hitachi seiki 10M, 16M, 18M Programming Manual

SEIKI - SEICOS å10M/16M/18M

INSTRUCTION MANUAL

6 PROGRAMMING

Edition 1.01 NP-0000-1-0221-E-1-01

Hitachi Seiki Deutschland

Werkzeugmaschinen GmbH

2

CONTENTS

1.	G CODE .............................................................................................			1-1
	1-1	List of G Code Group(SEICOSΣ 10M/16M/18M) ..........................................................		1-1
	1-2	List of G Codes (SEICOS Σ 10M/16M/18M) .................................................................		1-2
2.	INTERPOLATION FUNCTION ........................................................			2 - 1
	2-1	Positioning (G00) .......................................................................................................		2 - 1
	2-2	Linear Interpolation (G01) ..........................................................................................		2 - 2
	2-3 Circular Interpolation (G02, G03) ...............................................................................			2 - 3
	2-3-1		Radius Designation on Arc ..................................................................................	2 - 5
	2-4 Helical Interpolation (G02, G03) .................................................................................			2 - 7
	2-5	Virtual Axis lnterpolation (G07) .................................................................................		2 - 10
	2-5-1 SIN Interpolation (G02, G03, G07) .....................................................................			2 - 12
	2-6 Single Direction positioning (G60) ...........................................................................			2 - 12
	2-7 Involute Interpolation (G222, G223) ..........................................................................			2 - 15
	2-8	Cylindrical Interpolation (G271) ................................................................................		2 - 19
	2-8-1		Command Format .............................................................................................	2 - 19
	2-8-2		Feed Rate .........................................................................................................	2 - 19
	2-8-3		Cylindrical Interpolation Applied Axes.................................................................	2 - 20
	2-8-4		Cylindrical Interpolation Applied Plane ...............................................................	2 - 20
	2-8-5		Sample Program ..............................................................................................	2 - 20
	2-8-6		Cautions ............................................................................................................	2 - 21
	2-8-7		Associated Parameters ....................................................................................	2 - 22
	2-8-8		Associated Alarms ............................................................................................	2 - 22
	2-9 Polar Coordinate Interpolation (G120, G121) ...........................................................			2 - 23
	2-9-1		G Codes ............................................................................................................	2 - 23
	2-9-2		Command Format .............................................................................................	2 - 23
	2-9-3		Polar Coordinate Interpolation Axes ..................................................................	2 - 23
	2-9-4 Polar Coordinate Interpolation plane ..................................................................			2 - 24
	2-9-5		Program Command ..........................................................................................	2 - 24
	2-9-6 sample Program (X-axis: Linear Axis, C-axis: Rotary Axis) ...............................			2 - 25
	2-9-7		Feed Rate Clamp ..............................................................................................	2 - 26
	2-9-8		Rapid Traverse(G00) Operation ........................................................................	2 - 26
	2-9-9		Precautions .......................................................................................................	2 - 26
	2-9-10		Associated parameters .....................................................................................	2 - 27
	2-9-11		Associated Alarms ............................................................................................	2 - 28
3.	FEED FUNCTION ..............................................................................			3-1
	3-1 Feed per Minute (G94) .................................................................................................			3-1
	3-2 Feed per Rotary (G95) .................................................................................................			3-2
	3-3	Inverse Time (G93) ......................................................................................................		3-3
	3-4	Exact Stop (G09) .........................................................................................................		3-4

