Skip to main content
1
1badc203-Newcomer
3-Newcomer
June 16, 2023
Question

Where to set Absolute or Incremental for milling programs

  • June 16, 2023
  • 2 replies
  • 3374 views

I am trying to make a couple basic profile milling toolpaths and when posting out the program a G90 or G91 does not show up in the NC code. Initially I thought it was a problem with a setting in the gpost editor but after adding a bit of code I found on this message board into the FIL file it still does not show up. Looking at the .ncl file the command "SET / OFSETL, 90" is not found in the file. Is there a specific place in the mill, operation or toolpath setting where absolute of incremental programming can be set?

 

On another note I would like to be able to insert a G187 P1 into some of my programs, this if for HSM on a HAAS control. I found in the gpost GUI where I can add bits of code before or after a tool change which would almost work. The kicker is I would like to be able to add a number 1, 2 or 3 somewhere in the toolpath parameters that could be written into the P1 portion of the G code (1 is for rouging and 3 is for finishing). I'm assuming there is a way to do this using the FIL feature. Would anyone know of a clever way to do this?   

2 replies

K
KenFarley21-Topaz II
21-Topaz II
June 16, 2023

To the best of my knowledge, SET/OFSETL is only used to set the offset register. It's not a generic "I want this G-code output" command. It's only output from the parameters set for it in the NC sequence. To get a G90 into the post-processed G-code I have it printed by the FIL code when I see a "MACHIN /" command.

I don't know how you'll implement the G187 stuff you want. Perhaps someone has the same machine as you and has handled this kind of thing, or you could try contacting Austin NC to see if they could help you...

1
1badc203-NewcomerAuthor
3-Newcomer
June 16, 2023

Thank you for the response. I'm very unfamiliar with with the FIL coding language, is there a manual available that states what the different commands do?   

G
GabrielZaha14-Alexandrite
14-Alexandrite
June 16, 2023

GPost and FIL manuals used to be included with Creo under <Creo load point>\CommonFiles\x86e_win64\gpost. Or at least used to be up to Creo 6.

I didn't find the files in Creo 7. Not sure about Creo 8 - 10.

 

J
JonathanCook10-Marble
10-Marble
June 17, 2023

set the parameter LINTOL to 1, 2 or 3

 

in the fill file add 

SET187=0  $$ this is a global variable and can go near the top of the fill file

$$ *******************************************************
$$ * L I N T O L S E C T I O N *
$$ *******************************************************
CIMFIL/ON,LINTOL
TPCDE=POSTF(7,4)  $$ get the lintol value
CASE/TPCDE
WHEN/1 
SET187=1
DMY=POSTF(26,5,5,1) $$TURN OFF CIMFIL/GOTO FIL ROUTINE
WHEN/2
SET187= 2
DMY=POSTF(26,5,5,1) $$TURN OFF CIMFIL/GOTO FIL ROUTINE
WHEN/10 $$ TURN OFF G5 AND G5.1
SET187= 3
DMY=POSTF(26,5,5,1) $$TURN OFF CIMFIL/GOTO FIL ROUTINE
ENDCAS
CIMFIL/OFF

 

$$ ****************************************************
$$ *          GOTO POINT SECTION           *
$$ ****************************************************
CIMFIL/ON,GOTO
DMY = POSTF(20)
 
  CASE/SET187
   WHEN/1                 
  INSERT/'G187 P1'
  SET187=0             $$ RESET SET187 FLAG
   WHEN/2             
  INSERT/'G187 P2'
  SET187=0
   WHEN/3                
  INSERT/'G187 P3'
  SET187=0
   ENDCAS
DMY = POSTF(21)
DMY = POSTF(13)
DMY = POSTF(26,5,5,0)  $$ TURN OFF GOTO SECTION
CIMFIL/OFF  

 

1
1badc203-NewcomerAuthor
3-Newcomer
June 19, 2023

Thank you for the reply, this seems to be more what I was hoping for. One question though, is there a LINTOL parameter in the HSM Roughing tool paths? Also according to the documentation LINTOL specifies the interpolation used post processor for MULTAX sequences. TO be honest I do not know that this means, would someone be able to give a brief explanation?  

Terms & ConditionsCookie settingsAccessibility statement