How to show COMP for CONTOUR, POCKET tricks

[PcRobotic]

Hello everyone,
   I've been crazy with looking for COMPS if using or not especially the pocket, it only show G41 Dxx value nearly at the end of the toolpath.  Colin showed me how to trick out the post and I know you guys wonder how to do it too.

 

#Region Tool change common blocks
ptlchg_com      #Tool change common blocks
         pbld, no_spc$, "G43", [if comp_type = two & tool_typ$ > 9 | CompensationForFinishPasses = 2, spaces$ = 0, "(",*tloffno$,")"], *tlngno$, spaces$ = sav_spc,
         pfzout, next_tool$, [spaces$ = 0, "", spaces$ = sav_spc], scoolant, [spaces$ = 0, " ", pcan1, spaces$ = sav_spc], #Second G43
#endregion
 

#region  ptlchg0$         #Call from NCI null tool change (tool number repeats)
ptlchg0$         #Call from NCI null tool change (tool number repeats)
         pbld, no_spc$, "G43", [if comp_type = two & tool_typ$ > 9 | CompensationForFinishPasses = 2, spaces$ = 0, "(",*tloffno$,")"], *tlngno$, spaces$ = sav_spc, #No Tool Change
         pfzout, next_tool$, scoolant, pcan1, #Third G43
#endregion

 

#region pparameter
pparameter$ # Run parameter table
           if prmcode$ = 15570, CompensationForFinishPasses = rpar(sparameter$, 1)
#endregion

#region Custom Defined Variables
CompensationForFinishPasses: 0


++++++++++++++++++G CODE outputs+++++++++++++++

15( .3750,3/8 FLAT ENDMILL, HSS, USED TOOL,)
(4FLTS 1.500LOC, 2.00LOH)
G0 G17 G40 G49 G80 G90
G91 G28 Z0 M19
G28 Y0
T15 M6(Rough and finish 5x .9925 dia holes, CUT#17)
G90 G54 X-11.4408 Y1.7998 S6500 M3
G43(D15)H15 Z1. T3
M8(DOC= Z-1.3)
Z.0625
G1 Z-1.3 F10.
G41 D15 X-11.1318
G3 X-11.1318 Y1.7998 I-.309
X-11.1567 Y1.9214 R.309
G1 G40 X-11.4408 Y1.7998
G0 Z.125
X-6.5
Z.0625
G1 Z-1.3
G41 D15 X-6.191
G3 X-6.191 Y1.7998 I-.309
X-6.2159 Y1.9214 R.309
G1 G40 X-6.5 Y1.7998
G0 Z.125
X0.
Z.0625
G1 Z-1.3
G41 D15 X.309
G3 X.309 Y1.7998 I-.309
X.2841 Y1.9214 R.309
G1 G40 X0. Y1.7998
G0 Z.125
X6.5
Z.0625
G1 Z-1.3
G41 D15 X6.809
G3 X6.809 Y1.7998 I-.309
X6.7841 Y1.9214 R.309
G1 G40 X6.5 Y1.7998
G0 Z.125
X11.4408
Z.0625
G1 Z-1.3
G41 D15 X11.7498
G3 X11.7498 Y1.7998 I-.309
X11.7248 Y1.9214 R.309
G1 G40 X11.4408 Y1.7998
G0 Z1. M9
G91 G28 Z0. M5

[crazy^millman]

Thanks but no I have never really worried about such a thing. I appreciate your efforts so please don't take it I don't, but I post the code and as long as it makes a good part that is all I care about. When it doesn't make a good part then I will figure out why. I fix that issue and move on. Sorry you seem to be running into issues that require so much effort on your part to work it out in the post, but in my years of doing this a lot of what you keep fighting with has never been an issue for myself and all the different people and places I have worked with. Best of luck and thanks for posting that up.

[PcRobotic]

Hi 5th Axis CGI,
   What happened is, my company hired UNSKILLED machinist with cheap labor cost.  Most of the time, they don't see the entire picture of the program, so the only way is to make sure they understand what the programmers want and need.

[crazy^millman]

18 hours ago, PcRobotic said:

Hi 5th Axis CGI,
   What happened is, my company hired UNSKILLED machinist with cheap labor cost.  Most of the time, they don't see the entire picture of the program, so the only way is to make sure they understand what the programmers want and need.

They are not machinist then they are just operators. Where a good setup sheet and tool list help. We have run 2000 operations out of Mastercam on a part without any of the issues you keep seeing. 

[Guest]

I agree with Crazy, those issues are not "software" issues, they are operator issues. You could solve the active H/D by setting that stuff in the tool change cycle at the machine as well so you don't further complicate matters with heavy unnecessary post edits. 

 

JM2CFWIW YMMV

[jlw™]

IMO if you need CC to sneak up on something you need a separate op any way.