i

	3-5	Exact Stop Mode (G61) ................................................................................................	3-4
	3-6	Automatic Corner Override (G62) ................................................................................	3-5
	3-6-1 Automatic Override in Inner Corner Area ...............................................................		3-6
	3-6-2 Inner Arc Cutting Speed Change ...........................................................................		3-7
	3-7 Tapping Mode (G63) .....................................................................................................		3-9
	3-8	Cutting Mode (G64) ....................................................................................................	3-10
	3-9	Automatic Acceleration/Deceleration .........................................................................	3-11
	3-10	Dwell (G04) ................................................................................................................	3-11
4.	REFERENCE POINT ........................................................................		4-1
	4-1	Automatic Reference Point Return (G28) ....................................................................	4-1
	4-2	Reference Point Return Check (G27) ..........................................................................	4-2
	4-3	Return from Reference Point (G29).............................................................................	4-4
	4-4	2nd-4th Reference Point Return (G30) ........................................................................	4-5
	4-5	Reset of Floating Reference point (G301) ...................................................................	4-7
5.	COORDINATE SYSTEM ...................................................................		5-1
	5-1	Machine Coordinate System Selection (G53) ..............................................................	5-1
	5-2	Work Coordinate system selection (G54 - G59) ..........................................................	5-2
	5-3	Addition of Work Coordinate system Pairs (G540 - G599) ..........................................	5-3
	5-4	Local Coordinate System Setting (G52) ......................................................................	5-5
	5-5	Work Coordinate System Change (G92) .....................................................................	5-7
	5-6	Work Coordinate System Preset (G921) .....................................................................	5-9
	5-7	Work Coordinate System Shift (External Work Zero Point Offset Amount) ...............	5-11
	5-8 Plane Selection (G17, G18, G19) ..............................................................................		5-12
	5-9	Rotary Table Dynamic Fixture Offset .........................................................................	5-14
6.	COORDINATE ...................................................................................		6-1
	6-1	Absolute/Incremental Programming (G90,G91) ...........................................................	6-1
	6-2 Polar Coordinate Input (G15,G16) ...............................................................................		6-2
	6-3 Inch/Metric Input (G20, G21) ........................................................................................		6-5
7. SPINDLE FUNCTION (S FUNCTION) ..............................................			7-1
8. TOOL FUNCTION (T FUNCTION) ....................................................			8-1
9. Miscellaneous Function (M FUNCTION) ............................................			9-1
	9-1 Miscellaneous Function (M Function) ..........................................................................		9-1
	9-2	2nd Miscellaneous Function (B Function) ....................................................................	9-2
10. Canned Cycle ...................................................................................			10-1
	10-1	Canned Cycle (G73, G74, G76, G80 - G89) ..............................................................	10-1
	10-2 Direct Tap (G741, G841) ..........................................................................................		10-16
	10-3	Drilling Pattern Cycle (G70, G71, G72, G77) ...........................................................	10-22
	10-4 True Circular Cutting (G302 ~ G305) .......................................................................		10-25
	10-5 Square Outside Cutting (G322,323) ........................................................................		10-34
	10-6	Plane Cutting Cycle (G324, G325, G326) ................................................................	10-38
	10-7 Poketing (G327 ~ G333) ..........................................................................................		10-50
	10-7-1 Circular Poketing (G327) ...................................................................................		10-55
		ii

	10-7-2		Square Poketing (G328) ....................................................................................	10-59
	10-7-3		Track Inside (G329) ...........................................................................................	10-64
	10-7-4		Circle outside Pocketing (G330) .......................................................................	10-67
	10-7-5		Square Outside Cutting (G331) .........................................................................	10-70
	10-7-6		Track Outside (G332) ........................................................................................	10-73
	10-7-7		Circle (G333) .....................................................................................................	10-76
	10-7-8		Special Fixed Cycles (G322 ~ G333) Type 2 ....................................................	10-78
	10-8 ATC Canned Cycle (MO6) .......................................................................................			10-79
	10-8-1 ATC Canned Cycle, Type A (VK, VKC, VG, VkII) ................................................			10-82
	10-8-2 ATC CANNED CYCLE TYPE E (VM40III) ..........................................................			10-84
	10-8-3		ATC CANNED CYCLE TYPE F (HG) ................................................................	10-86
	10-8-4		ATC Canned Cycle, Type G (HK) ......................................................................	10-87
	10-8-5 ATC Canned Cycle, Type I (Initial HS500) .........................................................			10-89
	10-8-6		ATC Canned Cycle, Type J (VS) .......................................................................	10-91
	10-8-7		ATC Canned Cycle, Type K(HS630) .................................................................	10-93
	10-8-8		ATC Canned Cycle, Type L (New HS500) .........................................................	10-95
	10-8-9 ATC Canned Cycle, Type M (VS 16-tool) ..........................................................			10-96
	10-8-10		ATC Canned Cycle, Type N (MS400H) ..............................................................	10-98
	10-9	High-Speed Machining Cycle ...................................................................................		10-99
	10-9-1		Trochoid Cycle (G334) ......................................................................................	10-99
	10-9-2 Helical Drilling Cycle (G812, G813) .................................................................			10-103
	10-9-3 High Speed Side Face Cutting Cycle (G335) ..................................................			10-107
	10-9-4		Z Feed Fluting Cycle (G336) ............................................................................	10-111
	10-9-5		Corner Pocket Cycle (G337) ...........................................................................	10-113
	10-9-6		Square Pocket Cycle (G338) ..........................................................................	10-116
11.	COMPENSATION FUNCTION ........................................................			11-1
	11-1 Tool Length Compensation (G43, G44, G49) .............................................................			11-1
	11-2	Tool Offset (G45 - G48) .............................................................................................		11-6
	11-3 Tool Diameter Compensation (G38 - G42) ................................................................			11-9
	11-3-1 Detailed Description of Tool Diameter Compensation ......................................			11-15
	11-4 3-D Tool Offset (G40 - G41) .....................................................................................			11-27
	11-5 H and D Functions ...................................................................................................			11-31
	11-6 Tool Offset by Tool Number......................................................................................			11-33
12.	CONVERTING FUNCTION .............................................................			12-1
	12-1 Programmable Mirror Image (G501, G511) ...............................................................			12-1
	12-2	Setting Mirror Image ...................................................................................................		12-4
	12-3	Scaling (G50, G51) ....................................................................................................		12-7
	12-4 Coordinate Ratation (G68, G69) ..............................................................................			12-10
	12-5 Optional Angle Chamfering/Corner R (, C, R)..........................................................			12-15
13.	MEASURMENT ................................................................................			13-1
	13-1	Skip Function (G31) ...................................................................................................		13-1

