Fanuc Radius Compensation
Moderators: TomKerekes, dynomotion

 Posts: 9
 Joined: Mon Aug 27, 2018 10:15 am
Fanuc Radius Compensation
Hi,
While using radius compensation, I've been getting two errors:
“Gcode Error concave corner with radius comp”
“Cutter gouging with cutter radius comp”
I assume this is related to the default EMC/NIST entry move style, so I would like to set the Fanuc radius compensation entry move style. I followed the section on the wiki to enable this style by adding the following line to the Kmotion CNC setup file:
comp_entry_style FANUC_COMP_ENTRY_STYLE
Now I'm getting the error: "Unknown attribute comp_entry_style"
I'm using Kmotion 433
Am I missing something here?
While using radius compensation, I've been getting two errors:
“Gcode Error concave corner with radius comp”
“Cutter gouging with cutter radius comp”
I assume this is related to the default EMC/NIST entry move style, so I would like to set the Fanuc radius compensation entry move style. I followed the section on the wiki to enable this style by adding the following line to the Kmotion CNC setup file:
comp_entry_style FANUC_COMP_ENTRY_STYLE
Now I'm getting the error: "Unknown attribute comp_entry_style"
I'm using Kmotion 433
Am I missing something here?
 TomKerekes
 Posts: 270
 Joined: Mon Dec 04, 2017 1:49 am
Re: Fanuc Radius Compensation
Regards,
Tom Kerekes
Dynomotion, Inc.
Tom Kerekes
Dynomotion, Inc.

 Posts: 9
 Joined: Mon Aug 27, 2018 10:15 am
Re: Fanuc Radius Compensation
I've installed 434. The installation on a new machine did not go smooth. After installation I got 3 errors:
" The code execution cannot proceed because mfc140d.dll was not found. Reinstalling the program may fix this problem."
" The code execution cannot proceed because VCRUNTIME140D.dll was not found. Reinstalling the program may fix this problem."
" The code execution cannot proceed because ucrtbased.dll was not found. Reinstalling the program may fix this problem."
During installation the installer prompted me to install something from Microsoft (forgot what) on which I chose "yes". So I was surprised that there were dll's missing. Anyways, I searched the web for these dll's, found them (https://www.dllme.com) and put them in the C:\Windows\SysWOW64 folder, after which KMotionCNC started without error.
Then I chose the default settings file "C:\KMotion434\KMotion\Data\Default.set" and added a single line to the bottom "comp_entry_style FANUC_COMP_ENTRY_STYLE". I restarted KMotionCNC to be sure the settings are loaded.
The good thing is that the error "Unknown attribute comp_entry_style" did not appear anymore. However, after that I tried to run my Gcode that uses radius compensation in simulation mode. This did not work. I'm still getting the "concave corner with cutter radius comp" error. This is the small test Gcode that I'm trying to run. Tool #1 should be set to 5mm diameter.
G00 G49 G40 G17
(CONTOURBEWERKING )
M00 (T0001  RECHTE FREES 5 MM)
M6 T0001
M3 S2000
G40
G49
G00 X1. Y0.25
G00 G43 H0001 Z20.
Z2.
G01 Z1.5 F32
G41 D0001 X2.945 Y2.195 F100
G03 X1. Y3. R2.75
G01 X0.
X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X0.
X1.
G03 X2.945 Y2.195 R2.75
G01 X1. Y0.25 G40
X1.
Z3. F32
G41 D0001 X2.945 Y2.195 F100
G03 X1. Y3. R2.75
G01 X0.
X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X0.
X1.
G03 X2.945 Y2.195 R2.75
G01 X1. Y0.25 G40
X1.
G00 Z40.
M9
M5
G40
M30
" The code execution cannot proceed because mfc140d.dll was not found. Reinstalling the program may fix this problem."
" The code execution cannot proceed because VCRUNTIME140D.dll was not found. Reinstalling the program may fix this problem."
" The code execution cannot proceed because ucrtbased.dll was not found. Reinstalling the program may fix this problem."
During installation the installer prompted me to install something from Microsoft (forgot what) on which I chose "yes". So I was surprised that there were dll's missing. Anyways, I searched the web for these dll's, found them (https://www.dllme.com) and put them in the C:\Windows\SysWOW64 folder, after which KMotionCNC started without error.
Then I chose the default settings file "C:\KMotion434\KMotion\Data\Default.set" and added a single line to the bottom "comp_entry_style FANUC_COMP_ENTRY_STYLE". I restarted KMotionCNC to be sure the settings are loaded.
The good thing is that the error "Unknown attribute comp_entry_style" did not appear anymore. However, after that I tried to run my Gcode that uses radius compensation in simulation mode. This did not work. I'm still getting the "concave corner with cutter radius comp" error. This is the small test Gcode that I'm trying to run. Tool #1 should be set to 5mm diameter.
G00 G49 G40 G17
(CONTOURBEWERKING )
M00 (T0001  RECHTE FREES 5 MM)
M6 T0001
M3 S2000
G40
G49
G00 X1. Y0.25
G00 G43 H0001 Z20.
