brother TC-32B Programming Manual

TC-32B	Title

TC-32B

NC PROGRAMMING

MANUAL

Please read this manual carefully before starting operation.

2003/4/21	1	eTCOMNCPRT1.doc

TC-32B	Title

This manual describes the NC-Programming of the TC-32B.

The tapping centre is able to perform drilling, tapping, and facing.

We shall not bear any responsibility for accidents caused by user's special handling or handling deviating from the generally recognized safe operation.

The relation between the manuals is as follows.

-OPERATION MANUAL

This manual describes the operations of the machine.

-INSTALLATION MANUAL

This manual describes the installation of the machine.

-PROGRAMMING MANUAL

This manual describes the programming of the machine.

Keep this manual for future reference.

Please include this manual when reselling this product.

When this manual or labels are lost or damaged, please replace them (charged) from your nearest agency.

This manual is printed by using paper obtained from farmed trees.

2003/3/20

2

eTCOMNCPRT1.doc

TC-32B	Title

INTRODUCTION

Congratulations on your purchase of the Brother CNC

tapping center. Correct usage of the machine is of most importance to assure the expected machine capabilities and functions as well as operator's safety. Read this Manual thoroughly before starting operation.

*All rights reserved: No part of this manual may be reproduced, stored in a retrieval system, or transmitted in any form without prior permission of the manufacturer.

*The contents of this Manual are subject to change without notice.

*This manual are complied with utmost care. If you encounter any question or doubt, please contact your local dealer.

©Copyrigt 2004 BROTHER INDUSTRIES,LTD. Machinery & Solution Company. Machine Tools Field. ALL RIGHTS RESERVED.

2003/4/21

3

eTCOMNCPRT1.doc

TC-32B	Title

HOW TO USE THE MANUAL

This Instruction Manual consists of the following elements:

(1)General description Is an outline of the description given in the section.

(2)	Alarm	Is a alert given against a danger which may cause serious
		damage or death to human being or may damage the machine.
		The hazards are explained in this order:

degree of danger, subject of danger, expected damage, preventive measure,

(3)Operation procedure Is a procedure of activating a function.

(4) Screen

Is given to describe important points of a procedure given.

NOTE: This screen is only a representation of the information displayed on the actual screen and therefore differs somewhat from the actual screen

layout and screen fonts.

(5)Illustration Is a sketch, figure, view, etc. indicating dimensions, position or zone, given

	in the points where it is necessary to provide complementary information to the text
	description.
(2) Alarm	(3) Operation procedure	(1) General description

1.3Precautions of first

WARNING

Dropping a heavy object onto your foot may fracture your foot bones.

When lifting heavy objects, wear safety shoes.

1.3.1Before starting operation

Before starting operation careful to read bellow.

(1)Turn off the main power breaker handle on

the control box door. Never touch the primary side power source or the terminal of the main power breaker, as these have high voltage applied.

(2)Put up a signboard which says' Under Maintenance (3)Never allow people to approach the machine,

particularly moving areas.

(4)Do not place any unnecessary object around the machine.

(5)Wear a helmet and safety shoes.

1 - 2 1 - 3

(5) Illustration (4) Screen

2003/3/20

4

eTCOMNCPRT1.doc

TC-32B Contents

Chapter 1		Program Composition--------------------------------	1-1
1.1	Types and composition of program ------------------------------------		1-2
1.2	Composition of block -------------------------------------------------------		1-2
1.3	Composition of word --------------------------------------------------------		1-3
1.4	Numerical values ----------------------------------------------------------		1-3
1.5	Sequence number ---------------------------------------------------------------		1-4
1.6	Optional block skip -------------------------------------------------------------		1-4
1.7	Control out/in function---------------------------------------------------------		1-4

Chapter 2		Coordinate Command --------------------------------	2-1
2.1	Coordinate system and coordinate value-------------------------------		2-2
2.2	Machine zero point and machine coordinate system---------------		2-3
2.3	Working coordinate system--------------------------------------------------		2-3

Chapter 3			Preparation Function ---------------------------------	3-1
3.1	Outline of G code ----------------------------------------------------------------			3-2
3.2	Positioning (G00) ------------------------------------------------------------			3-9
3.3	Linear interpolation (G01) ----------------------------------------------------			3-10
	3.3.1 Chamfering to desired angle and cornering C ----------------------------------------------			3-11
3.4	Circular/helical interpolation (G02, G03) --------------------------------			3-14
	3.4.1	Circular interpolation ---------------------------------------------------------------------------		3-14
	3.4.1.1		Circular interpolation ----------------------------------------------------------------------	3-14
	3.4.1.2		XZ Circular interpolation -----------------------------------------------------------------	3-15
	3.4.1.3		YZ Circular interpolation -----------------------------------------------------------------	3-16
	3.4.2	Helical interpolation-----------------------------------------------------------------------------		3-20
	3.4.3 Spiral interpolation (G02, G03) ---------------------------------------------------------------			3-21
	3.4.4 Conical interpolation (G02, G03) -------------------------------------------------------------			3-23

