mazak Mazatrol Matrix Programming Manual

Download

PROGRAMMING MANUAL

Return to Library

for

MAZATROL MATRIX

(for Machining Centers)

EIA/ISO Program

MANUAL No. : H740PB0041E

Serial No. :

Before using this machine and equipment, fully understand the contents of this manual to ensure proper operation. Should any questions arise, please ask the nearest Technical Center or Technology Center.

IMPORTANT NOTICE

1. Be sure to observe the safety precautions described in this manual and the contents of the

safety plates on the machine and equipment. Failure may cause serious personal injury or material damage. Please replace any missing safety plates as soon as possible.

2. No modifications are to be performed that will affect operation safety. If such modifications are

required, please contact the nearest Technical Center or Technology Center.

3. For the purpose of explaining the operation of the machine and equipment, some illustrations

may not include safety features such as covers, doors, etc. Before operation, make sure all such items are in place.

4. This manual was considered complete and accurate at the time of publication, however, due to

our desire to constantly improve the quality and specification of all our products, it is subject to change or modification. If you have any questions, please contact the nearest Technical Center or Technology Center.

5. Always keep this manual near the machinery for immediate use.

6. If a new manual is required, please order from the nearest Technical Center or Technology

Center with the manual No. or the machine name, serial No. and manual name.

Issued by Manual Publication Section, Yamazaki Mazak Corporation, Japan

11. 2006

SAFETY PRECAUTIONS

Preface

Safety precautions relating to the CNC unit (in the remainder of this manual, referred to simply as the NC unit) that is provided in this machine are explained below. Not only the persons who create programs, but also those who operate the machine must thoroughly understand the contents of this manual to ensure safe operation of the machine.

Read all these safety precautions, even if your NC model does not have the corresponding functions or optional units and a part of the precautions do not apply.

Rule

1. This section contains the precautions to be observed as to the working methods and states usually expected. Of course, however, unexpected operations and/or unexpected working states may take place at the user site. During daily operation of the machine, therefore, the user must pay extra careful attention to its own working safety as well as to observe the precautions described below.

2. Although this manual contains as great an amount of information as it can, since it is not rare for the user to perform the operations that overstep the manufacturer-assumed ones, not all of “what the user cannot perform” or “what the user must not perform” can be fully covered in this manual with all such operations taken into consideration beforehand. It is to be understood, therefore, that functions not clearly written as “executable” are “inexecutable” functions.

SAFETY PRECAUTIONS

3. The meanings of our safety precautions to DANGER, WARNING, and CAUTION are as follows:

: Failure to follow these instructions could result in loss of life.

DANGER

: Failure to observe these instructions could result in serious harm to a human

life or body.

WARNING

: Failure to observe these instructions could result in minor injuries or serious

machine damage.

CAUTION

HGENPA0043E

S-1

Basics

SAFETY PRECAUTIONS

! After turning power on, keep hands away from the keys, buttons, or switches of the

operating panel until an initial display has been made.

WARNING

! Before proceeding to the next operations, fully check that correct data has been entered

and/or set. If the operator performs operations without being aware of data errors, unexpected operation of the machine will result.

! Before machining workpieces, perform operational tests and make sure that the machine

operates correctly. No workpieces must be machined without confirmation of normal operation. Closely check the accuracy of programs by executing override, single-block, and other functions or by operating the machine at no load. Also, fully utilize tool path check, Virtual Machining, and other functions, if provided.

! Make sure that the appropriate feed rate and rotational speed are designated for the

particular machining requirements. Always understand that since the maximum usable fee d rate and rotational speed are determined by the specifications of the tool to be used, those of the workpiece to be machined, and various other factors, actual capabilities differ from the machine specifications listed in this manual. If an inappropriate feed rate or rotational speed is designated, the workpiece or the tool may abruptly move out from the machine.

! Before executing correction functions, fully check that the direction and amount of

correction are correct. Unexpected operation of the machine will result if a correction function is executed without its thorough understanding.

! Parameters are set to the optimum standard machining conditions prior to shipping of the

machine from the factory. In principle, these settings should not be modified. If it becomes absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the functions of the corresponding parameters. Modifications usually affect any program. Unexpected operation of the machine will result if the settings are modified without a thorough understanding.

Remarks on the cutting conditions recommended by the NC

! Before using the following cutting conditions:

- Cutting conditions that are the result of the MAZATROL Automatic Cutting Conditions

WARNING

Determination Function

- Cutting conditions suggested by the Machining Navigation Function

- Cutting conditions for tools that are suggested to be used by the Machining Navigation

Function

Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiece fixturing/clamping and tool setup.

! Confirm that the machine door is securely closed before starting machining.

Failure to confirm safe machine setup may result in serious injury or death.

S-2

Programming

WARNING

SAFETY PRECAUTIONS

! Fully check that the settings of the coordinate systems are correct. Even if the designated

program data is correct, errors in the system settings may cause the machine to operate in unexpected places and the workpiece to abruptly move out from the machine in the event of contact with the tool.

! During surface velocity hold control, as the current workpiece coordinates of the surface

velocity hold control axes approach zeroes, the spindle speed increases significantly. For the lathe, the workpiece may even come off if the chucking force decreases. Safety speed limits must therefore be observed when designating spindle speeds.

! Even after inch/metric system selection, the units of the programs, tool information, or

parameters that have been registered until that time are not converted. Fully check these data units before operating the machine. If the machine is operated without checks being performed, even existing correct programs may cause the machine to operate differently from the way it did before.

! If a program is executed that includes the absolute data commands and relative data

commands taken in the reverse of their original meaning, totally unexpected operation of the machine will result. Recheck the command scheme before executing programs.

! If an incorrect plane selection command is issued for a machine action such as arc

interpolation or fixed-cycle machining, the tool may collide with the workpiece or part of the machine since the motions of the control axes assumed and those of actual ones will be interchanged. (This precaution applies only to NC units provided with EIA functions.)

! The mirror image, if made valid, changes subsequent machine actions significantly. Use

the mirror image function only after thoroughly understanding the above. (This precaution applies only to NC units provided with EIA functions.)

! If machine coordinate system commands or reference position returning commands are

issued with a correction function remaining made valid, correction may become invalid temporarily. If this is not thoroughly understood, the machine may appear as if it would operate against the expectations of the operator. Execute the above commands only after making the corresponding correction function invalid. (This precaution applies only to NC units provided with EIA functions.)

! The barrier function performs interference checks based on designated tool data. Enter the

tool information that matches the tools to be actually used. Otherwise, the barrier function will not work correctly.

! The system of G-code and M-code commands differs, especially for turning, between the

machines of INTEGREX e-Series and the other turning machines. Issuance of the wrong G-code or M-code command results in totally non-intended machine operation. Thoroughly understand the system of G-code and M-code commands before using this system.

Sample program Machines of INTEGREX e-Series Turning machines

S1000M3 S1000M203

The milling spindle rotates at 1000 min–1. The turning spindle rotates at 1000 min–1. The turning spindle rotates at 1000 min–1. The milling spindle rotates at 1000 min–1.

S-3

SAFETY PRECAUTIONS

! For the machines of INTEGREX e-Series, programmed coordinates can be rotated using

an index unit of the MAZATROL program and a G68 command (coordinate rotate command) of the EIA program. However, for example, when the B-axis is rotated through 180 degrees around the Y-axis to implement machining with the turning spindle No. 2, the plus side of the X-axis in the programmed coordinate system faces downward and if the program is created ignoring this fact, the resulting movement of the tool to unexpected positions may incite collisions. To create the program with the plus side of the X-axis oriented in an upward direction, use the mirror function of the WPC shift unit or the mirror imaging function of G-code command (G50.1, G51.1).

! After modifying the tool data specified in the program, be sure to perform the tool path

check function, the Virtual Machining function, and other functions, and confirm that the program operates properly. The modification of tool data may cause even a field-proven machining program to change in operational status. If the user operates the machine without being aware of any changes in program status, interference with the workpiece could arise from unexpected operation. For example, if the cutting edge of the tool during the start of automatic operation is present inside the clearance-including blank (unmachined workpiece) specified in the common unit of the MAZATROL program, care is required since the tool will directly move from that position to the approach point because of no obstructions being judged to be present on this path. For this reason, before starting automatic operation, make sure that the cutting edge of the tool during the start of automatic operation is present outside the clearance-including workpiece specified in the common unit of the MAZATROL program.

CAUTION

! If axis-by-axis independent positioning is selected and simultaneously rapid feed selected

for each axis, movements to the ending point will not usually become linear. Before using these functions, therefore, make sure that no obstructions are present on the path.

! Before starting the machining operation, be sure to confirm all contents of the program

obtained by conversion. Imperfections in the program could lead to machine damage and operator injury.

S-4

Operations

WARNING

SAFETY PRECAUTIONS

! Single-block, feed hold, and override functions can be made invalid using system variables

#3003 and #3004. Execution of this means the important modification that makes the corresponding operations invalid. Before using these variables, therefore, give thorough notification to related persons. Also, the operator must check the settings of the system variables before starting the above operations.

! If manual intervention during automatic operation, machine locking, the mirror image

function, or other functions are executed, the workpiece coordinate systems will usually be shifted. When making machine restart after manual intervention, machine locking, the mirror image function, or other functions, consider the resulting amounts of shift and take the appropriate measures. If operation is restarted without any appropriate measures being taken, collision with the tool or workpiece may occur.

! Use the dry run function to check the machine for normal operation at no load. Since the

feed rate at this time becomes a dry run rate different from the program-designated feed rate, the axes may move at a feed rate higher than the programmed value.

! After operation has been stopped temporarily and insertion, deletion, updating, or other

commands executed for the active program, unexpected operation of the machine may result if that program is restarted. No such commands should, in principle, be issued for the active program.

CAUTION

! During manual operation, fully check the directions and speeds of axial movement. ! For a machine that requires manual homing, perform manual homing operations after

turning power on. Since the software-controlled stroke limits will remain ineffective until manual homing is completed, the machine will not stop even if it oversteps the limit area. As a result, serious machine damage will result.

! Do not designate an incorrect pulse multiplier when performing manual pulse handle feed

operations. If the multiplier is set to 1000 times and the handle operated inadvertently, axial movement will become faster than that expected.

S-5

BEFORE USING THE NC UNIT

Limited Warranty

The warranty of the manufacturer does not cover any trouble arising if the NC unit is used for its non-intended purpose. Take notice of this when operating the unit.

Examples of the trouble arising if the NC unit is used for its non-intended purpose are listed below.

1. Trouble associated with and caused by the use of any commercially available software products (including user-created ones)

2. Trouble associated with and caused by the use of any Windows operating systems

3. Trouble associated with and caused by the use of any commercially available computer equipment

Operating Environment

1. Ambient temperature

During machine operation: 0° to 50°C (32° to 122°F)

2. Relative humidity

During machine operation: 10 to 75% (without bedewing) Note: As humidity increases, insulation deteriorates causing electrical component parts to

deteriorate quickly.

Keeping the Backup Data

Note: Do not attempt to delete or modify the data stored in the following folder.

Recovery Data Storage Folder: D:\MazakBackUp

Although this folder is not used when the NC unit is running normally, it contains important data that enables the prompt recovery of the machine if it fails.

If this data has been deleted or modified, the NC unit may require a long recovery time. Be sure not to modify or delete this data.

S-6

CONTENTS

Page

1 CONTROLLED AXES........................................................................... 1-1

1-1 Coordinate Words and Controlled Axes ............................................................. 1-1

2 UNITS OF PROGRAM DATA INPUT................................................... 2-1

2-1 Units of Program Data Input...............................................................................2-1

2-2 Units of Data Setting...........................................................................................2-1

2-3 Ten-Fold Program Data......................................................................................2-1

3 DATA FORMATS.................................................................................. 3-1

3-1 Tape Codes........................................................................................................3-1

3-2 Program Formats ...............................................................................................3-5

3-3 Tape Data Storage Format................................................................................. 3-6

3-4 Optional Block Skip ............................................................................................3-6

3-5 Program Number, Sequence Number and Block Number: O, N ........................3-7

3-6 Parity-H/V...........................................................................................................3-8

3-7 List of G-Codes ................................................................................................3-10

4 BUFFER REGISTERS.......................................................................... 4-1

4-1 Input Buffer.........................................................................................................4-1

4-2 Preread Buffer.................................................................................................... 4-2

5 POSITION PROGRAMMING................................................................ 5-1

5-1 Dimensional Data Input Method.........................................................................5-1

5-1-1 Absolute/Incremental data input: G90/G91............................................................. 5-1

C-1

5-2 Inch/Metric Selection: G20/G21..........................................................................5-3

5-3 Decimal Point Input ............................................................................................5-4

6 INTERPOLATION FUNCTIONS........................................................... 6-1

6-1 Positioning (Rapid Feed): G00...........................................................................6-1

6-2 One-Way Positioning: G60.................................................................................6-4

6-3 Linear Interpolation: G01....................................................................................6-5

6-4 Circular Interpolation: G02, G03.........................................................................6-6

6-5 Radius Designated Circular Interpolation: G02, G03..........................................6-9

6-6 Spiral Interpolation: G2.1, G3.1 (Option)..........................................................6-11

6-7 Plane Selection: G17, G18, G19......................................................................6-19

6-7-1 Outline .................................................................................................................. 6-19

6-7-2 Plane selection methods....................................................................................... 6-19

6-8 Virtual-Axis Interpolation: G07..........................................................................6-21

6-9 Spline Interpolation: G06.1 (Option).................................................................6-22

6-10 NURBS Interpolation: G06.2 (Option)...............................................................6-33

6-11 Cylindrical Interpolation: G07.1 ........................................................................6-40

6-12 Helical Interpolation: G02, G03 ........................................................................6-49

7 FEED FUNCTIONS.............................................................................. 7-1

7-1 Rapid Traverse Rates.........................................................................................7-1

7-2 Cutting Feed Rates.............................................................................................7-1

7-3 Asynchronous/Synchronous Feed: G94/G95.....................................................7-1

7-4 Selecting a Feed Rate and Effects on Each Control Axis...................................7-3

C-2

7-5 Automatic Acceleration/Deceleration..................................................................7-6

7-6 Speed Clamp......................................................................................................7-7

7-7 Exact-Stop Check: G09......................................................................................7-7

7-8 Exact-Stop Check Mode: G61..........................................................................7-10

7-9 Automatic Corner Override: G62...................................................................... 7-10

7-10 Tapping Mode: G63 ..........................................................................................7-15

7-11 Cutting Mode: G64 ...........................................................................................7-15

7-12 Geometry Compensation/Accuracy Coefficient: G61.1/,K................................7-16

7-12-1 Geometry compensation function: G61.1.............................................................7-16

7-12-2 Accuracy coefficient (,K)....................................................................................... 7-17

7-13 Inverse Time Feed: G93 (Option).....................................................................7-18

8 DWELL FUNCTIONS ........................................................................... 8-1

8-1 Dwell Command in Time: (G94) G04..................................................................8-1

8-2 Dwell Command in Number of Revolutions: (G95) G04.....................................8-2

9 MISCELLANEOUS FUNCTIONS......................................................... 9-1

9-1 Miscellaneous Functions (M3-Digit)....................................................................9-1

9-2 No. 2 Miscellaneous Functions (A8/B8/C8-Digit)................................................9-2

10 SPINDLE FUNCTIONS ...................................................................... 10-1

10-1 Spindle Function (S5-Digit Analog)...................................................................10-1

10-2 Spindle Clamp Speed Setting: G92..................................................................10-1

11 TOOL FUNCTIONS............................................................................ 11-1

11-1 Tool Function (4-Digit T-Code).........................................................................11-1

C-3

11-2 Tool Function (8-Digit T-Code).........................................................................11-1

12 TOOL OFFSET FUNCTIONS............................................................. 12-1

12-1 Tool Offset........................................................................................................12-1

12-2 Tool Length Offset/Cancellation: G43, G44, or T-Code/G49............................12-5

12-3 Tool Position Offset: G45 to G48......................................................................12-7

12-4 Tool Diameter Offset Function: G40, G41, G42 .............................................12-13

12-4-1 Overview............................................................................................................. 12-13

12-4-2 Tool diameter offsetting...................................................................................... 12-13

12-4-3 Tool diameter offsetting operation using other commands................................. 12-22

12-4-4 Corner movement............................................................................................... 12-29

12-4-5 Interruptions during tool diameter offsetting ....................................................... 12-29

12-4-6 General precautions on tool diameter offsetting................................................. 12-31

12-4-7 Offset number updating during the offset mode ................................................. 12-32

12-4-8 Excessive cutting due to tool diameter offsetting................................................ 12-34

12-4-9 Interference check.............................................................................................. 12-36

12-5 Three-Dimensional Tool Diameter Offsetting (Option)....................................12-43

12-5-1 Function description............................................................................................ 12-43

12-5-2 Programming methods ....................................................................................... 12-44

12-5-3 Correlationships to other functions..................................................................... 12-48

12-5-4 Miscellaneous notes on three-dimensional tool diameter offsetting................... 12-48

12-6 Programmed Data Setting: G10.....................................................................12-49

12-7 Tool Offsetting Based on MAZATROL Tool Data...........................................12-57

12-7-1 Selection parameters.......................................................................................... 12-57

12-7-2 Tool length offsetting .......................................................................................... 12-58