Z2.
G01 Z1.5 F32
G41 D0001 X2.945 Y2.195 F100
G03 X1. Y3. R2.75
G01 X0.
X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X0.
X1.
G03 X2.945 Y2.195 R2.75
G01 X1. Y0.25 G40
X1.
Z3. F32
G41 D0001 X2.945 Y2.195 F100
G03 X1. Y3. R2.75
G01 X0.
X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X22.
G03 X25. Y0. R3.
X22. Y3. R3.
G01 X0.
X1.
G03 X2.945 Y2.195 R2.75
G01 X1. Y0.25 G40
X1.
G00 Z40.
M9
M5
G40
M30
 TomKerekes
 Posts: 270
 Joined: Mon Dec 04, 2017 1:49 am
Re: Fanuc Radius Compensation
Hi BaxEDM,
Sorry you had trouble. Those are all Debug versions of Visual Studio libraries and should only be needed when trying to debug. Maybe you were running from the \KMotion\Debug directory rather than the \KMotion\Release directory? BTW you should be very careful downloading dll's as they are often infected with viruses. So only download them from Microsoft, Dynomotion, or someone you completely trust.
The radius compensation seems to work ok for me. Here is a tool path plot of your GCode with comp for a 5mm diameter Tool.
Here is a double plot with/without compensation. "Without" comp was created by setting the Tool diameter to 0.001mm (Tool image diameter is still 5mm)
I've also attached the Settings file (as a txt file) that was used.
Any special offsets or other settings you are using?
Sorry you had trouble. Those are all Debug versions of Visual Studio libraries and should only be needed when trying to debug. Maybe you were running from the \KMotion\Debug directory rather than the \KMotion\Release directory? BTW you should be very careful downloading dll's as they are often infected with viruses. So only download them from Microsoft, Dynomotion, or someone you completely trust.
The radius compensation seems to work ok for me. Here is a tool path plot of your GCode with comp for a 5mm diameter Tool.
Here is a double plot with/without compensation. "Without" comp was created by setting the Tool diameter to 0.001mm (Tool image diameter is still 5mm)
I've also attached the Settings file (as a txt file) that was used.
Any special offsets or other settings you are using?
You do not have the required permissions to view the files attached to this post.
Regards,
Tom Kerekes
Dynomotion, Inc.
Tom Kerekes
Dynomotion, Inc.

 Posts: 9
 Joined: Mon Aug 27, 2018 10:15 am
Re: Fanuc Radius Compensation
Hi,
Thanks! It works now, not sure what I did wrong though, might have navigated to the 433 settings file while I changed the 434 or something...
Regarding the dll's, I was running the Debug exe indeed, my mistake, I removed the dlls and ran the released version without problems.
Thanks! It works now, not sure what I did wrong though, might have navigated to the 433 settings file while I changed the 434 or something...
Regarding the dll's, I was running the Debug exe indeed, my mistake, I removed the dlls and ran the released version without problems.

 Posts: 8
 Joined: Sun Aug 26, 2018 10:13 pm
Re: Fanuc Radius Compensation
So I had the same issues and am using a Fanuc style post I believe. I was glad to see this post and was able to download the setup file that Tom posted which resolved the gouging and concave corner messages for me.
However, now I have constant errors with G03 moves, each one popping up with "Tool radius not less than arc radius with comp."
Am I missing something else? Changing the post processor is possible but not as easy for me to do as working with KMotionCNC if there is something easy that I am just missing.
Below is a short test example of code  it is using a 12.7mm endmill with an actual diameter of 12.72mm that is stored in the tool table. Let me know if you have seen this issue and how is best to resolve please... Appreciate the help!
(PROGRAM NAME: 0001)
(METRIC MODE / ABS COORDINATES)
( SETUP1  9/24/2018  08:09:32 )
( FEATURECAM  AP MINI )
( MACHINE TIME = 2.4 MIN. )
( FINISH BOSS BOSS1 )
(***START TOOL DIAMETER = 12.7mm***)
(***START TOOL = 1/2"x1.25"  Square, 3F  Carbide***)
()
N60 G21 G17 G90
N65 T17 M6
N70 G54 G90 G43 H17
N75 G0 X21.75 Y4.675 S2500 M3
N80 Z10.0 F286.
N85 Z3.0
N90 G1 Z2.5
N95 G41 D17 X21.6 Y4.101 F572.
N100 G3 X21.55 Y3.51 R3.492 F286.
N105 G1 Y2.5 F572.
N110 G2 X14.2 Y4.85 R7.35 F857.
N115 G1 X3.5 F572.
N120 G2 X3.85 Y2.5 R7.35 F857.
N125 G1 Y6.85 F572.
N130 G2 X3.5 Y14.2 R7.35 F857.
N135 G1 X14.2 F572.
N140 G2 X21.55 Y6.85 R7.35 F857.
N145 G1 Y2.5 F572.
N150 G2 X14.2 Y4.85 R7.35 F857.
N155 G1 X11.781 F572.