3.4.5Cutter compensation procedure for spiral interpolation and conical interpolation

		(G02, G03)----------------------------------------------------------------------------------------	3-26
3.5	Circle Cutting (G12, G13) -----------------------------------------------------		3-27
3.6	Plane Selection (G17, G18, G19) -------------------------------------------		3-28
3.7	Dwell (G04)-------------------------------------------------------------------------		3-29
3.8	Exact stop check (G09, G61, G64) -----------------------------------------		3-29
3.9	Programmable data input (G10) --------------------------------------------		3-31
3.10	Soft limit ----------------------------------------------------------------------------		3-34
	3.10.1	Stroke --------------------------------------------------------------------------------------------	3-34
	3.10.2	Stroke limit --------------------------------------------------------------------------------------	3-34
	3.10.3 Programmable stroke limit (G22) -----------------------------------------------------------		3-35
3.11	Return to the reference point (G28) ---------------------------------------		3-36
3.12	Return from the reference point(G29)------------------------------------		3-37
3.13	Return to the 2nd/3rd/4th reference point (G30)----------------------		3-37
3.14	Selection of machine coordinate system (G53)-----------------------		3-37
3.15	Selection of working coordinate system (G54~G59)----------------		3-38
3.16	Additional working coordinate system selection (G54.1) ---------		3-38
3.17	Scaling (G50, G51) --------------------------------------------------------------		3-39
3.18	Programmable Mirror Image (G50.1, G51.1)----------------------------		3-43
3.19	Rotational transformation function (G68,G69) ------------------------		3-46
3.20	Coordinate rotation using measured results(G168)-----------------		3-48
3.21	Absolute command and incremental command (G90, G91)------		3-48
3.22	Change of workpiece coordinate system(G92) -----------------------		3-50
3.23	Skip function (G31,G131,G132)---------------------------------------------		3-52
3.24	Continuous skip function (G31) --------------------------------------------		3-53
3.25	Change of tap twisting direction(G133,G134) -------------------------		3-53
3.26	High speed peck drilling cycle (G173)) ----------------------------------		3-54

2004/01/19

1

eTCOMNCPRC.doc

TC-32B		Contents
3.27	Peck drilling cycle (G183) ----------------------------------------------------	3-55
3.28	Local coordinate system function (G52) --------------------------------	3-56
3.29	Single direction positioning function(G60)-----------------------------	3-57
3.30	G code priority--------------------------------------------------------------------	3-58

Chapter 4			Preparation Function (tool offset function) ----		4-1
4.1	Tool Dia Offset(G40,G41,G42)-----------------------------------------------				4-2
	4.1.1	Tool dia offset function-------------------------------------------------------------------------			4-2
	4.1.1.1 Tool dia fine compensation---------------------------------------------------------------				4-2
	4.1.2	Cancel Mode -------------------------------------------------------------------------------------			4-3
	4.1.3	Start -up -------------------------------------------------------------------------------------------			4-4
	4.1.3.1		Inside cutting -------------------------------------------------------------------------------		4-4
	4.1.3.2		Outside cutting (90° ≤ θ <	180°)---------------------------------------------------------	4-5
	4.1.3.3		Outside cutting (θ < 90°)------------------------------------------------------------------		4-6
	4.1.4		Offset Mode-------------------------------------------------------------------------------------		4-7
	4.1.4.1		Inside cutting (180° ≤ θ ) ------------------------------------------------------------------		4-7
	4.1.4.2		Outside cutting (90° ≤ θ <	180°)---------------------------------------------------------	4-9
	4.1.4.3		Outside cutting (θ < 90°)------------------------------------------------------------------		4-10
	4.1.4.4		Exceptional case ----------------------------------------------------------------------------		4-11
	4.1.5	Offset Cancel -------------------------------------------------------------------------------------			4-12
	4.1.5.1		Inside cutting (180° ≤ θ ) ------------------------------------------------------------------		4-12
	4.1.5.2		Outside cutting (90° ≤ θ <	180°)---------------------------------------------------------	4-12
	4.1.5.3		Outside cutting (θ < 90°)------------------------------------------------------------------		4-14
	4.1.6	G40 single command----------------------------------------------------------------------------			4-15
	4.1.7 Change of offset direction in offset mode ---------------------------------------------------				4-16
	4.1.8 Change of offset direction in offset mode --------------------------------------------------				4-17
	4.1.8.1 When there is a cross point --------------------------------------------------------------				4-17
	4.1.8.2 When there is no cross point -------------------------------------------------------------				4-18
	4.1.8.3 When offset path becomes more than a circle -----------------------------------------				4-19
	4.1.9 G cord command for tool dia offset in offset mode----------------------------------------				4-20
	4.1.10 Notes on tool dia offset -------------------------------------------------------------------------				4-21
	4.1.11 Override function related to tool dia offset--------------------------------------------------				4-29
	4.1.11.1 Automatic corner override --------------------------------------------------------------				4-29
	4.1.11.2 Override of the inside circular cutting-------------------------------------------------				4-30
	4.2		Tool length offset (G43,G44,G49) -----------------------------------		4-31
	4.2.1 Tool length fine offset --------------------------------------------------------------------------				4-31