C-4

12-7-3 Tool diameter offsetting...................................................................................... 12-59

12-7-4 Tool data update (during automatic operation)................................................... 12-60

12-8 Shaping Function (Option)..............................................................................12-61

12-8-1 Overview............................................................................................................. 12-61

12-8-2 Programming format........................................................................................... 12-62

12-8-3 Detailed description............................................................................................ 12-62

12-8-4 Remarks ............................................................................................................. 12-69

12-8-5 Compatibility with the other functions.................................................................12-70

12-8-6 Sample program.................................................................................................12-71

13 PROGRAM SUPPORT FUNCTIONS................................................. 13-1

13-1 Hole Machining Pattern Cycles: G34.1/G35/G36/G37.1...................................13-1

13-1-1 Overview............................................................................................................... 13-1

13-1-2 Holes on a circle: G34.1 ....................................................................................... 13-2

13-1-3 Holes on a line: G35............................................................................................. 13-3

13-1-4 Holes on an arc: G36............................................................................................ 13-4

13-1-5 Holes on a grid: G37.1.......................................................................................... 13-5

13-2 Fixed Cycles.....................................................................................................13-7

13-2-1 Outline .................................................................................................................. 13-7

13-2-2 Fixed-cycle machining data format....................................................................... 13-8

13-2-3 G71.1 (Chamfering cutter CW)........................................................................... 13-11

13-2-4 G72.1 (Chamfering cutter CCW) ........................................................................ 13-12

13-2-5 G73 (High-speed deep-hole drilling)................................................................... 13-13

13-2-6 G74 (Reverse tapping) ....................................................................................... 13-14

13-2-7 G75 (Boring).......................................................................................................13-15

C-5

13-2-8 G76 (Boring).......................................................................................................13-16

13-2-9 G77 (Back spot facing)....................................................................................... 13-17

13-2-10 G78 (Boring) ....................................................................................................... 13-18

13-2-11 G79 (Boring) ....................................................................................................... 13-19

13-2-12 G81 (Spot drilling)............................................................................................... 13-19

13-2-13 G82 (Drilling)....................................................................................................... 13-20

13-2-14 G83 (Deep-hole drilling)...................................................................................... 13-21

13-2-15 G84 (Tapping)..................................................................................................... 13-22

13-2-16 G85 (Reaming) ................................................................................................... 13-23

13-2-17 G86 (Boring) ....................................................................................................... 13-23

13-2-18 G87 (Back boring)............................................................................................... 13-24

13-2-19 G88 (Boring) ....................................................................................................... 13-25

13-2-20 G89 (Boring) ....................................................................................................... 13-25

13-2-21 Synchronous tapping (Option)............................................................................ 13-26

13-3 Initial Point and R-Point Level Return: G98 and G99 .....................................13-30

13-4 Scaling ON/OFF: G51/G50.............................................................................13-31

13-5 Mirror Image ON/OFF: G51.1/G50.1..............................................................13-44

13-6 Subprogram Control: M98, M99 .....................................................................13-45

13-7 End Processing: M02, M30, M998, M999.......................................................13-52

13-8 Linear Angle Commands................................................................................13-53

13-9 Macro Call Function: G65, G66, G66.1, G67..................................................13-54

13-9-1 User macros ....................................................................................................... 13-54

13-9-2 Macro call instructions........................................................................................ 13-55

13-9-3 Variables............................................................................................................. 13-64

C-6

13-9-4 Types of variables............................................................................................... 13-66

13-9-5 Arithmetic operation commands.........................................................................13-84

13-9-6 Control commands.............................................................................................. 13-88

13-9-7 External output commands (Output via RS-232C).............................................. 13-92

13-9-8 External output command (Output onto the hard disk)....................................... 13-94

13-9-9 Precautions......................................................................................................... 13-96

13-9-10 Specific examples of programming using user macros ...................................... 13-98

13-10 Geometric Commads (Option)......................................................................13-102

13-11 Corner Chamfering and Corner Rounding Commands.................................13-103

13-11-1 Corner chamfering ( , C_)................................................................................. 13-103

13-11-2 Corner rounding ( ,R_)...................................................................................... 13-105

14 COORDINATE SYSTEM SETTING FUNCTIONS.............................. 14-1

14-1 Fundamental Machine Coordinate System, Workpiece Coordinate

Systems, and Local Coordinate Systems.........................................................14-1

14-2 Machine Zero Point and Second, Third, and Fourth Reference Points.............14-2

14-3 Fundamental Machine Coordinate System Selection: G53..............................14-3

14-4 Coordinate System Setting: G92......................................................................14-4

14-5 Automatic Coordinate System Setting..............................................................14-5

14-6 Reference Point Return: G28, G29 ..................................................................14-6

14-7 Second, Third, or Fourth Reference Point Return: G30....................................14-8

14-8 Reference Point Check Command: G27 ........................................................14-10

14-9 Workpiece Coordinate System Setting and Selection: (G92) G54 to G59......14-11

14-10 Additional Workpiece Coordinate System Setting and Selection: G54.1........14-16

C-7

14-11 Local Coordinate System Setting: G52...........................................................14-22

14-12 Reading/Writing of MAZATROL Program Basic Coordinates.........................14-27

14-12-1 Calling a macroprogram (for data writing) .......................................................... 14-27

14-12-2 Data reading ....................................................................................................... 14-27

14-12-3 Rewriting............................................................................................................. 14-28

14-13 Workpiece Coordinate System Rotation.........................................................14-29

14-14 Three-Dimensional Coordinate Conversion: G68...........................................14-42

15 MEASUREMENT SUPPORT FUNCTIONS........................................ 15-1

15-1 Skip Function: G31...........................................................................................15-1

15-1-1 Function description.............................................................................................. 15-1

15-2 Skip Coordinate Reading..................................................................................15-2

15-3 Amount of coasting in the execution of a G31 block.........................................15-3

15-4 Skip coordinate reading error...........................................................................15-4

15-5 Multi-Step Skip: G31.1, G31.2, G31.3, G04 .....................................................15-5

16 PROTECTIVE FUNCTIONS............................................................... 16-1

16-1 Pre-move Stroke Check ON/OFF: G22/G23 ....................................................16-1

17 THREADING: G33 (Option)................................................................ 17-1

17-1 Equal-Lead Threading......................................................................................17-1

17-2 Continuous Threading......................................................................................17-4

17-3 Inch Threading .................................................................................................17-4

18 DYNAMIC OFFSETTING: M173, M174 (Option) ............................... 18-1

C-8

19 HIGH-SPEED SMOOTHING CONTROL FUNCTION (OPTION)....... 19-1

19-1 Programming Format........................................................................................19-2

19-2 Commands Available in the High-Speed Smoothing Control Mode .................19-2

19-3 Additional Functions in the High-Speed Smoothing Control Mode...................19-3

19-4 Related Parameters..........................................................................................19-4

19-5 Remarks...........................................................................................................19-4

19-6 Related Alarms.................................................................................................19-4

20 FUNCTION FOR SELECTING THE CUTTING CONDITIONS........... 20-1

21 TORNADO TAPPING (G130)............................................................. 21-1

22 HIGH-SPEED MACHINING MODE FEATURE (OPTION)................. 22-1

23 AUTOMATIC TOOL LENGTH MEASUREMENT: G37 (OPTION) ..... 23-1

24 DYNAMIC OFFSETTING II: G54.2P0, G54.2P1 - G54.2P8

(OPTION)............................................................................................ 24-1

25 EIA/ISO PROGRAM DISPLAY........................................................... 25-1

25-1 Procedures for Constructing an EIA/ISO Program ...........................................25-1

25-2 Editing Function of EIA/ISO PROGRAM Display..............................................25-2

25-2-1 General................................................................................................................. 25-2

25-2-2 Operation procedure............................................................................................. 25-2

25-3 Macro-Instruction Input.....................................................................................25-8

25-4 Division of Display (Split Screen)......................................................................25-9

25-5 Editing Programs Stored in External Memory Areas ......................................25-12

C-9

- NOTE -

C-10

1 CONTROLLED AXES

1-1 Coordinate Words and Controlled Axes

Under standard specifications, there are three-dimensional controlled axes. With an added feature and a special option, the machine can control up to a maximum of six axes, including the three fundamental axes. The direction of machining can be designated using a predetermined coordinate word consisting of an alphabetic character.

For X-Y table

CONTROLLED AXES 1

+Y +X

Program coordinates

Workpiece X-Y table

For X-Y table and turntable

Table moving directions

Bed

MEP001

Table moving directions

Workpiece

Table turning direction

1-1

+Y +X

Program coordinates

MEP002

1 CONTROLLED AXES

- NOTE -

1-2

2 UNITS OF PROGRAM DATA INPUT

2-1 Units of Program Data Input

The movements on coordinate axes are to be commanded in the MDI mode or machining program. The movement data are expressed in millimeters, inches or degrees.

2-2 Units of Data Setting

Various data commonly used for control axes, such as offsetting data, must be set for the machine to perform an operation as desired. The units of data setting and those of program data input are listed below.

UNITS OF PROGRAM DATA INPUT 2

Units of program data input 0.0001 mm 0.00001 in. 0.0001 deg Units of data setting 0.0001 mm 0.00001 in. 0.0001 deg

Note 1: Inch/metric selection can be freely made using either bit 4 of parameter F91 (“0” for

metric, “1” for inches; validated through power-off and -on) or G-code command s (G20, G21). Selection using the G-code commands is valid only for program data input. Variables and offsetting data (such as tool offsetting data) should therefore be set beforehand using the appropriate unit (inch or metric) for the particular machining requirements.

Note 2: Metric data and inch data cannot be used at the same time.

2-3 Ten-Fold Program Data

Using a predetermined parameter, machining program data can be processed as set in units of one micron. There may be cases that a machining program which has been set in units of one micron is to be used with a numerical control unit based on 0.1 micron increment s. In such cases, use of this parameter allows the machine to perform the required machining operations without rewriting the program. Use bit 0 of user parameter F91 for this purpose. All types of coordinate data (axis movement data) not provided with the decimal point will be multiplied by a factor of 10. This does not apply, indeed, to preset tool-offsetting data designated with addresses H and D.

Linear axis

Metric system Inch system

Rotational axis

Linear axis

Rotational axis

Program

command

X1 (Y1 / Z1)

Moving distance when program commands are executed

NC (A) for which the

program was prepared

1 micron 0.1 micron 1 micron Applicable

0.001° 0.0001° 0.001° Applicable

Bit 0 of F91 = 0 Bit 0 of F91 = 1

MAZATROL (B)Controlled axis

2-1

Program

applicability

(A) → (B)

2 UNITS OF PROGRAM DATA INPUT

- NOTE -

2-2

3 DATA FORMATS

3-1 Tape Codes

This numerical control unit (in the remainder of this manual, referred to as the NC unit) uses

command information that consists of letters of the alphabet (A, B, C .... Z), numerics (0, 1, 2 ....

9), and signs (+, –, /, and so on). These alphanumerics and signs are referred to collectively as

characters. On paper tape, these characters are represented as a combination of a maximum of eight punched holes. Such a representation is referred to as a code. The NC unit uses either the EIA codes (RS-244-A) or the ISO codes (R-840).

Note 1: Codes not included in the tape codes shown in Fig. 3-1 will result in an error when they

are read.

Note 2: Of all codes specified as the ISO codes but not specified as the EIA codes, only the

following codes can be designated using the data I/O (Tape) parameters TAP9 to TAP14:

[ Bracket Open ] Bracket Close # Sharp ∗ Asterisk = Equal sign

:Colon However, you cannot designate codes that overlap existing ones or that result in parity error.

DATA FORMATS 3

Note 3: EIA/ISO code identification is made automatically according to the first EOB/LF code

appearing after the NC unit has been reset. (EOB: End Of Block, LF: Line Feed)

1. Significant information area (LABEL SKIP function)

During tape-based automatic operation, data storage into the memory, or data searching, the NC unit will ignore the entire information up to the first EOB code (;) in the tape when the unit is turned on or reset. That is, significant information in a tape refers to the information contained in the interval from the time a character or numeric code appears, following the first EOB code (;) after the NC unit has been reset, until a reset command is given.

2. Control Out, Control In

The entire information in the area from Control Out “(” to Control In “)” will be ignored in regard to machine control, while they will surely be displayed on the data display unit. Thus, this area can be used to contain information, such as the name and number of the command tape, that is not directly related to control. During tape storage, however, the information in this area will also be stored. The NC unit will enter the Control In status when power is turned on.

3-1

3 DATA FORMATS

Example of EIA Code

Control InControl Out

CON

P R 1 10

Name of tape is printed out

CON

1 1 1 1

Name of tape is punched in captital letters.

D E

R R R O

N U

.ONMARGO

N UL1

E O

1 1

E L

2DE

LCI

MEP003

Example of ISO Code

OBG0 X–8500 0 640 C U T T E R

Operator information is printed out.

Control Out

0 0 0

0 0 0G0 X 500 0 40 C U T T E R

(

The information at this portion is ignored and nothing is executed.

E T U R N )–

E T U R NR

Control In

E O B

3. EOR code (%)

In general, the EOR (End Of Record) code is punched at both ends of a tape and has the following functions:

- To stop rewinding (only when a rewinding device is provided)

- To start rewinding during tape data search (only when a rewinding device is provided)

- To terminate the storage of tape data.

MEP004

3-2

DATA FORMATS 3

4. Tape creation method for tape operation (Only when a rewinding device is used)

;

10 cm

2m First block Last block 2m

!!!!!!!!!

; ;

!!!!!!!!!

;

10 cm %%

TEP005

The two meters of dummy at both ends and the EOR (%) at the head are not required when a rewinding device is not used.

3-3

3 DATA FORMATS

EIA/ISO identification is made automatically by detecting whether EOB or LF initially appears after the NC unit has been reset.

EIA code (RS-244-A)

Feed holes

87654 321

Channel number

1 2 3 4 5 6 7 8 9 0

B C D E F G H I J K L M N O P Q R S T U V W X Y Z + – . , / EOR (End of Record) EOB (End of Block) or CR CO (2+4+5) CI (2+4+7)

Definable in parameters

BS (Back Space) TAB SP (Space) &

DEL (Delete)

S (All Space=Feed)* M (All Mark=EOB+DEL)*

ISO code (R-840)

Feed holes

87654 321

Channel number

1 2 3 4 5 6 7 8 9 0

B C D E F G H I J K L M N O P Q R S T U V W X Y Z + – . , / % LF (Line Feed) or NL ( (Control Out) ) (Control In) : # ? = [ ]

BS (Back Space) HT (Horizontal Tab) SP (Space) & CR (Carriage Return) $ ' (Apostrophe) ; < > ? @

" DEL (Delete) NULL DEL (Delete)

[1]

[2]

* The codes asterisked above are not EIA codes,

but may be used for the convenience’s sake.

Fig. 3-1 Tape codes

LF or NL acts as EOB and % acts as EOR.

MEP006

3-4

Codes in section [1] will only be stored as tape data when they are present in a comment section,

and ignored elsewhere in the significant information area. Codes in section [2] are non-operative and will always be ignored (but undergo the parity-V check). A dotted area indicates that the EIA Standard provides no corresponding codes.

3-2 Program Formats

A format predetermined for assigning control information to the NC unit is referred to as a program format. The program format used for our NC unit is word address format.

1. Words and addresses

A word is a set of characters arranged as shown below, and information is pro ce ssed in words.

DATA FORMATS 3

Word

Numeral

lphabet (address)

Word configuration

The alphabetic character at the beginning of a word is referred to as an address, which defines the meaning of its succeeding numeric information.

Table 3-1 Type and format of words

Item Metric command Inch command Program No. O8 Sequence No. N5 Preparatory function

Moving axis

Auxiliary axis

Dwell

Feed

Fixed cycle

Tool offset Miscellaneous function M3 × 4 Spindle function S5 Tool function No. 2 miscellaneous function B8, A8 or C8 Subprogram Variables number #5

Input unit

0.0001 mm (deg.),

0.00001 in.

0.0001 mm (deg.),

0.00001 in.

0.001 mm (rev),

0.0001 in.

0.0001 mm (deg.),

0.00001 in.

0.0001 mm (deg.),

0.00001 in.

X+54 Y+54 Z+54 α+54 X+45 Y+45 Z+45 α+45

I+54 J+54 K+54 I+45 J+45 K+45

F54 (per minute) F33 (per revolution)

R+54 Q54 P8 L4 R+45 Q45 P8 L4

G3 or G21

X54 P8 U54

F45 (per minute) F24 (per revolution)

H3 or D3

T4 or T8

P8 H5 L4

3-5

3 DATA FORMATS

1. Code O8 here indicates that program number can be set as an unsigned integer of eight digits following O, and for X+54, “+” indicates that the value can be signed (negative) and the two-digit number (54) indicates that the decimal point can be used and that five digits before and four after the decimal point are effective (5 + 4 = 9 digits are effective for a designation without decimal point).

2. The alpha sign ( rotational axis.

3. The number of digits in the words is checked by the maximum number of digits in the addresses.

4. When data with decimal point is used for address for which decimal input is not available, decimal figures will be ignored.

5. If the number of integral digits exceeds the specified format, an alarm will result.

6. If the number of decimal digits exceed the specified format, the excess will be rounded.

2. Blocks

A block, unit of instruction, contains a number of words which constitute information necessary for the NC machine to perform an operation. The end of each block must be indicated by an EOB (End Of Block) code.

