g98 in lathe drilling cycle

[Rocketmachinist]

How do I remove the g98 in the canned cycle drilling portion on a lathe post.

 

G97 S1000 M03

G0 X0. Z.25

M8

---> G98 G83 Z-1.3533 R.1 Q.3125 F.003

G80

 

Also how do i combine the go G28 U0. and G28 w0. into the same line?

 

The post I am using is Generic Haas SL 4X MT_Lathe.pst

 

Thanks in advance

[EX-wccprogrammer]

Find this:

 

lpeck$		 #Canned peck drill cycle, lathe
 pdrlcommonb
 pcan1, pbld, n$, *sgdrlref, *sgdrillf, pxout, pyout, pfzout, pcout,
 prdrlout, *peck1$, *feed, strcantext, e$
 pcom_movea

 

and delete ' *sgdrlref,' like this:

lpeck$		 #Canned peck drill cycle, lathe
 pdrlcommonb
 pcan1, pbld, n$, *sgdrillf, pxout, pyout, pfzout, pcout,
 prdrlout, *peck1$, *feed, strcantext, e$
 pcom_movea

 

The U0 and W0 calls are on the same line in my copy of this post.

[Rocketmachinist]

^ The previous guy that did all the lathe work around here wanted to see the post look a certain way (he was annoying like that) I want i changed back because it takes too much time for tool changes.

[EX-wccprogrammer]

OK, if you want to put it back, make your post look like this:

ltlchg$		 #Toolchange, lathe
 toolchng = one
 gcode$ = zero
 copy_x = vequ(x$)
 pcc_capture #Capture LCC ends, stop output RLCC
 c_rcc_setup$ #Setup LCC on first 60000
 plcc_lead_begin #Save original in sav_xa and shift copy_x for LCC comp.
 pcom_moveb #Get machine position, set inc. from c1_xh
 c_mmlt$	 #Position multi-tool sub, sets inc. current if G54...
 ptoolcomment
 comment$
 if home_type < two, #Toolchange G50/home/reference position
 [
 sav_xh = vequ(copy_x)
 sav_absinc = absinc$
 absinc$ = zero
 pmap_home #Get home position, xabs
 ps_inc_calc #Set start position, not incremental
 #Toolchange home position
 if home_type = one,
	 pbld, n$, *sgcode, pfxout, pfyout, pfzout, e$
 else,
	 [
	 #Toolchange g50 position
	 pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", e$ # <----------------------
	 toolno = t$ * 100 + zero
	 if home_type = m_one, pbld, n$, *sgcode, *toolno, e$
	 else, pbld, n$, *sg50, pfxout, pfyout, pfzout, e$
	 ]

 

And this:

pl_retract	 #Retract tool based on next tool gcode, lathe (see ptoolend)
 cc_pos$ = zero
 if home_type = one,
 [
 pmap_home #Get home position, xabs
 ps_inc_calc #Set inc.
 pbld, n$, psccomp, e$
 pcan1, pbld, n$, *sgcode, pfxout, pfyout, pfzout, *toolno, e$
 pbld, n$, pnullstop, strcantext, e$
 ]
 else,
 [
 #Retract to reference return
 pbld, n$, `sgcode, psccomp, e$
 if home_type = m_one, pbld, n$, *toolno, e$
 pcan1, pbld, n$, *sg28ref, "U0.", [if y_axis_mch, "V0."], "W0.", # <----------------------
	 pnullstop, strcantext, e$
 if home_type > m_one, pbld, n$, *toolno, e$
 ]

 

If this is for a mill-turn, there are two more areas involved. Let me know if you need that section of code.

[Rocketmachinist]

Mine look exactly the same except for the # at the end of the lines with the arrows

[EX-wccprogrammer]

If you are getting U0. and W0. on separate lines, then it is from some code that your predecessor inserted. This code will output both on the same line, with no line break.

[Rocketmachinist]

Thanks for your help I figured it out. I was modifying the wrong post. My machine def was one thing and the post was MPLmaster_haas