Cobra Series CNC Lathes

Transcription

1 PROGRAMMER S MANUAL TP1480B TP3264 TP2580 Cobra Series CNC Lathes Equipped with the GE Fanuc 21T Control Manual No. M-312C Litho in U.S.A. Part No. M C October, 1998

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 Cobra series CNC lathes equipped with the GE Fanuc 21T 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 , Hardinge Inc. M-312C

3 READ COMPLETE INSTRUCTIONS CAREFULLY BEFORE OPERATING MACHINE When this instruction book was printed, the information given was current. However, since we are constantly improving the design of our machine tools, it is possible that the illustrations and descriptions may vary from the machine you received. - 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 equipment be supplied to you. A complete list of the chemicals used with this machine, their reference data sheet numbers, and their suppliers appears as an insertion at the end of this manual. Refer to the applicable section of the Material Safety Data Sheets supplied with your machine when handling, storing, or disposing of chemicals. Machine should only be used with a bar feed approved by Hardinge Inc. HARDINGE 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 all equipment. Our recommendations are described below. READ THESE SAFETY RECOM- MENDATIONS BEFORE PROCEEDING ANY FURTHER. READ THE APPROPRIATE MANUAL OR INSTRUCTIONS before attempting operation or maintenance of the machine. Make sure you understand all instructions. CONSULT YOUR SUPERVISOR when in doubt as to the correct way to do a job. DON T OPERATE EQUIPMENT unless proper maintenance has been regularly performed and the equipment is known to be in good working order. DON T REMOVE any warning or instruction tags from machine. 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. MAKE SURE equipment is properly grounded. Consult National Electric Code and all local codes. DISCONNECT MAIN ELECTRICAL POWER before attempting repair or maintenance. DON T REACH into any control or power case area unless electrical power if OFF. DON T TOUCH ELECTRICAL EQUIPMENT when hands are wet or when standing on a wet surface. M-312C i

4 ALLOW ONLY AUTHORIZED PERSONNEL to have access to enclosures containing electrical equipment. DON T ALLOW the operation or repair of equipment by untrained personnel. REPLACE BLOWN FUSES with fuses of the same size and type as originally furnished. ASCERTAIN AND CORRECT cause of a shutdown caused by overload heaters before starting machine. WEAR SAFETY GLASSES AND PROPER FOOT PROTECTION at all times. When necessary, wear respirator, helmet, gloves and ear muffs or plugs. KEEP AREA THE AROUND THE MACHINE well lighted and dry. KEEP CHEMICAL AND FLAMMABLE MATERIAL away from electrical or operating equipment. HAVE THE CORRECT TYPE OF FIRE EXTINGUISHER handy when machining combustible material and keep chips clear of the work area. DON T USE a toxic or flammable substance as a solvent cleaner or coolant. MAKE SURE PROPER GUARDING is in place and all doors are closed and secured. TO REMOVE OR REPLACE the collet closer it is necessary to remove the guard door at left end of the machine. Make certain the guard door is replaced before starting the machine. DON T ALTER THE MACHINE to bypass any interlock, overload, disconnect or other safety device. DON T OPEN GUARD DOORS 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 chucks, closers, fixture plates and all other spindle-mounted work-holding devices are properly mounted and secured before starting machine. MAKE CERTAIN all tools are securely clamped in position before starting machine. REMOVE ANY LOOSE PARTS OR TOOLS left on machine or in the work area before operating machine. Always check machine and work area for loose tools and parts especially after work has been done 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 stop push buttons are located in case of an emergency. ii M-312C

5 CHECK THE LUBRICATION OIL LEVEL and the status of 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. CHECK THE TURRET POSITION before pressing the Cycle Start push button. CHECK SETUP, TOOLING AND SECURITY OF WORKPIECE if the machine has been OFF for any length of time. DRY CYCLE a new setup to check for programming errors. MAKE CERTAIN 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 newly machined workpieces. DON T REMOVE OR LOAD workpieces 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 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 gage. DON T ATTEMPT to brake or slow the machine with hands or any makeshift device. ANY ATTACHMENT, TOOL OR MACHINE MODIFICATION not obtained from Hardinge Inc., must be reviewed by a qualified safety engineer before installation. 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 job being performed. M-312C iii

6 USE ONLY a soft-faced hammer on turret tools and fixtures. DON T USE worn or broken tooling on machine. MAKE CERTAIN that all tool mounting surfaces are clean before mounting tools. INSPECT ALL CHUCKING DEVICES daily to make sure they are in good operating condition. REPLACE DEFECTIVE CHUCK before starting machine. USE MAXIMUM ALLOWABLE gripping pressure on the chuck. Consider weight, shape and balance of workpiece. 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 machine. DON T LEAVE the machine unattended while it is operating. DON T CLEAN the machine with an air hose. DON T OVERFILL tote pans. KEEP TOTE PANS a safe distance from machine. 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 spindle. If floormounted type, it must be securely bolted to floor. 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. DON T USE any chuck that is not a counterbalanced chuck. When a chuck is required for a machining operation, a counterbalanced chuck MUST be used. FOR YOUR PROTECTION - WORK SAFELY iv M-312C

7 - Contents - CHAPTER 1 - PART PROGRAM LANGUAGE Introduction Programming the GE Fanuc 21T Control Legal Programming Characters Special Programming Characters Programming Format Programming Sequence Tape Programming Sequence Keyboard Programming Sequence Program Number X and Z Axes 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 Data Setting ON G20 Inch Data Input G21 Metric Data Input G22 Stored Stroke Limits ON [Option] G23 Stored Stroke Limits OFF [Option] G28 Return to Reference Position G31 Skip Function G32 Threadcutting (Constant Lead) 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 [Option] G71 Automatic Rough Turning Cycle [Option] G72 Automatic Rough Facing Cycle [Option] G73 Automatic Rough Pattern Repeat Cycle [Option] G74 Automatic Drilling Cycle (Constant Depth Increments) [Option] G75 Automatic Grooving Cycle [Option] G76 Automatic Threading Cycle [Option] 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 M-312C v