Chapter 5		Preparation Function (canned cycle)------------	5-1
5.1	List of canned cycle function -----------------------------------------------		5-2
5.2	Basic motions in canned cycle ---------------------------------------------		5-3
5.3	General description of canned cycle ------------------------------------		5-4
	5.3.1	Command related to canned cycle motions------------------------------------------------	5-4
	5.3.2	Setting of data in absolute / incremental command --------------------------------------	5-4
	5.3.3	Types of return point (G98,G99) ------------------------------------------------------------	5-5
	5.3.4	Canned cycle motion conditions-------------------------------------------------------------	5-5
	5.3.5	Machining data of canned cycle -------------------------------------------------------------	5-6
	5.3.6	Repeat number of canned cycle--------------------------------------------------------------	5-7
5.4	Details of Canned Cycle-------------------------------------------------------		5-8
	5.4.1	High-speed peck drilling cycle (G73) ------------------------------------------------------	5-8
	5.4.2	Reverse tapping cycle (G74) -----------------------------------------------------------------	5-9
	5.4.3	Fine boring cycle (G76)-----------------------------------------------------------------------	5-10
	5.4.4	Tapping cycle (G77)---------------------------------------------------------------------------	5-11
	5.4.5	Reverse tapping cycle (Synchro mode) (G78) --------------------------------------------	5-12
	5.4.6	Drilling cycle (G81,G82) ---------------------------------------------------------------------	5-13
	5.4.7	Peck drilling cycle (G83) ---------------------------------------------------------------------	5-15
	5.4.8	Tapping cycle (G84)---------------------------------------------------------------------------	5-16
	5.4.9	Boring cycle (G85,G89) ----------------------------------------------------------------------	5-17
	5.4.10	Boring cycle (G86)-----------------------------------------------------------------------------	5-18
	5.4.11 Back boring cycle (G87) ----------------------------------------------------------------------		5-20

2004/01/23

2

eTCOMNCPRC.doc

TC-32B		Contents
5.4.12 End mill tap cycle (G177) --------------------------------------------------------------------		5-21
5.4.13 End mill tap cycle (G178) --------------------------------------------------------------------		5-22
5.4.14	Double drilling cycle (G181,G182) ---------------------------------------------------------	5-23
5.4.15	Double boring cycle (G185,G189) ----------------------------------------------------------	5-24
5.4.16	Double boring cycle (G186)------------------------------------------------------------------	5-25
5.4.17	Canned cycle of reducing step ---------------------------------------------------------------	5-26
5.4.18	Canned cycle cancel (G80) -------------------------------------------------------------------	5-32
5.4.19	Notes on canned cycle ------------------------------------------------------------------------	5-33

5.5 Canned cycle for tool change (non-stop ATC)(G100)---------------5-34

Chapter 6		Preparation Function (coordinate calculation)6-1
6.1	List of coordinate calculation function ----------------------------------		6-2
6.2	Coordinate calculation parameter -----------------------------------------		6-2
6.3	Details of coordinate calculation function------------------------------		6-3
	6.3.1	Bolt hole circle ---------------------------------------------------------------------------------	6-3
	6.3.2	Linear (Angle) ----------------------------------------------------------------------------------	6-4
	6.3.3	Linear (X,Y) ------------------------------------------------------------------------------------	6-4
	6.3.4	Grid --------------------------------------------------------------------------------------------	6-5
6.4	Usage of coordinate calculation function-------------------------------		6-6