iii

13-2 Automatic Measurement of Tool Length (G37)...........................................................			13-3
13-3 Safety Guard (Tool Length) ........................................................................................			13-5
13-4	Safety Guard (Comparison) .......................................................................................		13-9
14. DATA SETTING ...............................................................................			14-1
14-1	Data Setting (G10) .....................................................................................................		14-1
14-1-1 Tool offset amount setting ...................................................................................			14-1
14-1-2 Work coordinate system offset amount setting...................................................			14-1
14-2	Programmable Parameter Input (G10) ......................................................................		14-3
14-3	Plotting Parameter Setting .........................................................................................		14-5
15. SOFT OT .........................................................................................			15-1
15-1 Soft OT (Stored Stroke Limit 1) ..................................................................................			15-1
15-2 Stored Stroke Limits 2 and 3 (G22 and G23) .............................................................			15-3
15-3	Soft-OT before Move .................................................................................................		15-6
16. AXIS CONTROL ..............................................................................			16-1
16-1	Rotary Axis Controlling Function ................................................................................		16-1
16-2 Oscillation Function (G113, G114) .............................................................................			16-4
16-3 Normal Direction Control (G411, G421, G401) ..........................................................			16-8
17. HIGH-SPEED MACHINING .............................................................			17-1
17-1	Multibuffer (G251) ......................................................................................................		17-1
17-2 Feed Rate Clamp by Circular Arc Radius ..................................................................			17-3
17-3 PRECONTROLLING .................................................................................................			17-4
17-3-1		PRE-INTERPOLATION LINEAR ACCELERATION/DECELERATION ................	17-5
17-3-2		AUTO CORNER DECELERATION ....................................................................	17-6
17-4 HIGH PRECISION PROFILE CONTROL ..................................................................			17-8
17-5	Smooth Interpolation ................................................................................................		17-10
17-6	NURBS Interpolation ................................................................................................		17-12
17-7	SHG Machining ........................................................................................................		17-14
18. FIVE-FACE MACHINING ................................................................			18-1
18-1 Selecting the Machining Plane (G240-G245) .............................................................			18-1
18-2	Common Work Origin Offset .....................................................................................		18-2
18-3	Axis Changeover ........................................................................................................		18-5
18-3-1		Axis Changeover (Type A) ...................................................................................	18-5
18-3-2 Axis Changeover (Type B)...................................................................................			18-6
19. AUTOMATIC OPERATION .............................................................			19-1
19-1	Program Restart ........................................................................................................		19-1
19-2	Block Restart .............................................................................................................		19-6
19-3 Machining Break Point Return (G206) .....................................................................			19-11
19-4 Reverse Movement ..................................................................................................			19-14
19-5 Sequence Number Comparison and Stop ...............................................................			19-16
19-6 Reset (Reset Associated with Automatic Operation) ...............................................			19-18
19-6-1 Details of Reset (Reset Associated with Automatic Operation) ........................			19-18

iv

20. MANUAL OPERATION ....................................................................			21-1
20-1	Manual Absolute ON/OFF ..........................................................................................		21-1
21. TEST RUN .......................................................................................			21-1
21-1	Miscellaneous Function Lock .....................................................................................		21-1
21-2	Miscellaneous Function Finish ...................................................................................		21-1
22. CUSTOM MACROS.........................................................................			22-1
22-1	Outline .......................................................................................................................		22-1
22-2 Call Commands and Return Command ....................................................................			22-2
22-2-1		Types of Command .............................................................................................	22-2
22-2-2 Multi-call ..............................................................................................................			22-8
22-2-3		Argument Designation .......................................................................................	22-13
22-3	Variables ..................................................................................................................		22-18
22-4	Representation of Variables .....................................................................................		22-31
22-5	Citation of Variables .................................................................................................		22-31
22-6	Undefined Variables .................................................................................................		22-32
22-7	Expression and Computation ..................................................................................		22-33
22-8	Substitution Command ............................................................................................		22-36
22-9 Branch Command ...................................................................................................			22-37
22-10Repeat Command ...................................................................................................			22-38
22-11 Naming Command ..................................................................................................			22-39
22-12IF Command ............................................................................................................			22-40
22-13External Output Commands ....................................................................................			22-42
23. Interrupt Type Custom Macro ..........................................................			23-1
23-1 Custom Macro Interrupt Operation ............................................................................			23-1
23-2	How to Specify ...........................................................................................................		23-2
23-3 Interrupt Type Custom Macro Proper .........................................................................			23-2
23-4 Status Trigger Method and Edge Trigger Method (Parameters) .................................			23-2
23-5 Reversion and Modal Information ..............................................................................			23-3
23-6 System Variable in Interrupt Program ........................................................................			23-3
23-7	Custom Macro Interrupt and Custom Macro Modal Call ............................................		23-4
23-8 Interrupt Timing and Return Position in Each Mode ...................................................			23-4
23-9	Associated Parameters .............................................................................................		23-7
24. MEMORY OPERATION IN OTHER COMPANIES’ FORMATS ......			24-1
24-1	Memory Operation in FS15 Format ...........................................................................		24-1
24-2	Memory Operation in i80M Format ............................................................................		24-2

v

vi

1.G CODE

1-1 List of G Code Group(SEICOSΣ 10M/16M/18M)

Group	Function	Remarks
00	Non-modal
01	Positioning/liner interpolation/circular interpolation
02	Plane designation
03	Absolute programming/incremental programming
04	Stored stroke check
05	Inverse time/feed per minute/feed per revolution
06	Inch/metric conversion
07	Tool diameter compensation
08	Tool length compensation
09	Canned cycle
10	Initial point return/R point return
11	Scaling
12	Work coordinate system Selection
13	Cutting mode/exact stop mode/automatic corner override mode
14	Macro modal call
15	Programming mirror image
16	Coordinator rotation
17	Constant surface speed control	*1
18	Tool life management
19	Normal direction control	*1
20	Polar coordinate command
21	Oscillation function
22	Polar coordinate interpolation	*1
23	Spindle speed fluctuation detection	*1
24	Machining plane selection	*1
25	Tool nose interference check	*1
26	Axis switching/3-D coordinate conversion	*1
27		*2
28		*2
29		*2
30		*2
31		*2

(Note) *1 Reserved G code and not available for the moment *2 Spare G code group for function improvement.

1 - 1

1-2 List of G Codes (SEICOS Σ 10M/16M/18M)

	Code	Group	Function			Remarks
	G00		Positioning
	G01	01	Linear interpolation
	G02		Circular interpolation/helical interpolation CW
	G03		Circular interpolation/helical interpolation CCW
	G04		Dwell
	G05	00	High-precision profile control
	G07		Virtual axis interpolation
	G08		Antecedent control
	G09		Exact stop
	G10		Data setting
	G11		Data setting node cancel
	G15	20	Polar coordinate command cancel
	G16		Polar coordinate command
	G17		XP YP	plane	where: XP : x axis or its parallel axis
	G18	02	ZP XP	plane		YP : Y axis or its parallel axis
	G19		YP ZP	plane		ZP : Z axis or its parallel axis
	G20	06	Inch input
	G21		Metric input
	G22	04	Store stroke check ON
	G23		Stored stroke check OFF
	G25	23	Spindle speed fluctuation detection OFF				*1
	G26		Spindle speed fluctuation detection ON				*1
	G27		Reference point return check
	G28		Reference point return
	G29	00	Return from reference point
	G30		2nd, 3rd, 4th reference point return
	G31		Skip function
	G33	01	Thread cutting				*1
	G34		Variable lead thread cutting				*1
	G37		Tool length automatic measurement
	G38	00	Tool diameter compensation vector hold
	G39		Tool diameter compensation corner arc
	G40		Tool diameter compensation left/3-D tool offset cancel
	G41	07	Tool diameter left/3-D tool offset
	G42		Tool diameter compensation right

1 - 2

Code	Group	Function	Remarks
G43	08	Tool length compensation +
G44		Tool length compensation -
G45		Tool offset extension
G46	00	Tool offset contraction
G47		Tool offset double extension
G48		Tool offset double contraction
G49	08	Tool length compensation cancel
G50	11	Scaling cancel
G51		Scaling
G52	00	Local coordinate system Setting
G53		Machine coordinate system selection
C54		Work coordinate system 1 selection
G55		Work coordinate system 2 selection
G56	12	Work coordinate system 3 selection
G57		Work coordinate system 4 selection
G58		Work coordinate system 5 selection
G59		Work coordinate system 6 selection
G60	00	Single direction positioning	Group 01 by
			parameter change
G61		Exact stop mode
G62	13	Automatic corner override mode
G63		Tapping mode
G64		Cutting mode
G65	00	Macro call
G66	14	Macro modal call
G67		Macro modal call cancel
G68	16	Coordinate rotation
G69		Coordinate rotation cancel
G70		Bolt hole cycle
G71	00	Arc
G72		Arc
G73		Peck drilling cycle
G74	09	Counter tapping cycle
G76		Fine boring cycle
G77	00	Grid cycle

1 - 3

	Code	Group	Function	Remarks
	G80		Canned cycle cancel
	G81		Drilling cycle, spot boring
	G82		Drilling cycle, counter boring
	G83		Peck drilling cycle
	G84	09	Tapping cycle
	C85		Boring cycle
	G86		Boring cycle
	G87		Back boring cycle
	G88		Boring cycle
	G89		Boring cycle
	G90	03	Absolute programming
	G91		Incremental programming
	G92	00	Work coordinate system change/maximun spindle speed setting
	G93		Inverse tine feed
	G94	05	Feed per minute
	G95		Feed per revolution
	G96	17	Constant surface speed control	*1
	G97		Constant surface speed control	*1
	G98	10	Canned cycle initial level point return
	G99		Canned cycle R point level return
	G113	21	Oscillation node ON
	G114		Oscillation node OFF
	G120	22	polar coordinate interpolation mode cancel
	G121		Polar coordinate interpolation mode
	G130	18	Tool life management OFF
	G131		Tool life management ON
	G201		PMC data setting	*1
	G203	00	High-speed machining program registration start	*1
	G204		High-speed machining pro-gram registration end	*1
	G206		Tool retract amount setting
	G212		Circular thread cutting CW	*1
	G213	01	Circular thread cutting CCW	*1
	G216		Spline interpolation	*1

1 - 4

	Code	Group		Function		Remarks
	G222		Involute interpolation CW
	G223	01	Involute interpolation CCW
	G232		Exponential function interpolation CW			*1
	G233		Exponential function interpolation CCW			*1
	G240		Machining plane 0 selection		(Machining plane
					selection cancel)
	G241		Machining plane 1 selection
	G242	24	Machining plane 2 selection
	G243		Machining plane 3 selection
	G244		Machining plane 4 selection
	G245		Machining plane 5 selection		(Available for an optional
					horizontal/vertical angle)
	G248	26	Axis switching/3-D coordinate conversion ON
	G249		Axis switching/3-D coordinate conversion canel
	G251	00	Multi-buffer
	G264	25	Tool nose interference check ON			*1
	G265		Tool nose interference check OFF			*1
	G271		Cylindrical interpolation
	G301		Floating reference point return
	G302		Circular cutting inner diameter CW
	G303		Circular cutting inner diameter CCW
	G304		Circular cutting outer diameter CW
	G305		Circular cutting outer diameter CCW
	G311		Multi-step skip function 1			*1
	G312		Multi-step skip function 2			*1
	G313		Multi-step skip function 3			*1
	G314	00	Multi-step skip function 4			*1
	G322		Square outside cutting CW
	G323		Square outside cutting CCW
	G324		Square plane
	G325		Square plane 1-directional
	G326		Square plane 2-directional
	G327		Circle inside	(pocketing)
	G328		Square inside (pocketing)
	G329		Track inside	(pocketing)
	G330		circle outside	(pocketing)

1 - 5

Code		Group		Function	Remarks
G331			Square outside	(pocketing)
G332			Track outside	(pocketing)
G333			Circle	(pocketing)
G334		00	Trochoid cycle
G335			High-speed side cutting cycle
G336			Z feed fluting cycle
G337			Corner pocket cycle
G338			Square pocket cycle
G401			Normal direction control cancel node
G411		19	Normal direction control left side ON
G421			Normal direction control right side ON
C431		08	Tool axis direction tool length compensation		*1
G501		15	Programmable mirror image Cancel
G511			Programmable mirror image
G540~		12	Additional work coordinate system selection
G599			(60 pairs)
G611		00	Pre-interpolation acceleration/deceleration		*1
C653		00	Position check (Note) for Maintenance		*1
G661		14	Macro modal call B		*1
G721		00	Rotary copy		*1
G722			Parallel copy		*1
G741		09	Counter direct tap cycle
G841			Direct tap cycle
G812			Helical drilling cycle CW
G813			Helical drilling cycle CCW
G921		00	Work coordinate system preset
(Note 1)		*1 Reserved G code and not available for the noment
(Note 2)		The G code marked		in each group is selected in the reset state.

1 - 6

2.INTERPOLATION FUNCTION

2-1 Positioning (G00)

Each axis moves to a Program-specified position at an independent rapid traverse rate to perform positioning.

(1)	command format
	G90
	G91 G00 X_ Y_ Z_ ;
(2)	Sample program
	(a) Absolute programming		(b) Incremental programming
	G90 G00 X100. Y50.	:	G91 G00 X100. Y50.

Y

50.

100.

(3)Cautions

(a)The rapid traverse rate has been set independently for each axis.

(b)The tool path is non-linear. See to it that the tool does not interfere with the workpiece.

(c)Linear acceleration/deceleration is applied. Confirm imposition (an accumulated amount due to servo delay is within tolerance) at the end of the block, and then, proceed to the next block.

(d)G00, G90 are G91 ale modal G codes. Once they are specified, they remain effective until the next associated G code is specified.

(e)The tool path can be made linear by altering the parameter.

Y

50.

X

100.

(f)You can set with the parameter whether the reset state is to be the G00 or G01 mode.

2 - 1

(4)Associated parameters

No.1401, # 6 = 0 Dry run made invalid for rapid traverse command. 1 Dry run made valid for rapid traverse command.

No.1401, # 1= 0 Non-linear interpolation as positioning interpolation system 1 Linear interpolation as positioning interpolation system

No.3402, # 0= 0 G00 mode in reset state 1 G01 mode in reset state

2-2 Linear Interpolation (G01)

The tool moves linearly to a program-specified position at the cutting feed rate specified with an F code.

(1)	Command format
	{ G91G90 } G01 X_ Y_ Z_...F_ ;
(2)	Sample program
	(a) Absolute programming.	(b) Incremental programming
	G90 G01 X100. Y50. F200;	G90 G01 X100. Y50. F200;

Y

50.

100.

(3)Cutting feed rate

The cutting feed rate specified with an F code is the speed at which the tool moves linearly. In this case, the cutting feed rate is a composite speed of all the specified axes; the cutting feed rate of each axis is as follows.

G01 G91 Xa Yb Zc Ff:

X-axis cutting feed rate: Fx = afL , where; L= a2 + b2 + c2

bf

Y-axis cutting feed rate: Fy = L

cf z-axis cutting feed rate, Fz = L

When the rotary axis is specified in the identical block, linear interpolation is performed taking it as a linear axis in the units of degree.

2 - 2

End Point

G01 G91 X100. C90. F200 :

Cutting feed rate in the rotary axis (C axis) direction:

	Start	Fc =	90. x 200	(deg/min)
	Point
			L

where; L = 100.2 + 902 (mm)

(4)Cautions

(a)An alarm results when no F code has been specified in the G01 block or before.

(b)Exponential type acceleration/deceleration is applied.

(c)Set with the parameter whether the reset state is to be the G00 or G01 mode.

(5)Associated parameters

No.3402, #0 = 0 G00 mode in reset state

1G01 mode in reset state

(6)Associated alarm

No. 102

F0 was specified in the G01/G02/G03 mode.

2-3 Circular Interpolation (G02, G03)

The tool moves to a program-specified position along an arc within the plane selected with a plane selection G code (G17, G18, G19) at the cutting feed rate specified with an F code.

(1)Command format

(a)XP YP plane

G17 G02	X - Y -	R_		F_ ;
G03	P P	I_
			J_

(b) ZP -XP plane

G02		R_
G18 G03	ZP- YP-	K_		F_ ;
			I_

(c) XP -ZP plane

	G02		R_			F_ ;
G19			YP-ZP-	J_
	G03				K_
Where;			XP : X axis or its parallel axis
			YP : Y axis or its parallel axis
			ZP : Z axis or its parallel axis
(Note)		To specify with R instead of I, J or K is called radius designation on arc.

2 - 3

(2) Sample program
(a) Absolute programming	(b) Incremental programming
G17 G90 G00 X13.397 Y70. F200:	G17 C91 G02 X86.603 Y50
G02 X100. Y120. I86.603 J-50.:	I86.603 J-50. F200:

Y

120.

	100.	X	X
			100.

(3)Arc rotating direction G02 : Clockwise (CW)

G03 : Counterclockwise direction (CCW)

ZP

XP YP

(4)Arc plane

The arc plane is specified with C17, G18 or G19.

G17 : XP -YP plane

G18 : ZP -XP plane

G19 : YP -ZP plane

(5)Arc center

The arc center is specified with I, J or K corresponding to XP ,YP and ZP respectively. In this case, I, J and K are the vector components when viewing the arc center from its start point.

YP X

Point

ZP

2 - 4

(6)Cutting feed rate

The cutting feed rate specified with an F code is the speed at which the tool moves on the arc.

(7)Cautions

(a)An alarm results when no F code has been specified in the G02/G03 block or before.

(b)An alarm results if an arc radius = 0 is specified.

(c)I0, J0 and K0 are omissible.

(d)When there is no end point on the arc, the tool moves linearly the rest after moving along an arc if the end point error of circular interpolation is within the parameter set value. Also, an alarm results if it is other than the parameter set value.

End Point

End

Point error

Moves linearly

Start Point

Center

(e)An alarm results if the axis not for the arc plane is specified.

(f)When R is specified in the same block as I, J and K, R is given priority.

(g)When the rotary axis is specified in the same block, circular interpolation is performed taking it as a linear axis in the units of degree.

(h)Exponential type acceleration/deceleration is applied.

(8) Associated parameters

No.3459 Arc end tolerance

(9) Associated alarm
No.102	F0 has been command with G01, G02 and G03.
No.132	Arc interpolation error
(#001)	Center command, although available, is 0 in value.
(#002)	Difference in radius value between of start and end
(#003)	pints has exceeded parameter set value.

2-3-1 Radius Designation on Arc

In case of circular interpolation, an arc radius can be directly specified with R instead of specifying the arc center with I, J or K.

2 - 5

(1)Command format.

(a)XP-YP plane

	G17	{	G03G02	}	XP _ YP _ R ± _ F_ :
(b)	ZP-XP plane
	G18	{	G03G02	}	ZP_ YP _ R ± _ F_ :
(c)	YP-ZP plane
	G19	{	G03G02	}	YP-ZP_ R ± _ F_ :
	where;		XP: X axis or its parallel axis
			YP : Y axis or its parallel axis

ZP : Z axis or its parallel axis

R+ : Arc of less than 180°

R- : Arc of over 180°

(2)Sample program

(a)For the arc of less than 180° G17 G91 G02 X100. Y100. R-100. F200:

(b)For the arc of over 180° G17 G91 G02 X100. Y-100. R-100. F200 :

than 180°

X

(3)Cautions

(a)When I, J, K and R are specified in the same blocks, R is given priority.

(b)When the arc center is not calculated, an alarm results.

(c) When G91		G02	R_ : is specified, it is taken as a block without axial move.
		G03

(4) Associated parameters

2 - 6

(5)Associated alarms

No. 131 An arc radius R with which arc center position cannot be calculated has been commanded.

2-4 Helical Interpolation (G02, G03)

If an arc command and any one axis for other than arc are specified, helical interpolation is enabled by control which performs linear interpolation synchronously with arc movement.

(1) Command format

G17		G02	XP		_ YP _		R _		α_	F_ ;
		G03					I _
								J _
G18		G02	Z		_ Y _		R _		α_	F_ ;
				P
		G03			P		I _	J _
		G02					R _		α_
G19		G03	YP _ ZP _				I _			F_ ;
								J _
where;		XP : X axis or its parallel axis
		YP : Y axis or its parallel axis
		ZP : Z axis or its parallel axis
		α : Any optional linear axis for other than circulate interpolation (up to 2 axes)
		F : Arc speed
	Linear axis speed = F ×						Linear		arc length
								Arc length

2 - 7

(2)Sample program

G17 G91 G03 X-100. Y-100. R100. Z50. F200 :

Z

Point

Start

Tool Path

(3) The axes for	specified up to 2 axes in the same
block.
(Example) G17
I-
	V axis must be
	with the Y axis.

Y

X

(4)Cautions

(a)See to it that the linear axis speed does not exceed the maximum value.

(b)Tool diameter compensation is applied to circular interpolation.

(c)An alarm results if 3 or more linear axes are specified.

2 - 8

(5) Associated parameters

(6) Associated alarms

2 - 9

2-5 Virtual Axis lnterpolation (G07)

If the axis is specified as a virtual axis, it does not move.

Interpolation can be perfomed with this axis and other one.

(1)	Command format
	G07 α	0	;	Sets the α axis as the virtual axis.
	:			}	The α axis is the virtual axis
	:				in this section.
	G07 α	1	;	Cancels the a axis as the virtual axis.
	where ;		α	: Any one axis
(2)	Sample program
	G07	X0	;		Sets the X axis as the virtual axis.
	G17	G91 G02 X0 Y0 I50. Z-1. 0 F200 ; SIN interpolation
	G01	X5. F100;			Dwell state for the move time of the X axis
	G07	X1	;		Cancels the X axis as the virtual aixs.

(3)Cautions

(a)SIN interpolation results if one arc axis for helical interpolation is set as the virtual axis.

(b)The virtual axis is any one axis.

An alarm results if 2 or more axes are set as virtual axes.

(c)If a command is given as to only one axis specified as the virtual axis, the axis move time valve is placed in the dwell state.

(d)Program virtual axis interpolation in the incremental manner.

Since the virtual axis does not move at any time, it is necessary to be careful when programming in the absolute manner.

2 - 10

(4) Associated parameters

(5)Associated alarms

No.139 Two or more virtual axes have been specified.

2 - 11

2-5-1 SIN Interpolation (G02, G03, G07)

SIN interpolation can be performed by assuming one of axes for an arc command as a virtual axis in helical interpolation.

(1) Command format

G87 α

0

;

Sets the virtual axis.

specify helical interpolation.

G07 α

1

;

Cancels the virtual axis.

αis any one axis for the arc command.

(2)Sample program

G07 X0;

G17 G91 G03 X0 Y0 I-50. Z100. F200 ; G07 X1;

Y

Z

(3)Cautions

(a)Effective only for automatic operation of the virtual axis.

(b)Program the virtual axis in the incremental manner.

(c)An alarm results if 2 or more virtual axes are specified.

2-6 Single Direction positioning (G60)

Performs final positioning always from a specified single direction.

Using this function allows you to perform high-accuracy positioning.

(1)Command format

(a)For the one-shot G code

G60 X_Y_Z_... ; Effective only in the G60 specified block

2 - 12

(b)For the modal G code G60 X_ Y_ Z_... ; X_ Y_ Z_...;

:

:

G00 ;

(2) Sample program

(a)When moving in the

+direction

G60 G91 X100.;

Start Point

End

Point Approach

Amount

Single direction positioning

Cancels G60 if any G code in Group 01 other than G60 is given.

(b)When moving in the

-direction

G60 G91 X-100.;

End Point		Start Point

Approach

Amount

(3)Final positioning direction

Approach amount > 0 : The positioning direction is the + direction. Approach amount < 0 : The positioning direction is the - direction. Approach amount = 0 : Positioning is not performed in the - direction.

(4)Cautions

(a)Whether G610 is to be one-shot or modal is set with the parameter.

(b)In the canned cycle, hole positioning is performed with G60.

However, single positioning is disabled for the shift amount of G76 and G87.

(c)During the mirror image, it is disabled for the approach amount of single direction positioning.

(5)Associated parameters

2 - 13

(5) Associated parameters

No. 3458 Single positioning direction and approach amount of each axis No. 3400, #2 = 0 G60 is the G code of Group 00 (one-shot).

1 G60 is the G code of Group 01 (modal).

2 - 14

2-7 Involute Interpolation (G222, G223)

This function allows machining along an involute curve. It also provides cutter compensation.

(1)Involute curve

The involute curve in the X-Y plane is defined as following.

X(θ ) =R [cosθ + (θ - θ 0) sinθ ] +X0

Y(θ ) =R [sinθ + (θ - θ 0) cosθ ] +Y0

where;

X0, Y0:Central coordinate of the basic circle

R : Radius of the basic circle

θ0 : Angle of the point where the involute curve starts

θ: Angle of the contact of the tangent from the current position to the basic circle X(θ ), Y(θ ) :Current position of the X-and Y-axis

Y

Point

The involute curves in the Z-X and Y-Z planes are defined in the same manner as that in the X- Y plane.

2 - 15

(2)Command format

(a)XP -YP _ plane

	G17		G222	X _Y _ I_ J_ R_ F_ ;
			G223	P	P
(b)	ZP-XP Plane
	G18		G222	Z _ Y _ K_ J_ R_ F_;
			G223	P	P
(c)	YP-ZP plane
	G19		G222	Y _ Z J_ K_ R_ F_ ;
			G223	P	P
where;
	G222		: Clockwise involute interpolation
	G223		: Counterclockwise involute interpolation
	XP, YP, ZP : Coordinate value of the end point
	XP		: X-axis or its parallel axis
	YP		: Y-axis or its parallel axis
	ZP		: Z-axis or its parallel axis
	I, J, K		: Central position of the basic circle for the involute curve viewed from the
				start point
	R		: Radius of the basic circle

F: Cutting feed rate

(3)Start point and end point

The end point of the involute curve is specified with the address X, Y, or Z and expressed with an absolute or incremental value depending on G90 or G91. If the incremental value is used, specify the coordinate of the end point viewed from the start point of the involute curve.

When a start or end point command is within the basic circle, an alarm results. The same results when an offset vector is brought into the basic circle by cutter compensation. Care should be taken when an offset is applied, in particular, to the inside of the involute curve.

(4)Basic circle command

The center of the basic circle is specified with I, J, and K, corresponding to X, Y, and Z, respectively. However, the numerals following I, J, and K are vector components, when the center of the basic center is viewed from the start point of the involute curve.

They should be always programmed with incremental values, regardless of G90 or G91. Add a sign to I, J, and K as required.

2 - 16