8 X Word U Word Z Word W Word I Word K Word R Word Linear Interpolation (G01) Circular Interpolation (G02/G03) Tool Nose Radius Compensation (G41/G42) Defining Tapers P Word Q 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/Coolant OFF M08 Coolant ON M09 Coolant OFF M10 High Pressure Coolant ON (Cobra 51 & 65 lathes only) [Option] M11 High Pressure Coolant OFF (Cobra 51 & 65 lathes only) [Option] M13 Spindle Forward/Coolant ON M14 Spindle Reverse/Coolant ON M21 Open Collet M22 Close Collet M25 Part Catcher Retract [Option] M26 Part Catcher Extend [Option] M28 External Chucking Mode M29 Internal Chucking Mode M30 End of Program M31 Program Rewind and Restart M48 Enable Feedrate and Spindle Override M49 Disable Feedrate and Spindle Override M61 Load New Bars M84 Tailstock Quill Forward [Option] M85/M86 Tailstock Quill Retract [Option] M93 Steady Rest Open [Option] M94 Steady Rest Closed [Option] M98 Subprogram Call M99 Subprogram End Diameter Programming Programming Notes General Program Format vi M-312C

9 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 Canned Turning and Facing Cycles with Tool Nose Radius Compensation Active Modes in which Tool Nose Radius Compensation is not Performed Tool Moved Away from the Workpiece with Tool Nose Radius Compensation Active. 2-8 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 Alarm Messages for Insert Chamfer/Insert Corner Radius Circular Interpolation G02 Clockwise Arc G03 CounterClockwise Arc Sample Part Program Programming Notes for Circular Interpolation CHAPTER 4 - WORK SHIFT AND TOOL OFFSETS Work Shift (Zero Offset) To Store a Work Shift Offset from the Part Program Tooling and Tool Offsets Square Shank Tools Qualified Tool Holders Top Plate Configurations Round Shank Tools Double Tool Holder Positioning Left Hand/Right Hand Tooling Tool Offsets Tool Nose Radius Value and Tool Orientation Code To Store Tool Offsets from the Part Program Activating Tool Offsets M-312C vii

10 CHAPTER 5 - WORK COORDINATE SYSTEM How the Control Positions the Slides X and Z Axes Rectangular Coordinates Work Coordinate System 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 Multiple Repetitive Rough and Finish Turning [Option] Example 3: G71/G70 Turning Cycle G71 Turning Programming Rules G94 Canned Facing Cycle Example 4: G94 Straight Facing Example 5: G94 Taper Facing G72/G70 Multiple Repetitive Rough and Finish Facing [Option] G72 Programming Notes G73/G70 Automatic Rough and Finish Pattern Repeat [Option] G73 Programming Notes G70 Automatic Finishing Cycle [Option] G70 Programming Notes Automatic Drilling Cycles G74 Constant Depth Increment Auto Drilling Cycle [Option] Q Word Programming G74 Auto Drilling Sample Program Variable Depth Increment Auto Drilling Cycle Block Format Positioning the Drill Calculating the Drill Pass Increments Example Optional Z Word Example G75 Automatic Grooving Cycle [Option] P and Q Word Programming Tool Movement Sequence G75 Automatic Grooving Sample Program viii M-312C

11 CHAPTER 7 - THREADING CYCLES Single Block Threadcutting To Establish a Start Point for Threading G32 Programming Example 1: G32 Straight Threads Example 2: G32 Tapered Threads G92 Programming Example 3: G92 Straight Threads Example 4: G92 Tapered Threads Plunge Infeed Threading Compound Infeed Threading G76 Multiple Repetitive Threading Cycle [Option] Example 5: G76 Straight Threads Example 6: G76 Tapered Thread G76 Parameters G76 Execution Line G76 Programming Notes Tapping Example Sample Program Segment Left-Hand Threads CHAPTER 8 - MISCELLANEOUS Constant Surface Speed Subprograms Manual Data Input Keyboard Entry Tape or Floppy Disk Entry Subprogram Call Safe Start Subprograms Inch Mode Hardinge Permanent Macro Programs Macro 9115: Safe Tool Offset Macro 9136: Deep Hole Drilling Macro 9150: Collet Dwell Recommended Settings To Set the Delay Macro 9333: Parts Counter How the Parts Counter Macro Works Checking/Clearing Macro Variable # Programming the Parts Counter Macro Tailstock Programming [Option] Tailstock Quill Feedrate Tailstock M Codes M84 - Tailstock Quill Extend M85/M86 - Tailstock Quill Retract Tailstock Programming Recommendations English/Metric Mode Establishing English/Metric Mode M-312C ix

12 CHAPTER 9 - SAMPLE PART PROGRAM Safe Start Program Sample Program APPENDIX ONE Turret Travel Specifications Cobra 42 & 51 Lathes Hardinge Top Plate A1-1 VDI Top Plate A1-2 Cobra 65 Lathe Hardinge Top Plate A1-3 VDI Top Plate A1-4 Tailstock Travel Specifications Cobra 42 & 51 Lathes A1-5 Cobra 65 Lathe A1-5 Work Envelope with Qualified Square Shank Tooling Cobra 42 & 51 Lathes Hardinge Top Plate A1-6 VDI Top Plate A1-7 Cobra 65 Lathe Hardinge Top Plate A1-8 VDI Top Plate A1-9 Turret Top Plate Dimensions Cobra 42 & 51 Lathes Hardinge Top Plate A1-10 VDI Top Plate A1-11 Cobra 65 Lathe Hardinge Top Plate A1-12 VDI Top Plate A1-13 Sample Tooling Configurations with Maximum Workpiece Diameters Illustrated Cobra 42 & 51 Lathes Hardinge Top Plate A1-14 VDI Top Plate A1-15 Cobra 65 Lathe Hardinge Top Plate A1-16 VDI Top Plate A1-17 Spindle Drive Motor Horsepower/Torque Curves Cobra 42 Lathe A1-18 Cobra 51 Lathe A1-19 Cobra 65 Lathe Standard Spindle A1-20 High Torque Spindle [Option] A1-21 APPENDIX TWO Standard G Codes A2-1 Optional G Codes A2-1 Standard M Codes A2-2 Optional M Codes A2-2 Alarm Messages A2-3 Operator Messages A2-5 x M-312C

