VMC Series II Vertical Machining Centers PROGRAMMER S MANUAL. Equipped with the Hardinge / Fanuc System II, Fanuc 0i-M, or Fanuc 18-MC Control

Transcription

1 PROGRAMMER S MANUAL VMC Series II Vertical Machining Centers Equipped with the Hardinge / Fanuc System II, Fanuc 0i-M, or Fanuc 18-MC Control Revised: July 26, 2004 Manual No. M-377B Litho in U.S.A. Part No. M B October, 2002

2 - NOTICE - 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 VMC Series II Vertical Machining Centers equipped with the Hardinge / Fanuc System II, Fanuc 0i-M, or Fanuc 18-MC 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 THIS MANUAL - WARNINGS - Warnings must be followed carefully to avoid the possibility of personal injury or damage to the machine, tooling, or workpiece. - CAUTIONS - Cautions must be followed carefully to avoid the possibility of damage to the machine, tooling, or workpiece. - NOTES - Notes contain supplemental information. Hardinge Inc. One Hardinge Drive P.O. Box 1507 Elmira, New York USA , Hardinge Inc. M-377B

3 READ COMPLETE INSTRUCTIONS CAREFULLY BEFORE OPERATING OR PROGRAMMING HARDINGE VMC SERIES II VERTICAL MACHINING CENTERS. - WARNING - Occupational Safety and Health Administration (OSHA) Hazard Communication Standard , effective September 23, 1987, and various state employee right-to-know laws require that information regarding chemicals used with this machine be supplied to you. The list of chemicals appears in manual SP-134, the Material Safety Data Sheets (MSDS). Refer to the applicable section of the MSDS supplied with your machine when handling, storing, or disposing of chemicals. Store MSDS of other chemicals used with this machine in the same packet with manual SP-134. HARDINGE SAFETY RECOMMENDATIONS Your Hardinge machine is designed and built for maximum ease and safety of operation. Since some previously accepted shop practices may not reflect current safety regulations and procedures, they 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 all equipment. Our recommendations are described below. READ THESE SAFETY RECOMMEN- DATIONS BEFORE PROCEEDING ANY FURTHER. READ THE APPROPRIATE MANUAL OR INSTRUCTIONS before attempting operation, programming, 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. Wear a respirator, helmet, gloves, and ear muffs or plugs when necessary. DON T OPERATE EQUIPMENT unless proper maintenance has been regularly performed and the equipment is known to be in good working order. WARNING and INSTRUCTION TAGS are mounted on the machine for your safety and information. Do not remove them. DON T ALTER THE MACHINE to bypass any interlock, overload, disconnect switch, or other safety devices. DON T OPERATE ANY MACHINE while wearing rings, watches, jewelry, loose clothing, or neckties. Long hair must be contained by a net or shop cap for safety. MAKE CERTAIN that the equipment is properly grounded. Consult and comply with the National Electric Code and all local codes. M-377B i

4 DISCONNECT MAIN ELECTRICAL POWER before attempting repair or maintenance. DON T OPERATE EQUIPMENT if unusual or excessive heat, noise, smoke, or vibration occurs. Report any excessive or unusual conditions as well as any damaged parts to your supervisor. 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 any shutdown before restarting the machine. KEEP THE AREA AROUND THE MACHINE well lighted and dry. KEEP CHEMICALS AND FLAMMABLE MATERIAL away from operating equipment. HAVE THE CORRECT TYPE OF FIRE EXTINGUISHER handy when machining combustible material and keep the chips clear of the work area. DON T USE a toxic or flammable substance as a solvent cleaner or coolant. INSPECT ALL SAFETY DEVICES AND GUARDS to make certain that they are in good condition and are functioning properly. MAKE CERTAIN THAT PROPER GUARDS are in place and that all doors and covers are in place and secured before starting a machining cycle. DON T OPEN GUARDS while any machine component is in motion. Make certain that all people in the area are clear of the machine when opening the guard door. MAKE SURE that all spindle tools and any tool-holding devices are properly mounted. MAKE SURE that fixture plates and all other table-mounted work-holding devices are properly mounted. MAKE CERTAIN that all tooling is secured either in the tool magazine or spindle before starting the machine. DON T USE worn or defective hand tools. Use the proper size and type tool for the job being performed. ii M-377B

