1 Attachment(s)
Cutter Compensation problem
The rectangle I demonstrating is 2" x 4", When make part the dimension always off about .015 radius and I though I could use tool compensation to take care of it, however Mach3 give me quite a problem. If I put in .015 in tool offset diameter the machine will cut (G03 X3.1963 Y2.1759 I0.1875 J0 F25.) line on the left as shown in the picture, if I put in -.015 in tool offset diameter the machine will cut (G02 X7.1213 Y1.8509 I0 J-0.325 line on the right as shown in the picture. Does anyone know why? maybe there is some parameter in the Config that I missed?
By the way, if i put .015/-.015 in Tool Wear under Tool Offset nothing happen, nothing I mean the machine will cut just fine but then it is defeat the point have comp .
Thanks
%
O0
(MACHINE: FANUC 15MB MPost Library)
G17 G40 G80 G90
T1 M6
G00 G55 X3.0213 Y2.3634
G43 Z0.3 H1
M9
Z0.1
G01 Z-0.1 F25.
G41 X3.0088 F20. D11
G03 X3.1963 Y2.1759 I0.1875 J0 F25. (if .015 input this line start have problem)
G01 X6.7963 F20.
G02 X7.1213 Y1.8509 I0 J-0.325 (if -.015 input this line start have problem)
G01 Y0.2509
G02 X6.7963 Y-0.0741 I-0.325 J0
G01 X3.1963
G02 X2.8713 Y0.2509 I0 J0.325
G01 Y1.8509
G02 X3.1963 Y2.1759 I0.325 J0
G03 X3.3838 Y2.3634 I0 J0.1875 F25.
G01 G40 X3.3713
G00 Z0.3
X0.025 Y1.3125
Z0.1
G01 Z-0.1
G41 X0.0125 F20. D11
G03 X0.2 Y1.125 I0.1875 J0 F25.
G01 X1.8 F20.
G02 X2.125 Y0.8 I0 J-0.325
G01 Y0.2
G02 X1.8 Y-0.125 I-0.325 J0
G01 X0.2
G02 X-0.125 Y0.2 I0 J0.325
G01 Y0.8
G02 X0.2 Y1.125 I0.325 J0
G03 X0.3875 Y1.3125 I0 J0.1875 F25.
G01 G40 X0.375
G00 Z0.3
M9
G28G91 Z0
G90 G00 G59
X0 Y0
M30
%
Re: Cutter Compensation problem
Re: Cutter Compensation problem
i notice you are using t1 and h1 but d11. is that intentional? and are you adjusting the comp in the d11 spot?
Re: Cutter Compensation problem
aware of that but so far it doesn't make diffirence.
- - - Updated - - -
Quote:
Originally Posted by
RINES
i notice you are using t1 and h1 but d11. is that intentional? and are you adjusting the comp in the d11 spot?
Yes, it is program like that by design.
Re: Cutter Compensation problem
...this is not a long term fix for CAM post but, try running modified program below see if this fixes the problem...see notes.
%
O99 (changed to 99 from 0)
(MACHINE: FANUC 15MB MPost Library)
N10 G17 G40 G80 G90
N20 T1 M6
N30 G00 G55 X3.5 Y2.5 (changed XY start point)
N40 G43 Z0.3 H1
N50 M9
N60 Z0.1
N70 G01 Z-0.1 F25.
N80 G41 X3.0088 Y2.3634 F20. D11 (added/moved to here Y)
N90 G03 X3.1963 Y2.1759 I0.1875 J0 F25.
N100 G01 X6.7963 F20.
N110 G02 X7.1213 Y1.8509 I0 J-0.325
N120 G01 Y0.2509
N130 G02 X6.7963 Y-0.0741 I-0.325 J0
N140 G01 X3.1963
N150 G02 X2.8713 Y0.2509 I0 J0.325
N160 G01 Y1.8509
N170 G02 X3.1963 Y2.1759 I0.325 J0
N180 G03 X3.3838 Y2.3634 I0 J0.1875 F25.