13 - NOTES - M-312C xi

14 - NOTES - xii M-312C

15 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 outlined in each of the data word descriptions and are also listed in the table on page 1-2. PROGRAMMING THE GE FANUC 21T CONTROL Programming Hardinge Cobra series lathes equipped with the GE Fanuc 21T control 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 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. Block Skip code (/) 2. Sequence number (N Function) 3. Preparatory Functions (G Functions) 4. Axis Movement Instructions (X or U 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-312C 1-1

16 FUNCTION (Word) PREPARATORY COMMANDS INCH MODE (G20) METRIC MODE (G21) Format Min. Max. Format Min. Max. O (Prog. #) N (Block #) G (Command) M (Command) P (Block #) P (Dwell) Q (Block #) O4 N4 G3 M2 P4 P8 Q O4 N4 G3 M2 P4 P8 Q U (Coordinate) U (Dwell) W (Coordinate) X (Coordinate) 1 X (Coordinate) 2 X (Dwell) Z (Coordinate) 1 Z (Coordinate) 2 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 G00, G01, G02, G03 G04 G00, G01, G02, G03 G00, G01, G02, G03 U±2.4 U5.3 W±2.4 X±2.4 X±2.4 X5.3 Z±2.4 Z± U±3.3 U5.3 W±3.3 X±3.3 X±3.3 X5.3 Z±3.3 Z± X (Tool Offset) X (Wear Offset) X (Zero Offset) Z (Tool Offset) Z (Wear Offset) Z (Zero Offset) G10 G10 G10 G10 G10 G10 X±2.4 X±0.4 X±2.4 Z±2.4 Z±0.4 Z± X±3.3 X±2.3 X±3.3 Z±3.3 Z±2.3 Z± I (Circ. Inter.) K (Circ. Inter.) K (Lead Change) G02, G03 G02, G03 G34 I±3.4 K±3.4 K± I±4.3 K±4.3 K± F (per min) [X/U] F (per min) [Z/W] F (per rev) F (Thread Lead) G98 G98 G99 G32, G92 F3.2 F3.2 F1.6 F F5.0 F5.0 F3.4 F S (Spindle rpm) 3 S (Spindle rpm) 4 S (Spindle rpm) 5 S (Spindle rpm) 6 S (Surface Speed) G50, G97 G50, G97 G50, G97 G50, G97 G96 S4 S4 S4 S4 S S4 S4 S4 S4 S T (Tool Function) 7 T (Tool Function) T4 T T4 T C (Chamfer) R (Radius) R (Circ. Inter.) G01 G01 G02, G03 C2.4 R2.4 R C3.3 R3.3 R Table Data Word Formats and Min/Max Increments 1 - Cobra 42 & 51 lathes. 2 - Cobra 65 lathe. 3 - Cobra 42 lathe. 4 - Cobra 51 lathe. 5 - Cobra 65 lathe standard spindle drive. 6 - Cobra 65 lathe high torque spindle drive [Option]. 7 - Standard Feature. 8 - Optional Feature. 1-2 M-312C

17 LEGAL PROGRAMMING CHARACTERS Legal alpha characters for the GE Fanuc 21T control are those used as word addresses in a part program block that the control will accept and act on. All illegal alpha characters input through the RS-232 serial port 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: B, C, D, E, J, and L 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, it may be desirable to place an End of Record character between each of the programs. All End of Record characters 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 EOB 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. M-312C 1-3

18 PROGRAMMING FORMAT Programs to be executed by the GE Fanuc 21T 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, I, K, P, Q, R, A, F, S, T, M The software for the system is configured to provide the following programming resolution:.0001 inch [.001 mm] This 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 table 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. The general part program format is shown on page The Safe Start Subprogram shown in the program format is described in Chapter 8 of this manual. 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 an End of Record character. 6. A few inches of tape feed (trailer), as required. 1-4 M-312C

19 Keyboard Programming Sequence - NOTE - If necessary, refer to the Cobra series lathe operator s manual (M-313C) for information on using the Manual Data Input keyboard. To program from the keyboard, follow this procedure: 1. Activate Edit mode. 2. Set Protect Key to Release. 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. 4. Key in the letter O and the program number at the Manual Data Input keyboard. Example: O Press the Insert key. 6. Press the EOB key. 7. Press the Insert key. 8. Enter each data block as follows: a) Key in the letter addresses and values. b) Press the EOB key. c) Press the Insert key. 9. Set Protect Key to Protect. M-312C 1-5

20 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 entered on the Master Macro Tape. 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. X AND Z AXES The axis of motion parallel to the spindle face is the X axis and the axis of motion parallel to the spindle centerline is the Z axis. From this point on, the cross slide will be referred to as the X axis and the carriage as the Z axis. These letter designations for the two 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. 1-6 M-312C

21 DECIMAL POINT PROGRAMMING A decimal point should be used with the following address words: A, C, 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 (P or Q 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. 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 ±2.4. If Z4. is programmed, the control will assume Z CAUTION - 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 X2.0000; however, the command X2" (no decimal point) sends the cross slide to X Be sure the decimal point is programmed when allowed. In addition to 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-312C 1-7

22 DATA WORD DESCRIPTIONS On the following pages are descriptions of the data words used with the GE Fanuc 21T 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 1-6. 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. 1-8 M-312C

23 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 (M02/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 GE Fanuc 21T 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 G1 G00 Positioning (Group 1 G Code) This positioning command generates linear motion on one or more axes (X or Z) from the current position to the programmed end points at a rate determined by the Rapid Override switch. When this switch is set to 100%, axis motion takes place at the rapid traverse rates shown below. Rapid traverse rates are shown as inches per minute [millimeters per minute]. X Axis: 400 [10160] Cobra 42 Lathe X Axis: 472 [12000] Cobra 51 & 65 Lathes Z Axis: 630 [16000] Cobra 42 Lathe Z Axis: 787 [20000] Cobra 51 & 65 Lathes Axis distance may be expressed as X and Z for absolute moves or U 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 in both axes (X & Z), the axes execute a vectorial move at a traverse rate which is a result of the X and Z rapid traverse. 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. M-312C 1-9

