Re: MasterCAM post processor for EMC, anyone?

[Fred Proctor <frederick.proctor-at-nist.gov>]

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