N160 G3 X11.19 Y4.9 R3.493 F286.
N165 G1 G40 X10.616 Y5.05 F572.
N170 G0 Z10.0
N175 X26.201 Y10.535
N180 Z3.0
N185 G1 Z2.5 F286.
N190 G41 D17 X25.901 Y11.047 F572.
N195 G3 X25.519 Y11.501 R3.492 F286.
N200 G1 X21.272 Y15.748 F572.
N205 G2 X19.119 Y20.945 R7.35 F857.
N210 X21.272 Y26.143 R7.35
N215 G1 X39.303 Y44.174 F572.
N220 G2 X44.5 Y46.327 R7.35 F857.
N225 X49.697 Y44.174 R7.35
N230 G1 X67.728 Y26.143 F572.
N235 G2 X69.881 Y20.945 R7.35 F857.
N240 X67.728 Y15.748 R7.35
N245 G1 X49.697 Y2.283 F572.
N250 G2 X44.5 Y4.436 R7.35 F857.
N255 X39.303 Y2.283 R7.35
N260 G1 X21.984 Y15.036 F572.
N265 G3 X21.53 Y15.418 R3.492 F286.
N270 G1 G40 X21.018 Y15.718 F572.
N275 X13.749 Y21.574
N280 G41 D17 X13.32 Y21.299
N285 G3 X12.935 Y20.965 R3.492 F286.
N290 G2 X6.175 Y18.15 R9.525 F857.
N295 X3.35 Y27.675 R9.525
N300 X6.175 Y37.2 R9.525
N305 X15.7 Y27.675 R9.525
N310 X12.935 Y20.965 R9.525
N315 X6.175 Y18.15 R9.525
N320 X0.562 Y20.942 R9.525
N325 G3 X0.948 Y21.275 R3.493 F286.
N330 G1 G40 X1.377 Y21.548 F572.
N335 G0 Z10.0
N340 X1.425 Y41.027
N345 Z3.0
N350 G1 Z2.5 F286.
N355 G41 D17 X0.99 Y41.255 F572.
N360 G3 X0.527 Y41.42 R3.493 F286.
N365 G2 X4.85 Y48.5 R7.35 F857.
N370 G1 Y74.0 F572.
N375 G2 X2.5 Y81.35 R7.35 F857.
N380 G1 X28.0 F572.
N385 G2 X35.35 Y74.0 R7.35 F857.
N390 G1 Y48.5 F572.
N395 G2 X28.0 Y41.15 R7.35 F857.
N400 G1 X2.5 F572.
N405 G2 X4.85 Y48.5 R7.35 F857.
N410 G1 Y52.201 F572.
N415 G3 X4.885 Y52.691 R3.493 F286.
N420 G1 G40 X4.987 Y53.171 F572.
N425 G0 Z10.0
N430 X53.45
N435 Z3.0
N440 G1 Z2.5 F286.
N445 G41 D17 X53.6 Y53.745 F572.
N450 G3 X53.65 Y54.336 R3.492 F286.
N455 G1 Y74.0 F572.
N460 G2 X61.0 Y81.35 R7.35 F857.
N465 G1 X86.5 F572.
N470 G2 X93.85 Y74.0 R7.35 F857.
N475 G1 Y48.5 F572.
N480 G2 X86.5 Y41.15 R7.35 F857.
N485 G1 X61.0 F572.
N490 G2 X53.65 Y48.5 R7.35 F857.
N495 G1 Y59.336 F572.
N500 G3 X53.6 Y59.927 R3.493 F286.
N505 G1 G40 X53.45 Y60.501 F572.
N510 G0 Z10.0
N515 X76.34 Y34.922
N520 Z3.0
N525 G1 Z2.5 F286.
N530 G41 D17 X76.808 Y35.124 F572.
N535 G3 X77.241 Y35.392 R3.492 F286.
N540 G2 X82.825 Y37.2 R9.525 F857.
N545 X92.35 Y27.675 R9.525
N550 X82.825 Y18.15 R9.525
N555 X73.3 Y27.675 R9.525
N560 X77.241 Y35.392 R9.525
N565 X82.825 Y37.2 R9.525
N570 X90.564 Y33.228 R9.525
N575 G3 X90.89 Y32.837 R3.493 F286.
N580 G1 G40 X91.27 Y32.497 F572.
N585 G0 Z10.0
N590 X87.157 Y14.216
N595 Z3.0
N600 G1 Z2.5 F286.
N605 G41 D17 X87.573 Y13.955 F572.
N610 G3 X88.021 Y13.754 R3.493 F286.
N615 G2 X92.85 Y6.85 R7.35 F857.
N620 G1 Y2.5 F572.
N625 G2 X85.5 Y4.85 R7.35 F857.
N630 G1 X74.8 F572.
N635 G2 X67.45 Y2.5 R7.35 F857.
N640 G1 Y6.85 F572.
N645 G2 X74.8 Y14.2 R7.35 F857.
N650 G1 X85.5 F572.
N655 G2 X92.85 Y6.85 R7.35 F857.