24 G01 Linear Interpolation (Group 1 G Code) Linear Interpolation generates linear motion on one or more axes (X 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. The maximum programmable feedrate for the X and Z axes is 400 inches per minute [10160 millimeters per minute]. Axis distance may be expressed as X and Z for absolute moves or U and W for incremental moves. When both the X and Z axes are programmed for a taper cut, the control will compensate X and Z 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. G02 Clockwise Arc (Group 1 G Code) Refer to Figure 3.4 for the path traced by the tool for a clockwise arc. 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) Refer to Figure 3.4 for the path traced by the tool for a counter-clockwise arc. 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 M-312C

25 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 as follows:.001 to seconds. 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. G10 Data Setting ON (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 is non-modal when used for tool offset entry and must be programmed in each offset entry block. Refer to Chapter 4, Work Shift and Tool Offsets. M-312C 1-11

26 G20 Inch Data Input (Group 6 G Code) 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. - 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. G21 Metric Data Input (Group 6 G Code) 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. - 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. G22 Stored Stroke Limits ON [Option] (Group 9 G Code) With G22 active, stored stroke limit #2 is active. The tool cannot enter the stroke limits established by these stored stroke limits. - NOTE - Stored stroke limit #1 is active even if G22 is inactive. 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. G23 Stored Stroke Limits OFF [Option] (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-312C

27 G28 Return to Reference Position (Group 0 G Code) - CAUTION - Tool offsets and Tool Nose Radius Compensation should be canceled BEFORE commanding G28. - NOTE - The turret reference position is the intersection of the X and Z axis reference coordinates. The G28 command performs an automatic return of the turret to the reference position for one or both axes. The move may 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 turret to X axis reference coordinate or G28 W0. ; Move turret to Z axis reference coordinate or G28 U0. W0. ; Move turret to X and Z axis reference coordinates Move Through an Intermediate Position: G28 X4. Z6. ; Move turret to X4. Z6., then to X and Z axis reference coordinates 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 move currently being executed is not completed. G31 is non-modal and must be programmed each time it is to be effective. M-312C 1-13

28 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. The data word format is F1.6 in inch mode and 3.4 in metric mode. 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, Threading Cycles. 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, Tool Nose Radius Compensation M-312C

29 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, Tool Nose Radius Compensation. 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, Tool Nose Radius Compensation. 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 8 for additional information on Constant Surface Speed. 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 8 for additional information on the G65 Macro Call command. M-312C 1-15

30 G70 Automatic Finishing Cycle [Option] (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/G70 Multiple Repetitive Rough and Finish Turning, Chapter 6 G72/G70 Multiple Repetitive Rough and Finish Facing, Chapter 6 G73/G70 Rough and Finish Pattern Repeat, Chapter 6 G71 Automatic Rough Turning Cycle [Option] (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 G71/G70 Rough and Finish Turning Cycle, in Chapter 6, for additional information. G72 Automatic Rough Facing Cycle [Option] (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 G72/G70 Rough and Finish Facing Cycle, in Chapter 6, for additional information. G73 Automatic Rough Pattern Repeat Cycle [Option] (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 G73/G70 Rough and Finish Pattern Repeat, in Chapter 6, for additional information M-312C

31 G74 Automatic Drilling Cycle (Constant Depth Increments) [Option] (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 Constant Depth Increment Auto Drilling Cycle (G74), in Chapter 6, for additional information. G75 Automatic Grooving Cycle [Option] (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 G75 Auto Grooving Cycle, in Chapter 6, for additional information. G76 Automatic Threading Cycle [Option] (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 Multiple Repetitive Threading Cycle (G76), in Chapter 7, for additional information. 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 and Decrease push buttons, Feedrate Override switch, and Feed Hold push button are active. Refer to Canned Turning Cycle (G90), in Chapter 6, for additional information. M-312C 1-17

32 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 G92 Programming, in Chapter 7, for additional information. 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 Canned Facing Cycle (G94), in Chapter 6, for additional information. 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 Spindle Limitation 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 Constant Surface Speed, in Chapter 8, for more information M-312C

33 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. The F word format is F3.2 in inch mode (G20) and F5.0 in metric mode (G21). 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: F400 results in a feedrate of 4.00 inches per minute. Example 2: F400. 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. The F word format is F1.6 in inch mode (G20) and F3.4 in metric mode (G21). 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. M-312C 1-19

34 X WORD - CAUTION - Programming an X axis move without the correct Tool or Zero Offset active could cause the tool to strike the workpiece or optional tailstock. The X word is a DIAMETER DIMENSION for the 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 the 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 from the keyboard or tape, the control will act on the X command programmed closest to the End of Block character. The data word format is shown in the table on page 1-2. Assuming tool offsets are inactive, 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. A movement in the +X direction will cause the X axis to be positioned one-half the programmed distance behind the zero point. A movement in the -X direction will cause the X axis to be positioned one-half the programmed distance in front of the zero point. 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). The X word format in a G04 command is 4.4, in seconds. Refer to G04 Dwell, page M-312C

35 U WORD - CAUTION - Programming a U axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike the workpiece or optional tailstock. 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 from the keyboard or tape, the control will act on the U command programmed closest to the End of Block character. The data word format is shown in the table on page 1-2. 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). The U word format in a G04 command is 4.4, in seconds. Refer to G04 Dwell, page M-312C 1-21

36 Z WORD - CAUTION - Programming a Z axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike the workpiece, or optional tailstock. The Z word is a distance command for the carriage. It is measured relative to the 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 from the keyboard or tape, the control will act on the Z command programmed closest to the End of Block character. The data word format is shown in the table on page 1-2. 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 face in relation to the 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 face 5 inches from the spindle face. A command of Z9. with a feedrate will cause the control to position the carriage with the turret face 9 inches from the spindle face. A work shift (zero offset) is used to establish a work coordinate system in which Z0 does not coincide with the spindle face. If Z0 for the work coordinate system used is not the 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-312C

37 W WORD - CAUTION - Programming a W axis move without the correct Tool Offset or Zero Offset active could cause the tool to strike the workpiece or optional tailstock. 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 from the keyboard or tape, the control will act on the W command programmed closest to the End of Block character. The data word format is shown in the table on page 1-2. W is positive when the carriage is programmed to move away from the spindle face. W is negative when the carriage is programmed to move toward the 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. 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. The data word format is shown in the table on page 1-2. Refer to Circular Interpolation, in Chapter 3. K WORD 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. The data word format is shown in the table on page 1-2. Refer to Circular Interpolation, in Chapter 3. M-312C 1-23

