Help with Mastercam Post for Prototrak

[hall6ppc]

Hello, I need a little help modifying a post proseccor for Mastercam X . My post came from V9 and is leaving out my " Q" value when you post a G83 peck drill cycle. It always post a 0 value no matter what. Any idea what needs to be changed or added? Thanks for your help .

[Superman]

Looked at your PST file

The Q value is being read from "peck2$", the field that this value is read from in the drill cycle operation is "Subsequent peck" NOT the "1st peck" field

[hall6ppc]

Originally Posted by Superman Looked at your PST file The Q value is being read from "peck2$", the field that this value is read from in the drill cycle operation is "Subsequent peck" NOT the "1st peck" field

Thanks can you show me exactly what I need to change ? I am new to Mastercam post Processors and they look like Greek to me .

Thanks for your help !

[Superman]

Make a backup copy your post.

find this in the original

pg83       # Drill cycle for peck drill (G83)
           n$, "G00", *x$, *y$, e$
           n$,  initht$, e$
           n$, "G98", *sgdrill, *refht$, *depth$, *peck2$, *frplunge$, e$
           n$, "G80", e$

pg73       # Drill cycle for peck drill (G83)
           n$, "G00", *x$, *y$, e$
           n$,  initht$, e$
           n$, "G98", *sgdrill, *refht$, *depth$, *peck2$, *frplunge$, e$
           n$, "G80", e$

change to this

pg83       # Drill cycle for peck drill (G83)
           n$, "G00", *x$, *y$, e$
           n$,  initht$, e$
           n$, "G98", *sgdrill, *refht$, *depth$, *peck1$, *frplunge$, e$
           n$, "G80", e$

pg73       # Drill cycle for peck drill (G83)
           n$, "G00", *x$, *y$, e$
           n$,  initht$, e$
           n$, "G98", *sgdrill, *refht$, *depth$, *peck1$, *frplunge$, e$
           n$, "G80", e$

and save it

# means comments
n$ means sequence number is output
* means to force the string and value into the NC code, even if it is already stated previously
"" means the text inside is output to the NC code
e$ means end of line of NC code, start a new line

[hall6ppc]

Thanks for the help!!

[hall6ppc]

Worked Great !!!

Thanks again