Chapter 7		Macro-------------------------------------------------------		7-1
7.1	What is a Macro? ----------------------------------------------------------------			7-2
7.2	Variable Function----------------------------------------------------------------			7-3
	7.2.1	Outline of variable function ------------------------------------------------------------------		7-3
	7.2.2	Expression of variable-------------------------------------------------------------------------		7-3
	7.2.3	Undefined variable-----------------------------------------------------------------------------		7-4
	7.2.4	Types of variables------------------------------------------------------------------------------		7-5
	7.2.5	Variable display and setting ------------------------------------------------------------------		7-6
	7.2.6	System variable---------------------------------------------------------------------------------		7-7
7.3	Calculation		Function ---------------------------------------------------------	7-12
	7.3.1	Calculation type --------------------------------------------------------------------------------		7-12
	7.3.2	Calculation order -------------------------------------------------------------------------------		7-12
	7.3.3	Precautions for calculation -------------------------------------------------------------------		7-13
7.4	Control Function---------------------------------------------------------------			7-14
	7.4.1	GOTO	statement (unconditional branch)------------------------------------------------	7-14
	7.4.2	IF statement (conditional branch)-----------------------------------------------------------		7-14
	7.4.3	WHILE statement (repetition)---------------------------------------------------------------		7-15
	7.4.4	Precautions for control function-------------------------------------------------------------		7-16
7.5	Call	Function--------------------------------------------------------------------		7-18
	7.5.1	Simple call function ---------------------------------------------------------------------------		7-19
	7.5.2	Modal call function----------------------------------------------------------------------------		7-20
	7.5.3	Macro call argument --------------------------------------------------------------------------		7-21
	7.5.4	Difference between G65 and M98----------------------------------------------------------		7-23
	7.5.5	Multiple nesting call---------------------------------------------------------------------------		7-24

Chapter 8		Automatic work measurement---------------------	8-1
8.1	Before automatic work measurement ------------------------------------		8-4
8.2	Setting of data on automatic work measurement --------------------		8-4
8.3	Operation of automatic work measurement----------------------------		8-9
	8.3.1	Corner --------------------------------------------------------------------------------------------	8-9
	8.3.2	Parallel -------------------------------------------------------------------------------------------	8-13
	8.3.3	Circle ---------------------------------------------------------------------------------------------	8-16
	8.3.4	Z level --------------------------------------------------------------------------------------------	8-20
	8.3.5 Positioning to the measurement position---------------------------------------------------		8-20
8.4	Handling of measured results-----------------------------------------------		8-21
	8.4.1 Display of the measured results--------------------------------------------------------------		8-21
	8.4.2 Reflection of measured results on the workpiece coordinate system------------------		8-22
8.5	Lock key operations ------------------------------------------------------------		8-24

2004/01/19

3

eTCOMNCPRC.doc

TC-32B Contents

Chapter 9		High Accuracy Mode A---------------------------------	9-1
9.1	Outline-------------------------------------------------------------------------------		9-2
9.2	Usage --------------------------------------------------------------------------------		9-3
	9.2.1	User parameter setting ------------------------------------------------------------------------	9-3
	9.2.2	User parameter description -------------------------------------------------------------------	9-4
	9.2.3	Usage in a program ----------------------------------------------------------------------------	9-5
	9.2.4	Conditions available ---------------------------------------------------------------------------	9-6
	9.2.5	Conditions where high accuracy mode A is released ------------------------------------	9-6
9.3	Restrictions------------------------------------------------------------------------		9-7
	9.3.1	Functions available ----------------------------------------------------------------------------	9-7
	9.3.2	Additional axis travel command -------------------------------------------------------------	9-7
9.4	Effective Functions -------------------------------------------------------------		9-8
	9.4.1	Automatic corner deceleration function ----------------------------------------------------	9-8
	9.4.2	Automatic arc deceleration function -------------------------------------------------------	9-9
	9.4.3	Automatic curve approximation deceleration ---------------------------------------------	9-10

Chapter 10 Subprogram function ---------------------------------		10-1
10.1	Making subprogram ------------------------------------------------------------	10-2
10.2	Simple call ----------------------------------------------------------------------	10-3
10.3	Return No. designation from sub program-----------------------------	10-4
	10.3.1 Command by sub program--------------------------------------------------------------------	10-4
	10.3.2 Command by main program------------------------------------------------------------------	10-4