3. Programs

A number of blocks form one program.

4. Program end

M02, M30, M99, M998, M999 or % is used as program end code.

α) denotes additional axis address. +44 will be used when α is specified for

3-3 Tape Data Storage Format

As with tape operation, tape data to be stored into the memory can be either of ISO or EIA code. The first EOB code read in after resetting is used by the NC unit for automatic identification of the code system ISO or EIA. The area of tape data to be stored into the memeory is, if the NC unit has been reset, from the character immediately succeeding the first EOB code the EOR code, and in all other cases, from the current tape position to the EOR code. Usually, therefore, start tape data storage operation after resetting the NC unit.

3-4 Optional Block Skip

1. Function and purpose

Optional block skip is a function that selectively ignores that specific block within a machining program which begins with the slash code “/”. Any block beginning with “/” will be ignored if the [BLOCK SKIP] menu function is set to ON, or will be executed if the menu function is set to OFF. For example, if all blocks are to be executed for a type of parts but specific blocks are not to be executed for another type, then different parts can be machined using one and the same program that contains the “/” code at the beginning of the specific blocks.

3-6

2. Operating notes

1. Blocks that have already been read into the pre-read buffer cannot be skipped.

2. This function is valid even during sequence number search.

3. During tape data storage (input) or output, all blocks, including those having a “/” code, are in- or outputted, irrespective of the status of the [BLOCK SKIP] menu function.

3-5 Program Number, Sequence Number and Block Number: O, N

Program numbers, sequence numbers, and block numbers are used to monitor the execution status of a machining program or to call a machining program or a specific process within a machining program. Program numbers are assigned to command blocks as required. A program number must be set using the letter O (address) and a numeric of a maximum of eight digits that follow O. Sequence numbers identify command blocks forming a machining program. A sequence number must be set using the letter N (address) and a numeric of a maximum of five digits that follow N. Block numbers are counted automatically within the NC unit, and reset to 0 each time a program number or a sequence number is read. These numbers will be counted up by one if the block to be read does not have an assigned program number or sequence number. All blocks of a machining program, therefore, can be uniquely defined by combining program number, sequence number, and block number as shown in the table below.

DATA FORMATS 3

NC input machining program

O1234 (DEMO. PROG) G92X0Y0 G90G51X–150. P0.75 N100G00X–50. Y–25. N110G01X250. F300 Y–225. X–50. Y–25. N120G51Y–125. P0.5 N130G00X–100. Y–75. N140G01X–200. Y–175. X–100. Y–75. N150G00G50X0Y0 N160M02 %

NC monitor display

Program No. Sequence No. Block No.

1234 0 0

1234 0 1

1234 0 2

1234 100 0

1234 110 0

1234 110 1

1234 110 2

1234 110 3

1234 120 0

1234 130 0

1234 140 0

1234 140 1

1234 140 2

1234 140 3

1234 150 0

1234 160 0

3-7

3 DATA FORMATS

3-6 Parity-H/V

One method of checking if the tape is correctly created is by parity checks. Parity checks are performed to check a tape for errors in punched codes, that is, for punching errors. There are two types of parity checks: parity-H and parity-V.

1. Parity-H check

Parity-H checks are intended to check the quantity of punched holes which form one character, and performed during tape operation, tape loading, and sequence-number searching. A parity-H error occurs in the following cases:

- ISO Codes

If a code with an odd number of punched holes is present in the significant information area.

- EIA Codes

If a code with an even number of punched holes is present in the significant information area or if non-punched holes (sprockets only) are present after a significant code in one block.

Example 1: Parity-H error (for EIA codes)

This character leads to a Parity-H error.

One block

This non-punched character will result in a Parity-H error.

These non-punched characters will not result in a Parity-H error.

If a parity-H error occurs, the tape will stop at the position next to the error code.

MEP007

3-8

DATA FORMATS 3

2. Parity-V check

Parity-V checks will be performed during tape operation, tape loading, or sequence-number searching, if parity-V check item on the PARAMETER display is set to ON. Parity-V during memory operation, however, will not be checked. A parity-V error occurs in the following case: If an odd number of codes are present in the significant information area from the first significant code in the vertical direction to the EOB code (;), that is, if an odd number of characters are present in one block. In the event of a parity-V error, the tape stops at a code next to the EOB (;).

Example 2: An example of parity-V error

1234567

This block leads to a Parity-V error.

MEP009

Note 1: During a parity-V check, some types of code are not counted as characters. See Fig.

3-1, “Tape codes” for further details.

Note 2: Space codes in the area from the first EOB code to the first address code or slash code

“/” are not subjected to counting for parity-V check.

3-9

3 DATA FORMATS

3-7 List of G-Codes

G functions are described in the list below.

Positioning

Linear interpolation

Circular interpolation (CW) G02 01

Circular interpolation (CCW) G03 01

Spiral interpolation (CW) G02.1 01

Spiral interpolation (CCW) G03.1 01

Dwell G04 00

High-speed machining mode G05 00

Fine spline interpolation G06.1 01

NURBS interpolation G06.2 01

Virtual-axis interpolation G07 00

Cylindrical interpolation G07.1 00

Exact-stop check G09 00

Data setting mode ON G10 00

Command address OFF G10.1 00

Data setting mode OFF G11 00

X-Y plane selection

Z-X plane selection

Y-Z plane selection

Inch command

Metric command

Pre-move stroke check ON G22 04

Pre-move stroke check OFF ▲G23 04

Reference point check G27 00

Reference point return G28 00

Return from reference point G29 00

Return to 2nd, 3rd and 4th reference points G30 00

Skip function G31 00

Multi-step skip 1 G31.1 00

Multi-step skip 2 G31.2 00

Multi-step skip 3 G31.3 00

Thread cutting (straight, taper) G33 01

Variable lead thread cutting G34 01

Hole machining pattern cycle (on a circle) G34.1 00

Hole machining pattern cycle (on a line) G35 00

Hole machining pattern cycle (on an arc) G36 00

Hole machining pattern cycle (on a grid) G37.1 00

Automatic tool length measurement G37 00

Vector selection for tool radius compensation G38 00

Corner arc for tool radius compensation G39 00

Tool radius compensation OFF ▲G40 07

Tool radius compensation (left) G41 07

3-D tool radius compensation (left) G41.2 07

Tool radius compensation (right) G42 07

3-D tool radius compensation (right) G42.2 07

Tool length offset (+) G43 08

Function G-code Group

■G00

■G01

■G17

■G18

■G19

■G20

■G21

3-10

Function G-code Group

Tool tip point control (Type 1) ON G43.4 08

Tool tip point control (Type 2) ON G43.5 08

Tool length offset (–) G44 08

Tool position offset, extension G45 00

Tool position offset, reduction G46 00

Tool position offset, double extension G47 00

Tool position offset, double reduction G48 00

Tool position offset OFF ▲G49 08

Scaling OFF ▲G50 11

Scaling ON G51 11

Mirror image OFF ▲G50.1 19

Mirror image ON G51.1 19

Local coordinate system setting G52 00

Machine coordinate system selection G53 00

Selection of workpiece coordinate system 1 ▲G54 12

Selection of workpiece coordinate system 2 G55 12

Selection of workpiece coordinate system 3 G56 12

Selection of workpiece coordinate system 4 G57 12

Selection of workpiece coordinate system 5 G58 12

Selection of workpiece coordinate system 6 G59 12

Additional workpiece coordinate systems G54.1 12

Selection of fixture offset G54.2 23

One-way positioning G60 00

Exact stop mode G61 13

High-accuracy mode (Geometry compensation) G61.1 13

Automatic corner override G62 13

Tapping mode G63 13

Cutting mode ▲G64 13

User macro single call G65 00

User macro modal call A G66 14

User macro modal call B G66.1 14

User macro modal call OFF ▲G67 14

Programmed coordinate rotation ON G68 16

Programmed coordinate rotation OFF G69 16

3-D coordinate conversion ON G68 16

3-D coordinate conversion OFF ▲G69 16

Fixed cycle (Chamfering cutter 1, CW) G71.1 09

Fixed cycle (Chamfering cutter 2, CCW) G72.1 09

Fixed cycle (High-speed deep-hole drilling) G73 09

Fixed cycle (Reverse tapping) G74 09

Fixed cycle (Boring 1) G75 09

Fixed cycle (Boring 2) G76 09

Fixed cycle (Back spot facing) G77 09

Fixed cycle (Boring 3) G78 09

Fixed cycle (Boring 4) G79 09

Fixed cycle OFF ▲G80 09

Fixed cycle (Spot drilling) G81 09

Fixed cycle (Drilling) G82 09

Fixed cycle (Deep-hole drilling) G83 09

DATA FORMATS 3

3-11

3 DATA FORMATS

Fixed cycle (Tapping) G84 09

Fixed cycle (Synchronous tapping) G84.2 09

Fixed cycle (Synchronous reverse tapping) G84.3 09

Fixed cycle (Reaming) G85 09

Fixed cycle (Boring 5) G86 09

Fixed cycle (Back boring) G87 09

Fixed cycle (Boring 6) G88 09

Fixed cycle (Boring 7) G89 09

Absolute data input

Incremental data input

Coordinate system setting/Spindle clamp speed setting G92 00

Workpiece coordinate system rotation G92.5 00

Inverse time feed G93 05

Feed per minute (asynchronous)

Feed per revolution (synchronous)

Initial point level return in fixed cycles ▲G98 10

R-point level return in fixed cycles G99 10

Measurement macro, workpiece/coordinate measurement G136

Compensation macro G137

Function G-code Group

■G90

■G91

■G94

■G95

Notes:

1. The codes marked with ▲ are selected in each group when the power is turned ON or executing reset for initializing modal.

2. The codes marked with " are able to be selected by a parameter as an initial modal which is to become valid when the power is turned ON or executing reset for initializing modal. Changeover of inch/metric system, however, can be made valid only by turning the power ON.

3. G-codes of group 00 are those which are not modal, and they are valid only for commanded blocks.

4. If a G-code not given in the G-code list is commanded, an alarm is displayed. And if a Gcode without corresponding option is commanded, an alarm is displayed (808 MIS-SET G CODE).

5. If G-codes belong to different groups each other, any G-code can be commanded in the same block. The G-codes are then processed in order of increasing group number. If two or more G-codes belonging to the same group are commanded in the same block, a G-code commanded last is valid.

3-12

4 BUFFER REGISTERS

4-1 Input Buffer

1. Overview

During tape operation or RS-232C operation, when the preread buffer becomes empty, the contents of the input buffer will be immediately shifted into the pre-read buffer and, following this, if the memory capacity of the input buffer diminuishes to 248 × 4 characters or less, next data (up to 248 characters) will be preread from the tape and then stored into the input buffer. The input buffer makes block-to-block connections smooth by eliminating any operational delays due to the tape-reading time of the tape reader. These favorable results of prereading, however, will be obtained only if the execution time of the block is longer than the tape-reading time of the next block.

BUFFER REGISTERS 4

Tape

Keyboard

Input buffer

Memory

Mode selection

Preread buffer 5

Buffer 4

Buffer 3

Buffer 2

Buffer 1

Note:

One block of data is stored in one buffer.

2. Detailed description

- The memory capacity of the input buffer is 248 × 5 characters (including the EOB code).

- The contents of the input buffer register are updated in 248-character units.

Arithmetic

operation

process

TEP010

- Only the significant codes in the significant information area are read into the buffer.

- Codes, including “(” and “)”, that exist between Control Out and Control In, are read into the

input buffer. Even if optional block skip is valid, codes from / to EOB will also be read into the input buffer.

- The contents of the buffer are cleared by a reset command.

4-1

4 BUFFER REGISTERS

4-2 Preread Buffer

1. Overview

During automatic operation, one block of data is usually preread to ensure smooth analysis of the program. During tool radius compensation, however, maximal five blocks of data are prere ad to calculate crossing point or to check the interference. In the high-speed machining mode (G05P2), moreover, up to 8 blocks of data are preread, and in the mode of high-speed smoothing control up to 24 blocks of data are stored with the currently executed block in the middle (i. e. 12 blocks being preread).

2. Detailed description

- One block of data is stored into the prepared buffer.

- Only the significant codes in the significant information area are read into the pre-read buffer.

- Codes existing between Control Out and Control In are not read into the pre-read buffer. If

optional block skip is valid, codes from / to EOB will not also be read into the pre-read buffer.

- The contents of the buffer are cleared by a reset command.

- If the single block operation mode is selected during continuous operation, processing will stop

after pre-reading the next block data.

4-2

5 POSITION PROGRAMMING

5-1 Dimensional Data Input Method

5-1-1 Absolute/Incremental data input: G90/G91

1. Function and purpose

Setting of G90 or G91 allows succeeding dimensional data to be processed as absolute data or incremental data. Setting of arc radius (with address R) or arc center position (with addresses I, J, K) for circular interpolation, however, must always refer to incremental data input, irrespective of preceding G90 command.

2. Programming format

POSITION PROGRAMMING 5

G90 (or G91) Xx

Yy1 Zz1 αα1 (α : Additional axis)

where G90: Absolute data input

G91: Incremental data input

3. Detailed description

1. In the absolute data mode, axis movement will be performed to the program-designated position within the workpiece coordinate system, irrespective of the current position.

N1 G90G00X0 Y0

In the incremental data mode, axis movement will be performed through the programdesignated distance as relative data with respect to the current position.

N2 G91G01X200. Y50. F100

N2 G90G01X200. Y50. F100

200.

Tool

100. N1

100. 200. 300.

MEP011

Commands for a movement from the origin of the workpiece coordinate system are given with the same

values, irrespective of whether the absolute data mode or the incremental

data mode is used.

5-1

5 POSITION PROGRAMMING

2. The last G90 or G91 command works as a modal one for the following blocks.

(G90) N3 X100. Y100.

This block will perform a movement to the position of X = 100 and Y = 100 in the workpiece coordinate system.

(G91) N3 X-100. Y50.

This block will perform a movement of –100 on the X-axis and +50 on the Y-axis, and thus result in a movement to the position of X = 100 and Y = 100.

200.

100.

100. 200. 300.

MEP012

3. Multiple G90 or G91 commands can be set in one block, and thus only a specific address can be set as absolute data or incremental data.

N4 G90X300. G91Y100.

In this example, dimensional data X300 preceded by G90 will be processed as an absolute data input, and Y100 preceded by G91 as an incremental data input. Therefore, this block will result in a movement to the position of X = 300 and Y = 200 (100 + 100) in the workpiece coordinate system.

200.

100.

100. 200.

300. MEP013

Moreover, G91 (incremental data input mode) will work for the succeeding blocks.

4. Either the absolute data mode or the incremental data mode can be freely selected as initial mode by setting the bit 2 of user parameter F93.

5. Even in the MDI (Manual Data Input) mode, G90 and G91 will also be handled as modal commands.

5-2

5-2 Inch/Metric Selection: G20/G21

1. Function and purpose

Inch command/metric command selection is possible with G-code commands.

2. Programming format

G20: Inch command selection G21: Metric command selection

3. Detailed description

1. Changeover between G20 and G21 is effective only for linear axes; it is meaningless for rotational axes.

Example: Preset unit of data input and G20/G21 (for decimal-point input type Ι)

POSITION PROGRAMMING 5

Axis Example

X Y Z B

X100

Y100

Z100

B100

Initial Inch (parameter) OFF Initial Inch (parameter) ON

G21 G20 G21 G20

0.0100 mm 0.0254 mm 0.00039 inches 0.00100 inches

0.0100 deg 0.0100 deg 0.0100 deg 0.0100 deg

2. To perform G20/G21 changeover in a program, you must first convert variables, parameters, and offsetting data (such as tool length/tool position/tool diameter offsetting data) according to the unit of data input for the desired system (inch or metric) a nd then set all these types of data either on each data setting display or using the programmed parameter input function.

Example: If Initial inch selection is OFF and offsetting data is 0.05 mm, the offsetting data

must be converted to 0.002 (0.05 ÷ 25.4 ≈ 0.002) before changing the G21 mode over to the G20 mode.

3. In principle, G20/G21 selection should be done before machining. If you want this changeover to be performed in the middle of the program, temporarily stop the program by an M00 command after G20 or G21 and convert the offsetting data as required.

Example: G21 G92 Xx

Yy1 Zz

MM MM MM

G20 G92 Xx

Yy2 Zz

M00 → Convert offsetting data here.

F10 → Set an F (Feed rate) command anew.

Note: Do not fail to give an F command appropriate to the new unit system after

changeover between G20 and G21. Otherwise, axis movements would be performed using the last F value before the changeover, without any conversion, on the basis of the new unit system.

4. Whether G20 or G21 is to be selected upon switching-on can be specified by the bit 4 of user parameter F91 (Initial Inch parameter).

5-3

5 POSITION PROGRAMMING

5-3 Decimal Point Input

1. Function and purpose

The decimal point can be used to determin the units digit (mm or inch) of dimensional data or feed rate.

2. Programming format

!!!!!.!!!! Metric system

!!!!.!!!!! Inch system

3. Detailed description

1. Decimal-point commands are valid only for the distance, angle, time, speed, and scaling factor (only after G51) that have been set in the machining program.

2. As listed in the table below, the meaning of command data without the decimal point differs between decimal-point input types Ι and ΙΙ according to the type of command unit system.

