G41 and G42 Input path error

I never used it

( PART NAME=2mm )
( MACHINE=LINUXCNC )
(1.5MM CRB3FL 25 LOC)
G54 G0 G90 G21 G17 G40 G80
T1M6
G10 L1 P1 R0.5 (SET TOOL TABLE POSITION #1)
S12000 M03
M08
G00 X36.7 Y17.04
G43 Z-3. H01
G01 Z-7. F662.94
G41 X36.7 Y16. D1 F1988.82
X37. F2651.76
X54.284
X56.409 Y43.
X54.914
G40
G91 G28 Z0
G28 Z0Y0
G90
m30

D23 is taken from your selection of tools in your cam. you will surely find the value in the configuration. For example, I use Surfcam and I can tell the system which table number to use, you should be able to do the same. But you do not have the problem in D23 as table position, your problem is in the value of the diameter (3mm is too big for the length of entry to the path you have programmed), so that your program works well, your diameter should be smaller to 1mm. Remember you must always place the value of your tool diameter in the table in order to use G41 or G42. it is from there where the value to be compensated is taken.

If you want to use tool #3 change the D23 to D3, but the real problem is that your next move after the entry move is less than the tool radius - it moves from X36.7 to X37 = 0.3 Cutter needs to be less than 0.6 diameter. Change the first move after comp to X36.7 + more than half the tool#3 diameter and see if that works.

Refer to www.linuxcnc.org/docs/2.7/html/gcode/too...:cutter-compensation

Best way to learn cutter diameter compensation is to write the code by hand and understand what it is doing. Alternately, in you CAM just turn it off, and let the Gcode reflect the tool centreline path, rather than the coordinates of the part itself. Will work provided that the tool diameter used in CAM is same as actual tool diameter!

As for where the T01 and D23 comes from - that is some sort of issue with the CAM postprocessor.

The inside pocket I have in my design has a 2 mm radius and I prefer to use a bigger mill than to use a smaller one just because my cam software doesn't play nice with my CNC.

I tried using your input to edit my G code with no success(same error message) but I'm surely doing something wrong. But even if I got it figured it takes a lot to edit every G41 line in every G code.

In Solidworks CAM I can't find any option regarding cutter compensation
Only option left is to edit my postprocessor to stop using cutter compensation G41 as you said.
I am trying to learn UPG from a youtube clip but can't find how to remove G41 cutter compensation option.
In Solidworks CAM I can't find any option regarding cutter compensation
What do you use to edit your post-processor?

Thank you for your help and patience

Why don't you change your design to reflect your choice of tool? If you want to use a 10mm cutter it is normal for the pocket rad to be bigger than 5mm to allow the NC to "drive" around the corner, rather than stop and change direction, which will leave a dwell mark in the corner.

For the solidworks CAM questions, you might want repost those specific questions in the CAM section of the forum. I don't use solidworks but I think many do. In CATIA you usually have to explicitly turn on the compensation (see attached), many production CNC made parts suppliers don't use tool diameter compensation now anyway it seems.

Usually the post is supplied by the NC machine manufacturer, and they are usually not easily (if at all) tweak-able. CATIA generates an "NC Neutral" format APT file, which the post's generally convert to g-code. There are a few sample posts supplied with CATIA, and the FANUC 30 one generates g-code that works pretty well with linux CNC.