hello,
my mastercam is generating a R instead of I and J...
how can I change it?
thank you.
hello,
my mastercam is generating a R instead of I and J...
how can I change it?
thank you.
What version of mastercam and it is most likely a post setting.
What machine are you posting to?
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Cadcam
Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .
well, this is the last version with maintenance package...
I'm posting it to a old Cincinnati 5 axis quality center with openCNC app.
I know for a fact that this machine is I and J compatible.
I would agree with you must be the post setting,
how to change it?
thanks in advance
I am sorry to say you will most likely have to contact the dealer you got the post from as most dealer lock there 5axis posts.Does your post files contain a extra file with the prefix of .PSB this is the file that locks to your sim.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Cadcam
Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .
Open your post and look for a line similar to this
arcoutput : 0 # 0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
Change to 0 and you are set. Also look for arctype :, and what setting you need. We have an Okuma and a G & L, and they read I,J,K differently. One reads from center of arc, the other from center of arc back to origin. Make sure you save original, or modified post under different names.
Please review picture and caption.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Cadcam
Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .
sound fair, first of all I do have to say thank you guys for the quick help.
I'm starting to understand much better how the post thing system works, although I concluded that the settings are in fact set to generating the R and not the I and J.
I would prefer to figure this out myself than contact the dealer, this way I'll learn more and progress.
Soon and I'll start playing around with the post and see the output.
Hey Guys finally I got some time in here to start changing the post but,
This does not look good, my post does not even have
arcoutput : 0 # 0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
mine has
#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, *iout, *jout, kout #XY plane code - G17
if plane$ = one, iout, *jout, *kout #YZ plane code - G19
if plane$ = two, *iout, jout, *kout #XZ plane code - G18
!i$, !j$, !k$
and
#Arc output for R
if abs(sweep$)<=180 | (plane$ = 0 & arctype$ = five) | (plane$ = 1 & arctypeyz$ = five) |
(plane$ = 2 & arctypexz$ = five), result = nwadrs(srad, arcrad$)
else, result = nwadrs(srminus, arcrad$)
*arcrad$
with the
arctype$ : 2 #CD_VAR Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.,
#5 = R no sign, 6 = R signed neg. over 180
I understood that I have to remove the "*" asterisks on I J and K but this does not happens; I'm still generating the R, any help out there.
Have you gone into the Control Def (from within Mastercam) and changed the arc output type? I had a similar problem with my Haas post not breaking 360 degree arcs into segments (or posting as IJK).
If you open the Control Definition, you'll see an Arc option in there. It lets you choose the type of behavior you want with different types of arcs. I think this determines what Mastercam passes to the Post Processor. Your install is still passing R values so no matter what you do, it won't output IJK.
If you change the output type to IJK, that's what will be handed to the post and it should work.
I'm no expert but that's where I'd look next.
Greg