Command Command unit × 10 Type Ι Type ΙΙ

OFF 0.0001 (mm, inches, deg) 1.0000 (mm, inches, deg)

ON 0.0010 (mm, inches, deg) 1.0000 (mm, inches, deg)

3. Decimal-point commands are only valid for addresses X, Y, Z, U, V, W, A, B, C, I, J, K, E, F, P, Q and R, where address P only refers to a scaling factor.

4. The number of effective digits for each type of decimal-point command is as follows:

Move command

(Linear)

Integral part Decimal part Integral part Decimal part Integral part Decimal part Integral part Decimal part

mm 0. - 99999. .0000 - .9999 0. - 99999. .0000 - .9999 0. - 200000. .0000 - .9999 0. - 99999. .000 - .999

inch 0. - 9999.

.00000 .99999

Move command

(Rotational)

0. - 99999. (359.)

Feed rate Dwell

.0000 - .9999 0. - 20000.

.00000 .99999

0. - 99999. .000 - .999

5. Decimal-point commands are also valid for definition of variables data used in subprograms.

6. For data which can be, but is not specified with the decimal point, either the minimum program data input unit or mm (or in.) unit can be selected using bit 5 of parameter F91.

7. A decimal-point command issued for an address which does not accept the decimal point will be processed as data that consists of an integral part only. That is, all decimal digits will be ignored. Addresses that do not accept the decimal point are D, H, L, M, N, O, S and T. All types of variables command data are handled as the data having the decimal point.

5-4

4. Sample programs

A. Sample programs for addresses accepting the decimal point

POSITION PROGRAMMING 5

Command category

Program example

G0X123.45

(With the decimal point always given as the millimeter point)

G0X12345

#111=123 #112=5.55

X#111 Y#112

#113=#111+#112 (ADD) #114=#111–#112 (SUBTRACT) #115=#111#112 (MULTIPLY)

#116=#111/#112

#117=#112/#111 (DIVIDE)

For 1 = 1 µ For 1 = 0.1 µ 1 = 1 mm

X123.450 mm X123.450 mm X123.450 mm

X12.345 mm* X1.2345 mm** X12345.000 mm***

X123.000 mm Y5.550 mm

#113 = 128.550 #114 = 117.450 #115 = 682.650 #116 = 22.162

#117 = 0.045

* The least significant digit is given in 1 micron. ** The least significant digit is given in 0.1 micron. *** The least significant digit is given in 1 mm.

5-5

5 POSITION PROGRAMMING

B. Validity of decimal point for each address

Decimal

Address

D Invalid

E Valid Valid

F Valid Feed rate Valid

G Valid Preparatory function code

L Invalid

M Invalid Miscellaneous function code

point

command

Valid Coordinate position data Invalid Dwell time

Invalid

Valid Linear angle data Invalid Number of helical pitches

Valid Coordinate position data Invalid Offset amount (in G10)

Invalid

Valid Coordinate position data Valid

Invalid

Valid Corner chamfering amount

Invalid

Valid Coordinate of arc center U Valid Coordinate position data

Valid

Valid Coordinate of arc center W Valid Coordinate position data

Valid

Valid Coordinate of arc center

Valid

Valid Knot for NURBS curve Z Valid Coordinate position data

Rotary table Miscellaneous function code

Offset number (tool position, tool length and tool diameter)

Offset number (tool postion, tool length and tool diameter)

Intra-subprogram sequence number

Vector component for tool diameter offset

Vector component for tool diamater offset

Fixed cycle/subprogram repetition

Application Remarks Address

S Invalid Spindle function code

T Invalid Tool function code

V Valid Coordinate position data

Y Valid Coordinate position data

Decimal

point

command

Valid Subprogram call number

Valid Scaling factor

Invalid Rank for NURBS curve

Cutting depth for deep-hole drilling cycle

Valid Shift amount for back boring

Valid Shift amount for fine boring

Valid R point in fixed cycle

Radius of an arc with R selected

Radius of an arc for corner rounding

Valid Offset amount (in G10) Valid Weight for NURBS curve

Valid Coordinate position data

Valid Dwell time

Application Remarks

N Invalid Sequence number

O Invalid Program number

Note: The decimal point is valid in all the arguments for a user macroprogram.

5-6

6 INTERPOLATION FUNCTIONS

6-1 Positioning (Rapid Feed): G00

1. Function and purpose

Positioning command G00 involves use of a coordinate word. This command positions a tool by moving it linearly to the ending point specified by a coordinate word.

2. Programming format

INTERPOLATION FUNCTIONS 6

G00 Xx Yy Zz α The command addresses are valid for all additional axis.

input is used according to the status of G90/G91 existing at the particular time.

3. Detailed description

1. Once this command has been given, the G00 mode will be retained until any other G-code command that overrides this mode, that is, either G01, G02, G03, or G32 of command group 01 is given. Thus, a coordinate word will only need be given if the next command is also G00. This function is referred to as the modal function of the command.

2. In the G00 mode, acceleration/deceleration always takes place at the starting/ending point of a block and the program proceeds to the next block after confirming that the pulse command in the present block is 0 and the tracking error of the acceleration/deceleration cycle is 0. The width of in-position can be changed using a parameter (S13).

3. The G-code functions (G71.1 to G89) of command group 09 are canceled by the G00 command (G80).

4. The tool path can be made either linear or nonlinear using a parameter (F91 bit 6) but the positioning time remains unchanged.

- Linear path

As with linear interpolation (G01), the tool speed is limited according to the rapid feed rate of each axis.

α; (α: Additional axis)

The absolute or the incremental data

- Nonlinear path

The tool is positioned according to the separate rapid feed rate of each axis.

5. When no number following G address, this is treated as G00.

6-1

6 INTERPOLATION FUNCTIONS

–

4. Sample programs

Unit: mm

(Tool)

Starting point (+150, –100, +150)

+300

100

+150

120

+200

Ending point (–120, +200, +300)

MEP014

The diagram above is for:

G90 G00 X-120.000 Y200.000 Z300.000; Absolute data command G91 G00 X-270.000 Y300.000 Z150.000; Incremental data command

5. Remarks

1. If bit 6 of user parameter F91 is 0, the tool will take the shortest path connecting the starting and ending points. The positioning speed will be calculated automatically to give the shortest allocation time within the limits of the rapid feed rate of each axis. For example, if a rapid feed rate of 9600 mm/min is preset for both X- and Y-axes, then the command

G91 G00 X–300.000 Y200.000

will move the tool as shown in the figure below.

bit 6 = 0

F91

Ending point

300

X-axis effective feedrate:

9600 mm/min

Y-axis effective feedrate: 6400 mm/min

200

Starting point

Unit: mm

MEP015-1

6-2

INTERPOLATION FUNCTIONS 6

2. If bit 6 of user parameter F91 is 1, the tool will move from the starting point to the ending point according to the rapid feed rate of each axis. For example, if a rapid feed rate of 9600 mm/min is preset for both X- and Y-axes, then the command

G91 G00 X–300.000 Y200.000

will move the tool as shown in the figure below.

bit 6 = 1

F91

Ending point

X-axis effective feedrate:

9600 mm/min

300

200

Starting point

Y-axis effective feedrate: 9600 mm/min

Unit: mm

MEP015-2

3. The rapid feed rate that you can set for each axis using the G00 command varies from machine to machine. Refer to the relevant machine specification for further details.

4. Rapid feed (G00) deceleration check When processing of rapid feed (G00) is completed, the next block will be executed after the deceleration check time (Td) has passed. The deceleration check time (Td) is calculated by following expressions depending on the acceleration/deceleration type.

Linear acceleration/linear deceleration .............................. Td = Ts + a

Exponential acceleration/linear deceleration .....................Td = 2 × Ts + a

Exponential acceleration/exponential deceleration............Td = 2 × Ts + a

(Where Ts is the acceleration time constant, a = 0 to 14 msec)

The time required for the deceleration check during rapid feed is the longest among the rapid feed deceleration check times of each axis determined by the rapid feed acceleration/deceleration time constants and by the rapid feed acceleration/deceleration mode of the axes commanded simultaneously.

6-3

6 INTERPOLATION FUNCTIONS

(–)

6-2 One-Way Positioning: G60

1. Function and purpose

Highly accurate positioning free from any backlash error can be performed when the axis movement is controled by the G60 command so that the final access always takes place in one determined direction.

2. Programming format

G60 Xx Yy Zz α

α; (α: Additional axis)

3. Detailed description

1. The direction of final access and its creeping distance must be set in parameter I1.

2. After rapid approach to a position away from the ending point by the creeping distance, the final access is performed in the predetermined direction at a speed corresponding with the rapid feed.

G60 a

Starting point

Temporary stop

G60 creeping distance

Positioning point

Final access direciton

Ending point

Starting point

G60 –a

3. The positioning pattern described above also applies during machine locking or for a Z-axis command with the Z-axis cancellation activated.

(+)

MEP018

4. In the dry run mode (G00 mode), the whole positioning is carried out at the dry-running speed.

5. The creeping to the einding point can be halted with Reset, Emergency stop, Interlock, or Feed hold, or by setting the rapid feed override to 0 (zero). The creeping is performed according to the setting of the rapid feed, and the rapid feed override function is also effective for the creeping.

6. One-way positioning is automatically invalidated for the hole-drilling axis in hole-drilling fixed-cycle operations.

7. One-way positioning is automatically invalidated for shifting in fine-boring or back-boring fixed-cycle operations.

8. Usual positioning is performed for an axis not having a parameter-set creeping distance.

9. One-way positioning is always of non-interpolation type.

10. An axis movement command for the same position as the ending point of the preceding block (movement distance = 0) will cause reciprocation through the creeping distance so that the final access can be performed in the predetermined direction for an accurate positioning to the desired point.

6-4

6-3 Linear Interpolation: G01

1. Function and purpose

This command moves (interpolates) a tool from the current position to the ending point specified by a coordinate word, at the feed rate specified with address F. The specified feed rate acts here as the linear velocity relative to the direction of movement of the tool center.

2. Programming format

INTERPOLATION FUNCTIONS 6

G01 Xx Yy Zz α where x, y, z, and

α Ff; (α: Additional axis)

α each denote a coordinate. The absolute or the incremental data input is used

according to the status of G90/G91 existing at the particular time.

3. Detailed description

Once this command has been given, the G01 mode will be retained until any other G-code command that overrides this mode, that is, either G00, G02, G03 or G33 of command group 01 is given. Thus, it is merely required to input coordinate words for linear interpolations in the succeeding blocks unless the feed rate must be changed. A programming error will result if no F-code command has been given to the first G01 command. The feed rates for rotational axes must be set in deg/min. (Example: F300 = 300 deg/min) The G-code functions (G71.1 to G89) of command group 09 are cancelled by G01 (set to G80).

4. Sample program

The following shows a program for moving the tool at a cutting feed rate of 300 mm/min on the route of P1 → P2 → P3 → P4 → P1 (where the section from P0 → P1 forms a positioning route for the tool):

2020

G91 G00 X20. Y20. P0 → P

G01 X20. Y30. F300 P1 → P

X30. P2 → P X–20. Y–30. P3 → P X–30. P4 → P

6-5

Unit: mm

MEP019

6 INTERPOLATION FUNCTIONS

6-4 Circular Interpolation: G02, G03

1. Function and purpose

Commands G02 and G03 feed the tool along an arc.

2. Programming format

G02 (G03)

Xx Yy (Zz) Ii Jj (Kk) Ff ;

Coordinates of the

ending point Counterclockwise (CCW) Clockwise (CW)

Coordinates of

the arc center

Feedrate

X : Arc ending point coordinate, X-axis Y : Arc ending point coordinate, Y-axis Z : Arc ending point coordinate, Z-axis I : Arc center, X-axis J : Arc center, Y-axis K : Arc center, Z-axis F : Feed rate

Use addresses X, Y and Z (or their parallel axes) to specify the coordinates of the ending point of arc, and addresses I, J and K for the coordinates of arc center. Combined use of absolute and incremental data input is available for setting the coordinates of the ending point of arc. For the coordinates of the arc center, however, incremental data relative to the starting point must always be set.

3. Detailed description

1. Once the G02 (or G03) command has been given, this command mode will be retained until any other G-code command used to override the G02 (or G03) comma nd mode, that is, G00 or G01 of command group 01 is given.

6-6

2. The direction of circular movement is determined by G02/G03. G02: CW (Clockwise)

G03: CCW (Counterclockwise)

G02 G03

G03

G02

INTERPOLATION FUNCTIONS 6

G03

G02

G17 (X-Y) plane G18 (Z-X) plane

G02

G03

G02

G19 (Y -Z ) Plane

MEP020

3. Interpolation of an arc that spans multiple quadrants can be defined with one block.

4. To perform circular interpolation, the following information is required:

- Rotational direction ......................CW (G02) or CCW (G03)

- Arc ending point coordinates .......Given with address X, Y, Z.

- Arc center coordinates.................Given with address I, J, K. (Incremental dimension)

- Feed rate......................................Given with address F.

5. If none of the addresses I, J, K and R is specified, a program error will occur.

6. Addresses I, J and K are used to specify the coordinates of the arc center in the X, Y and Z directions respectively as seen from the starting point, therefore, care must be taken for signs.

6-7

6 INTERPOLATION FUNCTIONS

4. Sample programs

Example 1: Complete-circle command

Y-axis

Feedrate

F = 500 mm/min

X-axis

Circle ce nter J = 50 mm

Starting / Ending point

G02 J50.000 F500

Example 2: Three-quarter circle command

Y-axis

MEP021

Feedrate

F = 500 mm/min

X-axis

Circle ce nter J = 50 mm

Starting point

Ending point (x+50, y+50)

MEP022

G91 G02 X50.000 Y50.000 J50.000 F500

5. Notes on circular interpolation

1. Clockwise (G02) or Counterclockwise (G03) during circular interpolation refers to the rotational direction in the right-handed coordinate system when seen from the plus side toward the minus side of the coordinate axis perpendicular to the plane to be interpolated.

2. If the coordinates of the ending point are not set or if the starting and ending points are set at the same position, designating the center using address I, K or J will result in an arc of 360 degrees (true circle).

6-8

INTERPOLATION FUNCTIONS 6

3. The following will result if the starting-point radius and the ending-point radius are not the same.

- If error ∆R is larger than the parameter F19 (tolerance for radial value difference at ending

point), a program error (817 INCORRECT ARC DATA) will occur at the starting point of the arc.

G02 X80. I50.

larm stop

Center Ending point

Starting

point

Radius at

starting point

Radius at

ending point

∆

MEP023

- If error ∆R is equal to or smaller than the parameter data, interpolation will take a spiral

form heading for the programmed ending point of the arc.

G02 X90. I50.

Starting

point

Radius at

starting point

Center Ending point

Spiral interpolation

Radius at

ending point

∆

MEP024

The examples shown above assume that excessively large parameter data is given to facilitate your understanding.

6-5 Radius Designated Circular Interpolation: G02, G03

1. Function and purpose

Circular interpolation can be performed by designating directly the arc radius R as well as specifying conventional arc center coordinates (I, J, K).

2. Programming format

G02 (G03) Xx Yy Rr Ff;

where x : X-axis coordinate of the ending point

y : Y-axis coordinate of the ending point r : Radius of the arc f : Feed rate

6-9

6 INTERPOLATION FUNCTIONS

3. Detailed description

The arc center is present on the mid-perpendicular to the segment which connects the starting point and the ending point. The crossing point of the mid-perpendicular and that circle of the designated radius r that has the center set at the starting point gives the center coordinates of the designated arc. A semi-circle or smaller will be generated if R is a positive value. An arc larger than the semi-circle will be generated if R is a negative value.

Path of an arc with a negative-signed R

Ending point

Path of a n arc with a positive R

O1, O2 : Center point

TEP023

Starting point

To use the radius-designated arc interpolation commands, the following requirement must be met:

≤

•

where L denotes the length of the line from the starting point to the ending point. If radius data and arc center data (I, J, K) are both set in the same block, the circular interpolation by radius designation will have priority in general. For complete-circle interpolation (the ending point = the starting point), however, use centerdesignation method with addresses I, J and K, since the radius-specification command in this case will immediately be completed without any machine operation.

4. Sample programs

- G02 Xx

- G03 Zz

- G02 Xx

Yy1 Rr1 Ff

Xx1 Rr1 Ff

Yy1 Jj1 Rr1 Ff

- G17 G02 Ii

Ji1 Rr1 Ff

X-Y plane, radius-designated arc Z-X plane, radius-designated arc X-Y plane, radius-designated arc

(If radius data and center data (I, J, K) are set in the same block, circular interpolation by radius designation will have priority.)

X-Y plane, center-designated arc

(Radius-specification is invalid for complete circle)

6-10

6-6 Spiral Interpolation: G2.1, G3.1 (Option)

1. Function and purpose

INTERPOLATION FUNCTIONS 6

Commands G2.1 connected

and G3.1 provide such an interpolation that the starting and ending points are

smoothly for an arc command where the radii of the both points differ from each

other.

