tool radius compensation

This way you can use tooltable and compensate wear, without G41/G42
#5410 is diameter of loaded tool.
Just remembered G64. If there is not something like 'G64 P.005' , it may give unwanted results

I tested this program, but the diameter was huge..
I changed the cutter from 12mm to 10mm, the tool diameter compensation worked..

 

I have another question... does linuxcnc interpret a Macro program?
I use this program on the Fanuc command.
N50T1(RIGHT SIDE RUNNER MILLER DAY 50MM)
N55M6
N60G54S763F450M3
N65T1(NEXT TOOL)
N70G0X109.771Y108.998M8
N75G43G0Z10.D1H1
N80#1=0(INITIAL Z)
N85#2=-119.(FINAL Z)
N90#3=3.4(DEPTH CUT)
N95#4=[#1-#3]
N100G1Z#4
N105WHILE[#4LE#2]DO1
N110G1X98.999Y71.468
N115G2X98.999Y-71.468R122.1
N120G1X110.519Y-97.078
N125G3X110.519Y97.078R147.1F1000
N130G1X109.771Y108.998F450
N135G1X103.088Y104.935
N140G1X82.029Y58.119
N145G1X76.40Y59.3
N150G3X76.4Y31.3R14.
N155G1X62.816Y39.620
N160G1X64.1Y0
N165G1X62.816Y-39.620
N170G1X76.40Y-31.3
N175G3X76.40Y-59.3R14.
N180G1X82.029Y-58.119
N185G1X95.434Y-87.898
N190G1X103.088Y104.935
N195G1X109,771Y108,998
N200#4=#4-#3
N205END1
N210G0Z10.
N220G53G0Z0H0M5

If you try this with 'sem ferramenta' , but #5410 is only usable with loaded tool. I have a few parametric routines built this way and it works.
*
I would change following in the Macro and try:

• G94 is missing (feed per minute)
• N105WHILE[#4LE#2]DO1   to     o105 WHILE[#4 LE #2] 
• N205END1                              to     o105 ENDWHILE
• N220G53G0Z0H0M5           to      N220 G53 G0 Z0 G49 M5
• Normally #1 to #30 are used and overwritten in subroutines, as they are global. I would name numbered parameters outside this range.

Hey, someone in another thread had the same issue the other day

forum.linuxcnc.org/38-general-linuxcnc-q...thout-gouging#264366


question, do you use diameter control with your fanuc controller? generally I use wear compensation with 10% of diameter with lead in arc/length, and never have issues. Im wondering how full diameter control works with the same parameters on fanuc, or if it will give the same issue as linuxcnc

I get the sense that using diameter compensation has fallen out of favor compared to wear compensation, or at least it seems uncommon compared to wear

The machine I work with is a CNC Romi Fanuc command ... I only use tool radius compensation

I'm going to study these macros to use in Linuxcnc...
thank you for your attention
thanks