Adding empty lines between tool operations

[Jake E.]

Hey guys,
I am working in Baltimore now with a new company, and working on some new projects. One thing i need some help with is modifying the post processor to add empty lines between the end of one tool (M01) and the next tool change (T2M06), as well as putting the tool name above the comments (3/4 ENDMILL). I am using the MCAMX5 Generic Fanuc 3X Mill post.

The other changes I am working on are adding 3 General Information lines from the Setup Sheet done in the Operations Manager.

Below is how I am trying to make it look.

%
O5742(4491157-42)
(NC FILE - C:\DOCUMENTS AND SETTINGS\JAKE_E\MY DOCUMENTS\MY MCAMX5\MILL\NC\4491157-42.NC)
(PROJECT - 18352 )
(DRAWING - 4491157 )
(REVISION - E )
(MATERIAL - PLASTIC - ABS)

(X ORIGIN IS - )
(Y ORIGIN IS - )
(Z ORIGIN IS - )

( T9020 | 4" FACE MILL | H20 )
( T8 | 3/4 FLAT ENDMILL | H8 | D8 | CONTROL COMP | TOOL DIA. - .75 )
( T1 | 1/4 X 90 SPOTDRILL | H1 )
( T2 | NO. 29 DRILL | H2 )
( T3 | NO. 8-32 TAPRH | H3 )
( T4 | 33/64 DRILL | H4 )
( T5 | 1/2-13 STI TAP | H5 )
( T6 | 17/64 DRILL | H6 )
( T7 | 1/4-20 STI TAP | H7 )


N100 G20
N102 G0 G17 G40 G49 G80 G90

( 4" FACE MILL )
( FACE TOP OF PART )
N104 T9020 M6
N106 G0 G90 G54 X-14.45 Y-1.0001 S1000 M3
N108 G43 H20 Z1. T8
N110 /M8
N112 Z.15
N114 G1 Z0. F20.
N116 X2.4 F7.5
N118 G2 Y-3.2499 R1.1249
N120 G1 X-14.45
N122 G0 Z1.
N124 M9
N126 G91 G28 Z0. M5
N128 M01

( 3/4 FLAT ENDMILL )
( CUT LENGTH TO SIZE )
N130 T8 M6
N132 G0 G90 G54 X-12.6 Y-4.71 S1500 M3
N134 G43 H8 Z1. T1
N136 /M8
N138 Z.1
N140 G1 Z-1.5 F20.
N142 G41 D8 Y-5.1 F12.
N144 G3 X-11.85 Y-4.35 R.75
N146 G1 Y-4.25
N148 Y0.
.
.
.
%

Similar Threads:

• Need Help!- Tool library not showing in operations
• Newbie- Tool Path & Operations
• Need Help!- Adding laser lines
• Just IN- Locus CAE … a NEW tool that estimates tolerance consumption for machining operations.
• Bold Tool Path Lettering in MasterCam Operations Manager

[txcncman]

Null input.

[Superman]

You seem comfortable in editing posts, so I won't state the usual "Save a copy" before doing any edits


To place an empty line, you need to find the correct placement in the post & insert
" ", e$ note....put a space between the quotes
or if you want open/close comments only, then insert
"()", e$

for the placement after the M00/M01 output, look for

ptlchg$          #Tool change                                        
      toolchng = one
      if mi1$ = one, #Work coordinate system
        [
        pfbld, n$, *sg28ref, "X0.", "Y0.", e$
        pfbld, n$, sg92, *xh$, *yh$, *zh$, e$
        ]
      if prog_stop = 1, pbld, n$, *sm01, e$
      if prog_stop = 2, pbld, n$, *sm00, e$
      pcom_moveb
      pcheckaxis
      c_mmlt$ #Multiple tool subprogram call
      pcan
      "()", e$  <---- HERE
      ptoolcomment
      pbld, n$, *t$, sm06, e$
      pbld, n$, pstagetool, e$
      "()", e$  <---- HERE
      comment$
      result = newfs(15, feed)  #Reset the output format for 'feed'
      sav_absinc = absinc$

You could try my post in this thread, it is very close... I use () instead of an empty line. It's also got a few "enhancements"

PS it is a 4 axis post, it will not ouput ABC's unless they are defined in the Machine definition file

[Jake E.]

I have the changes made now for the spacing in the program, as well as the tool name before each tool. Now i just need to see if the information from the setup sheet can be linked to the post.

Attached are the two nc files, the post and a screenshot of the Setup Sheet General Information window.

Superman, i appreciate the input. I had gotten those parts figured out before I left work yesterday.

[Jake E.]

The Setup Sheet information is not really feasible so gonna do it by hand.

Now onto the lathe posts, lol....

[Jake E.]

I am now trying to modify a lathe post now.. I have three 2-axis lathes that I am trying to get up and running as well.

Attached are the files I am looking to do.
Any help is appreciated.

[GMkly]

Jake, what did you change to add you tool information to the tool change. I got the space to work but not the tool information after the tool change.