Hello Guest it is December 11, 2019, 11:45:31 AM

Author Topic: g41 - Tool Compensation Help  (Read 2238 times)

0 Members and 1 Guest are viewing this topic.

g41 - Tool Compensation Help
« on: May 24, 2013, 07:44:30 AM »
ok heres my original code

( Made using CamBam - http://www.cambam.co.uk )
( part1.4_edit1 5/24/2013 12:15:47 PM )
( T0 : 8.0 )
G21 G90 G64 G40
G0 Z3.0
( T0 : 8.0 )
M6 T6
( Engrave1 )
G17
M3 S3200
G0 X13.1711 Y11.4362
G0 Z1.0
G1 F100.0 Z-1.0
G2 F250.0 X10.3813 Y9.539 I-2.7898 J1.1026
G1 X9.5
G3 X2.7825 Y6.7566 I-0.0127 J-9.4697
G3 X0.0 Y0.0391 I6.685 J-6.7041
G3 X2.7825 Y-6.6784 I9.4689 J-0.0129
G3 X9.5 Y-9.4609 I6.7046 J6.6865
G1 X10.3813
G2 X13.1711 Y-11.3579 I0.0005 J-2.9992
G3 X17.7278 Y-19.2571 I28.7178 J11.3021
G3 X23.1285 Y-24.5608 I24.133 J19.1726
G1 X22.5313 Y-24.0918
G3 X28.4181 Y-27.8276 I19.5263 J24.2629
G3 X36.9545 Y-30.5523 I13.6395 J27.9987
G1 X37.7051 Y-30.6673
G3 X44.8702 Y-30.8354 I4.3005 J30.5187
G3 X53.3971 Y-28.7897 I-2.8636 J30.7299
G3 X70.829 Y-11.3578 I-11.3947 J28.8265
G2 X73.6188 Y-9.4608 I2.7898 J-1.1029
G1 X74.5
G3 X78.3004 Y-8.67 I0.0113 J9.4724
G3 X81.2175 Y-6.6782 I-3.789 J8.6815
G3 X83.9999 Y0.0393 I-6.6869 J6.7047
G3 X81.2175 Y6.7567 I-9.4673 J0.0135
G3 X74.5 Y9.5391 I-6.7045 J-6.6862
G1 X73.6188
G2 X70.8289 Y11.4363 I0.0002 J3.0001
G3 X66.6274 Y18.8798 I-28.7197 J-11.3037
G3 X60.8714 Y24.6392 I-24.4859 J-18.7149
G1 X61.4687 Y24.1702
G3 X51.5402 Y29.5357 I-19.527 J-24.2645
G3 X47.0455 Y30.6306 I-9.598 J-29.6277
G1 X46.2949 Y30.7457
G3 X38.7146 Y30.8722 I-4.3005 J-30.5166
G3 X30.6029 Y28.8681 I3.2791 J-30.6899
G3 X13.1711 Y11.4362 I11.3947 J-28.8265
G0 Z3.0
M5
M30


now im using an 8mm cutter and want mach3 to take this into account so i want to use the g41 command.

so did this

( Made using CamBam - http://www.cambam.co.uk )
( part1.4_edit1 5/24/2013 12:15:47 PM )
( T0 : 8.0 )
G21 G90 G64 G40
G0 Z3.0
( T0 : 8.0 )
M6 T6
( Engrave1 )
G17
M3 S3200
G41 D8
G0 X13.1711 Y11.4362
G0 Z1.0
G1 F100.0 Z-1.0
G2 F250.0 X10.3813 Y9.539 I-2.7898 J1.1026
G1 X9.5
G3 X2.7825 Y6.7566 I-0.0127 J-9.4697
G3 X0.0 Y0.0391 I6.685 J-6.7041
G3 X2.7825 Y-6.6784 I9.4689 J-0.0129
G3 X9.5 Y-9.4609 I6.7046 J6.6865
G1 X10.3813
G2 X13.1711 Y-11.3579 I0.0005 J-2.9992
G3 X17.7278 Y-19.2571 I28.7178 J11.3021
G3 X23.1285 Y-24.5608 I24.133 J19.1726
G1 X22.5313 Y-24.0918
G3 X28.4181 Y-27.8276 I19.5263 J24.2629
G3 X36.9545 Y-30.5523 I13.6395 J27.9987
G1 X37.7051 Y-30.6673
G3 X44.8702 Y-30.8354 I4.3005 J30.5187
G3 X53.3971 Y-28.7897 I-2.8636 J30.7299
G3 X70.829 Y-11.3578 I-11.3947 J28.8265
G2 X73.6188 Y-9.4608 I2.7898 J-1.1029
G1 X74.5
G3 X78.3004 Y-8.67 I0.0113 J9.4724
G3 X81.2175 Y-6.6782 I-3.789 J8.6815
G3 X83.9999 Y0.0393 I-6.6869 J6.7047
G3 X81.2175 Y6.7567 I-9.4673 J0.0135
G3 X74.5 Y9.5391 I-6.7045 J-6.6862
G1 X73.6188
G2 X70.8289 Y11.4363 I0.0002 J3.0001
G3 X66.6274 Y18.8798 I-28.7197 J-11.3037
G3 X60.8714 Y24.6392 I-24.4859 J-18.7149
G1 X61.4687 Y24.1702
G3 X51.5402 Y29.5357 I-19.527 J-24.2645
G3 X47.0455 Y30.6306 I-9.598 J-29.6277
G1 X46.2949 Y30.7457
G3 X38.7146 Y30.8722 I-4.3005 J-30.5166
G3 X30.6029 Y28.8681 I3.2791 J-30.6899
G3 X13.1711 Y11.4362 I11.3947 J-28.8265
G0 Z3.0
G40
M5
M30


just added g41 d8 and then g40 at the end
but it isnt actually turning on in mach3
under tooling t6 is set to 8mm dia
can someone help?

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: g41 - Tool Compensation Help
« Reply #1 on: May 24, 2013, 12:24:53 PM »
G41 D8 means use the diameter of tool #8.
You probably want G41 D6.
You also need to add a lead in move.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: g41 - Tool Compensation Help
« Reply #2 on: May 24, 2013, 10:03:49 PM »
If I remember how I used to do this, its been about 15 years.  For the lead in move I'd just subtract about 0.010 from the X or Y of the G0 move after the G41.  Then after the G0 I'd finish the distance by doing and X or Y G1 0.010 move.  At this move the tool will move over then advance the 0.010, putting the edge of the tool on the cutting line, before plunging in the Z direction.  I like to put all the cutting moves in a subroutine too.  Then I can make a roughing cut, change the tool diameter and make a finish pass along the same path, after pausing to measure the part.

Gary H. Lucas

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: g41 - Tool Compensation Help
« Reply #3 on: May 25, 2013, 06:54:59 AM »
The lead in move needs to be at least 1/2 the tool diameter, preferably a little more. .01 probably won't work.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: g41 - Tool Compensation Help
« Reply #4 on: May 25, 2013, 07:04:32 AM »
Sometimes it's difficult to add a leadin to existing g-code.
In this case, you either run into a bug in the comp, or poor code that is causing problems with the comp.

Here's a quick change that get's comp working (somewhat), but there are issues that will probably ruin the part. This could be caused by a poor drawing to start with, possibly duplicate lines or points in the drawing.

G17
M3 S3200
G0 Z1.0
G0 X25 Y16
G41 D6
G0 X13.1711 Y11.4362
G1 F100.0 Z-1.0
G2 F250.0 X10.3813 Y9.539 I-2.7898 J1.1026
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html