precix post processor

pfiske · Post by **pfiske** » Sat May 02, 2009 10:51 am

The controller for my Precix router does not handle drilling as created. Can I change the post processor so that drilling is simply a set of G0 calls to the location and G1 calls to the depth? or do I have to edit the g-code file manually? Precix seems nearly out of business.

The code that does not work:
G0 Z0.13
X4.134 Y51.367
G20 S4000M3
G83X4.134Y51.367Z-0.854R0.1F80.0Q0.25

Mitch Heynick · Post by **Mitch Heynick** » Sat May 02, 2009 1:53 pm

A friend with a Charly Robot mill has the same problem, they don't support drill cycles. The stock post for a Charly (which works for him) includes the following "substitute" code for a drill cycle using G0/G1:

For Standard drill, in the cycle code box, change the G81 to G0. In the box below that, clear out what's in there and paste in the following:

[SEQ_PRECHAR][SEQNUM][OUTPUT_UNITS_CODE][SPINDLE_BLK]
[SEQ_PRECHAR][SEQNUM] G0 X[NEXT_NONMDL_X] Y[NEXT_NONMDL_Y]
[SEQ_PRECHAR][SEQNUM] Z[CYCL_Z+CLEAR]
[SEQ_PRECHAR][SEQNUM] G1 Z[CYCL_Z-DEPTH] F[CYCL_IPM]
[SEQ_PRECHAR][SEQNUM] G0 Z[CYCL_Z+CLEAR]

You may need to play around with it a bit, but basically it moves to the XY location of the next hole in G0, drops down to the safety distance also in G0, then drills with G1 to the hole depth, and retracts to the safety level with G0.

Peck drilling would be a bit harder to program...

--Mitch

Post by **MecSoft Support** » Sat May 02, 2009 6:57 pm

Yes, Mitch is right. You could look at the CharlyRobotEnglish.spm for the actual code.