N660 G1 Y3.071 F572.
N665 G3 X92.885 Y2.581 R3.493 F286.
N670 G1 G40 X92.987 Y2.101 F572.
N675 G0 Z10.0
( END OF PROGRAM )
N685 M101
N690 M30
%
However, now I have constant errors with G03 moves, each one popping up with "Tool radius not less than arc radius with comp."
Am I missing something else? Changing the post processor is possible but not as easy for me to do as working with KMotionCNC if there is something easy that I am just missing.
Below is a short test example of code  it is using a 12.7mm endmill with an actual diameter of 12.72mm that is stored in the tool table. Let me know if you have seen this issue and how is best to resolve please... Appreciate the help!
(PROGRAM NAME: 0001)
(METRIC MODE / ABS COORDINATES)
( SETUP1  9/24/2018  08:09:32 )
( FEATURECAM  AP MINI )
( MACHINE TIME = 2.4 MIN. )
( FINISH BOSS BOSS1 )
(***START TOOL DIAMETER = 12.7mm***)
(***START TOOL = 1/2"x1.25"  Square, 3F  Carbide***)
()
N60 G21 G17 G90
N65 T17 M6
N70 G54 G90 G43 H17
N75 G0 X21.75 Y4.675 S2500 M3
N80 Z10.0 F286.
N85 Z3.0
N90 G1 Z2.5
N95 G41 D17 X21.6 Y4.101 F572.
N100 G3 X21.55 Y3.51 R3.492 F286.
N105 G1 Y2.5 F572.
N110 G2 X14.2 Y4.85 R7.35 F857.
N115 G1 X3.5 F572.
N120 G2 X3.85 Y2.5 R7.35 F857.
N125 G1 Y6.85 F572.
N130 G2 X3.5 Y14.2 R7.35 F857.
N135 G1 X14.2 F572.
N140 G2 X21.55 Y6.85 R7.35 F857.
N145 G1 Y2.5 F572.
N150 G2 X14.2 Y4.85 R7.35 F857.
N155 G1 X11.781 F572.
N160 G3 X11.19 Y4.9 R3.493 F286.
N165 G1 G40 X10.616 Y5.05 F572.
N170 G0 Z10.0
N175 X26.201 Y10.535
N180 Z3.0
N185 G1 Z2.5 F286.
N190 G41 D17 X25.901 Y11.047 F572.
N195 G3 X25.519 Y11.501 R3.492 F286.
N200 G1 X21.272 Y15.748 F572.
N205 G2 X19.119 Y20.945 R7.35 F857.
N210 X21.272 Y26.143 R7.35
N215 G1 X39.303 Y44.174 F572.
N220 G2 X44.5 Y46.327 R7.35 F857.
N225 X49.697 Y44.174 R7.35
N230 G1 X67.728 Y26.143 F572.
N235 G2 X69.881 Y20.945 R7.35 F857.
N240 X67.728 Y15.748 R7.35
N245 G1 X49.697 Y2.283 F572.
N250 G2 X44.5 Y4.436 R7.35 F857.
N255 X39.303 Y2.283 R7.35
N260 G1 X21.984 Y15.036 F572.
N265 G3 X21.53 Y15.418 R3.492 F286.
N270 G1 G40 X21.018 Y15.718 F572.
N275 X13.749 Y21.574
N280 G41 D17 X13.32 Y21.299
N285 G3 X12.935 Y20.965 R3.492 F286.
N290 G2 X6.175 Y18.15 R9.525 F857.
N295 X3.35 Y27.675 R9.525
N300 X6.175 Y37.2 R9.525
N305 X15.7 Y27.675 R9.525
N310 X12.935 Y20.965 R9.525
N315 X6.175 Y18.15 R9.525
N320 X0.562 Y20.942 R9.525
N325 G3 X0.948 Y21.275 R3.493 F286.
N330 G1 G40 X1.377 Y21.548 F572.
N335 G0 Z10.0
N340 X1.425 Y41.027
N345 Z3.0
N350 G1 Z2.5 F286.
N355 G41 D17 X0.99 Y41.255 F572.
N360 G3 X0.527 Y41.42 R3.493 F286.
N365 G2 X4.85 Y48.5 R7.35 F857.
N370 G1 Y74.0 F572.
N375 G2 X2.5 Y81.35 R7.35 F857.
N380 G1 X28.0 F572.
N385 G2 X35.35 Y74.0 R7.35 F857.
N390 G1 Y48.5 F572.
N395 G2 X28.0 Y41.15 R7.35 F857.
N400 G1 X2.5 F572.
N405 G2 X4.85 Y48.5 R7.35 F857.
N410 G1 Y52.201 F572.
N415 G3 X4.885 Y52.691 R3.493 F286.
N420 G1 G40 X4.987 Y53.171 F572.
N425 G0 Z10.0
N430 X53.45
N435 Z3.0
N440 G1 Z2.5 F286.
N445 G41 D17 X53.6 Y53.745 F572.
N450 G3 X53.65 Y54.336 R3.492 F286.
N455 G1 Y74.0 F572.