5 USE CAUTION around exposed mechanisms and tooling especially when setting up. Be careful of sharp edges on tools. USE ONLY a soft-faced hammer on table work-holding devices and fixtures. MAKE CERTAIN that all tool mounting surfaces are clean before mounting tools. DON T USE worn or broken tooling on the machine. INSPECT ALL WORK-HOLDING DEVICES daily to make certain that they are in good operating condition. Replace any defective devices before operating the machine. ANY ATTACHMENT, TOOL, OR MACHINE MODIFICATION obtained from any source other than Hardinge Inc., must be reviewed by a qualified safety engineer before installation. USE MAXIMUM ALLOWABLE gripping pressure on work-holding devices. Consider the weight, shape, and balance of the tooling. DON T EXCEED the rated capacity of the machine. DON T LEAVE tools, workpieces, or other loose items where they can come in contact with a moving component of the machine. REMOVE ANY LOOSE PARTS OR TOOLS from the work area before operating the machine. Always clear the machine and work area of tools and parts, especially after work has been completed by maintenance personnel. REMOVE SPINDLE WRENCHES before starting the machine. CHECK THE SETUP, TOOLING, AND SECURE THE WORKPIECE if the machine has been turned OFF for any length of time. CHECK THE LUBRICATION AND COOLANT LEVELS and the status of control indicator lights before operating the machine. KNOW where all EMERGENCY STOP push buttons are located. MAKE CERTAIN THAT PROPER FUNCTIONS are programmed and that all controls are set in the desired modes before pressing the Cycle Start push button. DRY CYCLE a new setup to check for programming errors. DON T ADJUST tooling, workpiece, or coolant hoses while the machine is running. KEEP CLEAR of any pinch point and any potentially hazardous situation. DON T LEAVE the machine unattended while it is operating. M-377B iii

6 DON T REMOVE OR LOAD workpieces while any part of the machine is in motion. BE CAREFUL of sharp edges when handling newly machined workpieces. DON T CHECK the finish or dimension of a workpiece near a running spindle or moving slide. DON T ATTEMPT to brake or slow the machine with hands or any makeshift device. DON T REMOVE CHIPS with hands. Make certain that all machine movement has stopped and then use a hook or similar device to remove chips and shavings. DON T CLEAN the machine with an air hose. KEEP TOTE PANS a safe distance from machine. Don t overfill the tote pans. 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. FOR YOUR PROTECTION - WORK SAFELY iv M-377B

7 - Contents - CHAPTER 1 - PART PROGRAM LANGUAGE Programming the Control Introduction Legal Characters (Excluding Macro Language) Data Word Format Charts English Mode Metric Mode Special Programming Characters Programming Format Programming Sequence Tape Programming Sequence Keyboard Programming Sequence Program Number X, Y, and Z Axes Decimal Point Programming Data Word Descriptions O Word N Word G Word G00 Positioning G01 Linear Interpolation G02 Circular Interpolation (Clockwise Arc) G03 Circular Interpolation (Counterclockwise Arc) G04 Dwell G09 Exact Stop G10 Data Setting Mode ON G11 Data Setting Mode OFF G12 Circular Pocket Milling - Clockwise Motion G13 Circular Pocket Milling - Counterclockwise Motion G15 Polar Coordinate Programming OFF G16 Polar Coordinate Programming ON G17 XY Plane Selection G18 XZ Plane Selection G19 YZ Plane Selection G20 Inch Data Input G21 Metric Data Input G22 Stored Stroke Limits ON G23 Stored Stroke Limits OFF G27 Reference Position Return Check G28 Return to Reference Position G29 Return from Reference Position G30 Return to Tool Change Position G31 Skip Function G39 Corner Offset Circular Interpolation G40 Tool Diameter Compensation Cancel G41 Tool Diameter Compensation Active - Tool Left of Part G42 Tool Diameter Compensation Active - Tool Right of Part G43 Tool Length Compensation Active G49 Tool Length Compensation Cancel G50 Scaling Mode OFF M-377B v