(Normal circular interpol ation)

(Spiral interpolation)

Starting point

2. Programming format

G17 G2.1 (or G3.1) Xp_ Yp_ I_ J_ (α_) F_ P_

Ending point

re = r

Ending point

≠

Center

Arc center coordinates Arc ending point coordinates

MEP031

G18 G2.1 (or G3.1) Zp_ Xp_ K_ I_ (α_) F_ P_

G19 G2.1 (or G3.1) Yp_ Zp_ J_ K_ (α_) F_ P_

P : Number of pitches (revolutions) (P can be omitted if equal to 0.) α : Any axis other than circular interpolation axes (For helical cutting only) F : Rate of feed along the tool path

3. Detailed description

1. Circular movement directions of G2.1 and G3.1 correspond with those of G02 and G03, respectively.

2. Radius designation is not available for spiral interpolation. (The starting and ending points must lie on the same arc for a radius designation.)

Note: When a radius is designated, this command will be regarded as a radius-

designated circular interpolation.

3. Conical cutting or tapered threading can be done by changing the radii of the arc at its starting and ending points and designating a linear-interpolation axis at the sa me time.

4. Even for normal circular command G2 or G3, spiral interpolation will be performed if the difference between the radii of the starting point and the ending point is smaller than the setting of parameter F19.

6-11

6 INTERPOLATION FUNCTIONS

Example: When the following program is executed, the feed rates for each of the points will

be as shown in the diagram below.

CEDB

G28 X0 Y0 G00 Y–200. G17 G3.1 X–100. Y0 I–150. J0 F3000 P2 M30

3000 mm/min B 2500 C 2000 D 1500 E 1000

MEP032

6-12

INTERPOLATION FUNCTIONS 6

4. Sample programs

Example 1: Spiral cutting

Shown below is an example of programming for spiral contouring with incremental data input of the arc center (X = 0, Y = 45.0) and absolute data input of the arc ending point (X = 0, Y = –15.0).

G91 G28 Z0 G80 G40 T15 T00 M06 G54.1 P40 G94 G00 X0 Y-45.0 G43 Z30.0 H01 Z3.0 S1500 M03 M50 G01 Z-1.0 F150 G2.1 X0 Y-15.0 I0 J45.0 F450 P2

G00 Z3.0 M05 M09 Z30.0 M30

D735PB001

Zero point return on the Z-axis Fixed-cycle cancellation Tool change Coordinate system setting Approach in the XY-plane to the starting point (0, –45.0) Positioning on the Z-axis to the initial point

Normal rotation of the spindle Air blast ON Infeed on the Z-axis Command for spiral interpolation with arc ending point =

(0, –15.0), arc center = (0, 0)*, and pitch = 2. * I- and J-values refer to increments to the starting point.

Return on the Z-axis Spindle stop and Air blast OFF

End of machining

The rate of feed at the starting point is 450 mm/min, as specified in the block of G2.1, and the rate of feed at the ending point can be calculated as follows:

(Ending point’s radius/Starting point’s radius) × Command value of the rate of feed.

As the radius of the starting point = 45.0, that of the ending point = 15.0, and the command rate of feed (F) = 450, the rate of feed results in

(15.0/45.0) × 450 = 150 mm/min

at the ending point. Note 1: Take care not to use radius designation (argument R) for spiral interpolation; otherwise

a normal circular interpolation (by G02 or G03) will be executed.

Note 2: It is not possible to give the command for a spiral interpolation the starting and ending

points of which should have different centers specified.

6-13

6 INTERPOLATION FUNCTIONS

Example 2: Heart-shaped cam (by absolute data input)

D735PB002

G91 G28 Z0 G80 G40 T15 T00 M06 G54.1 P40 G94 G00 X0 Y-70.0 G43 Z30.0 H01 S1500 M03 Z3.0 M50 G01 Z-1.0 F150 G2.1 X0 Y1.0 I0 J70.0 F450 X0 Y-70.0 I 0 J-1.0 G00 Z3.0 M05 M09 Z30.0 M30

Zero point return on the Z-axis Fixed-cycle cancellation Tool change Coordinate system setting Approach in the XY-plane to the starting point (0, –70.0) Positioning on the Z-axis to the initial point Normal rotation of the spindle

Air blast ON Infeed on the Z-axis Command for the left-hand half curve Command for the right-hand half curve Return on the Z-axis Spindle stop and Air blast OFF

End of machining

6-14

INTERPOLATION FUNCTIONS 6

Example 3: Heart-shaped cam (by incremental data input)

(100.)

MEP033

Starting and Ending points

(30.)

The difference (b–a) between the radii of the starting point and ending point denotes a displacement for heart shape. Use two blocks for programming separately the right-half and the left-half shape.

A sample program in incremental data input:

G3.1 Y130. J100. F1000............... (Right half)

a+b b

G3.1 Y–130. J–30

........................ (Left half)

–a–b –a

a = 30. (Minimum arc radius)

b = 100. (Maximum arc radius)

a + b = 130. (Ending-point coordinate of the right half-circle)

–a – b = –130. (Ending-point coordinate of the left half-circle)

6-15

6 INTERPOLATION FUNCTIONS

Example 4: Large-size threading

To perform large-size threading, use three heilical-interpolation blocks for programming separately infeed section, threading section and upward-cutting section. Spiral interpolation is required to designate the amounts of diameter clearance for both the infeed block and the upward-cutting block. (The starting and ending points are shifted through the designated clearance amounts from the circumference of threading section.)

Clearance

Threading

Infeed

G3.1 X–i1–i2 Y0 Zz1 I–i1 J0 Ff1(Infeed block, half-circle) G03 X0 Y0 Zz G3.1 Xi

2+i3

* The number of pitches, p

l. Note that the value p

Ii2 J0 Pp

(Threading block, complete circle)

Y0 Zz3 Ii2 J0 (Upward-cutting block, half-circle )

, in the threading block is given by dividing the stroke z2 by the pitch

must be an integer.

Upward cutting

MEP034

6-16

Example 5: Tapered threading

As shown in the figure below, tapered helical cutting that begins at any angle can be performed.

INTERPOLATION FUNCTIONS 6

MEP035

Data with addresses X, Y and Z must be the increments x1, y1 and z1 respectively, from the starting point s to the ending point e; data of I and J must be the increments i

and j1 respectively,

from the starting point s to the circular center, and data of P must be equal to the number of pitches p

G3.1 Xx

Yy1 Zz1 Ii1 Jj1 Pp1 Ff

The amount of taper t and the pitch l are calculated as follows:

2(re – rs)

t =

where rs =

+ j

, re =

(x1 – i1)2 + (y1 – j1)

;

l =

(2π • π

where θ = θe – θs = tan

+ θ) / 2π

j1 – y i1 – x

– tan

–1

–j

–1

–i

where rs and re denote the radii at the starting point and the ending point respectively, and qs and qe denote the angles at the starting point and the ending point respectively.

6-17

6 INTERPOLATION FUNCTIONS

Example 6: Conical cutting

Conical cutting is an application of tapered threading, and have its starting or ending point on the center line. Tapering results from gradually increasing or decreasing the arc diameter. The pitch is determined by z

1/p1

MEP036

G2.1 X–x1 Y0 Zz1 I–x1 Pp1 Ff

x1: Radius of the base

: Height

: Number of pitches

: Feed rate

Note: Use the TRACE display to check the tool path during spiral interpolation.

6-18

6-7 Plane Selection: G17, G18, G19

6-7-1 Outline

1. Function and purpose

Commands G17, G18 and G19 are used to select a plane on which arc interpolation, tool nose radius compensation, etc. are to be done. Registering the three fundamental axes as parameters allows you to select a plane generated by any two non-parallel axes. These commands are also used to select a plane where figures or prog ram coordinates are to be rotated.

2. Programming format

INTERPOLATION FUNCTIONS 6

G17; (X-Y plane selection) G18; (Z-X plane selection) G19; (Y-Z plane selection)

YXZ

G03

G02

G17 (XY) plane G18 (ZX) plane G19 (YZ) plane

6-7-2 Plane selection methods

Plane selection by parameter setting is explained in this section.

1. Which of the fundamental axes or their parallel axes are to form the plane you want to select is determined by the type of plane selection command (G17, G18 or G19) and the axis address specified in the same block.

X, Y, and Z denote respective coordinate axes or their corresponding parellel axes.

G03 G03

G02

TEP024’

YXZ

G17X Y; G18X Z; G19Y Z;

G03 G03

G02

TEP025’

G02

G03

G02

2. Automatic plane selection does not occur for blocks that do not have an issued planeselection command (G17, G18 or G19)

G18 X_ Z_; Z-X plane

Y_ Z_; Z-X plane (No plane change)

6-19

6 INTERPOLATION FUNCTIONS

3. If axis addresses are not set for blocks having an issued plane-selection command (G17, G18 or G19), the fundamental three axes will be regarded as set.

G18_; (Z-X plane = G18 XZ ;)

Note 1: Use bits 0 and 1 of parameter F92 to set the initial plane which is to be selected upon

power-on or resetting.

Note 2: The G-codes for plane selection (G17, G18 or G19) should be commanded in a block

independently. If such a G-code is commanded in a block containing the axis move command, a movement independent from the selected plane can be caused.

6-20

6-8 Virtual-Axis Interpolation: G07

–

1. Function and purpose

Specify with G07 code one of the two circular-interpolation axes for helical or spiral interpolation with synchronous linear interpolation as a virtual axis (a pulse-distributed axis without actual movement), and an interpolation on the plane defined by the remaining circular axis and the linear axis can be obtained along the sine curve which corresponds with the side view of the circular interpolation with synchronous linear interpolation.

2. Programming format

G07 α0 To set a virtual axis M To interpolate with the virtual axis G07 α1 To cancel the virtual axis

3. Detailed description

1. Only helical or spiral interpolation can be used for the virtual-axis interpolation.

2. In the program section from G07α0 to G07α1, the “alpha” axis is processed as a virtual axis. If, therefore, the alpha axis is included independently in this section, the machine will remain in dwell status until pulse distribution to the virtual axis is completed.

INTERPOLATION FUNCTIONS 6

3. The virtual axis is valid only for automatic operation; it is invalid for manual operation.

4. Protective functions, such as interlock, stored stroke limit, etc., are valid even for the virtual axis.

5. Handle interruption is also valid for the virtual axis. That is, the virtual axis can be shifted through the amount of handle interruption.

4. Sample program

G07 Y0 Sets the Y-axis as a virtual axis. G17G2.1X0Y–5.I0J–10.Z40.P2F50 Sine interpolation on the XZ plane G07 Y1 Resets the Y-axis to an actual axis.

X-axis

10.

20.

Z-axis

40.

Y-axis

X-axis

–10.

MEP037

6-21

6 INTERPOLATION FUNCTIONS

6-9 Spline Interpolation: G06.1 (Option)

1. Function and purpose

The spline interpolation automatically creates a curve that smoothly traces specified points, and thus enables a high-speed and high-accuracy machining for free shapes along smoothly curved tool path.

2. Programming format

G06.1 Xx

3. Detailed description

A. Setting and cancellation of spline interpolation mode

The spline interpolation mode is set by the preparatory function G06.1, and cancelled by another Group 01 command (G00, G01, G02 or G03).

Example 1:

N100 G00 X_Y_ N200 G06.1 X_Y_ N201 X_Y_ N202 X_Y_ N203 X_Y_

MM N290 X_Y_ N300 G01 X_Y_

n+1

Fig. 6-1 Interpolated line by spline interpolation

In the above example, the spline interpolation is activated at N200 (block for movement from P to P2) and it is cancelled at N300. Therefore, a spline curve is created for a group of ending points from P

to Pn, and interpolation is applied along the created curve.

For creating a spline interpolation curve, it is generally required to specify two or more blocks (at least three points to be traced) in the mode. If the spline interpolation mode is set just for one block, the path to the ending point of the block is interpolated in a straight line.

Example 2:

N100 G01 X_Y_ N200 G06.1 X_Y_ N300 G01 X_Y_

Linear interpolation for the single spline-interpolation block

Fig. 6-2 Spline interpolation applied to a single block

6-22

INTERPOLATION FUNCTIONS 6

B. Division of spline curve in spline-interpolation mode

The spline interpolation mode generally creates a continuous curve that smoothly connects all specified points from the beginning of the mode to the end of it. However, the spline curve is divided into two discontinuous curves as often as one of the following conditions is satisfied:

- When the angle between linear movement lines of two neighboring blocks is beyond the

spline-cancel angle,

- When the movement distance of a block exceeds the spline-cancel distance, or

- When there is a block without any movement command in the spline-interpolation mode.

1. When the relative angle of two neighboring blocks is beyond the spline-cancel angle

Spline-cancel angle LLL Parameter F101

As to the sequence of points P1, P2, P3, L Pn in a spline interpolation mode, when the angle

made by two continuous vectors

i–1 Pi

and

PiP

is larger than

i+1

, the point Pi is

F101

regarded as a corner. In that event, the point group is divided into two sections of P and Pi to Pn at Pi, and spline curve is individually created for each section. When the spline-cancel angle is not set (

= 0), this dividing function is not available.

F101

Example 1: F101 = 80 deg

F101

not set

F101

Forms a corner

to P

Fig. 6-3 Spline cancel depending on angle

6-23

6 INTERPOLATION FUNCTIONS

When there are more than one point where θ

> F101, such points are treated as corners to

divide the point group and multiple spline curves are created for respective sections.

F101

Fig. 6-4 Multiple-cornered spline curve depending on angle When any two corner points (where θi > F101) successively exist, the block for the second

point is automatically set under control of linear interpolation. Therefore, it can be omitted to specify G01 code in each intermediate block of pick feed, for example, during 2.5dimensional machining, which considerably simplifies the programming.

Example 2: F101 < 90 (deg)

In the following program (shown in Fig. 6-5), the angle of the Y-directional pick feed to the X-Z plane (of spline interpolation) is always 90°. If F101 is set slightly smaller than 90°, spline interpolation is automatically cancelled in the pick-feed blocks (N310, N410, !!!), which are then linearly interpolated each time. If no value is set for F101, it is required to specify G-codes parenthesized in the program below to change the mode of interpolation.

N100 G00 X_Y_Z_ N200 G06.1 X_Z_ N210 X_Z_

N300 X_Z_

(G01)

N310

(G06.1)

N320

N400 X_Z_

(G01)

N410

(G06.1)

N420

N700 X_Z_ N710 G01

Y_ X_Z_

i+1

i+2

j+1

j+2

i+1

Fig. 6-5 Linear interpolation for pick feed in spline-interpolation mode

6-24

INTERPOLATION FUNCTIONS 6

2. When the movement distance of a block exceeds the spline-cancel distance

Spline-cancel distance LLL Parameter F100

As to the sequence of points P1, P2, P3, !!! Pn in a spline interpolation mode, when the length

PiP

of the vector

i+1

PiP

is longer than

i+1

, the block for point P

F100

is automatically set

i+1

under control of linear interpolation, while the preceding and succeeding sections P and P In this case, the inclination of the tangent vector at P inclination of the tangent vector at P

correspond to that of the line segment

to Pn are individually interpolated in spline curves.

i+1

(at the beginning of spline P

i+1

PiP

in general.

i+1

(at the end of spline P1 to Pi) and the

to Pn) do not

i+1

to P

When the spline-cancel distance is not set (F100 = 0), this dividing function is not available.

(a) P4P

F100

≤

F100

iPi+1

Interpolated as follows:

P P P

for other blocks

P4P

F100

to P4: Spline curve,

to P5: Straight li ne,

to P8: Spline curve.

(b)

F100

is not specified

The whole path P1 to P8 is interpolated in one spline curve.

Fig. 6-6 Spline cancel depending on movement distance of a block When there are more than one block where

PiP

i+1

, all those blocks will individually

F100

undergo the linear interpolation.

3. When there is a block without any movement command in the spline-interpolation mode Any block without movement command temporarily cancels the spline interpolation, and the sections before and after such a block will independently be spline-interpolated.

N100 G01 X_Y_

P5 (Not moved) P

Spline from

Forms a corner

to P

Spline from

to P

N110 G06.1 X_Y_ N120 X_Y_

N300 X_Y_ N310 X0 N320 X_Y_

N500 X_Y_ N510 G01 X_Y_

Fig. 6-7 Spline cancel by a block without movement command

6-25

6 INTERPOLATION FUNCTIONS

C. Fine spline function (curved shape correction)

The fine spline function works with spline interpolation and automatically corrects the shape of a spline curve, as required, to make the path of the curve smoother. More specifically, the fine spline function works in the following two cases:

- The case that the curve errors in blocks are significant

- The case that an unusually short block exists (automatic correction in this case is referred to as

fairing.)

Automatic correction in the above cases is explained below.

1. Automatic correction for significant curve errors in blocks When the curve data in CAD undergoes micro-segmentation with CAM, approximation

using a polygonal line is usually executed with a curve tolerance (chord error) of about 10 microns. At this time, if any inflection points are included in the curve, the micro-segment block including the inflection points may increase in length (see

Also, if the length of this block becomes unbalanced against those of the immediately preceding and succeeding blocks, the spline curve in this zone may have a significant error with respect to the original curve.

P3 P

. in the figure below)

CAD curve

Tolerance (minus side)

Spline curve (deviation from the CAD c urve i s significant)

Tolerance (plus side)

Tolerance

Inflection point in the original curve

Fig. 6-8 Spline curve having a significant chord error (inflection points present) This function detects the sections whose chord errors in the curve due to the presence of

inflection points become significant, and corrects the shape of the spline curve in that zone automatically so that the chord errors in the curve fall within the data range of the specified parameter.