N190 G01 G40 X3.3713
N200 G00 Z0.3
N210 X0.5 Y1.5 (changed XY start point)
N220 Z0.1
N230 G01 Z-0.1
N240 G41 X0.0125 Y1.3125 F20. D11 (added/moved to here Y)
N250 G03 X0.2 Y1.125 I0.1875 J0 F25.
N260 G01 X1.8 F20.
N270 G02 X2.125 Y0.8 I0 J-0.325
N280 G01 Y0.2
N290 G02 X1.8 Y-0.125 I-0.325 J0
N300 G01 X0.2
N310 G02 X-0.125 Y0.2 I0 J0.325
N320 G01 Y0.8
N330 G02 X0.2 Y1.125 I0.325 J0
N340 G03 X0.3875 Y1.3125 I0 J0.1875 F25.
N350 G01 G40 X0.375
N360 G00 Z0.3
N370 M9
N380 G28 G91 Z0
N390 G90 G00 G59
N400 X0 Y0
N410 M30
%
START POINT MAYBE WRONG...ADJUST AS NEEDED
Re: Cutter Compensation problem
The changes that machinehop5 did should solve the problem
I will assume you are using .0000 as the start of the radial value for the end mill
Your starting point is X3.0213 and the move to set the cutter comp is X3.0088 this is .0125 distance that will be all that you can have for cutter comp
after .0125 the control should say g41/g42 comp interference
Re: Cutter Compensation problem
Thanks everyone for the help. However, it didn't solve weird move. I have software that can be easily offset it just annoying, kept play with it I will figure it out.
Re: Cutter Compensation problem
Quote:
Originally Posted by
CNCRim
The rectangle I demonstrating is 2" x 4", When make part the dimension always off about .015 radius and I though I could use tool compensation to take care of it, however Mach3 give me quite a problem. If I put in .015 in tool offset diameter the machine will cut (G03 X3.1963 Y2.1759 I0.1875 J0 F25.) line on the left as shown in the picture, if I put in -.015 in tool offset diameter the machine will cut (G02 X7.1213 Y1.8509 I0 J-0.325 line on the right as shown in the picture. Does anyone know why? maybe there is some parameter in the Config that I missed?
By the way, if i put .015/-.015 in Tool Wear under Tool Offset nothing happen, nothing I mean the machine will cut just fine but then it is defeat the point have comp .
Thanks
%
O0
(MACHINE: FANUC 15MB MPost Library)
G17 G40 G80 G90
T1 M6
G00 G55 X3.0213 Y2.3634
G43 Z0.3 H1
M9
Z0.1
G01 Z-0.1 F25.
G41 X3.0088 F20. D11
G03 X3.1963 Y2.1759 I0.1875 J0 F25. (if .015 input this line start have problem)
G01 X6.7963 F20.
G02 X7.1213 Y1.8509 I0 J-0.325 (if -.015 input this line start have problem)
G01 Y0.2509
G02 X6.7963 Y-0.0741 I-0.325 J0
G01 X3.1963
G02 X2.8713 Y0.2509 I0 J0.325
G01 Y1.8509
G02 X3.1963 Y2.1759 I0.325 J0
G03 X3.3838 Y2.3634 I0 J0.1875 F25.
G01 G40 X3.3713
G00 Z0.3
X0.025 Y1.3125
Z0.1
G01 Z-0.1
G41 X0.0125 F20. D11
G03 X0.2 Y1.125 I0.1875 J0 F25.
G01 X1.8 F20.
G02 X2.125 Y0.8 I0 J-0.325
G01 Y0.2
G02 X1.8 Y-0.125 I-0.325 J0
G01 X0.2
G02 X-0.125 Y0.2 I0 J0.325
G01 Y0.8
G02 X0.2 Y1.125 I0.325 J0
G03 X0.3875 Y1.3125 I0 J0.1875 F25.