8 G51 Scaling Mode ON G52 Local Coordinate System G54 ~ G59 Standard Work Coordinate Systems (G54 Default) G54 P_ Additional Work Coordinate Systems G60 Single Direction Positioning G61 Exact Stop Mode G62 Automatic Corner Override G63 Tapping Mode G64 Cutting Mode G65 Non-Modal Macro Program Call G66 Modal Macro Program Call G67 Modal Macro Program Call Cancel G68 Coordinate Rotation G69 Coordinate Rotation Cancel G71 Rectangular Pocket Milling - Clockwise Motion G72 Rectangular Pocket Milling - Counterclockwise Motion G73 High Speed Peck Drilling Cycle G74 Left-Hand Tapping Cycle G76 Fine Boring Cycle G80 Cycle Cancel G81 Drilling Cycle G82 Drilling Cycle G83 Peck Drilling Cycle G84 Right-Hand Tapping Cycle G85 Boring Cycle G86 Boring Cycle G87 Back Boring Cycle G88 Boring Cycle (with Manual Retract) G89 Boring Cycle G90 Absolute Positioning Mode G91 Incremental Positioning Mode G92 Coordinate Shift / Constant Surface Speed RPM Limit G94 Inches / Millimeter Per Minute Feedrate G95 Inches / Millimeter Per Revolution Feedrate G96 Constant Surface Speed G97 Direct RPM Programming G98 Return to Initial Point in Cycle G99 Return to R Point in Cycle X Word Absolute Positioning Incremental Positioning Dwell Command Y Word Absolute Positioning Incremental Positioning Z Word Absolute Positioning Incremental Positioning I Word J Word K Word C Word vi M-377B

9 R Word P Word Q Word D Word H Word F Word S Word T Word M Word M00 Program Stop M01 Optional Stop M02 End of Program M03 Spindle Forward M04 Spindle Reverse M05 Spindle Stop M06 Automatic Tool Change M08 Coolant Pump ON M09 Coolant Pump OFF M10 Rotary Table Brake ON [Option] M11 Rotary Table Brake OFF [Option] M13 Spindle Forward / Coolant ON M14 Spindle Reverse / Coolant ON M15 Spindle Stop / Coolant OFF M16 Air Blast OFF M17 Air Blast ON M19 Spindle Orient M20 Spindle Orient Cancel M21 X Axis Mirror Image ON M22 Y Axis Mirror Image ON M23 Mirror Image Cancel M24 Work Light ON M25 Work Light OFF M29 Rigid Tapping Mode M30 End of Program M41 Spindle Low Gear (High Torque Machine Only) M42 Spindle High Gear (High Torque Machine Only) M48 Enable Feedrate and Spindle Override M49 Disable Feedrate and Spindle Override M51 Chip Coolant ON M52 Chip Coolant OFF M53 Thru-Spindle Coolant ON [Option] M54 Thru-Spindle Coolant OFF [Option] M68 Chip Conveyor ON M69 Chip Conveyor OFF M71 Tool Magazine 1 Home M72 Tool Magazine 1 Extend M73 Tool Magazine 1 Spindle Tool Clamp M74 Tool Magazine 1 Spindle Tool Unclamp M75 Search Spindle Tool Number (Magazine 1) M76 Activate Tool Change Mode (Magazine 1) M77 Cancel Tool Change Mode (Magazine 1) M80 Automatic Power OFF Active M-377B vii

10 M81 Tool Magazine 2 Home [Option] M82 Tool Magazine 2 Extend [Option] M83 Tool Magazine 2 Spindle Tool Clamp [Option] M84 Tool Magazine 2 Spindle Tool Unclamp [Option] M85 Search Spindle Tool Number (Magazine 2) M86 Activate Tool Change Mode (Magazine 2) M87 Cancel Tool Change Mode (Magazine 2) M98 Subprogram Call M99 Subprogram End M100 Circular Pocket Milling - Clockwise Motion M101 Circular Pocket Milling - Counterclockwise Motion M102 Rectangular Pocket Milling - Clockwise Motion M103 Rectangular Pocket Milling - Counterclockwise Motion Program Format CHAPTER 2 - TOOL COMPENSATION Introduction Tool Offset Definitions Tool Diameter Offset Tool Length Offset Tool Compensation Codes Plane Selection Activating Tool Compensation Programming Comparison Entering and Exiting the Workpiece with Tool Compensation Active Switching G41 / G42 Code Tool Moved Away from the Workpiece with Tool Compensation Active Canceling Tool Compensation Tool Diameter Compensation Programming Rules CHAPTER 3 - LINEAR AND CIRCULAR INTERPOLATION Feedrate Absolute and Incremental Programming Absolute Incremental Interpolation Linear Interpolation Insert Chamfer or Corner Radius Insert Chamfer Insert Corner Radius Alarm Messages for Insert Chamfer / Insert Corner Radius Circular Interpolation G02 Clockwise Arc (CW) G03 Counterclockwise Arc (CCW) Plane Selection Automatic Corner Override Helical Interpolation Sample Part Program Structure Programming Notes for Circular Interpolation Circular Interpolation Parameter Definitions viii M-377B