Curve error 1 LLL Parameter F102

6-26

INTERPOLATION FUNCTIONS 6

If a block in the spline interpolation mode is judged to have inflection points in the spline curve and the maximum chord error of the spline curve from the segment is greater than the value of F102, the shape of that spline curve will be corrected for a maximum chord error not exceeding the value of F102.

Uncorrected spline curve

Corrected spline curve

or less

F102

Fig. 6-9 Shape correction 1 for spline curve

The shape of a curve can also be corrected if the chord error in the spline curve increases due to an imbalance in the lengths of adjoining blocks occurs for any reasons other than the presence of inflection points or for other reasons.

Curve error 2 LLL Parameter F104

If a blocks in the spline interpolation mode is judged to have no inflection points in the splin e curve and the maximum chord error in the spline curve an d block is greater than the value of F104, the shape of that spline curve will be corrected for a maximum chord error not exceeding the value of F104.

Uncorrected spline curve

Correction

Corrected spline curve

or less

F104

Fig. 6-10 Spline curve having a significant chord error (no inflection points)

Remark 1: In all types of spline curve correction, the curve correction function works only for

the corresponding block. Therefore, the tangential vectors at the boundaries with the immediately preceding and succeeding blocks become discontinuous.

Remark 2: If parameter F102 is set to 0, all blocks regarded as including inflection points will

become linear. If parameter F104 is set to 0, all blocks regarded as including no inflection points will become linear.

Remark 3: Curved-shape correction based on parameter F102 or F104 usually becomes

necessary when adjoining blocks are unbalanced in length. If the ratio of the adjoining block lengths is very large, however, spline interpolation may be temporarily cancelled between the blocks prior to evaluation of the chord error.

6-27

6 INTERPOLATION FUNCTIONS

2. Automatic correction of the spline curve in an unusually short block (Fairing) When CAD data is developed into micro-segments by CAM, a very small block may be created in the middle of the program because of internal calculation errors. Such a block is often created during creation of a tool diameter offset program which requires convergence calculation, in particular. Since this unusually small block usually occurs at almost right angles to the direction of the spline curve, this curve tends not to become smooth.

Fig. 6-11 Distortion of a spline curve due to the effects of a very small block

Distorted spline curve

Very small block

If it detects such an extremely small block during spline interpolation, the shape correction function will remove that block and then connect the preceding and succeeding blocks directly (this is referred to as fairing) to create a smooth spline curve free from distortion.

Block fairing length LLL Parameter F103

Assume that the length of the i-th block in spline interpolation mode is taken as li and that the following expressions hold:

> F103 × 2

i – 1

≤ F103

> F103 × 2

i + 1

In the above case, the ending point of the (i–1)-th block and the starting point of the i+1 block are moved to the mid-point of the ith block and as a result, the ith block is deleted. Spline interpolation is executed for the sequence of points that has thus been corrected.

≤

F103

× 2

F103

i–1

F103

× 2

i+1

Correction of the passing point

Fig. 6-12 Correction of spline curve passing points by fairing

6-28

Created spline curve

INTERPOLATION FUNCTIONS 6

Assume that the first block in spline interpolation mode is very small and that the following expressions hold:

≤ F103

> F103 × 2

In the above case, the starting point of the second block is changed to that of the first block and as a result, the first block is deleted.

≤

F103

Non-spline block

Deletion of the passi ng point

× 2

F103

Created spline curve

Fig. 6-13 Fairing at the starting point of a spline curve

Assume that the last block in spline interpolation mode is very small and that the following expressions hold:

> F103 × 2

n–1

≤ F103

In the above case, the ending point of the (n–1)-th block is changed to that of the nth block and as a result, the nth block is deleted.

≤

F103

n–1

Created spline curve

F103

× 2

Non-spline block

Deletion of the passi ng point

Fig. 6-14 Fairing at the ending point of a spline curve

This function is executed preferentially over the curve slitting function based on the angle of spline cancellation.

6-29

6 INTERPOLATION FUNCTIONS

D. Feed-rate limitation in spline-interpolation mode

The modal cutting feed rate F remains valid in general for the spline interpolation; however, if the feed rate should be kept constant, it would yield excessively high acceleration at portions where the curvature is big (the curvature radius is small) as shown in Fig. 6-15.

Curvature: Small

cceleration: Lo

Curvature: Big

Fig. 6-15 Change of acceleration depending on curvature

In the spline-interpolation mode of our NC, the feed rate can be controlled so that it does not exceed the allowable limit, calculated from the related parameters, for pre-interpolation acceleration. To obtain an appropriate feed rate for each block of spline interpolation, the limit feed rate F' is calculated by the equation [1] shown below where the smaller between two radii Rs (curvature radius at the starting point of the block) and Re (curvature radius at its ending point) will be regarded as the reference radius R for the block. The modal feed rate F will then be temporarily overridden by F' for the respective block if F>F', so that the whole spline curve can be interpolated block-by-block at the appropriate feed rate according to the curvature radius.

cceleration: High

F’

j+1

Fig. 6-16 Feed-rate limitation for spline interpolation

F' =

∆V =

R × ∆V × 60 × 1000

G1bF (mm/min)

G1btL (msec)

......... [1]

F : Modal feed rate (mm/min) Rs : Curvature radius at the starting

point of block (mm)

Re : Curvature radius at the ending

point of block (mm)

R : Reference curvature radius for

the block (mm) R = min {Rs, Re}

V : Maximum of pre-interpolation

∆

acceleration

F’ : Limit feed rate (mm/min)

6-30

INTERPOLATION FUNCTIONS 6

E. Spline interpolation during tool-diameter offset

The spline interpolation can be performed during tool-diameter offset as follows.

1. Tool-diameter offset (2-dimensional) Shown in Fig. 6-17 is an example that the command route is straight in the section P

polygonal line in the section P in the section P

. The interpolation route with tool-diameter offset is created by the

nPn+1

. . . Pn that is the object of spline interpolation, and straight

1P2

following procedure.

1) In the first step is created a polygonal line P

tool-diameter offset value r compared with the original polygonal line P

2) Next, a point P

points P

(i = 2, 3, . . . n–1) other than the starting point P1 and the ending point Pn of the

'' where

= r on the vector P

PiPi''

0'P1'P2

' . . . Pn'P

' is determined for all the pass

iPi

' that is offset by the

n+1

. . . PnP

0P1P2

spline curve.

3) Spline interpolation is now conducted for the polygonal line P

''P3'' . . . P

1'P2

''Pn' and

n–1

the curve thus created will act an offset path of tool center for the commanded spline curve.

P1'

P2'

P3'

Pn'

n-1

n+1

P0'

0P1

n+1

P2''

P0'

P2'

P1'P

n-1

n+1

Spline curve for commanded

points offset

P0'

P1'

n-1

P2''

Spline curve for commanded

n-1

Pn'

n-1

n+1

Fig. 6-17 Spline interpolation during tool-diameter offset

The spline curve created in the above-mentioned procedure is not the strict offset, indeed, of the commanded spline curve, but an approximation of it.

6-31

6 INTERPOLATION FUNCTIONS

2. 3-dimensional tool-diameter offset In the 3-dimensional tool-diameter offset, each point defined with programmed coordinates

is first offset through the tool radius “r” in the direction of the specified normal vector (i, j, k) and then, the serial points thus offset in the spline-interpolation section are connected in a smooth curve, which will act as the path of tool-radius center for the 3-dimensional spline interpolation.

F. Others

1. The spline interpolation targets the basic coordinate axes of X, Y and Z; however, it is not always required to specify objective axes on commanding the spline interpolation. Moreover, the spline-interpolation command code (G06.1) can be given in a block without any movement command.

Example: N100 G06.1 X_Y_Z0 → N100 G06.1 X_Y_

N200 X_Y_Z_ N200 X_Y_Z_ N300 X_Y_Z_ N300 X_Y_Z_

M M M M

N100 G06.1 F_ ( ← No movement commands) N200 X_Y_Z_ N300 X_Y_Z_

M M

2. The spline-interpolation command (G06.1) falls under the G-code group 01.

3. In the single-block operation mode, the spline interpolation is cancelled and all the respective blocks will individually undergo the linear interpolation.

4. In tool-path check, the blocks of spline interpolation are not actually displayed in a spline curve but in a polygonal line that connects linearly the repective points, which, in case of tool-diameter offset, will have been offset in the same manner as described in the foregoing article E.

5. During spline interpolation, when feed hold is executed, the block for which the feed hold function has been executed will be interpolated, at the beginning of the restart operation along the spline curve existing before the feed hold function was executed, and then the spline curve in the next block onward will be re-created and interpolation executed.

6. Althouth spline interpolation can also be executed in the high-speed maching mode (G05P2 mode), curve shape correction by fairing becomes invalid in the G05P2 mode.

6-32

6-10 NURBS Interpolation: G06.2 (Option)

1. Function

The NURBS interpolation function provides interpolation by performing NURBS-defined CNCinternal computations on the command issued from the CAD/CAM system in the NURBS format. With this optional function, a very smooth interpolation path can be obtained since the interpolation process is performed directly without dividing a NURBS-formatted free-form curve into minute line segments.

2. Definition of the NURBS curve

NURBS, short for Non-Uniform Rational B-Spline, provides rationalization of the B-spline function. The NURBS curve is defined as follows:

INTERPOLATION FUNCTIONS 6

(t)wiP

i,m

i=0

n–1

P(t) =

i,1

(t) =

i=0

1 (xi ≤ t ≤ x 0 (t < x

i,m

(t)w

, x

≤ t ≤ x

m–1

)

i+1

< t)

i+1

n+1

)

Fig. 6-18 NURBS curve

P(t)

i,k

(t) =

(t – xi) N

i+k–1

i,k–1

– x

(t)

– t) N

i+k

- “Pi” and “wi” denote respectively a control point and the weight on the control point.

- “m” denotes the rank, and the NURBS curve of rank “m” is a curve of the (m–1)-th order.

- “x

” denotes a knot (xi ≤ x

), and an array of knots [x0 x1 x2 ... x

i+1

] is referred to as the knot

n+m

vector.

- A variation in parameter “t” from x

- N

(t) is the B-spline basis function expressed by the above recurrence equation.

i, k

m–1

to x

produces NURBS curve P(t).

n+1

Thus the NURBS curve is uniquely defined from the weighted control points and the knot vector.

3. Programming format

G6.2[P] K_X_Y_Z_[R_][F_] ← NURBS interpolation ON

K_X_Y_Z_[R_] K_X_Y_Z_[R_] K_X_Y_Z_[R_]

K_X_Y_Z_[R_] K_ K_ K_ K_ ← NURBS interpolation OFF

P : Rank (omissible) X, Y, Z : Coordinates of the control

point

R : Weight on the control point

(omissible) K : Knot F : Speed of interpolation

(omissible)

– x

i+1,k–1

i+1

MEP300

(t)

6-33

6 INTERPOLATION FUNCTIONS

4. Detailed description

Set the G6.2 code to select the NURBS interpolation mode. Subsequently, designate the rank, the coordinates and weights of the control points, and the knots to determine the shape of the NURBS curve. The modal code G6.2, which belongs to group 1 of G-codes, is of temporary validity and the modal function relieved by a G6.2 code will automatically be retrieved upon cancellation (termination) of the NURBS interpolation. The G6.2 code can only be omitted for an immediately subsequent setting of the next NURBS curve.

Address P is used to set the rank, and the NURBS curve of rank “m” is of the (m–1)-th order, that is, set as the rank

- P2 for a straight line (curve of the first order),

- P3 for a quadratic curve (of the second order) or

- P4 for a cubic curve (of the third order).

Setting another value than 2, 3 and 4 will cause an alarm, and P4 will be used in default of argument P. The rank, moreover, should be specified in the first block (containing the G6.2 code). Designate the control points in as many sequential blocks as required by specifying their respective coordinates and weights at addresses X, Y, Z and R. Argument R denotes the weight proper to each control point (R1.0 will be used in default), and the more the weight is applied, the closer will be drawn the NURBS curve to the control point.

Address K is assigned to knots, and the NURBS curve of rank “m” for an “n” number of control points requires an (n+m) number of knots. The required array of knots, referred to as knot vecto r, is to be designated in sequential blocks, namely: the first knot in the same block as the first control point, the second knot in the same block as the second control point, and so forth. Following the “n” blocks entered thus, designate the remaining “m” knots in single-command blocks. The leading single-command block of argument K also notifies the NC of the completion of entering the control points, and the NURBS interpolation function itself will be terminated with the last block for the “m” knots.

5. Remarks

1. Only the fundamental axes X, Y and Z can undergo the NURBS interpolation.

2. Do not fail to explicitly designate all the required axes X, Y and/or Z in the first block (containing G6.2). Designating a new axis in the second block onward will cause an alarm.

3. Since the first control point serves as the starting point of the NURBS curve, set in the first block (with G6.2) the same coordinates as the final point of the previous block. Otherwise, an alarm will be caused.

4. The setting range for the weight (R) is from 0.0001 to 99.9999. For a setting without decimal point, the least significant digit will be treated as units digit (for example, 1 = 1.0).

5. The knot (K) must be designated for each block. Omission results in an alarm.

6. Knots, as with the weight, can be set down to four decimal digits, and the least significant digit of a setting without decimal point will be regarded as units digit.

7. Knots must be monotonic increasing. Setting a knot smaller than that of the previous block will result in an alarm.

8. The order of addresses in a block can be arbitrary.

6-34

INTERPOLATION FUNCTIONS 6

9. The shape of the NURBS curve can theoretically be modified very flexibly by changing the rank, the positions and weights of the control points, and the knot vector (the relative intervals of knots). In practice, however, manual editing is almost impossible, and a special CAD/CAM system should be used to edit the NURBS curve and create the program for the interpolation. Generally speaking, do not edit manually the program created by a CAD/CAM system for the NURBS interpolation.

6. Variation of curve according to knot vector

The NURBS curve, which in general passes by the control points, can be made to pass through a specific control point by setting a certain number of knots in succession with the same value. In particular, setting as many leading and trailing knots as the rank (value of P) with the respective identical values will cause the NURBS curve to start from the first control point (P the last one (P

The examples given below exhibit a variation of the NURBS curve according to the knot vector with the control points remaining identical.

Example 1: Rank : 4

Number of control points : 6 Knot vector : [ 0.0 1.0 2.0 3.0 4.0 5.0 6.0 7.0 8.0 9.0 ]

) and to end in

The starting point of t he curve differs from the first control point.

Fig. 6-19 NURBS curve for continuously increasing knots

Example 2: Rank : 4

Number of control points : 6 Knot vector : [ 0.0 0.0 0.0 0.0 1.0 2.0 3.0 3.0 3.0 3.0

[1] [2]

Point [1]: The first four (=rank) knots have the same value assigned. Point [2]: The last four (=rank) knots have the same value assigned.

The curve starts from the first control point.

The final point of the curve differs from the last control

oint.

MEP301

]

The curve ends in the last control point.

Fig. 6-20 NURBS curve for some identical knots

MEP302

6-35

6 INTERPOLATION FUNCTIONS

Note 1: The NURBS interpolation can be performed only for the NURBS curve that starts and

ends from the first and in the last control point. Do not fail, therefore, to set as many leading and trailing knots as the rank with the respective identical values.

Note 2: The NURBS interpolation is executed at the designated feed rate (F-code). During the

shape correction mode, however, the interpolation speed is controlled in order that the maximum available acceleration may not be exceeded in the section of a considerable curvature.

7. Compatibility with the other functions

The tables in this section specify the compatibility of the NURBS interpolation with the other functions. Pay attention to the incompatible functions, especially G-codes.

A. Preparatory, feed and auxiliary functions

The table below enumerates the G-codes, F-, M-, S-, T- and B-codes with regard to their availability before, with and after G6.2.

Function Code before G6.2 with G6.2 after G6.2 G-codes of group 00 all G-codes of group 01 all

G-codes of group 04

G-codes of group 06

G-codes of group 07

G-codes of group 09 G-codes of group 12 G54 - G59

G-codes of group 13

G-codes of group 14

G-codes of group 16

G-codes of group 23

High-speed machining mode

Feed function F Auxiliary function MSTB

G54.2P1 - P8 × × ×

!: available ×: not available

G17 G18G-codes of group 02 G19 G22××× G23 G93 G98G-codes of group 05 G99 G20 G21 G40 G41××× G42××× G80

the others × × ×

G61.1 G61.2

G61××× G62××× G63××× G64

G66××× G66.1 × × × G66.2 × × ×

G67 G68.5 × × × G69.5

G54.2P0

G5P0 G5P2×××

××

! (*) ×

××

× ×× ××

××

×× ××

××

× ××

(*) The G-code given last in the block takes priority in group 01.

6-36

INTERPOLATION FUNCTIONS 6

B. Skip instructions

The table below enumerates the skip instructions with regard to their availability before, with and after G6.2.

": available ×: not available

Instruction before G6.2 with G6.2 after G6.2 Optional block skip Control Out/In

× ×

Note: Designating another address than X, Y, Z, R and K in the mode of (i. e. after) G6.2 will

cause an alarm.

C. Interruption and restart

The table below enumerates the functions for interrupting and restarting the program flow with regard to their availability before, with and after G6.2.

": available ×: not available

Function before G6.2 with G6.2 after G6.2 Single-block operation Feed hold Reset Program stop Optional stop Manual interruption

(Pulse feed and MDI) Restart Comparison stop

"""

× " (Note) ×

×× ××

××

×× ××

Note: The single-block stop only occurs between blocks with different knots.