38 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. The data word format is R2.4 in inch mode and R3.3 in metric mode. 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. The data word format is R2.4 in inch mode and R3.3 in metric mode. 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. The data word format is R1.4 in inch mode and R2.3 in metric mode. Refer to Tool Nose Radius Compensation, in Chapter 2. 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: Canned Turning Cycle (G90), Chapter 6 Canned Threading Cycle (G92), Chapter 7 Canned Facing Cycle (G94), Chapter M-312C

39 P WORD The P word is used in the following functions: Automatic Finishing Cycle (G70), Chapter 6 Multiple Repetitive Rough Turning Cycle (G71), Chapter 6 Multiple Repetitive Rough Facing Cycle (G72), Chapter 6 Rough Pattern Repeat Cycle (G73), Chapter 6 Subprogram Calling, Chapter 8 Storing Work Shift from Program, Chapter 4 Storing Tool Offsets from Program, Chapter 4 The P word may also be used to establish a time factor for a G04 Dwell. The P word has the data word format P8 when used to specify dwell. Refer to G04 Dwell, page NOTE - Decimal Point programming cannot be used with the P word. Leading zero suppression must be used. When used with subprogram calling, the P word appears in the M98 calling block of the main part program and specifies the program I.D. number of the subprogram to be called. The data word format is P4. Leading zeros may be omitted. When used with tape entry of tool offsets or work shift offsets, the P word specifies the offset number and has the following numerical ranges: Work Shift: P00 when used with work shift offset Standard Tool Offsets: P01 to P16 when used with tool wear offsets P10001 to P10016 when used with tool geometry offsets Optional Tool Offsets: P01 to P32 when used with tool wear offsets P10001 to P10032 when used with tool geometry offsets Refer to Chapter 4 for information on storing tool offsets in memory. Q WORD The Q word is used in the following functions: Automatic Finishing Cycle (G70), Chapter 6 Multiple Repetitive Rough Turning Cycle (G71), Chapter 6 Multiple Repetitive Rough Facing Cycle (G72), Chapter 6 Rough Pattern Repeat Cycle (G73), Chapter 6 Storing Tool Offsets from Program, Chapter 4 Programming Multiple Start Threads, Chapter 7 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-312C 1-25

40 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. The word format is F3.2 for inch mode (G20) and F5.0 for metric mode (G21). The decimal point must be programmed. When used with the G99 command, it expresses the feedrate in inches or millimeters per revolution. The word format is F1.6 for inch mode (G20) and F3.4 for metric mode (G21). The decimal point must be programmed. If more than one feedrate is programmed in a data block, the last feedrate programmed will be the active feedrate. Due to the maximum feedrates on the X 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/rev) = inches per minute rev/min Maximum Feedrate (mm/rev) = mm per minute rev/min The maximum programmable feedrate for the X and Z axes is 400 inches per minute [10160 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. 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 8. When used in G97 direct rpm mode, the word format is S4. Maximum spindle speeds are listed in the table on page 1-2. The S word is modal and, once programmed, need not be programmed again until a different spindle speed is required. Do not program a decimal point with the S word M-312C

41 T WORD 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 G04 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. - CAUTION - 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. 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. - NOTE - When the Hardinge Safe-Start formats are used, it is not necessary to program T0" before indexing to a new turret station. T0" is included in the Safe-Start subprograms. Refer to Chapter 8 for information on Safe Start subprograms. Refer to Tool Offsets, in Chapter 4, for additional information. M-312C 1-27

42 M WORD The M words convey action to the machine. They are known as miscellaneous functions and are designated by a programmed M word having the format M2. 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. The following M codes have been assigned to Cobra series lathes equipped with the GE Fanuc 21T control: M00 Program Stop The M00 command stops the program, stops the spindle, and turns the coolant off. The Collet/Chuck 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, or M14 to restart the spindle or live tooling (Option) 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, or M14 to restart the spindle or live tooling (Option) and/or coolant pump when restarting the program after an M01 Optional Stop. M02 End of Program M02 indicates the end of a part program and is usually found in the last block programmed. It stops the spindle and turns the coolant off. The Collet Open/Close push button is enabled. Refer also to M30. M03 Spindle Forward The M03 command causes the 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 headstock end of the machine. M03 remains active until canceled by M00, M01, M02, M04, M05, M14, M30, or by pressing the Reset key or Emergency Stop push button. M04 Spindle Reverse The M04 command causes the 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 headstock end of the machine. M04 remains active until canceled by M00, M01, M02, M03, M05, M13, M30, or by pressing the Reset key or Emergency Stop push button M-312C

43 M05 Spindle Stop/Coolant OFF The M05 command causes the 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, M02, M30, Reset, and Emergency Stop. M08 Coolant ON M08 turns the coolant pump ON and remains active until canceled by M00, M01, M02, M05, M09, M30, Reset, or Emergency Stop. M09 Coolant OFF M09 turns the coolant pump OFF and remains active until canceled by M08, M13, or M14. M09 is active at machine start-up and is activated by M00, M01, M02, M05, M30, Reset, or Emergency Stop. M10 High Pressure Coolant ON (Cobra 65 lathes only) [Option] M10 turns the high pressure coolant ON if this option is activated. The spindle must be rotating and the guard door must be closed to turn high pressure coolant ON. M10 remains active until canceled by M00, M01, M02, M11, M30, or Emergency Stop. M11 High Pressure Coolant OFF (Cobra 65 lathes only) [Option] M11 turns the high pressure coolant OFF. M11 is active at machine start-up and remains active until canceled by M10. M13 Spindle Forward/Coolant ON The M13 command causes the spindle to run in the forward direction at the programmed spindle speed (S word) and turns the coolant pump ON. The spindle is running in the forward direction when rotating clockwise as viewed from the headstock end of the machine. M13 remains active until canceled by M00, M01, M02, M04, M05, M14, M30, or by pressing the Reset key or Emergency Stop push button. If M04 is programmed after M13, the spindle will run in the reverse direction and the coolant pump will remain ON. M14 Spindle Reverse/Coolant ON The M14 command causes the spindle to run in the reverse direction at the programmed spindle speed (S word) and turns the coolant pump ON. The spindle is running in the reverse direction when rotating counterclockwise as viewed from the headstock end of the machine. M14 remains active until canceled by M00, M01, M02, M04, M05, M13, M30, or by pressing the Reset key or Emergency Stop push button. If M03 is programmed after M14, the spindle will run in the forward direction and the coolant pump will remain ON. M-312C 1-29