N460 G2 X61.0 Y81.35 R7.35 F857.
N465 G1 X86.5 F572.
N470 G2 X93.85 Y74.0 R7.35 F857.
N475 G1 Y48.5 F572.
N480 G2 X86.5 Y41.15 R7.35 F857.
N485 G1 X61.0 F572.
N490 G2 X53.65 Y48.5 R7.35 F857.
N495 G1 Y59.336 F572.
N500 G3 X53.6 Y59.927 R3.493 F286.
N505 G1 G40 X53.45 Y60.501 F572.
N510 G0 Z10.0
N515 X76.34 Y34.922
N520 Z3.0
N525 G1 Z2.5 F286.
N530 G41 D17 X76.808 Y35.124 F572.
N535 G3 X77.241 Y35.392 R3.492 F286.
N540 G2 X82.825 Y37.2 R9.525 F857.
N545 X92.35 Y27.675 R9.525
N550 X82.825 Y18.15 R9.525
N555 X73.3 Y27.675 R9.525
N560 X77.241 Y35.392 R9.525
N565 X82.825 Y37.2 R9.525
N570 X90.564 Y33.228 R9.525
N575 G3 X90.89 Y32.837 R3.493 F286.
N580 G1 G40 X91.27 Y32.497 F572.
N585 G0 Z10.0
N590 X87.157 Y14.216
N595 Z3.0
N600 G1 Z2.5 F286.
N605 G41 D17 X87.573 Y13.955 F572.
N610 G3 X88.021 Y13.754 R3.493 F286.
N615 G2 X92.85 Y6.85 R7.35 F857.
N620 G1 Y2.5 F572.
N625 G2 X85.5 Y4.85 R7.35 F857.
N630 G1 X74.8 F572.
N635 G2 X67.45 Y2.5 R7.35 F857.
N640 G1 Y6.85 F572.
N645 G2 X74.8 Y14.2 R7.35 F857.
N650 G1 X85.5 F572.
N655 G2 X92.85 Y6.85 R7.35 F857.
N660 G1 Y3.071 F572.
N665 G3 X92.885 Y2.581 R3.493 F286.
N670 G1 G40 X92.987 Y2.101 F572.
N675 G0 Z10.0
( END OF PROGRAM )
N685 M101
N690 M30
%
 TomKerekes
 Posts: 270
 Joined: Mon Dec 04, 2017 1:49 am
Re: Fanuc Radius Compensation
Hi a_j_p,
It isn't clear to me what you are trying to do. Are you trying to cut pockets or leave material standing up.
Here is a plot of the GCode with no compensation which should show how the material should look after the Job runs.
Also shown is a tool with diameter 12.72mm.
If you are trying to cut pockets the tool is too big to fit in radius.
If you are trying to leave standing material the tool will gouge the adjacent material.
What are you trying to do?
It isn't clear to me what you are trying to do. Are you trying to cut pockets or leave material standing up.
Here is a plot of the GCode with no compensation which should show how the material should look after the Job runs.
Also shown is a tool with diameter 12.72mm.
If you are trying to cut pockets the tool is too big to fit in radius.
If you are trying to leave standing material the tool will gouge the adjacent material.
What are you trying to do?
You do not have the required permissions to view the files attached to this post.
Regards,
Tom Kerekes
Dynomotion, Inc.
Tom Kerekes
Dynomotion, Inc.

 Posts: 8
 Joined: Sun Aug 26, 2018 10:13 pm
Re: Fanuc Radius Compensation
I am trying to cut bosses, the first image attached called 'boss outline and setup' should hopefully explain. The second picture called 'centerline' is a centerline simulation in the software I use (FeatureCAM) showing the finish pass (same as the G Code I posted earlier) but it also includes a wireframe outline of the tool, which does not gouge any adjacent material...
I have not used cutter compensation before now, I have not had the need to do so until recently, so it very well could be something I am doing wrong but I have been trying to figure it out for a while now without much success. It is pretty difficult however to get the FeatureCAM guys to support when the machine is not something that has a manufacturer's manual they can follow along to make post processor adjustments. The post I have from them is based on a Fanuc system with only small changes to add custom M Codes that I can have KMotionCNC execute specific items with.
If it helps at all, below is the same file's G Code post with cutter compensation turned off in FeatureCAM. I have used this file to run a part and it works just fine, just without the cutter comp...
Again I appreciate the help! Let me know if there is anything more I can provide, etc.
Andrew
( FINISH BOSS BOSS1 )
(***START TOOL DIAMETER = 12.7mm***)
(***START TOOL = 1/2"x1.25"  Square, 3F  Carbide***)
()
N60 G21 G17 G90
N65 T17 M6
N70 G54 G90 G43 H17
N75 G0 X21.75 Y4.675 S2500 M3
N80 Z10.0 F286.
N85 Z3.0
N90 G1 Z2.5
N95 X21.6 Y4.101 F572.
N100 G3 X21.55 Y3.51 R3.492 F286.
N105 G1 Y2.5 F572.
N110 G2 X14.2 Y4.85 R7.35 F857.
N115 G1 X3.5 F572.
N120 G2 X3.85 Y2.5 R7.35 F857.
N125 G1 Y6.85 F572.
N130 G2 X3.5 Y14.2 R7.35 F857.
N135 G1 X14.2 F572.
N140 G2 X21.55 Y6.85 R7.35 F857.
N145 G1 Y2.5 F572.
N150 G2 X14.2 Y4.85 R7.35 F857.
N155 G1 X11.781 F572.
N160 G3 X11.19 Y4.9 R3.493 F286.
N165 G1 X10.616 Y5.05 F572.
N170 G0 Z10.0
N175 X26.201 Y10.535
N180 Z3.0
N185 G1 Z2.5 F286.
N190 X25.901 Y11.047 F572.
N195 G3 X25.519 Y11.501 R3.492 F286.
N200 G1 X21.272 Y15.748 F572.
N205 G2 X19.119 Y20.945 R7.35 F857.
N210 X21.272 Y26.143 R7.35
N215 G1 X39.303 Y44.174 F572.
N220 G2 X44.5 Y46.327 R7.35 F857.
N225 X49.697 Y44.174 R7.35
N230 G1 X67.728 Y26.143 F572.
N235 G2 X69.881 Y20.945 R7.35 F857.
N240 X67.728 Y15.748 R7.35
N245 G1 X49.697 Y2.283 F572.
N250 G2 X44.5 Y4.436 R7.35 F857.
N255 X39.303 Y2.283 R7.35
N260 G1 X21.984 Y15.036 F572.
N265 G3 X21.53 Y15.418 R3.492 F286.
N270 G1 X21.018 Y15.718 F572.
N275 X13.749 Y21.574
N280 G3 X12.935 Y20.965 R3.492 F286.
N285 G2 X6.175 Y18.15 R9.525 F857.
N290 X3.35 Y27.675 R9.525
N295 X6.175 Y37.2 R9.525
N300 X15.7 Y27.675 R9.525
N305 X12.935 Y20.965 R9.525
N310 X6.175 Y18.15 R9.525
N315 X0.562 Y20.942 R9.525
N320 G3 X0.948 Y21.275 R3.493 F286.
N325 G1 X1.377 Y21.548 F572.
N330 G0 Z10.0
N335 X1.425 Y41.027
N340 Z3.0
N345 G1 Z2.5 F286.
N350 X0.99 Y41.255 F572.
N355 G3 X0.527 Y41.42 R3.493 F286.
N360 G2 X4.85 Y48.5 R7.35 F857.
N365 G1 Y74.0 F572.
N370 G2 X2.5 Y81.35 R7.35 F857.
N375 G1 X28.0 F572.
N380 G2 X35.35 Y74.0 R7.35 F857.
N385 G1 Y48.5 F572.
N390 G2 X28.0 Y41.15 R7.35 F857.
N395 G1 X2.5 F572.
N400 G2 X4.85 Y48.5 R7.35 F857.
N405 G1 Y52.201 F572.
N410 G3 X4.885 Y52.691 R3.493 F286.
N415 G1 X4.987 Y53.171 F572.
N420 G0 Z10.0
N425 X53.45
N430 Z3.0
N435 G1 Z2.5 F286.
N440 X53.6 Y53.745 F572.
N445 G3 X53.65 Y54.336 R3.492 F286.
N450 G1 Y74.0 F572.
N455 G2 X61.0 Y81.35 R7.35 F857.
N460 G1 X86.5 F572.
N465 G2 X93.85 Y74.0 R7.35 F857.
N470 G1 Y48.5 F572.
N475 G2 X86.5 Y41.15 R7.35 F857.
N480 G1 X61.0 F572.
N485 G2 X53.65 Y48.5 R7.35 F857.
N490 G1 Y59.336 F572.
N495 G3 X53.6 Y59.927 R3.493 F286.
N500 G1 X53.45 Y60.501 F572.
N505 G0 Z10.0
N510 X76.34 Y34.922
N515 Z3.0
N520 G1 Z2.5 F286.
N525 X76.808 Y35.124 F572.
N530 G3 X77.241 Y35.392 R3.492 F286.
N535 G2 X82.825 Y37.2 R9.525 F857.
N540 X92.35 Y27.675 R9.525
N545 X82.825 Y18.15 R9.525
N550 X73.3 Y27.675 R9.525
N555 X77.241 Y35.392 R9.525
N560 X82.825 Y37.2 R9.525
N565 X90.564 Y33.228 R9.525
N570 G3 X90.89 Y32.837 R3.493 F286.
N575 G1 X91.27 Y32.497 F572.
N580 G0 Z10.0
N585 X87.157 Y14.216
N590 Z3.0
N595 G1 Z2.5 F286.
N600 X87.573 Y13.955 F572.
N605 G3 X88.021 Y13.754 R3.493 F286.
N610 G2 X92.85 Y6.85 R7.35 F857.
N615 G1 Y2.5 F572.
N620 G2 X85.5 Y4.85 R7.35 F857.
