hello,
my mastercam is generating a R instead of I and J...
how can I change it?
thank you.
Printable View
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?
well, this is the last version with maintenance package...Quote:
Originally Posted by cadcam
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.
Quote:
Originally Posted by cadcam
no, does not have any file with the prefix .PSB, only .PST
what I got is the post name.PST
I know I can contact the dealer but theses guys taking forever to do things....
if you or anyone could just post an example on how can I change it , I would
be happy.
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.
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.
Yes I have gone to the Control Definition but, I changed and changed and still the same, first of all in the Control Definition there no IJK output or I can not find it, looks like this post processor is different than others I've seen.Quote:
Originally Posted by Donkey Hotey
Thanks
It's in there. This is what you're looking for:Quote:
Originally Posted by casta-baga
http://cnczone.com/forums/attachment...3&d=1208482740
It's not called IJK. It's called Delta Start to Center, Delta Center to Start or one of those (depending on how your control defines IJK arcs).
This is also how you tell it to handle complete circles like circular pockets and helical plunges (whether to break the arcs or not).
Hi Donkey Hotey
Yesterday before I left work I edited the post processor text and made it work, my problem was, it was generating an R on entry and exit point and the I and J on the circular interpolation.
Can I ask you what setting are you using on XZ plane and YZ plane just to make Sure?
I got another question, I want to change the way it generates the G codes, for example I like to generate a M01 after tool change and after reading the work coordinates etc,
Is this as well post processor settings and where?
Have a good day and thank you.
Sorry, but I'm not at all versed on editing the post processor. I can read it and kinda' see what is going on but that's it.
As for my settings for the circular planes, it's the default. But that doesn't matter. Mine is for a Haas. There is no guarantee yours will handle it the same.
That's why those settings are in there. You need to change them to match whatever your machine wants to see.
cool, works perfect with the machine that I'm trying to figure out.Quote:
Originally Posted by Donkey Hotey