44 M21 Open Collet The M21 command causes the collet closer to release the workpiece. M21 remains active until canceled by M22. M22 Close Collet The M22 command causes the collet closer to grip the workpiece. M22 remains active until canceled by M21. M25 Part Catcher Retract [Option] The M25 command causes the part catcher to move toward the machine headwall, away from the part pickup position. This is a linear motion. M26 Part Catcher Extend [Option] The M25 command causes the part catcher to move toward the part pickup position, away from the machine headwall. This is a linear motion. M28 External Chucking Mode M28 commands the control to use the collet closer with external-gripping style work-holding devices. The position of the collet closer is checked on power-up and the closer is initialized accordingly; for example, if the collet closer is open at power-up, it will remain open. Refer to the Cobra series lathe operator s manual (M-313C) for information on establishing chucking modes. M29 Internal Chucking Mode M29 commands the control to use the collet closer with internal-gripping style work-holding devices. The position of the collet closer is checked on power-up and the closer is initialized accordingly; for example, if the collet closer is open at power-up, it will remain open. Refer to the Cobra series lathe operator s manual (M-313C) for information on establishing chucking modes. M30 End of Program M30 indicates the end of a program and is usually found in the last block programmed. It stops the spindle, turns the coolant off, and rewinds the program to its beginning. The Collet Open/Close push button is enabled. Refer also to M02. M31 Program Rewind and Restart The M31 command causes the program to be restarted automatically, when followed by an M30 command M-312C

45 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 M02, M30, M48, a control OFF, or a control Reset. M61 Load New Bars If an M61 command is read by the CNC control and an End of Bar condition exists, the magazine bar feed system is commanded to load a new bar. If an M61 command is read by the CNC control and an End of Bar condition does not exist, program execution will continue. M84 Tailstock Quill Forward [Option] M84 causes the tailstock quill to move toward the machine spindle. Refer to Chapter 8 for information on programming the tailstock. M85/M86 Tailstock Quill Retract [Option] M85 causes the tailstock quill to move away from the machine spindle. M86 performs the same function. Refer to Chapter 8 for information on programming the tailstock. M93 Steady Rest Open [Option] M93 commands the steady rest to release the workpiece. M94 Steady Rest Closed [Option] M93 commands the steady rest to clamp the workpiece. 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 8. 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 8. M-312C 1-31

46 DIAMETER PROGRAMMING Hardinge Cobra series 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, Work Shift and Tool Offsets. - CAUTION - 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. Data word formats for diameter programming: X ±2.4 in inch mode (G20) and X ±3.3 in metric mode (G21). Maximum resolution is inches [.0005 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-312C

47 GENERAL PROGRAM FORMAT BEGINNING OF PROGRAM % Stop Code (End of Record) O Letter O and the Program Number G65 P9150 H Collet Dwell Macro (Cobra 42 lathes only) G20 or G21 Inch or Metric Mode N ( ) G97 S1000 M13 (or) M14 M98 P1 T X Z BEGINNING OF OPERATION Sequence Search Number and Message 1000 RPM and Spindle Direction Call: Safe Start Subprogram Index to Tool Station and Call Offset Move Tool To Activate Tool Offset G50 S G96 S IF USING CONSTANT SURFACE SPEED Maximum RPM Limit Surface Feet (Meters) Per Minute Speed IF USING TOOL NOSE RADIUS COMPENSATION G1 G41 (or) G42 X Z F100. Tool Nose Radius Compensation, Non-Cutting Move Required, IPM Feedrate G1 G99 X Z F Machine Part, Inches [mm] Per Revolution Feed X (and/or) Z M98 P1 (or) M98 P2 M01 Clear Part by 3 Times the Tool Tip Diameter Call: Safe O.D. or I.D. End Subprogram Operation Stop PROGRAM ENDING M30 Rewind Program - Stop Machine % Stop Code (End of Record) BAR JOB Activate Repeat Mode, on the Software Operator s Panel M-312C 1-33

48 - NOTES M-312C

49 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 +Z Z-AXIS TOUCH-OFF POINT TOOL NOSE REFERENCE POINT X-AXIS TOUCH-OFF POINT X-AXIS TOUCH-OFF POINT TI2373 Figure Tool Nose with X and Z-Axis Touch-off Points TI2374 Figure Tool Nose with an X-Axis Touch-off Point M-312C 2-1

50 TI2375 C(X.6 Z-.75) B(X.6 Z-.1732) 30 r= A(X.4 Z0.) +X START POINT (X.4 Z.2) C L.1732 Z ZERO +Z N40 G01 G99 ; N50 Z0. F.01 ; N60 X.6 Z ; N70 Z-.75 ; 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 (See Figure 2.3) 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 The tool does not reach the full depth of cut, represented by the dashed line in Figure 2.3. The actual cut, represented by the solid line parallel to the dashed 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-312C

51 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. 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 Tool Nose Radius Compensation entry block. The G41 or G42 Tool Nose Radius Compensation 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 Figure 2.6) The GE Fanuc 21T 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 2.7 for an comparison of programmed tool paths with and without Tool Nose Radius Compensation based on similar workpiece contours Spindle Face Turret Top Plate +X 5 7 +Z 1 SPINDLE 6 2 TURRET FACE TI2376 Figure Tool Nose Radius Orientation Codes -X +Z Centerline of I.D. Tool Holder +X +Z +X -Z Tool Reference Position Figure Tool Dimension Signs TI3637 M-312C 2-3

52 +X +X +Z +Z C L C L C L C L G41 G42 Figure G41/G42 Diagram TI2378 Compensation Compensation C L C L COMPENSATION NOT ACTIVE COMPENSATION ACTIVE Compensation Compensation C L C L TI2379 Figure Tool Path Comparisons 2-4 M-312C

53 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 2.8 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 2.9 for an illustration of incorrect axis motion and boxing the tool in. G42 EXIT WORKPIECE ENTRY G42 Figure Correct Axis Motion TI2380 G42 EXIT G42 ENTRY WORKPIECE TI2381 Figure Incorrect Axis Motion M-312C 2-5