G01 G40 X0.375
G00 Z0.3
M9
G28G91 Z0
G90 G00 G59
X0 Y0
M30
%
Try this, you may have a problem with the G41 cutter comp activating as the moves you have in the second part of the program may not work, the move has to be at least the tool diameter
D11 is not going to work
%
O0
G17 G40 G80 G90
T1 M6
G00 G55 X3.0213 Y2.3634
G43 Z0.3 H1
M9
Z0.1
G01 Z-0.1 F25.
G41 X3.0088 P.015 F20.
G03 X3.1963 Y2.1759 I0.1875 J0 F25.
G01 X6.7963 F20.
G02 X7.1213 Y1.8509 I0 J-0.325
G01 Y0.2509
G02 X6.7963 Y-0.0741 I-0.325 J0
G01 X3.1963
G02 X2.8713 Y0.2509 I0 J0.325
G01 Y1.8509
G02 X3.1963 Y2.1759 I0.325 J0
G03 X3.3838 Y2.3634 I0 J0.1875 F25.
G01 G40 X3.3713
G00 Z0.3
X0.025 Y1.3125
Z0.1
G01 Z-0.1
G41 X0.0125 P.015 F20.
G03 X0.2 Y1.125 I0.1875 J0 F25.
G01 X1.8 F20.
G02 X2.125 Y0.8 I0 J-0.325
G01 Y0.2
G02 X1.8 Y-0.125 I-0.325 J0
G01 X0.2
G02 X-0.125 Y0.2 I0 J0.325
G01 Y0.8
G02 X0.2 Y1.125 I0.325 J0
G03 X0.3875 Y1.3125 I0 J0.1875 F25.
G01 G40 X0.375
G00 Z0.3
M9
G53 Z0
X0 Y0
M30
%
Re: Cutter Compensation problem
Quote:
Originally Posted by
mactec54
Try this, you may have a problem with the G41 cutter comp activating as the moves you have in the second part of the program may not work, the move has to be at least the tool diameter
D11 is not going to work
%
O0
G17 G40 G80 G90
T1 M6
G00 G55 X3.0213 Y2.3634
G43 Z0.3 H1
M9
Z0.1
G01 Z-0.1 F25.
G41 X3.0088 P.015 F20.
G03 X3.1963 Y2.1759 I0.1875 J0 F25.
G01 X6.7963 F20.
%
Heya Mactec.
So can you interperate to me how this line works please?.
I might need to play with it myself also.
I've put an idea of how I think it reads. Just need you to tell me I'm stupid and correct me.
G41- Start cuuter radius compensation (left).
X3.0088 - X axis starting point ready for lead in.
P.015 - Amound added to tool (0.015 larger diameter). So a P-.015 would make it smaller?.
F20 - Our starting ffedrate.
Thanks.
This document from machmotion is probarbly quite a useful indepth read to many.
Explains quite a lot on how the g-code language works:
https://machmotion.com/documentation...-Reference.pdf
Re: Cutter Compensation problem
Quote:
Originally Posted by
dazp1976
Heya Mactec.
So can you interperate to me how this line works please?.
I might need to play with it myself also.
I've put an idea of how I think it reads. Just need you to tell me I'm stupid and correct me.
G41- Start cuuter radius compensation (left).
X3.0088 - X axis starting point ready for lead in.
P.015 - Amound added to tool (0.015 larger diameter). So a P-.015 would make it smaller?.
F20 - Our starting ffedrate.
Thanks.
This document from machmotion is probarbly quite a useful indepth read to many.
Explains quite a lot on how the g-code language works:
https://machmotion.com/documentation...-Reference.pdf
No it is not normal add a - or a + sign to this number the G41 is going to move the P.015 there must be an axis move by a minimum of half the tool diameter before cutter comp will activate
No the P0.15 will make it .015" smaller
Using the D word can also cancel the cutter comp in some controls so may be part of his problem
It will not activate any cutter comp unless the axis moves the right amount before engagement this is where most mess up
