[MauserBob]

We just bought an AXYZ gantry router at the turn of the year, and after much headaches and troubleshooting related to a bad board installed, we're up and running.

Ran two separate 1-up programs no sweat, and now we're trying to get a multiple-up program running, but we're having trouble getting the machine to accept the NC code for subroutine call-up. Here is a snippet of the code the machine will not accept and errors on:

...G00Z1.
G00X31.3995Y9.18
M98P5
G00G90X8.8795Y22.91
M98P5
G00G90X31.3995Y22.91
M98P5
X70.(RACK-IN-THE-BACK)
M30



O5
G91
G00Z-.8
G01Z-.22F5.
G01X-.025F13.
G02X.051I31.4J9.18
G02X-.051I31.4J9.18
G02X.0019Y.0098I31.4J9.18
G01X.0231Y-.0096
G01Z.22F500.
G00Z.8
G00X1.9Y-.0002...



The documentation from their site says P specifies sub number, and the subs themselves require an O...all normal stuff, nothing unexpected there. Also says that an "L" is optional for repeats, but I'm not using any. I'm just trying to run a pattern and transform it one time over to the right and then one time up in "Y", producing a 2-x-2 pattern. The machine will verify (in the graphics of the File manager) that the pattern from the main prog runs right but each of the three subs called up produce a ballooned-up pattern of ever-growing circles off the main pattern. I'm not sure how else to program the sub call up; there aren't too many variables to try. Playing phone-tag with them is a no-go today, so does anyone have any experience with AXYZ subroutine execution? We needed a custom post-processor from Cimquest to use Mastercam with this machine and this seems to work fine posting 1-up NC code. Any help at all would be appreciated, and apologies if this is posted in the wrong place.

Rob.

[he1957]

Not sure what errors you are seeing but you have a G91 (Incremental Positioning) so try G90.

Usually, these settings are at the start of a program to pre-set machine operation such as positioning in metric, imperial, disable compensations etc. such the machine starts from a knows set of conditions and parameters.

What did you use to generate the G-code?

[Superman]

looks like your IJ arc centers are set to absolute positioning .... but you have switched to incremental (G91) .... thus making the IJ relative to the arc start point.

see if the machine control parameters can be altered that support an incremental IJ & also modify post processor to match the new settings

[MauserBob]

Thanks for the replies, guys.

We're using Mastercam, running a custom-built post-processor for this machine from Cimquest because they didn't have an off-the-shelf version for AXYZ routers.

The program runs a 4-up, 2 x 2 layout where the first part is the pattern and then the following three are transformed/translated through subprograms (using standard M98/M99 commands ). The way we have always done it here dating back to MasterCam 8 & 9 @ 20 years ago is, the main body is always in G90 absolute mode and the subprograms are always in G91 Incremental. So, what you guys are seeing in my code is indeed what was intended up to a point. I did not intend the subprogram to post those I-value arc-swings in absolute, though...I believe that must be something the post-processor is doing and I never noticed it until reading your replies, so, thanks again! Now I just have to get on the horn to Cimquest...

[Superman]

It is only a simple mastercam setting to output R... that is if the control can use it.

open the MACHINE file, then open the CONTROL file.... go to the Arcs tab and set to signed Radius.... save while backing out
post a file and check.