11 CHAPTER 4 - WORK COORDINATE SYSTEMS Introduction Zero Return (Reference Home) X, Y, and Z Axes Rectangular Coordinates Coordinate System Displays Standard Programmable Work Coordinate Systems Additional Programmable Work Coordinate Systems To Store Coordinate System Data from a Program G52 Local Coordinate System Introduction Activating G Restrictions Canceling G G92 Absolute Coordinate Shift G92 Programming Notes Polar Coordinates G Codes Plane Selection Positioning Modes Absolute Positioning Incremental Positioning Polar Coordinate Programming Examples Sample Program Segment for a Bolt Circle CHAPTER 5 - TOOL SELECTION AND OFFSETS Automatic Tool Changer Commanding Tool Changes Tool Magazine M06 Command Drum Tool Magazine Swing Arm Tool Magazine Suggested Programming Format Tool Offsets Tool Length Offsets (H Word) Tool Diameter Offsets (D Word) To Store Tool Offsets from the Part Program Activating Tool Offsets Canceling Tool Offsets CHAPTER 6 - STANDARD MILLING Introduction G90/G91 Programming Compensation Factors Tool Compensation G41 Cutter Left of Workpiece G42 Cutter Right of Workpiece Tool Offset Compensation Length Compensation Diameter Compensation Programming Example Sample Program Segment M-377B ix

12 CHAPTER 7 - POCKET MILLING Introduction Pocket Milling G Codes Pocket Milling M Codes Tool Offsets for Pocket Milling Tool Offset Memory B Tool Offset Memory C [Option] Circular Pocket Milling Rough Pocket Programming Formats Data Word Definitions Sample Program Segment Single Finish Pass Programming Formats Data Word Definitions Sample Program Segment Rectangular Pocket Milling Rough Pocket Programming Formats Data Word Definitions Sample Program Segment CHAPTER 8 - DRILLING CYCLES Introduction G90/G91 Programming G98/G99 Programming Canceling Drilling Cycles Peck Drilling Cycles Data Words Formats Definitions Sample Program Segment Tool Movement in the G73 Cycle Tool Movement in the G83 Cycle Single Pass Drilling Cycles Data Words Formats Definitions Sample Program Segment Drilling Multiple Holes Sample Program Segment Program Notes x M-377B

13 CHAPTER 9 - BORING CYCLES Introduction G90/G91 Programming G98/G99 Programming Canceling Boring Cycles General Descriptions Orientation Angle Parameter Definitions Establishing the Offset Axis and Direction G76 Fine Boring Cycle Data Words Formats Definitions Tool Movement in the G76 Cycle Sample Program Segment G85 Boring Cycle Data Words Formats Definitions Tool Movement in the G85 Cycle Sample Program Segment G86 Boring Cycle Data Words Formats Definitions Tool Movement in the G86 Cycle Sample Program Segment G87 Boring Cycle Data Words Formats Definitions Tool Movement in the G87 Cycle Sample Program Segment G88 Boring Cycle Data Words Formats Definitions Tool Movement in the G88 Cycle Sample Program Segment G89 Boring Cycle Data Words Formats Definitions Tool Movement in the G89 Cycle Sample Program Segment Boring Multiple Holes Sample Program Segment Sample Program Notes M-377B Revised: May 7, 2003 xi

