Multicam Post Problems for Drag Knife

[terravan4x4]

Hello,
I'm having problems with the G72 and G73 circular moves in the post processor. It appears that the I and J values are posting as though the program is in a G91 (incremental mode). However, the post is calling for a G90 (Absolute mode). I modified the post to use G02 and G03 commands hoping for better results. So far I'm not having much luck. Below is the posted file:

G90
G74
//Part: TEST
//Operation: Knife, 1, T1: Drag knife, 0.1969 inch offset, 0.25 inch Deep
G00 T1 (EDIT TOOL NUMBER) Drag knife, 0.1969 inch offset
G00 Z-0.5
G00 X7.8031 Y4.0
G00 Z0.0039
G02 X8.0 Y4.1969 I0.1969 J0.0 F20.0
G00 Z0.25
G01 Y8.1969
G00 Z0.0039
G03 X7.8031 Y8.0 I0.0 J-0.1969
G00 Z0.25
G01 X3.8031
G00 Z0.0039
G03 X4.0 Y7.8031 I0.1969 J0.0
G00 Z0.25
G01 Y3.8031
G00 Z0.0039
G03 X4.1969 Y4.0 I0.0 J0.1969
G00 Z0.25
G01 X8.1969
G00 Z-0.5
G00 X0.1969 Y0.0
G00 Z0.0039
G03 X0.0 Y0.1969 I-0.1969 J0.0
G00 Z0.25
G01 Y12.1969
G00 Z0.0039
G02 X0.1969 Y12.0 I0.0 J-0.1969
G00 Z0.25
G01 X12.1969
G00 Z0.0039
G02 X12.0 Y11.8031 I-0.1969 J0.0
G00 Z0.25
G01 Y-0.1969
G00 Z0.0039
G02 X11.8031 Y0.0 I0.0 J0.1969
G00 Z0.25
G01 X-0.1969
G00 Z-0.5
M05
M02

I used the same geometry in Mastercam, added corner geometry for the drag knife, and the posted file looks like this:

M90
G90
G75
G00 T1
G00 Z-.25
G00 X7.8031 Y4.
M12
G00 Z-.1
G01 Z.25 F20
G02 X8. Y4.1969 I8. J4.
G01 Y8.1969
G03 X7.8031 Y8. I8. J8.
G01 X3.8031
G03 X4. Y7.8031 I4. J8.
G01 Y3.8031
G03 X4.1969 Y4. I4. J4.
G01 X7.8031
G00 Z-.25
G97 S50
G00 X.1969 Y0.
G00 Z-.1
G01 Z.25
G03 X0. Y.1969 I0. J0.
G01 Y12.1969
G02 X.1969 Y12. I0. J12.
G01 X12.1969
G02 X12. Y11.8031 I12. J12.
G01 Y-.1969
G02 X11.8031 Y0. I12. J0.
G01 X.1969
G00 Z-.25
M22
G00 X0. Y0.
M02

Thanks in advance for your help.

Cheers,
Dave

[Les Newell]

Most machines specify I and J as incremental, even in G90. It looks like your setup is configured to use absolute I and J. Go to Options->machine->post processor and click on the 'edit post' button.

Look for this chunk of code:

Code: Select all

function OnArc()
   if&#40;arcAngle <0&#41; then
      post.Text &#40;" G73"&#41;
   else
      post.Text &#40;" G72"&#41;
   end
   post.NonModalNumber &#40;" X", endX * scale, "0.0###"&#41;
   post.NonModalNumber &#40;" Y", endY * scale, "0.0###"&#41;
   post.ModalNumber &#40;" Z", &#40;endZ + toolOffset&#41; * &#40;-scale&#41;, "0.0###"&#41;
   post.Text &#40;" I"&#41;
   post.Number &#40;&#40;arcCentreX - currentX&#41; * scale, "0.0###"&#41;
   post.Text &#40;" J"&#41;
   post.Number &#40;&#40;arcCentreY - currentY&#41; * scale, "0.0###"&#41;
   post.ModalNumber &#40;" F", feedRate * scale, "0.0###"&#41;
   post.Eol&#40;&#41;
end

Change it to:

Code: Select all

function OnArc()
   if&#40;arcAngle <0&#41; then
      post.Text &#40;" G73"&#41;
   else
      post.Text &#40;" G72"&#41;
   end
   post.NonModalNumber &#40;" X", endX * scale, "0.0###"&#41;
   post.NonModalNumber &#40;" Y", endY * scale, "0.0###"&#41;
   post.ModalNumber &#40;" Z", &#40;endZ + toolOffset&#41; * &#40;-scale&#41;, "0.0###"&#41;
   post.Text &#40;" I"&#41;
   post.Number &#40;&#40;arcCentreX&#41; * scale, "0.0###"&#41;
   post.Text &#40;" J"&#41;
   post.Number &#40;&#40;arcCentreY&#41; * scale, "0.0###"&#41;
   post.ModalNumber &#40;" F", feedRate * scale, "0.0###"&#41;
   post.Eol&#40;&#41;
end

Save the modified post and give it a try.

[terravan4x4]

Hi Les,

Thank you for the prompt reply to my post. This morning I messed around with the Multicam post processor. The string of code you sent me didn't work. It looks like the Multicam does not like G72 and G73 commands. Below you will find what I was able to get to work:

function OnArc()
if(arcAngle <0) then
post.Text (" G03")
else
post.Text (" G02")
end
post.NonModalNumber (" X", endX * scale, "0.0###")
post.NonModalNumber (" Y", endY * scale, "0.0###")
post.ModalNumber (" Z", (endZ + toolOffset) * (-scale), "0.0###")
post.Text (" I")
post.Number ((arcCentreX - currentX) * scale, "0.0###")
post.Text (" J")
post.Number ((arcCentreY - currentY) * scale, "0.0###")
post.ModalNumber (" F", feedRate * scale, "0.0###")
post.Eol()
end

All I did was revert back to your original and changed the G72 and G73 to G02 and G03.

Other changes I made included forcing the tool number to number 1. For some reason the post is ignoring the tool number in Sheetcam. For the immediate, I'll use tool station 1 for the drag knife. If you have a fix I'd love to apply it to the post.

Best regards,

Dave Daum
dave@kingspaddlesports.com