N625 G1 X74.8 F572.
N630 G2 X67.45 Y2.5 R7.35 F857.
N635 G1 Y6.85 F572.
N640 G2 X74.8 Y14.2 R7.35 F857.
N645 G1 X85.5 F572.
N650 G2 X92.85 Y6.85 R7.35 F857.
N655 G1 Y3.071 F572.
N660 G3 X92.885 Y2.581 R3.493 F286.
N665 G1 X92.987 Y2.101 F572.
N670 G0 Z10.0
( END OF PROGRAM )
N680 M101
N685 M30
I have not used cutter compensation before now, I have not had the need to do so until recently, so it very well could be something I am doing wrong but I have been trying to figure it out for a while now without much success. It is pretty difficult however to get the FeatureCAM guys to support when the machine is not something that has a manufacturer's manual they can follow along to make post processor adjustments. The post I have from them is based on a Fanuc system with only small changes to add custom M Codes that I can have KMotionCNC execute specific items with.
If it helps at all, below is the same file's G Code post with cutter compensation turned off in FeatureCAM. I have used this file to run a part and it works just fine, just without the cutter comp...
Again I appreciate the help! Let me know if there is anything more I can provide, etc.
Andrew
( FINISH BOSS BOSS1 )
(***START TOOL DIAMETER = 12.7mm***)
(***START TOOL = 1/2"x1.25"  Square, 3F  Carbide***)
()
N60 G21 G17 G90
N65 T17 M6
N70 G54 G90 G43 H17
N75 G0 X21.75 Y4.675 S2500 M3
N80 Z10.0 F286.
N85 Z3.0
N90 G1 Z2.5
N95 X21.6 Y4.101 F572.
N100 G3 X21.55 Y3.51 R3.492 F286.
N105 G1 Y2.5 F572.
N110 G2 X14.2 Y4.85 R7.35 F857.
N115 G1 X3.5 F572.
N120 G2 X3.85 Y2.5 R7.35 F857.
N125 G1 Y6.85 F572.
N130 G2 X3.5 Y14.2 R7.35 F857.
N135 G1 X14.2 F572.
N140 G2 X21.55 Y6.85 R7.35 F857.
N145 G1 Y2.5 F572.
N150 G2 X14.2 Y4.85 R7.35 F857.
N155 G1 X11.781 F572.
N160 G3 X11.19 Y4.9 R3.493 F286.
N165 G1 X10.616 Y5.05 F572.
N170 G0 Z10.0
N175 X26.201 Y10.535
N180 Z3.0
N185 G1 Z2.5 F286.
N190 X25.901 Y11.047 F572.
N195 G3 X25.519 Y11.501 R3.492 F286.
N200 G1 X21.272 Y15.748 F572.
N205 G2 X19.119 Y20.945 R7.35 F857.
N210 X21.272 Y26.143 R7.35
N215 G1 X39.303 Y44.174 F572.
N220 G2 X44.5 Y46.327 R7.35 F857.
N225 X49.697 Y44.174 R7.35
N230 G1 X67.728 Y26.143 F572.
N235 G2 X69.881 Y20.945 R7.35 F857.
N240 X67.728 Y15.748 R7.35
N245 G1 X49.697 Y2.283 F572.
N250 G2 X44.5 Y4.436 R7.35 F857.
N255 X39.303 Y2.283 R7.35
N260 G1 X21.984 Y15.036 F572.
N265 G3 X21.53 Y15.418 R3.492 F286.
N270 G1 X21.018 Y15.718 F572.
N275 X13.749 Y21.574
N280 G3 X12.935 Y20.965 R3.492 F286.
N285 G2 X6.175 Y18.15 R9.525 F857.
N290 X3.35 Y27.675 R9.525
N295 X6.175 Y37.2 R9.525
N300 X15.7 Y27.675 R9.525
N305 X12.935 Y20.965 R9.525
N310 X6.175 Y18.15 R9.525
N315 X0.562 Y20.942 R9.525
N320 G3 X0.948 Y21.275 R3.493 F286.
N325 G1 X1.377 Y21.548 F572.
N330 G0 Z10.0
N335 X1.425 Y41.027
N340 Z3.0
N345 G1 Z2.5 F286.
N350 X0.99 Y41.255 F572.
N355 G3 X0.527 Y41.42 R3.493 F286.
N360 G2 X4.85 Y48.5 R7.35 F857.
N365 G1 Y74.0 F572.
N370 G2 X2.5 Y81.35 R7.35 F857.
N375 G1 X28.0 F572.
N380 G2 X35.35 Y74.0 R7.35 F857.
N385 G1 Y48.5 F572.
N390 G2 X28.0 Y41.15 R7.35 F857.
N395 G1 X2.5 F572.
N400 G2 X4.85 Y48.5 R7.35 F857.
N405 G1 Y52.201 F572.
N410 G3 X4.885 Y52.691 R3.493 F286.
N415 G1 X4.987 Y53.171 F572.
N420 G0 Z10.0
N425 X53.45
N430 Z3.0
N435 G1 Z2.5 F286.
