311 Wait for a high signal on AUXI08 (input X42.7) Standard M312 Wait for a high signal on AUXI07 (input X42.6) Standard M313 Wait for a high signal on AUXI06 (input X42.5) Standard M314 Wait for a high signal on AUXI05 (input X42.4) Standard M315 Wait for a high signal on AUXI04 (input X42.3) Standard A2-6 M-504A

415 M Code Definition Standard / Option M316 Wait for a high signal on AUXI03 (input X42.3) Standard M317 Wait for a high signal on AUXI02 (input X42.1) Standard M318 Wait for a high signal on AUXI01 (input X42.0) Standard M321 Turns ON AUXO03 (output Y30.2) Standard M322 Turns ON AUXO02 (output Y30.1) Standard M323 Turns ON AUXO01 (output Y30.0) Standard M326 Turns OFF AUXO03 (output Y30.2) Standard M327 Turns OFF AUXO02 (output Y30.1) Standard M328 Turns OFF AUXO01 (output Y30.0) Standard M-504A A2-7

416 - NOTES - A2-8 M-504A

417 DOCUMENT REVISION RECORD Date Document Revision Level Description October 29, Initial Release. November 12, November 17, Removed M08 coolant command, pages 1-54 & Corrected BMT 45 tooling chart, page 4-4. Modified tailstock programming formats, pages 9-11 & Updated Table of Contents entries for chapter 9. Corrected entrapment warning, page iii. Added Hardinge top plate X & Z travel limits to tables on pages 1-2 & 1-4. November 30, Removed M77 command. Updated programming examples. December 8, Added P98 to sample program segment, page December 13, December 20, February 25, April 15, May 12, Changed + Z axis software limit. Added Collet Dwell macro 9150 to Chapter 9. Added E axis work shift information to Chapters 4 & 14. Updated workpiece transfer program examples in Chapter 14. Added automatic swing-down tool probe option. Added tool limitation for automatic swing-down tool probe option. Updated sub-spindle part catcher information. Changed sub-spindle part catcher capacity specifications. Updated tailstock programming. Corrected data word formats and minimum / maximum values. Updated T-42 lathe spindle motor power and torque curves. Updated T-42 lathe live tool motor power and torque curves. Updated turret illustrations showing sub-spindle tool plate. Removed spindle nose layout. Changed + Z axis software limits. Added travel specifications for machine with 20C Big-Bore spindle. February 1, 2012 A Added T-51 and T-65 lathes. April 30, 2012 A Added turret top plate alignment caution. July 30, 2012 A Added M90 command. August 9, 2012 A Removed sub-spindle thermal compensation commands. Added M77 command. Updated programming example. September 23, 2013 A Added spare M codes. January 10, 2014 A Updated General Warnings and Cautions. June 20, 2014 A Corrected M codes in Chapter 14. July 2, 2014 A Updated spare M codes. M-504A R-1

418 Date Document Revision Level Description March 20, 2015 A Updated spindle synchronization in Chapter 14. R-2 M-504A

419 - NOTES - M-504A R-3

420 Hardinge Inc. Elmira, New York USA Phone: FAX: