How it Works
hitachi seiki
Loading...
10M
Operating Manual
230 pgs2.23 Mb4
Instruction Manual
386 pgs18.71 Mb2
Programming Manual
392 pgs2.02 Mb2

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(SEICOSΣ10M/16M/18M) ..........................................................1-1
1-2 List of G Codes (SEICOS Σ10M/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
2-9-1 1 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
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 T apping Mode (G63)..................................................................................................... 3-9
3-8 Cutting Mode (G64).................................................................................................... 3-10
3-9 Automatic Acceleration/Deceleration ......................................................................... 3-1 1
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 A TC Canned Cycle (MO6)....................................................................................... 10-79
10-8-1 A TC Canned Cycle, Type A (VK, VKC, VG, VkII) ................................................ 10-82
10-8-2 A TC CANNED CYCLE TYPE E (VM40III).......................................................... 10-84
10-8-3 A TC CANNED CYCLE TYPE F (HG)................................................................ 10-86
10-8-4 A TC Canned Cycle, Type G (HK)...................................................................... 10-87
10-8-5 A TC Canned Cycle, Type I (Initial HS500) ......................................................... 10-89
10-8-6 A TC Canned Cycle, Type J (VS) ....................................................................... 10-91
10-8-7 A TC Canned Cycle, Type K(HS630) ................................................................. 10-93
10-8-8 A TC Canned Cycle, Type L (New HS500)......................................................... 10-95
10-8-9 A TC Canned Cycle, Type M (VS 16-tool) .......................................................... 10-96
10-8-10 A TC 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, G51 1) ............................................................... 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 (G1 13, G114) ............................................................................. 16-4
16-3 Normal Direction Control (G41 1, 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-INTERPOLA TION LINEAR ACCELERA TION/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 (T ype A)................................................................................... 18-5
18-3-2 Axis Changeover (T ype 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 V ariables ................................................................................................. 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 T ype Custom Macro Proper......................................................................... 23-2
23-4 St atus Trigger Method and Edge T rigger 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(SEICOS
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
ΣΣ
Σ10M/16M/18M)
ΣΣ
(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
ΣΣ
Σ10M/16M/18M)
ΣΣ
Code G00 G01 G02 G03 G04 G05 G07 G08 G09 G10 G1 1 G15 G16 G17 G18 G19 G20 G21 G22 G23 G25 G26 G27 G28 G29 G30 G31 G33 G34 G37 G38 G39 G40 G41 G42
Group
01
00
20
02
06
04
23
00
01
00
07
Function Remarks Positioning Linear interpolation Circular interpolation/helical interpolation CW Circular interpolation/helical interpolation CCW Dwell High-precision profile control Virtual axis interpolation Antecedent control Exact stop Data setting Data setting node cancel Polar coordinate command cancel Polar coordinate command XP YP plane where:XP : x axis or its parallel axis ZP XP plane YP : Y axis or its p arallel axis YP ZP plane ZP : Z axis or its parallel axis Inch input Metric input Store stroke check ON Stored stroke check OFF Spindle speed fluctuation detection OFF *1 Spindle speed fluctuation detection ON *1 Reference point return check Reference point return Return from reference point 2nd, 3rd, 4th reference point return Skip function Thread cutting *1 Variable lead thread cutting *1 Tool length automatic measurement Tool diameter compensation vector hold Tool diameter compensation corner arc Tool diameter compensation left/3-D tool offset cancel Tool diameter left/3-D tool offset Tool diameter compensation right
1 - 2
Code
G43 G44 G45 G46 G47 G48 G49 G50 G51 G52 G53 C54 G55 G56 G57 G58 G59 G60 G61 G62 G63 G64 G65 G66 G67 G68 G69 G70 G71 G72 G73 G74 G76 G77
Group
08
00
08 11
00
12
00
13
00 14
16
00
09
00
Function Remarks Tool length compensation + Tool length compensation ­Tool offset extension Tool offset contraction Tool offset double extension Tool offset double contraction Tool length compensation cancel Scaling cancel Scaling Local coordinate system Setting Machine coordinate system selection Work coordinate system 1 selection Work coordinate system 2 selection Work coordinate system 3 selection Work coordinate system 4 selection Work coordinate system 5 selection Work coordinate system 6 selection Single direction positioning Exact stop mode Automatic corner override mode Tapping mode Cutting mode Macro call Macro modal call Macro modal call cancel Coordinate rotation Coordinate rotation cancel Bolt hole cycle Arc Arc Peck drilling cycle Counter tapping cycle Fine boring cycle Grid cycle
Group 01 by parameter change
1 - 3
Code
G80 G81 G82 G83 G84 C85 G86 G87 G88 G89 G90 G91 G92 G93 G94 G95 G96 G97 G98
G99 G113 G114 G120 G121 G130 G131 G201 G203 G204 G206 G212 G213 G216
Group
09
03 00
05
17
10
21
22
18
00
01
Function Remarks Canned cycle cancel Drilling cycle, spot boring Drilling cycle, counter boring Peck drilling cycle Tapping cycle Boring cycle Boring cycle Back boring cycle Boring cycle Boring cycle Absolute programming Incremental programming
Work coordinate system change/maximun spindle speed setting
Inverse tine feed Feed per minute Feed per revolution Constant surface speed control *1 Constant surface speed control *1 Canned cycle initial level point return Canned cycle R point level return Oscillation node ON Oscillation node OFF polar coordinate interpolation mode cancel Polar coordinate interpolation mode Tool life management OFF Tool life management ON PMC data setting *1 High-speed machining program registration start *1 High-speed machining pro-gram registration end *1 Tool retract amount setting Circular thread cutting CW *1 Circular thread cutting CCW *1 Spline interpolation *1
1 - 4
Code G222 G223 G232 G233 G240 G241 G242 G243 G244 G245 G248 G249 G251 G264 G265 G271 G301 G302 G303 G304 G305 G311 G312 G313 G314 G322 G323 G324 G325 G326 G327 G328 G329 G330
Group
01
24
26 00 25
00
Function Remarks Involute interpolation CW Involute interpolation CCW Exponential function interpolation CW *1 Exponential function interpolation CCW *1 Machining plane 0 selection
(Machining plane selection cancel)
Machining plane 1 selection Machining plane 2 selection Machining plane 3 selection Machining plane 4 selection Machining plane 5 selection
(Available for an optional horizontal/vertical angle)
Axis switching/3-D coordinate conversion ON Axis switching/3-D coordinate conversion canel Multi-buffer Tool nose interference check ON *1 Tool nose interference check OFF *1 Cylindrical interpolation Floating reference point return Circular cutting inner diameter CW Circular cutting inner diameter CCW Circular cutting outer diameter CW Circular cutting outer diameter CCW Multi-step skip function 1 *1 Multi-step skip function 2 *1 Multi-step skip function 3 *1 Multi-step skip function 4 *1 Square outside cutting CW Square outside cutting CCW Square plane Square plane 1-directional Square plane 2-directional Circle inside (pocketing) Square inside (pocketing) Track inside (pocketing) circle outside (pocketing)
1 - 5
Code G331 G332 G333 G334 G335 G336 G337 G338 G401 G411 G421 C431 G501 G511
G540~
G599 G611 C653 G661 G721 G722 G741 G841 G812 G813 G921
Group
00
19
08 15
12 00
00 14
00
09
00
Function Remarks Square outside (pocketing) Track outside (pocketing) Circle (pocketing) Trochoid cycle High-speed side cutting cycle Z feed fluting cycle Corner pocket cycle Square pocket cycle Normal direction control cancel node Normal direction control left side ON Normal direction control right side ON Tool axis direction tool length compensation *1 Programmable mirror image Cancel Programmable mirror image Additional work coordinate system selection (60 pairs) Pre-interpolation acceleration/deceleration *1 Position check (Note) for Maintenance *1 Macro modal call B *1 Rotary copy *1 Parallel copy *1 Counter direct tap cycle Direct tap cycle Helical drilling cycle CW Helical drilling cycle CCW 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
 
G00 X_ Y_ Z_ ;
G91
 
(2) Sample program
(a) Absolute programming (b) Incremental programming
G90 G00 X100. Y50. : G91 G00 X100. Y50.
50.
Y
End point
Start point
X
100.
Y
Start point
100. End point
50.
X
(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.
Start point
End point
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
G90
{ }
G91
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
100. End point
50.
Start point
50.
Y
End point
Start point
100.
X
(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.
X
G01 G91 Xa Yb Zc Ff:
X-axis cutting feed rate: Fx = , where; L= a
Y-axis cutting feed rate: Fy =
z-axis cutting feed rate, Fz =
af L
bf L
cf L
2
+ b2 + c
2
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
G01 G91 X100. C90. F200 :
End Point
Cutting feed rate in the rotary axis (C axis) direction:
Start Point
Fc = (deg/min)
where; L = 100.
90. x 200 L
2
+ 90
2
(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
1 G01 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) X
plane
P YP
G02
 
G17 XP- YP- F_ ;
 
G03
(b) ZP -XP plane
G02
 
G18 ZP- YP- F_ ;
 
G03
(c) XP -ZP plane
G02
 
G19 YP-ZP- F_ ;
 
G03
Where; XP : X axis or its parallel axis
Y Z
(Note) To specify with R instead of I, J or K is called radius designation on arc.
R_
   
I_ J_
R_
   
K_ I_
R_
   
J_ K_
: Y axis or its p arallel axis
P
: Z axis or its parallel axis
P
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.
G02
Start point
186.603
End point
J=50
Center
100.
(3) Arc rotating direction
G02 : Clockwise (CW) G03 : Counterclockwise direction (CCW)
Y
100.
X
G02
X
P
Z
G03
G03
G02
G02
Start point
186.603
P
G03
G02
100.
End point
J=50
Y
P
X
(4) Arc plane
The arc plane is specified with C17, G18 or G19.
G17 : X G18 : Z G19 : Y
-YP plane
P
-XP plane
P
-ZP plane
P
(5) Arc center
The arc center is specified with I, J or K corresponding to X
,YP and ZP respectively. In this
P
case, I, J and K are the vector components when viewing the arc center from its start point.
Y
P
End Point
J I
Center point
Start Point
X
P
X
P
End Point
I K
Center point
Start Point
Z
P
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 error
Start Point
End Point
Moves linearly
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) X
P-YP
plane
G17 X
(b) Z
P-XP
G02
{ }
G03
plane
_ YP _ R ±_ F_ :
P
G02
G18 Z
(c) Y
P-ZP
{ }
G03
plane
_ YP _ R ±_ F_ :
P
G02
G19 Y
{ }
G03
where; X
P-ZP
: X axis or its parallel axis
P
: Y axis or its p arallel axis
Y
P
Z
: Z axis or its parallel axis
P
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:
_ R ±_ F_ :
°
(b) For the arc of over 180°
G17 G91 G02 X100. Y-100. R-100. F200 :
Y
End Point
R100.
Start Point
Center
Less than 180°
X
Y
Start Point
End Point
R100.
Center
(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.
G02
(c) When G91 R_ : is specified, it is taken as a block without axial move.
   
G03
(4) Associated parameters
More than 180°
X
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
G02
G17 X
G18 Z
G19 Y
where; X
   
G03 G02
   
G03 G02
   
G03
: X axis or its parallel axis
P
: Y axis or its p arallel axis
Y
P
Z
: Z axis or its parallel axis
P
α : Any optional linear axis for other than circulate interpolation (up to 2 axes)
F : Arc speed
Linear axis speed = F
R _
_ YP _ α_ F_ ;
P
_ YP _ α_ F_ ;
P
_ ZP _ α_ F_ ;
P
   
I _ J _ R _
   
I _ J _ R _
   
I _ J _
Linear arc length
×
Arc length
2 - 7
(2) Sample program
G17 G91 G03 X-100. Y-100. R100. Z50. F200 :
Z
End Point
Start Point
X
(3) The axes for other than circular interpolation can be specified up to 2 axes in the same
block. (Example) G17 G91 G03 I-100. Z100. V50. F200 :
I-100. Z100.V50.;
Z
Tool Path
Y
The V axis must be parallel 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
α 0 ; Sets the α axis as the virtual axis.
G07 : The
: in this section. G07
α 1 ; Cancels the a axis as the virtual axis.
where ;
(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.
α : Any one axis
α axis is the virtual axis
}
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 α0 ; Sets the virtual axis.
specify helical interpolation.
G07
α1 ; Cancels the virtual axis.
α is 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_...;
:
Single direction positioning
:
G00 ;
Cancels G60 if any G code in Group 01 other than G60 is given.
(2) Sample program
(a) When moving in the (b) When moving in the
+ direction - direction G60 G91 X100.; G60 G91 X-100.;
Start Point
End Point
Approach Amount
End Point
Approach Amount
Start Point
(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.
θ) =R [cosθ + (θ- θ0) sinθ ] +X0
X(
θ) =R [sinθ + (θ- θ0) cosθ ] +Y0
Y(
where;
X0, Y0:Central coordinate of the basic circle R : Radius of the basic circle
θ 0 : 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
θ ), Y(θ ) :Current position of the X-and Y-axis
X(
Y
Start Point
involute Carve
(X, Y)
R
(X0, Y0)
Basic Circle
The involute curves in the Z-X and Y-Z planes are defined in the same manner as that in the X­Y plane.
θ 0
θ
End Point
2 - 15
(2) Command format
(a) X
_ plane
P -YP
G222
 
G17 XP _YP _ I_ J_ R_ F_ ;
 
G223
(b) ZP-XP Plane
G222
 
G18 ZP _ YP_ K_ J_ R_ F_;
 
G223
(c) YP-ZP plane
G222
 
G19 YP_ ZP J_ K_ R_ F_ ;
 
G223
where;
G222 : Clockwise involute interpolation G223 : Counterclockwise involute interpolation X
, YP, ZP: Coordinate value of the end point
P
X
P
Y
P
Z
P
: X-axis or its parallel axis : Y-axis or its parallel axis : Z-axis or its parallel axis
I, J, K : Central position of the basic circle for the involute curve viewed from the
R : Radius of the basic circle F : Cutting feed rate
start point
(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
Loading...
+ 362 hidden pages
Buy Points How it Works FAQ Contact Us Questions and Suggestions Privacy Policy Cookie Policy Terms of Use