D. Tool path check

The tool path in a section of the NURBS interpolation can only be displayed as if the control points were linearly interpolated (in the mode of G01).

6-37

6 INTERPOLATION FUNCTIONS

8. Sample program

The program section below refers to a NURBS interpolation of rank 4 (cubic curve) for seven control points.

Control points: P

P1 P2 P3 P4 P5 P

Knot vector: [ 0.0 0.0 0.0 0.0 1.0 2.0 3.0 4.0 4.0 4.0 4.0 ]

M M

G90 G01 X0 Y120.F3000

Y100. ............. P

G6.2 P4 X0 Y100.R1.K0... P

X10.Y100.R1.K0.......... P

X10.Y60.R1.K0........... P

X60.Y50.R1.K0........... P

X80.Y60.R1.K1........... P

X100.Y40.R1.K2.......... P

X100.Y0 R1.K3........... P

0 0 1 2 3 4 5 6

K4. K4. K4. K4.

G01 X120................ P

M M

Fig. 6-21 NURBS interpolation and linear interpolation

NURBS interpolation for the control points

Linear interpolation for the control points

MEP303

6-38

9. Related alarms

The table below enumerates the alarms related to the NURBS interpolation.

Alarm list

Alarm

No. 806 ILLEGAL ADDRESS Another address than those for the

807 ILLEGAL FORMAT

809 ILLEGAL NUMBER

816 FEEDRATE ZERO The feed rate (F-code) has not yet been

936 OPTION NOT FOUND The system is not equipped with the

955 START AND END

956 RESTART OPERATION

957 MANUAL INTERRUPT

Alarm message Cause Remedy

nominated axes (X, Y and/or Z), the weight (R) and the knot (K) is set in the G6.2 mode.

1. The modal condition is not appropriate to set G6.2.

2 A block in the G6.2 mode is set without

knot (K).

3. The number of blocks with the same knot in succession does not reach the rank.

1. The number of digits exceeds the

INPUT

POINT NOT AGREE

NOT ALLOWED

specification of axis commands (X, Y or Z).

2. The rank (P) is not admissible. 2. Set 2, 3 or 4 at address P.

3. The value of a knot is not admissible. 3. Set a value in a range of 0.0001 to

4. The knot vector is not monotonic increasing.

designated.

optional function of the NURBS interpolation.

The axis coordinates designated in the block of G6.2 do not correspond to the final point of the previous block.

The designated restart block falls within the mode of G6.2.

An interruption by pulse handle or MDI operation is commanded in the midst of the G6.2 mode.

INTERPOLATION FUNCTIONS 6

Clear the inadequate address.

1. Satisfy the modal condition with reference to item 7-A.

2. Do not fail to set a knot in each block in the G6.2 mode.

3. Set an appropriate knot vector with reference to example 2 given in item 6.

1. Specify the axis command within eight digits.

99.9999.

4. Check the blocks for a decreasing knot.

Set an F-code before or in the same block as the G6.2 code.

Purchase and install the optional function.

Designate in the first block of the NURBS interpolation the same position as the final point of the previous block.

Restart operation is not allowed from the midst of the NURBS interpolation.

Manual interruption is not allowed in the midst of the NURBS interpolation.

6-39

6 INTERPOLATION FUNCTIONS

6-11 Cylindrical Interpolation: G07.1

1. Function and purpose

Cylindrical interpolation refers to a function by which the cylindrical surface of a workpiece can be machined according to a program prepared on its development plane. This function i s amo ng others very efficient in the creation of a cam grooving program.

2. Programming format

A. Selection and cancellation of the cylindrical interpolation mode

- When the A-axis functions as the rotational axis:

G07.1 Ar; Cylindrical interpolation mode ON (r = radius of cam groove bottom) G07.1 A0; Cylindrical interpolation mode OFF

- When the B-axis functions as the rotational axis:

G07.1 Br; Cylindrical interpolation mode ON (r = radius of cam groove bottom) G07.1 B0; Cylindrical interpolation mode OFF

Note 1: The above preparatory function (G-code) must be given in a single-command block. Note 2: Enter a precise value for the radius of the cam groove bottom (r), which is used for the

internal calculation of the dimensions and the rate of feed in the developed plane.

Note 3: Enter a positive value for the radius of the cam groove bottom (r). Note 4: In the mode of cylindrical interpolation the radius of the cam groove bottom (r) cannot

be otherwise modified than to zero. That is, the modification must be done after canceling the mode temporarily.

Note 5: Cylindrical interpolation is not available for machines with a linear type rotational axis

(F85 bit 2 = 1; HV-machines or machines with a tilting table).

Note 6: The figure below refers to a vertical machining center. To perform machining on the

surface of the cylinder, position the tool on the Y-axis to the axis of the cylinder first, perform an infeed on the Z-axis even to the groove bottom and then select the mode of a cylindrical interpolation with simultaneous control of the X- and A-axis.

Fig. 6-22 Diagrammatic view of cylindrical interpolation (1/2)

6-40

INTERPOLATION FUNCTIONS 6

Note 7: The next figure shows a machining center with the fixture mounted perpendicular to the

Y-axis. To use the cylindrical interpolation on such a machine, position the tool on the X-axis to the axis of the cylinder first, perform an infeed on the Z-axis even to the groove bottom and then select the mode of a cylindrical interpolation with simultaneous control of the Y- and B-axis.

Fig. 6-23 Diagrammatic view of cylindrical interpolation (2/2)

B. Commands in the cylindrical interpolation mode

GgXxAaRrIiJjDdPpFf; GgYyBbRrIiJjDdPpFf;

Gg: Refer to Table 6-2 (in paragraph 1 under 3-B) for the available G-codes. Xx/Aa: Cylindrical interpolation occurs in the X-A plane or Y-B plane. Yy/Bb: The values of X (or Y) and A (or B) are of linear and angular dimensions, respectively. Rr: Radius for a circular interpolation Ii: Abscissa (incremental) of the center for a circular interpolation Jj: Ordinate (incremental) of the center for a circular interpolation Dd: Offset number for tool diameter offset Pp/Xx: Dwell time

Ff: Rate of feed (Refer to the detailed description in paragraph 2 under 3-B.)

6-41

6 INTERPOLATION FUNCTIONS

3. Detailed description

A. Conditions necessary for the selection of the cylindrical interpolation mode

The G-code modal states required for the cylindrical interpolation mode selection are as follows:

Table 6-1 Conditions necessary for the mode selection

G-code group Condition G-code group 1 G0/G1 (Positioning or Linear interpolation only) G-code group 2 G17 (X-Y plane only) G-code group 3 G90/G91 (Absolute/Incremental programming) [unconditional] G-code group 4 G22/G23 (Stroke check ON/OFF) [unconditional] G-code group 5 G94/G95 (Asynchronous/Synchronous feed) [unconditional] G-code group 6 G20/G21 (Inch/Metric data input) [unconditional] G-code group 7 G40 (Tool diameter offset OFF) (Note 1) G-code group 8 G43/G49 (Tool length offset ON/OFF) [unconditional] G-code group 9 G80 (Fixed cycle OFF) G-code group 10 Invalid (Return level selection [between initial and R-point] is only valid for fixed

G-code group 11 G50 (Scaling OFF) G-code group 12 G-code group 13 G64 (Cutting mode) G-code group 14 G67 (User macro modal call OFF) G-code group 15 G40.1 (Shaping OFF) G-code group 16 G69 (Programmed coordinates rotation OFF) (Note 2) G-code group 19 G50.1/G51.1 (Mirror image ON/OFF) [unconditional] (Note 3) G-code group 19 No selection of a plane for five-surface machining G-code group 23 G54.2P0 (Dynamic offsetting II OFF) Others G5P0 (High-speed machining OFF) Others G7.1B0 (Cylindrical interpolation OFF)

cycles.)

G54 to G59

，G54.1 (Standard/Additional workpiece coordinate system) [unconditional]

Otherwise the selection will only lead to an alarm. Note 1: Select and cancel the tool diameter offset as required in the mode of cylindrical inter-

polation. An alarm will be caused if the cylindrical interpolation is selected in the mode of tool diameter offset.

Note 2: The cylindrical interpolation cannot be selected in the mode of G68 (3-dimensional

coordinate conversion). On an HV machining center, therefore, the cylindrical interpolation function is not available to an inclined or top surface.

Note 3: To use the cylindrical interpolation with the mirror image function being selected, take

the following precautions in order to prevent errors from occurring in the development of the cylindrical surface:

[1] Set the mirroring center to 0° for the rotational axis of the cylindrical interpolation. [2] Select the cylindrical interpolation with the rotational axis being positioned at its

workpiece origin (0°).

[3] Also cancel the cylindrical interpolation with the rotational axis being positioned at

its workpiece origin (0°).

An example of programming is given later in the sample program under 5-B.

6-42

INTERPOLATION FUNCTIONS 6

B. Commands in the cylindrical interpolation mode

1. The table below enumerates the G-codes available in the cylindrical interpolation mode. Any other G-code will cause an alarm.

Table 6-2 Available G-codes

G-code Function

G0 Rapid positioning G1，G2，G3

G4 Dwell G9 Exact-stop check G17 Plane selection (Note 1) G40，G41，G42

Linear and circular interpolation

Tool diameter offset (

Note 2)

Note 1: After the mode selection by a block of G7.1, do not fail to give a plane selection

command of the following format in order to specify the cylindrical interpolation plane determined by the corresponding linear and rotational axes:

G17X＿A＿ when the A-axis functions as the rotational axis. G17Y＿B＿ when the B-axis functions as the rotational axis.

Note 2: Select and cancel the tool diameter offset as required in the mode of cylindrical inter-

polation. An alarm will be caused if the cylindrical interpolation is selected in the mode of tool diameter offset.

2. In the mode of the cylindrical interpolation the rate of feed refers to a resultant speed (of Fx and Fa, or Fy and Fb) in the plane onto which the surface of the cylinder is developed.

The speed on each component axis is calculated for a block of G1XxAaFf; as follows:

(+x

360

(+x

360

=Fx

=Fa

f•

)r2

f•

)r2

x: metric (0.001 mm) a: degree (0.001°) r: radius of cam groove bottom f: command value of speed

The speed on each component axis is calculated for a block of G1YyBbFf; as follows:

(+y

360

(+y

y b

360

=Fy

=Fb

f•

)r2

f•

)r2

y: metric (0.001 mm) b: degree (0.001°) r: radius of cam groove bottom f: command value of speed

The speed of rapid traverse and the upper limit of cutting feed, both specified in a parameter, are expressed in an angular velocity (°/min) for a rotational axis. The actual linear speed on the rotational axis of the cylindrical interpolation is therefore allowed to increase in the developed plane just in proportion to the radius of the groove bottom.

6-43

6 INTERPOLATION FUNCTIONS

4. Remarks

A. Positioning accuracy (on the rotational axis)

Each angular dimension entered is internally converted into linear one on the circumference, which is to be used in the calculation of the interpolation with the other linear axis. The actual angular motion is then determined by the results of that calculation. As a result, dependi ng on the cylinder radius, positioning errors on the rotational axis may occur in the level of the least significant digit, but they are not cumulative.

0.002 mm

0.001 mm

0.001

0.001°

57.296 85.944 114.432 114.592

Fig. 6-24 Positioning error according to the angle and radius

Error: 0.0005

Error: 0.0009

Radius of cylinder

Unit: mm

B. Changing the radius of the groove bottom

In the mode of cylindrical interpolation, as mentioned before, the radius of the cam groove bottom cannot be otherwise modified than to zero. That is, the modification must be done after canceling the mode temporarily.

C. Rotational axis of the cylindrical interpolation

Only one rotational axis can be used for the cylindrical interpolation. It is not possible to designate multiple rotational axes in a command of G7.1.

D. Manual interruption

1. With “manual absolute” ON

The “manual absolute” function is suspended during cylindrical interpolation, and the first motion block after the cancellation of cylindrical interpolation is executed for the very target position as programmed by canceling the amount of manual interruption. Refer to the example given later under 5-D.

2. With “manual absolute” OFF

The amount of manual interruption remains intact, irrespective of the selection and cancellation of cylindrical interpolation. See the example given under 5-D.

E. Restart operation

For restarting in the middle of the cylindrical interpolation, follow the normal restart procedure to ensure normal operation by retrieving the necessary modal information (on the radius of groove bottom, etc.). Never use the [RESTART 2] menu function that skips the preceding blocks.

F. Resetting

Resetting (by the RESET key on the operating panel) cancels the cylindrical interpolation mode.

6-44

INTERPOLATION FUNCTIONS 6

5. Sample programs

Note: The examples in this section are all given for a cylindrical interpolation in the Y-B plane

(with respect to a machining center as shown in Fig. 6-23). Replace the axis names X, Y and B with Y, X and A, respectively, for a cylindrical interpolation in the X-A plane (on a vertical machining center as shown in Fig. 6-22).

A. Cam grooving program

50. N06

N14

0° 45° 135° 180° 270° 315° 360°

Tool radius

N07

N15

[Offset amount] = [Groov e wi dth] – [Tool radius]

N08

N16

N09

N17

N10

N18

Groove width

Programmed contour

N11

N19

Fig. 6-25 Cam grooving program

N01 G54G0G90X0Y0B0; ..Positioning to the cylinder axis N02 Z0S800M3; N03 G1Z-5.F2000;

........Infeed to the groove bottom

N04 G7.1B63.662;........Cylindrical interpolation ON

N05 G17G1G41Y0B0D1; N06 G2B45.R30.; N07 G3B135.R60.; N08 G1Y50.B180.; N09 G2B270.R60.; N10 G1Y0B315.; N11 G3B360.R30.; N12 G1G40;

N13 G1G42Y0B360.; N14 G2B45.R30.; N15 G3B135.R60.; N16 G1Y50.B180.; N17 G2B270.R60.; N18 G1Y0B315.; N19 G3B360.R30.; N20 G1G40; N21 G7.1B0;

..........Cylindrical interpolation OFF

6-45

6 INTERPOLATION FUNCTIONS

B. Use of mirror image function

50.

–50.

0°

Fig. 6-26 Use of mirror image function

270

N104

300

Main program

N01 G54G0G17G90X0Y0B0; N02 Z0S800M3; N03 M98P2000; N04 G55G0G17G90X0Y0B0; N05 Z0S800M3; N06 G51.1B0; N07 M98P2000; N08 G50.1B0;

..................Mirror image ON

..................Mirror image OFF

N103

45.

G55

135° 225°

45.

N104

G54

60° 90°

Subprogram

N100 G7.1 B47.746 ; N101 G17 G0 Y45.B0 ; N102 G1 Z-5.F1000 ; N103 G2 B60.R25.; N104 G3 B90.R12.5 ; N105 G0 Z0 ; N106 G0 B0 ; N107 G7.1 B0 ; N108 M99 ;

Table 6-3 Workpiece origin data

G54 G55 X0. 0. Y 0. –50. Z0. 0. B 225. 135.

6-46

C. Use of circular interpolation commands

INTERPOLATION FUNCTIONS 6

(mm)

85.

47.5

10.

Radius of groo ve bottom = 63.662 mm

N04

N03

50. 50.

45° 50

90° 100

135° 180°

Fig. 6-27 Use of circular interpolation commands

N01 G90 G1 Y47.5 F1000 ; N02 G7.1 B63.662 ; N03 G17 G1 Y47.5 B45.; N04 G2 B90.R62.5 ; N05 G1 B180.; N06 G3 B270.I50.J37.5 ;

N05

200

(47.5 – 10)

r =

= 62.5 mm

N06

225° 250

270° 300

+ 50

360° 400 (mm)

D. Operation examples with manual interruption

1. With “manual absolute” ON

N1 - N6: Programmed contour N2 - N4: In the mode of cylindrical interpolation

Programmed

contour

Cylindrical interpolation ON

Manual interruption

Fig. 6-28 With “manual absolute” ON

N3: Manual interruption N3 - N4: “Manual absolute” function i gnored (N3’ and N4’) N5: “Manual absolute” function retrieved (N5’)

N3’

Cylindrical interpolation

N4’

N5’

OFF

6-47

6 INTERPOLATION FUNCTIONS

2. With “manual absolute” OFF

Programmed

contour

Fig. 6-29 With “manual absolute” OFF

Manual interruption

Cylindrical interpolation ON

N1 - N6: Programmed contour N2 - N4: In the mode of cylindrical interpolation N3: Manual interruption N3 - N6: “Manual absolu te” function OFF (N3’ to N6’)

N3’

Cylindrical interpolation

N4’

OFF

N5’

N6’

6. Related parameters

1. Set the type of the rotational axis (A or B) as “rotational” (with short-cut approach) in order that the initial angular movement should not occur on the roundabout route for a command of tool diameter offset given in the vicinity of the 0° position.

