Post Processor Issue

[SteveLucas]

This is for all the post processor gurus.

I have a post for a Makino vertical mill where if I just use a tool once it works fine, But if I have more than one operation or If I use the same tool more than once it messes up my cutter comp line so I have to go in and edit it manually. I can't figure out what is causing it so I am looking for some help.

Before I edit

(TOOL NAME : BNEM_C4_1875_010_RLF)
(TOOL_TYPE : BULL MILL)
(CUTTER_DIAM : 0.187500)
G91G28Z0.
G90G49
M250
M01
T12
M06
S7640M03
G01G43X.7Y-1.1504Z.1F300.H12M07
Z-.175

After I edit

(TOOL NAME : BNEM_C4_1875_010_RLF)
(TOOL_TYPE : BULL MILL)
(CUTTER_DIAM : 0.187500)
G91G28Z0.
G90G49
M250
M01
T12
M06
S7640M03
G00X.7Y-1.1504Z.1F300.M07
G43Z.1H12
Z-.175

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[AustinN.C.,Inc.]

Steve,

I don't think this is the post causing the problem. Look in your NCL file,
I think the first move after tool change is at feed and not in RAPID. The
post does not split the output for G01 moves.

Fred Nemecek
Austin N.C., Inc.
512/458-1112 x119



_____

[SteveLucas]

Fred Nemecek found the problem with my post.
" I don't think this is the post causing the problem. Look in your NCL file, I think the first move after tool change is at feed and not in RAPID. The post does not split the output for G01 moves. "
Then I found my site file for that machine had a free feed set to 300 ipm same as the NCL file. Once that was removed everything posted fine
Kudos to Fred N.