54 SWITCHING G41/G42 CODE WITH TOOL NOSE RADIUS COMPENSATION ACTIVE - CAUTION - 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 compensation 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 below. 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 shown in Figure 2.10, G41 is activated in the move to Point A (Block N60). 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 Tool Nose Radius Compensation code to G42. No Z axis motion takes place as a result of the G41/G42 switch. If 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. A(X1.2 Z0.) B(X.8 Z0.) B (X.79 Z0.) A C(X0. Z0.) C L C (X-.01 Z0.) D(X.8 Z0.) B C(X0. Z0.) C L C (X-.01 Z0.) r=.01 N50 G00 G41 X1.2 Z.1 ; N60 G01 G99 Z0. F.01 ; N70 X-.02 ; N80 G42 ; N90 X.8 ; N100 Z-5. ; Figure Axis Reversal with Tool Nose Radius Compensation Active TI M-312C

55 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. Be aware of the tool nose radius overshoot at the end of the move prior to the reversal. CANNED TURNING AND FACING 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 (Figure 2.11): 1. 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. 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 Start Point G94 Canned Facing Cycle (Figure 2.12): 1. 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. 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. TI2383 Figure Axis Motion During a G90 Canned Turning Cycle with Tool Nose Radius Compensation Active Rapid Traverse Feed Start Point C L TI2384 Figure Axis Motion During a G94 Canned Facing Cycle with Tool Nose Radius Compensation Active M-312C 2-7

56 MODES IN WHICH TOOL NOSE RADIUS COMPENSATION IS NOT PERFORMED Tool Nose Radius Compensation is not performed in the G32 or G92 Threading Cycle. If Tool Nose Radius Compensation is active before this cycle is executed, Tool Nose Radius Compensation is deactivated during the cycle and then reactivated after the cycle is completed. 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 There are a number of alarm messages generated by the GE Fanuc control that relate to tool nose radius compensation. Refer to the GE Fanuc 21T operator s manual for an explanation of these alarm messages. DEACTIVATING TOOL NOSE RADIUS COMPENSATION To deactivate Tool Nose Radius Compensation, program a G40 along with a non-cutting linear move in both axes. As with Tool Nose Radius Compensation activation, it is important that the motion in this block be non-cutting due to the way Tool Nose Radius Compensation is interpolated. Alarm 034 Program will appear if circular motion is programmed in the exit block. Alarm 039 Program will appear if an Insert Chamfer or Insert Radius is programmed in the Tool Nose Radius Compensation exit block. 2-8 M-312C

57 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 during G32 or G92 threading. 6. 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. 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-312C 2-9

58 - NOTES M-312C

59 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 X and Z axes on Cobra series lathes is 400 inches per minute [10160 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: in/min rev/min = in/rev Metric: mm/min rev/min = mm/rev To convert in/rev [mm/rev] to in/min [mm/min], multiply the in/rev [mm/rev] feedrate by the programmed spindle speed: English: in/rev x rev/min = in/min Metric: mm/rev x rev/min = mm/min The machine operator has the capability of overriding programmed feedrates through the use of the Feedrate Override switch. The Feedrate Override switch is disabled during threading cycles, except when set to 0%. - CAUTION - If the machine operator sets the Feedrate Override switch is set to 0% during a threading cycle, X and Z axis motion will STOP. M-312C 3-1

60 ABSOLUTE AND INCREMENTAL PROGRAMMING In absolute programming, the X 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 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 W = Incremental distance on the Z axis W- = Toward the face of the spindle W+ = Away from the face of the 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 data word 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-312C

61 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 GE Fanuc 21T CNC 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. M-312C 3-3

62 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. 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 signed..010r.010r N15 G01 G99 X0. Z0. F.008 ;.010R N20 X.5 C-.01 ; N25 Z-.5 C.01 ; N30 X1. R-.01 ; N35 W-.5 R.01 ; N40 X1.5 R-.01 ; N45 Z-1.5 ; N50 Z-1.5 ; TI2367 Figure Insert Chamfer/Radius Sample Program 3-4 M-312C

63 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 signed. ALARM MESSAGES FOR INSERT CHAMFER/INSERT CORNER RADIUS Alarm 050: Chamfer or corner radius is commanded in a block which also includes a threadcutting command. Alarm 051: The move direction or move amount in the block following a block specifying a chamfer or corner radius was not adequate. Alarm 052: The block after a block specifying a chamfer or corner radius is not in G01 mode. (For example, the second block is in G02 or G03 mode). Alarm 053: C or R has been commanded more than once for the same corner or radius. Alarm 054: The next G01 block commands tapered motion (both X and Z data words are programmed) along with a command for inserting a chamfer or corner radius. Alarm 055: The axis motion in the second block is less than the chamfer or corner radius value specified in the first block. M-312C 3-5

64 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 ARC +X +R -R +Z +R -R Z(W) ±R X(U) +X -R -R +Z +R +R Figure Insert Chamfer/Insert Arc Diagram TI M-312C Revised: December 10, 1998

65 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 Tool motion during a G02 arc will appear clockwise, as viewed by the machine operator. G03 CounterClockwise Arc 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 3.4. 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, Tool Nose Radius Compensation. Sample Part Program Figure 3.3 illustrates a sample tool path and the basic program structure required for Circular Interpolation. The tool tip is programmed to move to the start point of each arc using G01 (Linear Interpolation). The program block commanding Circular Interpolation specifies the type of arc (G02 or G03), the end point of the arc, and the radius. G01 is programmed to cancel Circular Interpolation after each arc has been completed. M-312C 3-7

66 +X N7 N6 +Z N1 G1 G99 X0. Z0. F.01 ; N2 X1. ; N3 Z-1. ; N4 G2 X1.2 Z-1.1 R.1 ; N5 G1 X2. ; N6 G3 X2.5 Z-1.35 R.25 ; N7 G1 Z-2. ;.25 Radius N5 N4 N3.10 Radius N2 C L N1 (X0. Z0.) Figure Circular Interpolation Sample Program TI2702 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, alarm message 038 Program will appear on the control display screen. This 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. 3-8 M-312C

