Re: MasterCAM post processor for EMC, anyone?

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

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
>