N440 X53.6 Y53.745 F572.
N445 G3 X53.65 Y54.336 R3.492 F286.
N450 G1 Y74.0 F572.
N455 G2 X61.0 Y81.35 R7.35 F857.
N460 G1 X86.5 F572.
N465 G2 X93.85 Y74.0 R7.35 F857.
N470 G1 Y48.5 F572.
N475 G2 X86.5 Y41.15 R7.35 F857.
N480 G1 X61.0 F572.
N485 G2 X53.65 Y48.5 R7.35 F857.
N490 G1 Y59.336 F572.
N495 G3 X53.6 Y59.927 R3.493 F286.
N500 G1 X53.45 Y60.501 F572.
N505 G0 Z10.0
N510 X76.34 Y34.922
N515 Z3.0
N520 G1 Z2.5 F286.
N525 X76.808 Y35.124 F572.
N530 G3 X77.241 Y35.392 R3.492 F286.
N535 G2 X82.825 Y37.2 R9.525 F857.
N540 X92.35 Y27.675 R9.525
N545 X82.825 Y18.15 R9.525
N550 X73.3 Y27.675 R9.525
N555 X77.241 Y35.392 R9.525
N560 X82.825 Y37.2 R9.525
N565 X90.564 Y33.228 R9.525
N570 G3 X90.89 Y32.837 R3.493 F286.
N575 G1 X91.27 Y32.497 F572.
N580 G0 Z10.0
N585 X87.157 Y14.216
N590 Z3.0
N595 G1 Z2.5 F286.
N600 X87.573 Y13.955 F572.
N605 G3 X88.021 Y13.754 R3.493 F286.
N610 G2 X92.85 Y6.85 R7.35 F857.
N615 G1 Y2.5 F572.
N620 G2 X85.5 Y4.85 R7.35 F857.
N625 G1 X74.8 F572.
N630 G2 X67.45 Y2.5 R7.35 F857.
N635 G1 Y6.85 F572.
N640 G2 X74.8 Y14.2 R7.35 F857.
N645 G1 X85.5 F572.
N650 G2 X92.85 Y6.85 R7.35 F857.
N655 G1 Y3.071 F572.
N660 G3 X92.885 Y2.581 R3.493 F286.
N665 G1 X92.987 Y2.101 F572.
N670 G0 Z10.0
( END OF PROGRAM )
N680 M101
N685 M30
You do not have the required permissions to view the files attached to this post.
 TomKerekes
 Posts: 270
 Joined: Mon Dec 04, 2017 1:49 am
Re: Fanuc Radius Compensation
Hi a_j_p,
Thanks for the information.
It seems the specified paths in your GCode in both cases (with and without compensation) is exactly the same.
Maybe the confusion is that there are basically 2 approaches to Tool Diameter Compensation.
#1  is where the GCode specifies the final result without any compensation at all. In this case the Tool Table entry contains the true Tool Diameter of the tool and the GCode Interpreter does all the compensation.
#2  is where the CAM software does all the compensation and specifies in the GCode the tool path based on a theoretical tool diameter. In this case the Tool Table entry contains a small +/ difference between the actual tool diameter and the theoretical tool diameter used by the CAM. The GCode Interpreter then makes only a small adjustment to the tool path to compensate.
Do you understand the difference? Which approach are you intending to use?
Thanks for the information.
It seems the specified paths in your GCode in both cases (with and without compensation) is exactly the same.
Maybe the confusion is that there are basically 2 approaches to Tool Diameter Compensation.
#1  is where the GCode specifies the final result without any compensation at all. In this case the Tool Table entry contains the true Tool Diameter of the tool and the GCode Interpreter does all the compensation.
#2  is where the CAM software does all the compensation and specifies in the GCode the tool path based on a theoretical tool diameter. In this case the Tool Table entry contains a small +/ difference between the actual tool diameter and the theoretical tool diameter used by the CAM. The GCode Interpreter then makes only a small adjustment to the tool path to compensate.
Do you understand the difference? Which approach are you intending to use?
Regards,
Tom Kerekes
Dynomotion, Inc.
Tom Kerekes
Dynomotion, Inc.

 Posts: 8
 Joined: Sun Aug 26, 2018 10:13 pm
Re: Fanuc Radius Compensation
Hey Tom,
I was planning (at least in my head it seemed the easiest) to have the CAM software setup with the theoretical/nominal tool diameter and specify the end result. The Tool Table would contain the actual tool diameter and the GCode interpreter would offset itself half the distance of the diameter in the tool table to yield that end result.
If I understand what you have written correctly, I believe this would be your option #1.
Is that not what I am doing?
Again, thanks for the help!
I was planning (at least in my head it seemed the easiest) to have the CAM software setup with the theoretical/nominal tool diameter and specify the end result. The Tool Table would contain the actual tool diameter and the GCode interpreter would offset itself half the distance of the diameter in the tool table to yield that end result.
If I understand what you have written correctly, I believe this would be your option #1.
Is that not what I am doing?
Again, thanks for the help!