14 CHAPTER 10 - TAPPING CYCLES Introduction Tapping Modes Conventional Tapping Rigid Tapping Tapping Feedrate G90/G91 Programming G98/G99 Programming Canceling Tapping Cycles Single Pass Tapping Cycles Data Words Formats Definitions Sample Program Segment Tapping Multiple Holes Sample Program Segment Program Notes CHAPTER 11 - TOOL LIFE MANAGEMENT General Information Introduction Tool Life Measurement Units Number of Parts Amount of Machining Time General Program Description Tool Life Management Program Program Format Inputting New Data Updating Existing Data Deleting Existing Data Data Word Definitions P Word - Tool Group Number L Word - Tool Life Value Data Word T Word - Tool Number H Word - Tool Length Offset D Word - Tool Diameter Offset Programming Notes Sample Tool Life Management Program (Inputting New Data) Data Block Definitions Part Program Tool Commands Combining Tool Commands Sample Part Program Structure using Combined Tool Commands xii M-377B

15 CHAPTER 12 - OPTIONS AND MISCELLANEOUS FEATURES Inch / Metric Mode Establishing Inch / Metric Mode Subprograms Subprogram Call G96 Constant Surface Speed Introduction Programming Format Data Word Definitions Scaling Mode Types of Scaling Uniform Scaling Independent Scaling Examples Scale Factors for Magnification Scale Factors for Reduction Mirror Imaging Example Scaling Mode Notes Macro Programs Non-Modal Macro Call Modal Macro Call Macro Call Format Single Direction Positioning (G60) Introduction Determining Direction and Distance Machines Equipped with Hardinge / Fanuc System II Control Direction Distance Machines Equipped with Fanuc 0i-M or Fanuc 18-MC Control Direction Distance Examples Sample Positioning Programming Notes Programming the 4th Axis [Option] Introduction Formulas Description of Sample Operation Sample Part Calculations Sample Program M-377B Revised: May 7, 2003 xiii

16 APPENDIX Travel Specifications X and Y Axis VMC600II Machining Center A-1 VMC800II Machining Center A-2 VMC1000II Machining Center A-3 VMC1250II Machining Center A-4 VMC1500II Machining Center A-5 Z Axis VMC 600II, 800II, and 1000II Machining Centers A-6 VMC1250II and 1500II Machining Centers A-7 Tool Slot Locations and Configuration VMC600II Machining Center A-8 VMC800II Machining Center A-9 VMC1000II Machining Center A-10 VMC1250II Machining Center A-11 VMC1500II Machining Center A-12 G Code List A-13 M Code List A-16 Alarm Messages A-19 xiv M-377B

17 - NOTES - M-377B xv

18 - NOTES - xvi M-377B

19 CHAPTER 1 - PART PROGRAM LANGUAGE 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 outlined in each of the data word descriptions and are also listed in the tables on pages 1-2 and 1-4. PROGRAMMING THE CONTROL INTRODUCTION Programming Hardinge machining centers requires an understanding of the machine, tooling, and control. Extreme care must be exercised when writing a part program or punching a tape 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 of 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. Block Delete code (/) 2. Sequence number (N Function) 3. Preparatory Functions (G Function) 4. Axis Movement Instructions (X, Y, and Z Functions) 5. Feedrate Command (F Function) 6. Spindle Speed Command (S Function) 7. Tool and Offset Selection (T, D, and H Functions) 8. Miscellaneous Functions (M Function) A block MUST contain a valid End of Block character. LEGAL CHARACTERS (Excluding Macro Language) Legal alpha characters for the control are those used as word addresses in a part program block that the control will accept and act on. All illegal alpha characters on tape or disk will be loaded into memory, but will result in a decoding error when program execution is attempted. The illegal character must be removed or replaced with a legal character. The following characters are illegal: E, U, V, and W M-377B 1-1

