iso circular interpolation with heidenhain

[jmlwoods]

Is there a toggle in the post or in the configuration def's that will force mastercam to post the full code for each circular move. I am running mc9 with a heidenhain 430 control and the supplyed MPHEID.I post. The code looks like such..

N80G3X-.9889Y.5573I-.9264J.5573
N90G1Y-.8057
N100G3X-.9264Y-.8682J-.8057

in line 100 I need the "I-.9264" to be posted again. The control for some reason won't accept the repeated "I" from the previous line not being there.

I have the post mostly the way I want it and this seems to be my only hitch.

Any suggestions would be appreciated

[Superman]

***COPY your post ***
save the copy in another location, and restore if any problem arises

Putting an "*" in front of a string forces Mcam to output the contained values to the NC-code,
the IJK output also depends on the interpolating plane, G17 uses only I & J etc.

find in your post
parc #Select the arc output
if arcoutput = zero | full_arc_flg | arc_pitch,
[
#Arc output for IJK
i, j, k
replace with
parc #Select the arc output
if arcoutput = zero | full_arc_flg | arc_pitch,
[
#Arc output for IJK
# If you do NOT want to force out the I,J,K values,
# remove the "*" asterisks on the *i, *j, *k 's below...
if plane = zero, *i, *j, k #XY plane code - G17
if plane = one , i, *j, *k #YZ plane code - G19
if plane = two , *i, j, *k #XZ plane code - G18

the part in red was taken from the MPOKUMA.PST

[jmlwoods]

Thankyou very much !! That nailed it on the button.