Chapter 11			Feed function--------------------------------------------	11-1
Chapter 12			S,T,M function-------------------------------------------	12-1
12.1	S function --------------------------------------------------------------------------			12-2
12.2	T function --------------------------------------------------------------------------			12-2
	12.2.1 Commanded by tool No. ----------------------------------------------------------------------			12-2
	12.2.2 Commanding by pot No. (magazine No.) --------------------------------------------------			12-2
	12.2.3 Commanded by group No.--------------------------------------------------------------------			12-2
12.3	M function--------------------------------------------------------------------------			12-3
	12.3.1	Program stop (M00) ---------------------------------------------------------------------------		12-7
	12.3.2	Optional stop (M01) ---------------------------------------------------------------------------		12-7
	12.3.3 End of program (M02, M30) -----------------------------------------------------------------			12-7
	12.3.4 Commands on the spindle (M03, M04, M05, M19, M111)-----------------------------			12-7
	12.3.4.1		Spindle orientation to desired angle (M19) ---------------------------------------	12-7
	12.3.5 M signal level output (M400~M409) -------------------------------------------------------			12-7
	12.3.6	Tool change (M06)-----------------------------------------------------------------------------		12-8
	12.3.7 Workpiece counter specification (M211~M214) -----------------------------------------			12-12
	12.3.8 Workpiece counter cancel (M221~M224) -------------------------------------------------			12-12
	12.3.8.1		Tool life counter -----------------------------------------------------------------------	12-12
	12.3.9	Automatic corner deceleration (M232, M233) ------------------------------------------		12-12
	12.3.10 Tool breakage detection (M120 and M121)----------------------------------------------			12-12
	12.3.11 Tool breakage detection (M200 and M201)----------------------------------------------			12-12
	12.3.12 Tap time constant selection (M241 to 250) ----------------------------------------------			12-13
	12.3.13 Pallet related M codes (M410, M411, M430, and M431) -----------------------------			12-13
	12.3.14 Unclamping and clamping C axis (M430 and M431) ----------------------------------			12-13
	12.3.15 Unclamping and clamping B axis (M440 and M441) ----------------------------------			12-13
	12.3.16 Unclamping and clamping A axis (M442 and M443) ----------------------------------			12-13
	12.3.17 One-shot output (M450, M451, M455, and M456)-------------------------------------			12-13
	12.3.18 Waiting until response is given (M460 to M469) ---------------------------------------			12-14
	12.3.19 Magazine rotate speed (M435 to M437)--------------------------------------------------			12-14
	12.3.20 Magazine rotate to tool setting position (M501 to M599) -----------------------------			12-14
	12.3.21 Positioning finished check distance (M270 to M279)----------------------------------			12-14

2004/01/23

4

eTCOMNCPRC.doc

TC-32B	Contents
Chapter 13 Option------------------------------------------------------	13-1

13.1Programming precautions when using rotation axis

(index table) -----------------------------------------------------------------------

13-2

2004/01/19

5

eTCOMNCPRC.doc

TC-32B	Contents

(This page is a blank.)

2004/01/23

6

eTCOMNCPRC.doc

TC-32B

Quick index

	Chpt. 1	PROGRAM COMPOSITION
	Chpt. 2	COORDINATE COMMAND
	Chpt. 3	PREPARATION FUNCTION
	Chpt. 4	PREPARATION FUNCTION
		(TOOL OFFSET FUNCTION)
	Chpt. 5	PREPARATION FUNCTION (CANNED CYCLE)
	Chpt. 6	PREPARATION FUNCTION
		(COORDINATE CALCULATION))
	Chpt. 7	MACRO
	Chpt. 8	AUTOMATIC WORK MEASUREMENT
	Chpt. 9	HIGH ACCURACY MODE
	Chpt.10	SUBPROGRAM FUNCTION
	Chpt.11	FEED FUNCTION
	Chpt.12	S, T, M FUNCTION
	Chpt.13	OPTION

1

2

3

4

5

6

7

8

8

9

10

11

12

13

2004/01/16

1

eTCOMPRIN.doc

Quick index

TC-32B

(This page is a blank.)

2003/04/14

2

TCOMCOOP8-2

TC-32B	Chapter 1 Program Composition

1

CHAPTER 1

PROGRAM COMPOSITION

1.1Types and composition of program

1.2Composition of block

1.3Composition of word

1.4Numerical values

1.5Sequence number

1.6Optional block skip

1.7Control out/in function

2004/01/22

1 - 1

eTCOMNCPR1-1.doc

Chapter 1 Program Composition	TC-32B

1.1Types and Composition of Program

The program is divided into the main program and the subprogram.

(1) Main program

The main program is for machining one workpiece. While the main program is in use, a 1 subprogram can be called to use the program more efficiently.

Command M02 (or M30) to finish the main program.

Main program

N0001 G92X100;

N0002 G00Z30

:

:

:

M02;

(2) Subprogram

A subprogram is used by calling it from the main program or other subprograms. Command M99 to finish the subprogram.

Subprogram

N0100 G91X10;

:

:

:

M99;

1.2Composition of Block

The program is composed of several commands. One command is called a block. A block is composed of one or more words. One block is discriminated from another block by an end of block code (EOB).

This manual expresses the end of block code by the symbol ";".

;

N0001 G92X100

;

;

M02

;

Block

Block

(Note 1) The end of block code

ISO code : [LF] 0A(hexadecimal) EIA code : [CR] 80(hexadecimal)

(Note 2) One block has maximum 128 characters.

2004/01/22

1 - 2

eTCOMNCPR1-1.doc

TC-32B	Chapter 1 Program Composition

1.3Compositiom of Word

A word is composed of an address and some digit of figures as shown below. (Algebraic sign + or - may added before a numerical value.)

X	-1000	1
Address numerical value

Word

(Note 1) The address uses one of the alphabetical letters.

(Note 2) The address "O" can not be used except for comments.