20 DATA WORD FORMAT CHARTS English Mode Refer to the key on page 1-3. Function (Data Word) Preparatory Commands Format Minimum Value Maximum Value O (Program Number) - O N (Block Number) - N G (Command) - G M (Command) - M P (Dwell) G04 P P (Subprogram) - P P (Offset) G10 P Q (Depth of Cut) G73,G83 Q X (Absolute) 1 G90,G00,G01,G02,G03 X± X (Absolute) 2 G90,G00,G01,G02,G03 X± X (Absolute) 3 G90,G00,G01,G02,G03 X± X (Absolute) 4 G90,G00,G01,G02,G03 X± X (Absolute) 5 G90,G00,G01,G02,G03 X± X (Incremental) G91,G00,G01,G02,G03 X± X (Dwell) G04 X Y (Absolute) 6 G90,G00,G01,G02,G03 Y± Y (Absolute) 7 G90,G00,G01,G02,G03 Y± Y (Incremental) G91,G00,G01,G02,G03 Y± Z (Absolute) 6 G90,G00,G01,G02,G03 Z± Z (Absolute) 7 G90,G00,G01,G02,G03 Z± Z (Incremental) G91,G00,G01,G02,G03 Z± X (Zero Offset) G10 X± Y (Zero Offset) G10 Y± Z (Zero Offset) G10 Z± D (Tool Diameter Offset) G41,G42 D H (Tool Length Offset) G43 H I (Circular Interpolation) G02,G03 I± J (Circular Interpolation) G02,G03 J± K (Circular Interpolation) G02,G03 K± F (Feedrate, per min) G94 F F (Feedrate, per rev) G95 F S (Spindle Speed) 8 - S S (Spindle Speed) 9 - S S (Spindle Speed) 10 - S M-377B

21 T (Tool Select) 11 - T T (Tool Select) [Option] 12 - T T (Tool Select) [Option] 13 - T C (Insert Chamfer) G01 C R (Insert Radius) G01 R R (Radius) G02,G03 R R (Coordinate Rotation) G68 R Key for Data Word Format Charts 1. VMC600II Machining Center 2. VMC800II Machining Center 3. VMC1000II Machining Center 4. VMC1250II Machining Center 5. VMV1500II Machining Center 6. VMC600II, 800II, and 1000II Machining Centers 7. VMC1250II, and 1500II Machining Centers 8. Machining Center equipped with standard or optional high torque spindle 9. Machining Center equipped with optional 12,000 rpm high speed spindle 10. Machining Center equipped with optional 15,000 rpm high speed spindle 11. Machining Center equipped with one drum tool magazine 12. Machining Center equipped with two drum tool magazines [Option] 13. Machining Center equipped with one swing arm tool magazine [Option] M-377B 1-3

22 Metric Mode Refer to the key on page 1-3. Function (Data Word) Preparatory Commands Format Minimum Value Maximum Value O (Program Number) - O N (Block Number) - N G (Command) - G M (Command) - M P (Dwell) G04 P P (Subprogram) - P P (Offset) G10 P Q (Depth of Cut) G73,G83 Q X (Absolute) 1 G90,G00,G01,G02,G03 X± X (Absolute) 2 G90,G00,G01,G02,G03 X± X (Absolute) 3 G90,G00,G01,G02,G03 X± X (Absolute) 4 G90,G00,G01,G02,G03 X± X (Absolute) 5 G90,G00,G01,G02,G03 X± X (Incremental) G91,G00,G01,G02,G03 X± X (Dwell) G04 X Y (Absolute) 6 G90,G00,G01,G02,G03 Y± Y (Absolute) 7 G90,G00,G01,G02,G03 Y± Y (Incremental) G91,G00,G01,G02,G03 Y± Z (Absolute) 6 G90,G00,G01,G02,G03 Z± Z (Absolute) 7 G90,G00,G01,G02,G03 Z± Z (Incremental) G91,G00,G01,G02,G03 Z± X (Zero Offset) G10 X± Y (Zero Offset) G10 Y± Z (Zero Offset) G10 Z± D (Tool Diameter Offset) G41,G42 D H (Tool Length Offset) G43 H I (Circular Interpolation) G02,G03 I± J (Circular Interpolation) G02,G03 J± K (Circular Interpolation) G02,G03 K± F (Feedrate, per min) G94 F F (Feedrate, per rev) G95 F S (Spindle Speed) 8 - S S (Spindle Speed) 9 - S S (Spindle Speed) 10 - S M-377B

23 T (Tool Select) 11 - T T (Tool Select) [Option] 12 - T T (Tool Select ) [Option] 13 - T C (Insert Chamfer) G01 C R (Insert Radius) G01 R R (Radius) G02,G03 R R (Coordinate Rotation) G68 R M-377B 1-5