N21 bit 0 = 0: Setting the type of the rotational axis as rotational

= 1: Short-cut approach valid

2. Set the B- and A-axis as the primary parallel ones to the axis of abscissa and that of the ordinate, respectively.

SU2 = 66: Setting the B-axis as parallel axis 1 for the axis of abscissa SU5 = 65: Setting the A-axis as parallel axis 1 for the axis of the ordinate

3. The following parameter setting is required for a cylindrical interpolation in the X-A plane on vertical machining centers:

F85 bit 7 = 1

4. The following parameter setting is required for inch data input in order that the speed of the angular movement may be calculated appropriately:

F85 bit 4 = 1

7. Related alarms

Table 6-4 Related alarms

Alarm

No. 806 ILLEGAL

2110 ILLEGAL

808 MIS-SET G

936 OPTION NOT

Alarm message Description Remedy

ADDRESS

FORMAT

CODE

FOUND (7, 0, 0)

The address of argument in the block of selecting the cylindrical interpolation does not refer to any rotational axis.

The necessary conditions for the selection of cylindrical interpolation are not yet all satisfied.

An unavailable G-code is given in the mode of cylindrical interpolation.

The optional function for cylindrical interpolation is not provided.

6-48

Use the correct address.

Refer to Table 6-1.

Refer to Table 6-2.

Equip the machine with the option as required.

6-12 Helical Interpolation: G02, G03

1. Function and purpose

Command G02 or G03 with a designation for the third axis allows synchronous circular interpolation on the plane specified by plane-selection command G17, G18 or G19 with the line ar interpolation on the third axis.

2. Programming format

INTERPOLATION FUNCTIONS 6

G17 G02 Xx

Yy1Zz1Ii1 Jj1Pp1Ff

(G03)

G17 G02 Xx

Yy2Zz2 Rr

(G03)

3. Detailed description

1 ;

Pp2Ff

1st

2ndp1-th

2 ;

Feed rate Number of pitches Arc center coordinates Linear axis ending point coordinate Arc ending point coordinates

Feed rate Number of pitches Arc radius Linear axis ending point Arc ending point coordinates

H734P0001

1. For helical interpolation, movement designation is additionally required for one to two linear axes not forming the plane for circular interpolation.

2. The velocity in the tangential direction must be designated as the feed rate F.

3. The pitch l is calculated as follows:

= θe – θs = tan

p1 + θ)/2

π •

–1

– tan–1

0 ≤ θ < 2

（

）

where (xs, ys): relative coordinates of starting point with respect to the arc center

(xe, ye): relative coordinates of ending point with respect to the arc center

4. Address P can be omitted if the number of pitches is 1.

6-49

6 INTERPOLATION FUNCTIONS

5. Plane selection As with circular interpolation, the circular-interpolation plane for helical interpolation is determined by the plane-selection code and axis addresses. The basic programming procedure for helical interpolation is: selecting a circular-interpolation plane using a planeselection command (G17, G18 or G19), and then designating the two axis addresses for circular interpolation and the address of one axis (perpendicular to the circular-interpolation plane) for linear interpolation.

- X-Y plane circular, Z-axis linear

After setting G02 (or G03) and G17 (plane-selection command), set the axis addresses X, Y and Z.

- Z-X plane circular, Y-axis linear

After setting G02 (or G03) and G18 (plane-selection command), set the axis addresses Z, X and Y.

- Y-Z plane circular, X-axis linear

After setting G02 (or G03) and G19 (plane-selection command), set the axis addresses Y, Z and X.

4. Sample programs

Example 1:

G91 G28 X0 Y0 Z0; G92 X0 Z0 Y0; G17 G03 X100. Y50. Z-50. R50. F1000;

Example 2:

G91 G28 X0 Y0 Z0; G92 X0 Z0 Y0; G17 G03 X100. Y50. Z-50. R50. P2 F1000;

Ending

point

Ending

point

–50.

50.

100.

Starting point

100.

Starting point

H734P0002

6-50

H734P0003

7 FEED FUNCTIONS

7-1 Rapid Traverse Rates

A separate rapid traverse rate can be set for each axis. The maximum rate of rapid traverse, however, is limited according to the particular machine specifications. Refer to the Operating manual for the machine for rapid traverse rates. Two types of tool paths are available for positioning: an interpolation type, which uses a line to perform interpolation from the starting point through the ending point, and a non-interpolation type, which moves the tool at the maximum speed of each axis. Use a parameter to select the interpolation type or the non-interpolation type. The positioning time is the same for both types.

7-2 Cutting Feed Rates

A cutting feed rate must be designated using address F and an eight-digit number (F8-digit direct designation). The F8 digits must consist of five integral digits and three decimal digits, with the decimal point. Cutting feed rates become valid for commands G01, G02, G03, G33 and G34.

FEED FUNCTIONS 7

Example: Feed rate

G01 X100. Y100. F200* 200.0 mm/min G01 X100. Y100. F123.4 123.4 mm/min G01 X100. Y100. F56.789 56.789 mm/min

* It means the same if F200. or F200.000 is set in stead of F200.

Note: An alarm (No. 713) will result if a feed rate command is not set for the first cutting

command (G01, G02, G03, G33 or G34) that is read firstly after power-on.

7-3 Asynchronous/Synchronous Feed: G94/G95

1. Function and purpose

Command G95 allows a feed rate per revolution to be set using an F-code. Command G94 retrieves the mode of asynchronous feed (per minuite).

2. Programming format

G94: Feed per minute (/min) [Asynchronous feed] G95: Feed per revolution (/rev) [Synchronous feed]

Since command G95 is modal, it will remain valid until command G94 is issued.

7-1

7 FEED FUNCTI ONS

3. Detailed description

1. Feed rates that can be set using F-codes are listed in the table below.

The table below also lists synchronous feed rates, which are to be set in millimeters (or inches) per spindle revolution using F-codes.

Input in mm 1 to 240000 mm/min (F1 to F240000) 0.0001 to 500.0000 mm/rev (F1 to F5000000) Input in inches 0.01 to 9600.00 in./min (F1 to F960000) 0.000001 to 9.999999 in./rev (F1 to F9999999)

2. The effective feed rate per revolution, that is, the actual moving speed of the machine, can

be calculated as follows: FC = F × N × OVR (Expression 1) where FC: Effective feed rate (mm/min or inches/min)

If multiple axes are selected at the same time, effective feed rate FC given by expression 1 above will become valid for the corresponding vectorial direction.

G94F_ (Feed per minute) G95F_ (Feed per revolution)

F: Designated feed rate (mm/rev or inches/rev) N: Spindle speed (rpm) OVR: Cutting feed override

4. Remarks

1. On the POSITION display, FEED denotes an effective feed rate that is expressed in a feed

rate per minute (mm/min or inches/min), based on the selected feed rat e, the spindle speed, and the cutting feed override.

2. If the effective feed rate should become larger than the cutting feed limit speed, that limit

speed will govern.

3. In the dry run mode, feed will become asynchronous and the machine will operate at an

externally preset feed rate (mm/min or inches/min).

4. According to the setting of bit 1 of parameter F93, synchronous or asynchronous feed mode

(G95 or G94) is automatically made valid upon power-on or by execution of M02 or M30.

7-2

7-4 Selecting a Feed Rate and Effects on Each Control Axis

As mentioned earlier, the machine has various control axes. These control axes can be broadly divided into linear axes, which control linear motions, and rotational axes, which control rotation al motions. Feed rates for control axes have different effects on the tool speed, which is of great importance for machining quality, according to the particular type of axis controlled. The amount of displacement must be designated for each axis, whereas the feed rate is to be designated as a single value for the intended tool movement. Before letting the machine control two or more axes at the same time, therefore, you must understand how the feed rate designated will act on each axis. In terms of this, selection of a feed rate is described below.

1. Controlling linear axes

The feed rate that has been selected using an F-code acts as a linear velocity in the moving direction of the tool, irrespective of whether only one axis is to be controlled or multiple axes simultaneously.

Example: If linear axes (X- and Y-axes) are to be controlled using a feed rate of f:

FEED FUNCTIONS 7

(Tool ending point)

(Tool starting point)

“f” denotes the velocity in this direction.

MEP038

When only linear axes are to be controlled, setting of a cutting feed rate itself is only required. The feed rate for each axis refers to that component of the specified feed rate which corresponds with the ratio of movement stroke on the respective axis to the actual movement distance.

In the example shown above:

X-axis feed rate = f ×

Y-axis feed rate = f ×

+ y

2. Controlling a rotational axis

When a rotational axis is to be controlled, the selected feed rate act s as the rotating speed of the rotational axis, that is, as an angular velocity. Thus, the cutting speed in the moving direction of the tool, that is, a linear velocity varies according to the distance from the rotational center to the tool. This distance must be co nsi dered when setting a feed rate in the program.

7-3

7 FEED FUNCTI ONS

Example 1: If a rotational axis (C-axis) is to be controlled using a feed rate of f (deg/min):

In this case, the cutting speed in the moving direction of the tool (linear velocity) “fc” is calculated by:

fc = f ×

Hence, the feed rate to be programmed for the required value fc is:

f = fc ×

Note: If the tool is to be moved by controlling linear axes along the circumference using the

(Tool ending point)

“f” denotes the angular velocity.

!r!

180

MEP034

Center of

rotation

•

180

•

The linear velocity is obtainable from

(Tool ending point)

circular interpolation function, the feed rate programmed is the velocity acting in the moving direction of the tool, that is, in the tangential direction.

Example 2: If linear axes (X- and Y-axes) are to be controlled at a feed rate of f using the

circular interpolation function:

“f” denotes this linear speed.

MEP040

In this case, the X- and Y-axis feed rates will change with the movement of the tool. The resultant velocity, however, will be kept at the constant value, f.

7-4

FEED FUNCTIONS 7

3. Controlling a linear axis and a rotational axis at the same time

The NC unit controls linear axes and rotational axes in exactly the same manner. For control of rotational axes, data given as a coordinate word (with A, B or C) is handled as an angle, and data given as a feed rate (F) is handled as a linear velocity. In other words, an angle of one degree for a rotational axis is handled as equivalent to a moving distance of 1 mm for a linear axis. Thus, for simultaneous control of a linear axis and a rotational axis, the magnitudes of the individual axis components of the data that has been given by F are the same as those existing during linear axis control described previously in Subparagraph 1. above. In this case, however, the velocity components during linear axis control remain constant in both magnitude and direction, whereas those of rotational axis control change in direction according to the movement of the tool. Therefore, the resulting feed rate in the moving direction of the tool changes as the tool moves.

Example: If a linear axis (X-axis) and a rotational axis (C-axis) are to be controlled at the same

time at a feed rate of f:

Center of rotation

- “fx” is constant in both size and direction.

- “fc” is constant in size, but varies in direction.

- “ft” varies in both size and direction.

MEP036

X-axis incremental command data is expressed here as x, and that of C-axis as c. The X-axis feed rate (linear velocity), fx, and the C-axis feed rate (angular velocity), ω, can be calculated as follows:

fx = f ×

!!!!!!! [1]

+ c

= f ×

+ c

!!!!!!! [2]

The linear velocity “fc” that relates to C-axis control is expressed as:

π •

fc =

•

180

!!!!!!! [3]

If the velocity in the moving direction of the tool at starting point P

is taken as “ft”, and its X- and

Y-axis components as “ftx” and “fty” respectively, then one can express “ftx” and “fty” as follows:

ftx = –r sin (

fty = –r cos (

180

θ) ×

ω + fx !!!!!!! [4]

180

!!!!!!! [5]

where r denotes the distance (in millimeters) from the rotational center to the tool, and q denotes the angle (in degrees) of starting point P

to the X-axis at the rotational center.

7-5

7 FEED FUNCTI ONS

π90π

From expressions [1] through [5] above, the resultant velocity “ft” is:

x2 – x

• c •

r sin (

180

x2 + c

ft =

= f ×

ftx2 + ft

The feed rate f that is to be set in the program must be therefore:

x2 + c

f = ft ×

x2 – x

• c •

r sin (

180

In expression [6], “ft” is the velocity at starting point P of θ which changes according to the rotational angle of the C-axis. To keep cutting speed “ft” as constant as possible, the rotational angle of the C-axis in one block must be minimized to ensure a minimum rate of change of θ.

7-5 Automatic Acceleration/Deceleration

The rapid traverse and manual feed acceleration/deceleration pattern is linear acceleration and linear deceleration. Time constant T 1 msec steps within a range from 1 to 500 msec. The cutting feed (not manual feed) acceleration/deceleration pattern is exponential acceleration/deceleration. Time constant T independently for each axis using parameters in 1 msec steps within a range from 1 to 500 msec. (Normally, the same time constant is set for each axis.)

R can be set independently for each axis using parameters in

)

• r •

+ ( )

180

!!!!!!! [6]

!!!!!!! [7]

180

and thus the value of ft changes with that

• r •

+ ( )

)

C can be set

Rapid feed acceleration/deceleration pattern

= Rapid feed time constant)

= Deceleration check time)

Continuous command

Cutting feed acceleration/deceleration pattern

= Cutting feed time constant)

Continuous command

TEP037

During rapid traverse and manual feed, the following block is executed after the command pulse of the current block has become “0” and the trackin g error of the acceleration/deceleration circuit has become “0”. During cutting feed, the following block is executed as soon as the command pulse of the current block becomes “0” and also the following block can be executed when an external signal (error detection) can detect that the tracking error of the acceleration/d eceleration circuit has reached “0”. When the in-position check has been made valid (selected by machine parameter) during the deceleration check, it is first confirmed that the tracking error of the acceleration/deceleration circuit has reached “0”, then it is checked that the position deviation is less than the parameter setting, and finally the following block is executed.

7-6

7-6 Speed Clamp

This function exercises control over the actual cutting feed rate in which override has been applied to the cutting feed rate command so that the speed clamp value preset independently for each axis is not exceeded.

Note: Speed clamping is not applied to synchronous feed.

7-7 Exact-Stop Check: G09

1. Function and purpose

Only after the in-position status has been checked following machine deceleration and stop or after deceleration checking time has been passed, may you want to start the next block command in order to reduce possible machine shocks due to abrupt changes in tool feed rate and to minimize any rounding of workpieces during corner cutting. An exact-stop check function is provided for these purposes.

2. Programming format

G09 G01 (G02, G03) ;

FEED FUNCTIONS 7

Exact-stop check command G09 is valid only for the cutting command code (G01, G02, or G03) that has been set in that block.

3. Sample program

N001 G09 G01 X100.000 F150; The next block is executed after an in-position status

check following machine deceleration and stop.

N002 Y100.000 ;

(Selected feedrate)

X-axis

N001

Y-axis

N002

The solid line indicates a feedrate pattern with the G09 available. The dotted line indicates a feedrate pattern without the G09.

Fig. 7-1 Validity of exact-stop check

Time

N001

Without G09

Tool

With G09 available

N002

TEP038

7-7

7 FEED FUNCTI ONS

4. Detailed description A. Continuous cutting feed commands

Preceding block

Fig. 7-2 Continuous cutting feed commands

B. Cutting feed commands with in-position status check

Preceding block Next block

Ts Ts

Next block

TEP039

TEP040

Fig. 7-3 Block-to-block connection in cutting feed in-position status check mode

In Fig. 7-2 and 7-3 above,

Ts: Cutting feed acceleration/deceleration time constant Lc: In-position width

As shown in Fig. 7-3, in-position width Lc represents the remaining distance within the block immediately preceding the next block to be executed.

The in-position width helps keep any rounding of workpieces during corner cutting within a fixed level.

If rounding of workpieces at corners is to

Next block

be completely suppressed, include dwell command G04 between cutting blocks.

Preceding block

TEP041

7-8

mazak Mazatrol Matrix Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

Preface

Rule

Basics

Remarks on the cutting conditions recommended by the NC

Programming

Operations

BEFORE USING THE NC UNIT

Limited Warranty

Operating Environment

Keeping the Backup Data

1 CONTROLLED AXES

1-1 Coordinate Words and Controlled Axes

2 UNITS OF PROGRAM DATA INPUT

2-1 Units of Program Data Input

2-2 Units of Data Setting

2-3 Ten-Fold Program Data

3 DATA FORMATS

3-1 Tape Codes

3-2 Program Formats

3-3 Tape Data Storage Format

3-4 Optional Block Skip

3-5 Program Number, Sequence Number and Block Number: O, N

3-6 Parity-H/V

3-7 List of G-Codes

4 BUFFER REGISTERS

4-1 Input Buffer

4-2 Preread Buffer

5 POSITION PROGRAMMING

5-1 Dimensional Data Input Method

5-1-1 Absolute/Incremental data input: G90/G91

5-2 Inch/Metric Selection: G20/G21

5-3 Decimal Point Input

6 INTERPOLATION FUNCTIONS

6-1 Positioning (Rapid Feed): G00

6-2 One-Way Positioning: G60

6-3 Linear Interpolation: G01

6-4 Circular Interpolation: G02, G03

6-5 Radius Designated Circular Interpolation: G02, G03

6-6 Spiral Interpolation: G2.1, G3.1 (Option)

6-7 Plane Selection: G17, G18, G19

6-7-1 Outline

6-7-2 Plane selection methods

6-8 Virtual-Axis Interpolation: G07

6-9 Spline Interpolation: G06.1 (Option)

6-10 NURBS Interpolation: G06.2 (Option)

6-11 Cylindrical Interpolation: G07.1

6-12 Helical Interpolation: G02, G03

7 FEED FUNCTIONS

7-1 Rapid Traverse Rates

7-2 Cutting Feed Rates

7-3 Asynchronous/Synchronous Feed: G94/G95

7-4 Selecting a Feed Rate and Effects on Each Control Axis

7-5 Automatic Acceleration/Deceleration

7-6 Speed Clamp

7-7 Exact-Stop Check: G09