1.4Numerical Values

(1) Decimal point programming

Numerical values can be input in the following two ways and set by the user parameter (Switch 1).

Command type 1 (Standard)

Programmed command		Commanded axis	Actual amount (mm)	Actual amount (inch)
	1	Feed axis	1mm	1 inch
		Rotation axis	1 deg	1 deg
	1.	Rotation axis	1 mm	1 inch
		Rotation axis	1 deg	1 deg
Command type 2 (Minimum)
Programmed command		Commanded axis	Actual amount (mm)	Actual amount (inch)
	1	Feed axis	0.001 mm	0.0001 inch
		Rotation axis	0.001 deg	0.001 deg
	1.	Rotation axis	1 mm	1 inch
		Rotation axis	1 deg	1 deg
(Note)	User parameter : Refer to Instruction manual.

(2) Programmable range of address

The maximum number of digits is 9.

The digits less than the minimum range are ignored.

2004/01/22

1 - 3

eTCOMNCPR1-1.doc

Chapter 1 Program Composition	TC-32B

1.5Sequence Number

A sequence number (1~99999) can be used following the address N for each block.

		Command format		N *****;
	1	i)	A sequence number is used following the address N.
		ii)	A sequence number can be specified with up to 5-digit number.

(Note 1) The sequence number "N0" should not be used. (Note 2) It is used at the head of a block.

Ex.) N0100 G90X100;

When a block has a slash (/) code at the head of block (the optional block skip is commanded), a sequence number can be used either before or after it.

Ex.) N0100/ G90X100; or /N0100 G90X100;

(Note 3)

The order of sequence numbers is arbitary and need not be consecutive. (Note 4)

The sequence number is recognized as numerical values. Therefore such numerical values as 0001, 001, 01 and 1 are regarded as the same number.

1.6Optional Block Skip

When a block has a slash (/) code at the start and [BLOCK SKIP] key on the operation panel is turned ON, all information in the block with the slash code is ignored during the automatic operation.

If the [BLOCK SKIP] key is OFF, information in the block with the slash code is effective. That is, the block with a slash code can selectively be skipped.

..... ;

/ N0100 G00X100 .....

;

N0101 .....

Ignore these words

(Note 1)

A slash (/) code must be put at the start of a block. If it is placed elsewhere in the block, an alarm is generated.

This code can be also put right after a sequence number. (Note 2)

In the single block mode during automatic operation, when the [BLOCK SKIP] key is ON the operation does not stop at a block with a slash code, but stops at the next block.

1.7Control Out/In Function

For a easier look at the program, comments can be inserted in the program.

The comment is discriminated from operation by "(" and ")" at the start and the end.

(		............. )
(Ex.)	N1000 G00X200 (PRO-1);

(Note)

A comment including the control out and in codes should not be longer than one block.

2004/01/22

1 - 4

eTCOMNCPR1-1.doc

TC-32B	Chapter2 Coordinate Command

2

CHAPTER 2

COORDINATE COMMAND

2.1Coordinate system and coordinate value

2.2Machine zero point and machine coordinate system

2.3Working coordinate system

2004/01/22

2 - 1

eTCOMNCPR2-1.doc

Chapter2 Coordinate Command	TC-32B

2.1Coordinate system and coordinate value

Coordinate values should be set in one coordinate system to specify a tool movement.

There are two types of coordinate systems.

(i)Machine coordinate system

(ii)Working coordinate system

The coordinate values are expressed by each component of the program axes (X, Y and Z for this unit).

2

Z

Y

Tool target position:

CommandedX20.Y10.Z15

15

10

X

0	20

eNCPR2.01.ai

2004/01/22

2 - 2

eTCOMNCPR2-1.doc

TC-32B	Chapter2 Coordinate Command

2.2Machine Zero Point and Machine Coordinate System

(1) Machine zero point

The machine zero point is the reference point on the machine.

(2) Machine coordinate system
The coordinate systen with the machine zero point as its reference point is called the machine
coordinate system. Each machine has its own coordinate system.					2
			Machine zero point
		X axis stroke	(0,0,0)
	-X

Y axis stroke

Table

-Y

eNCPR2.02.ai

2.3Working Coordinate System

The working coordinate system is used to specify a tool motion for each workpiece.

A coordinate system previously set in the "Data Bank" is once selected, programming afterward can be easily done by specifying that coordinate system.

Each coordinate system is set by using an offset amount from the machine zero point to the working zero position.

(Note) Data Bank : Refer to Instruction manual.

2004/01/22

2 - 3

eTCOMNCPR2-1.doc

Chapter2 Coordinate Command	TC-32B

2

( This page is a blank.)