24 SPECIAL PROGRAMMING CHARACTERS An End of Record character (%) should be the first and last character on a punched tape which is to be uploaded to the machine control by means of the RS-232 serial port. If multiple programs are to be loaded from a single punched tape, it may be desirable to place an End of Record character between each of the programs. All End of Record characters must 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 part programs loaded through the RS-232 serial port, 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, Y, Z, I, J, K, C, R, P, Q, D, H, F, S, T, M The software for the system was configured to provide a programming resolution of.0001 inch [.001 mm], which causes specific data word formats to be applied to the associated values. These formats are outlined in each of the data word descriptions and are also listed in the tables on pages 1-2 and 1-4. These numbers designate 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. The program format shown on page 1-46 outlines the part program format taught and used by the Hardinge Customer Training School. - NOTE - It is strongly recommended that the programmer follow the Hardinge Programming Format. 1-6 M-377B

25 PROGRAMMING SEQUENCE Tape Programming Sequence The sequence in which a tape should be programmed is as follows: 1. A few inches of tape feed (leader), as required. 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 (M02, M30) in the last data block. All data blocks must end with a valid End of Block character. 5. Enter the End of Record character. 6. A few inches of tape feed (trailer), as required. Keyboard Programming Sequence To program from the keyboard, follow this procedure: 1. Select Edit mode. 2. Enable program editing. Refer to the machine operator s manual (M-400) for information on enabling program editing. 3. Press the Program key. - NOTE - Part 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. An example of a program number is O2222". 4. Enter the program ID code and program number; then, press the Insert key. The currently active program is cleared from the display. The new program number and the End of Record character are displayed. - NOTE - A valid End of Block character must be entered at the end of each data block. Each letter address and value must be inserted separately. 5. Key in each letter address and value. 6. Press the Insert key. 7. Press the End of Block key and the Insert key at the end of each data block. 8. The End of Program command (M02 or M30) must be placed at the end of the program, followed by a valid End of Block character. 9. Disable program editing. M-377B 1-7

26 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 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 entered on the Master Macro Tape. These numbers cannot be assigned to other part programs or macros. 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. - 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. X, Y, AND Z AXES The axes of motion parallel to the spindle face are the X and Y axes. The axis of motion parallel to the spindle centerline is the Z axis. These letter designations for the three axes are recommended by the Electronic Industries Association (E.I.A.). In an effort to promote interchangeability and prevent misunderstandings between CNC manufacturers and purchasers, recommended standards have been set forth by E.I.A. These standards include the following: axis designation, axis motion nomenclature, character codes for perforated tape, operational command format, data format, and electrical interface between controls and machine tools. 1-8 M-377B

27 DECIMAL POINT PROGRAMMING A decimal point should be used with the following address words: A, B, C, F, I, K, R, X, Y, and Z. If a decimal point is programmed in a word in which a decimal point is not allowed (G, M, N, O, P, Q, S, or T word) 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. - CAUTION - The programmer must make certain all decimal points are correctly positioned to prevent undesirable machine behavior. 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 (G20), the format for the Z word is ±2.4. If Z4. is programmed, the control will assume Z 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. The following example is written in inch mode (G20). Example: The command X2. sends the table to coordinate X2.0000, however, the command X2 sends the table to X Be sure the decimal point is programmed when allowed. Besides specifying the location of the assumed decimal point, data word formats also indicates the maximum number of digits which can appear to the left and right of the decimal point. Refer to the tables on pages 1-2 and 1-4. M-377B 1-9

28 DATA WORD DESCRIPTIONS On the following pages are descriptions of the data words used with the control. 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 1-8. 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 gives 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 tool offset to be used during that operation. For example, when using tool offset #6, N6 will be the block number to start that 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 from 0 to 152. Certain G codes are default codes automatically activated by the control under the following conditions: 1. Machine Power-up 2. Reading an End of Program Code (M02/M30) 3. Control Reset 4. Emergency Stop The G codes are of two types: 1. Non-modal or one-shot G codes are effective only in the block in which they are programmed. 2. Modal G codes are effective until replaced by another G code in the same group. A chart in the Appendix 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-377B