Re: MasterCAM post processor for EMC, anyone?

["Darrell Gehlsen" <darrell-at-machinemaster.com>]

Fred, still waiting for those files.
Darrell

----- Original Message -----
From: "Darrell Gehlsen" <darrell-at-machinemaster.com>
To: "Multiple recipients of list" <emc-at-nist.gov>
Sent: Tuesday, August 01, 2000 9:49 AM
Subject: Re: MasterCAM post processor for EMC, anyone?


>
> Fred,
> Send me the .MC7 and .NCI files that generated the errors and I will make
> the changes.
> Darrell
>
> ----- Original Message -----
> From: "Fred Proctor" <frederick.proctor-at-nist.gov>
> To: "Multiple recipients of list" <emc-at-nist.gov>
> Sent: Tuesday, August 01, 2000 7:39 AM
> Subject: Re: MasterCAM post processor for EMC, anyone?
>
>
> >
> > Darrell and EMC CAD/CAM users,
> >
> > Darrell posted a MasterCAM post processor for the EMC NC dialect. It
> > almost works. Here are my notes:
> >
> > 1. The .pst file caused a handful of complaints when the code part
> > wasn't indented the required 14 spaces. This caused "illegal character"
> > errors that were easy to track down and fix. I don't know if the version
> > of MasterCAM we have (7.2) is pickier than previous versions.
> >
> > 2. The leading and trailing "%" characters are not needed. We should
> > ignore these in our interpreter, but we don't, so for the time being the
> > post shouldn't generate them.
> >
> > 3. The "O0000" ("Oh-zero-zero-zero-zero") subprogram number is not
> > needed and causes an error.
> >
> > 4. G0 can't be used without a move. This was done at the beginning to
> > set the modal G code to G0. We should allow this to just set the mode,
> > but the spec doesn't say this so we don't. It should just be left out
> > and explicitly put in the first move.
> >
> > The offending line was:
> > N102G0G40G49
> >
> > It should be:
> > N102G40G49
> >
> > If something has to go there, put a G80 to cancel any modes.
> >
> > 5. The preparatory moves for tool changing can be replaced with this
> > simpler sequence:
> >
> > G53 G0 Z0
> >
> > which cancels work offsets for that block only (G53), then rapids to
> > spindle home. In the current post, the code generated uses incremental
> > mode (G91) for this, which is unnecessary.
> >
> > The first offending code was this:
> >
> > N106G91G53Z0.
> > N108G53X0.Y0.
> > N110G92X0.Y0.Z0.
> > N112T1M6
> >
> > which should just be
> > N106G53G0Z0.
> > N112T1M6
> >
> > Also, for machines that have manual tool changing, an M0 should be
> > inserted after the tool change to pause motion until the operator
> > resumes at the GUI. A message can be popped up to prompt him. For tool
> > length compensation, the G43 H<tool #> should be used. This would look
> > like this:
> >
> > N106G53G0Z0.
> > N112T1M6
> > (MSG,Load tool 1)
> > N113G43H1
> > N113M0
> >
> > Darrell, can you make these changes? anyone else?
> >
> > Thanks everyone.
> >
> > --Fred
> >
>
>