67 PARAMETER COMMAND DEFINITION Rotational Direction G02 G03 +X +X +Z +Z Definition (Tool Compensation Not Active) Incremental distance from the center of the tool nose radius at the start point to the arc center. Definition (Tool Compensation Active) Location of Arc Center I,K R IMPORTANT: This value must be signed. (Also note that this incremental distance depends on the size of the tool nose radius.) Refer to Figure 3.5. Radius of the arc. The 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.) Incremental distance from the 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 Figure 3.6. Radius of the arc. The 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 180 degrees. NOTE: The R word can only be used when the arc 180 degrees. Refer to Figure 3.5. Refer to Figure 3.6. X,Z Coordinates 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.) 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.) Location of Arc End Point U,W Refer to Figure 3.7. 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 Figure 3.7. Refer to Figure 3.8. Incremental distance from the arc start point to the arc end point as measured on the workpiece. (The incremental distance is independent of the size of the tool nose radius and geometric configuration of the tool nose.) Refer to Figure 3.8. Figure Circular Interpolation Parameters M-312C 3-9

68 R ARC CENTER K +X +Z TI2369 K I R I C L Figure Arc Center Parameters (Tool Nose Radius Compensation Not Active) C L ARC CENTER R ARC CENTER K +X +Z TI2371 I R I C L K C L ARC CENTER Figure Arc Center Parameters (Tool Nose Radius Compensation Active) 3-10 M-312C

69 W +X TI2370 (X,Z) ARC CENTER (X,Z) +Z U U W C L C L ARC CENTER Figure Arc End Point Parameters (Tool Nose Radius Compensation Not Active) W +X TI2372 (X,Z) ARC CENTER (X,Z) +Z U U W C L C L ARC CENTER Figure Arc End Point Parameters (Tool Nose Radius Compensation Active) M-312C 3-11

70 - NOTES M-312C

71 CHAPTER 4 - WORK SHIFT AND TOOL OFFSETS WORK SHIFT (Zero Offset) The work shift offset shifts the origin of the work coordinate system. Work Shift values (Z) are stored in the Work Shift file. The value stored in this file is active at all times. - CAUTION - The Work Shift file contains an X and a Z shift register. The X axis register in the Work Shift file should be set to zero at all times. The value entered into the Z axis Work Shift file must be a negative number. 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. Typically, the part length is stored as the Z Work Shift offset and the X Work Shift offset IS 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. TO STORE A WORK SHIFT OFFSET FROM THE PART PROGRAM The Work Shift offset may be input directly from the part program by using the G10 code. - CAUTION - The Work Shift file contains an X and a Z SHIFT VALUE register. It is strongly recommended that the X SHIFT VALUE register in the Work Shift file be set to zero at all times. Programming Format: G10 P0 X0 Z ; or G10 P0 X0 W ; P0: Selects the Work Shift offset as the offset file to be modified. X: Offset value on the X axis (absolute) Z: Offset value on the Z axis (absolute) W: Offset value on the Z axis (incremental) In an absolute command, the value(s) specified in addresses X and/or Z are set as the Work Shift Offset value. In an incremental command, the value specified in address W is added to the current Z Work Shift Offset. Use of this command in a program allows the work shift Z to advance incrementally. M-312C 4-1

72 TOOLING AND TOOL OFFSETS SQUARE SHANK TOOLS - NOTE - Hardinge Inc. recommends the exclusive use of left-hand tooling. This ensures that all cutting forces will be directed into the machine base, resulting in maximum tool life. Hardinge Cobra series lathes are designed to use qualified square shank tool holders. Since these tools are length, width, and height qualified, both set-up time and downtime due to tool replacement are greatly reduced. Qualified Tool Holders Qualified tool holder dimensions are held to ±.003 inch [.076 mm]. A left-hand square shank qualified tool holder is illustrated in Figure 4.1. Top Plate Configurations - NOTE - Hardinge Cobra series lathes are available with a Hardinge top plate or a VDI top plate. HARDINGE TOP PLATES Information relating to Hardinge top plates is available in Appendix One. Information relating to square shank tool holder assemblies designed for Hardinge top plates is available in Figure 4.1. VDI TOP PLATES Cobra 42 & 51 lathes can be equipped with VDI top plates conforming to DIN-69880, VDI30. Cobra 65 lathes can be equipped with VDI top plates conforming to DIN-69880, VDI40. Information relating to tool holder assemblies designed for VDI top plates should be obtained from the appropriate tooling catalog. 4-2 M-312C

73 +X +Z Turret Top Plate A Centerline of Tool Holder Mounting Hole B Turret X Axis Reference Position C E X Axis Tool Offset = 2 x (B + C) Z Axis Tool Offset = D + E Tool Tip Position D Turret Z Axis Reference Position TI3967 Figure Qualified Tool Holder for Square Shank Tools (Hardinge Top Plate) Cobra 42 & 51 Lathes Inches [Millimeters] Cobra 65 Lathe Inches [Millimeters] Dimension English Tools Metric Tools English Tools Metric Tools A.315 [8].315 [8].394 [10].394 [10] B [30.25] [30.25] [38.25] [38.25] C * * * * D * * * * E.772 [19.61].734 [18.64].915 [23.24].936 [23.77] * Refer to the specific tooling catalog for this dimension. M-312C 4-3

74 ROUND SHANK TOOLS Double Tool Holder Positioning - CAUTION - Read this section thoroughly before assigning turret stations for double tool holders on Cobra 42 & 51 lathes. On Cobra 42 & 51 lathes, DO NOT assign double round shank tool holders to turret stations that will be positioned 90 from the active turret station when commanding the turret top plate to a position close to the spindle face. A potential interference condition exists between the tool or double tool holder and the Z axis way cover wiper as the turret approaches the spindle. When programming operations that require the turret top plate to be close to the spindle face, be sure to assign any required double tool holders to turret stations other than the station positioned 90 from the spindle centerline. Refer to Figure 4.2 for the position of the interference condition in relation to the machine spindle. Refer to Figures 4.3 and 4.4 for photographs showing a tool in close proximity to the Z axis way cover wiper. +X -X Interference Position Active Turret Station Spindle Z Axis Way Cover Figure Double Tool Holder (Viewed from Headstock) TI4092 Figure Tool Interference TP3080 Figure Tool Interference (Close-Up View) TP M-312C