2004/01/22

2 - 4

eTCOMNCPR2-1.doc

TC-32B	Chapter 3 Preparation Function

CHAPTER 3

3

PREPARATION FUNCTION

3.1Outline of G code

3.2Positioning (G00)

3.3Linear interpolation (G01)

3.4Circular/helical interpolation (G02, G03)

3.5Circle cutting (G12, G13)

3.6Plane selection (G17, G18, G19)

3.7Dwell (G04)

3.8Exact stop check (G09, G61, G64)

3.9Programmable data input (G10)

3.10Soft limit

3.11Return to the reference point (G28)

3.12Return from the reference point (G29)

3.13Return to the 2nd/3rd/4th reference point (G30)

3.14Selection of machine coordinate system (G53)

3.15Selection of working coordinate system (G54~G59)

3.16Additional working coordinate system selection (G54.1)

3.17Scaling (G50, G51)

3.18Programmable mirror image (G50.1, G51.1)

3.19Coordinate rotation function (G68, G69)

3.20Coordinate rotation using measured results (G168)

3.21Absolute command and incremental command (G90, G91)

3.22Change of working coordinate system (G92)

3.23Skip function (G31, G131, G132)

3.24Continuous skip function (G31)

3.25Change of tap twisting direction (G133, G134)

3.26High speed peck drilling cycle (G173)

2004/01/22

3 - 1

eTCOMNCPR3.doc

Chapter 3 Preparation Function	TC-32B

3.27Peck drilling cycle (G183)

3.28Local coordinate system function (G52)

3.29Single direction positioning function (G60)

3.30G code priority

3

2004/01/22

3 - 2

eTCOMNCPR3.doc

TC-32B	Chapter 3 Preparation Function

3.1Outline of G code

Within 3-digit number following the address G determines the meaning of the command of the block concerned.

The G codes are divided into the following two types.

	Type	Meaning
	Modal	The G code is effective until another G code in the
		same group is commanded.
	One-shot	The G code is effective only at the block in which it is
		specified.

3

2004/01/22

3 - 3

eTCOMNCPR3.doc

	Chapter 3 Preparation Function				TC-32B
		Group	G cord	Contents	Modal
			G00*	Positioning
			G01	Linear interpolation
			G02	Circular/ helical interpolation (CW)
			G03	Circular / helical interpolation (CCW)	Modal
			G102	XZ Circular interpolation (CW)
			G103	XZ Circular interpolation (CCW)
3
			G202	YZ Circular interpolation (CW)
			G203	YZ Circular interpolation (CCW)
			G04	Dwell	One-shot
			G09	Exact stop check	One-shot
			G10	Programmable data input	One-shot
			G13	Circular cutting CCW	One-shot
			G17*	XY plane selection
			G18	YZ plane selection	Modal
			G19	ZX plane selection
			G22*	Programmable stroke limit on	Modal
			G23	Programmable stroke limit cancel
			G28	Return to the reference point
			G29	Return from the reference point	One-shot
			G30	Return to the 2nd /3rd/4th reference point
			G31	Skip function	One-shot
			G36	Coordinate calculation function (Bolt hole circle)
			G37	Coordinate calculation function (Line-angle)	One-shot
			G38	Coordinate calculation function (Line-angle)
			G39	Coordinate calculation function (Grid)
			G40*	Tool dia offset cancel
			G41	Tool dia offset left	Modal
			G42	Tool dia offset right

The G codes with * mark indicates the modal status when the power is turned ON.

(Note1)	Details of coordinate calculation functions are described in " Chapter 6 ".
(Note2)	Details of tool dia offset are described in " Chapter 4 ".

2004/01/22

3 - 4

eTCOMNCPR3.doc

TC-32B			Chapter 3 Preparation Function
	Group	G cord	Contents	Modal
		G43	Tool length offset +
		G44	Tool length offset -	Modal
		G49*	Tool length offset cancel
		G50*	Scaling cancel	Modal
		G51	Scaling
		G50.1	Mirror image cancel	Modal
						3
		G51.1	Mirror image
		G52	Local coordinate system	One-shot
		G53	Machine coordinate system selection
		G54*	Working coordinate system selection 1
		G55	Working coordinate system selection 2
		G56	Working coordinate system selection 3
		G57	Working coordinate system selection 4	Modal
		G58	Working coordinate system selection 5
		G59	Working coordinate system selection 6
		G54.1	Extended working coordinate system selection
		G60	Single direction positioning	One-shot
		G61	Exact stop mode	Modal
		G64*	Cutting mode
		G65	Macro call	One-shot
		G66	Macro modal call	Modal
		G67*	Cancel macro modal call
		G68	Coordinate rotation function
		G69*	Coordinate rotation function cancel	Modal
		G168	Coordinate rotation using measured results

2004/01/22

3 - 5

eTCOMNCPR3.doc

	Chapter 3 Preparation Function				TC-32B
		Group	G cord	Contents	Modal
			G90*	Absolute command	Modal
			G91	Incremental command
			G92	Working coordinate system setting	One-shot
			G94	Feed rate per minute
			G98*	Return to the initial point level	Modal
3			G99	Return to the R point level
			G73	Canned cycle (High-speed peck drilling cycle)
			G74	Canned cycle (Reverse tapping cycle)
			G76	Canned cycle (Fine boring cycle)
			G77	Canned cycle (Tapping cycle, synchro mode)
			G78	Canned cycle (Reverse tapping cycle, synchro
				mode)
			G80*	Canned cycle cancel
			G81	Canned cycle (Drill, spot drilling cycle)	Modal
			G82	Canned cycle (Drill, spot drilling cycle)
			G83	Canned cycle (Peck drilling cycle)
			G84	Canned cycle (Tapping cycle)
			G85	Canned cycle (Boring cycle)
			G86	Canned cycle (Boring cycle)
			G87	Canned cycle (Back boring cycle)
			G89	Canned cycle (Boring cycle)

2004/01/22

3 - 6

eTCOMNCPR3.doc

TC-32B			Chapter 3 Preparation Function
	Group	G cord	Contents	Modal
		G173	Canned cycle (High-speed peck drilling cycle)	One-shot
		G177	Canned cycle (End mill tap cycle)	Modal
		G178	Canned cycle (End mill tap cycle)
		G181	Canned cycle (Double drilling cycle)	Modal
		G182	Canned cycle (Double drilling cycle)
		G183	Canned cycle cancel (Peck drilling cycle)	One-shot
		G185	Canned cycle (Double boring cycle)			3
		G186	Canned cycle (Double boring cycle)	Modal
		G189	Canned cycle (Double drilling cycle)
		G100	Non-stop automatic tool change	One-shot

2004/01/22

3 - 7

eTCOMNCPR3.doc

	Chapter 3 Preparation Function				TC-32B
		Group	G cord	Contents	Modal
			G120	Positioning to the measuring point	One-shot
			G121	Automatic measurement Corner (Boss)
			G122	Automatic measurement Parallel (Groove)
			G123	Automatic measurement Parallel (Boss)
			G124	Automatic measurement Circle center (Hole, 3 points)
			G125	Automatic measurement Circle center (Boss, 3 points)	One-shot
3
			G126	Automatic measurement Circle center (Hole, 4 points)
			G127	Automatic measurement Circle center (Boss, 4 points)
			G128	Automatic measurement Z-axis height
			G129	Automatic measurement Corner (Groove)
			G31	Measurement feed
			G131	Measurement feed	One-shot
			G132	Measurement feed
			G133	Changeover of tap twisting direction (CW)	One-shot
			G134	Changeover of tap twisting direction (CCW)

(Note)

Commands G120 to G129 are described in detail in " Option, Automatic Measurement " in the instruction manual.

2004/01/22

3 - 8

eTCOMNCPR3.doc

TC-32B	Chapter 3 Preparation Function

3.2Positioning (G00)

A tool moves from its current position to the end point at the rapid traverse rate in each axis direction independently. Therefore, a tool path is not always a linear line.

Command format	G00 X_Y_Z_A_B_C_ ;

When the additional axis is commanded and the optional additional axis is not installed, an alarm will occur.

In the positioning mode actuated by the G00 code, the execution proceeds to the next block after confirming the in-position check. (Note 1)

3

eNCPR3.01.ai

(Note 1)

In-position check is to confirm that the machine detecting position is within the specified range around the target (end) point.

(This range is set by the machine parameter for each axis.) (Note 2)

The rapid traverse rate is set by the machine parameter for each axis. Accordingly, rapid traverse rate cannot be specified by the F command.

2004/01/22

3 - 9

eTCOMNCPR3.doc

Chapter 3 Preparation Function	TC-32B

3.3Linear interpolation (G01)

Linear interpolation moves a tool linearly from the current position to the target position at the specified feedrate.

Command format	G01 X_Y_F_ ;

Up to X,Y,X and one additional axis can be controlled simultaneously.

When the additional axis is commanded and the optional additional axis is not installed, an alarm will occur.

3	The feedrate is commanded by the address F. Once the feedrate is commanded, it is effective until
	another value is specified.
	When the X, Y, and Z axes are commanded, the feedrate is determined by the value entered to mm
	/ min.

When the additional axis is commanded, the feedrate is determined by the value entered to /min.

End

point

Start

point

eNCPR3.2.ai

(Note 1) Feedrate along each axis is as follows:

When "G01 G91 Xα YβFf ;" is programmed:

	α
Feedrate along X axis:	Fx ─── •	f
	L
	β
Feedrate along Y axis:	Fy ─── •	f
	L
( L = α2 + β2	)

2004/01/22

3 - 10

eTCOMNCPR3.doc