Modifying Mastercam post processor.
I am trying to figure out how to edit the post to add a g94 z.1 after the x,y g94 position move. As it posts now it will move in all 3 axis at the same time and that is not good. Here are the examples the first is all 3 axis in motion at once. The second is after I added the additional g94. Thanks in advance.
( original )
%
O9999(ROUGH THICKNESS)
( T10 | 3" FACE MILL | H10 | D10 | WEAR COMP | TOOL DIA. - 2.25 | XY STOCK TO LEAVE - -.02 | Z STOCK TO LEAVE - 0. )
N1 G90 G54 G64 G50 G17 G40 G80 G49
N2 G20
N3 G54
N4 M8
N5 M998
N6 T10 G43 H10 M6
N7 S4000 M3
N8 G0 G94
N9 X6.7 Y-1.005 Z.1-------current line
N10 G1 Z-.0291 F40.
N11 X-1.7
N12 G0 Z.1
N13 X6.7
N14 G1 Z-.0582
N15 X-1.7
N16 G0 Z.1
N17 X6.7
N18 G1 Z-.0873
N19 X-1.7
N20 G0 Z.1
N21 X6.7
N22 G1 Z-.1164
N23 X-1.7
N24 G0 Z.1
N25 X6.7
N26 G1 Z-.1455
N27 X-1.7
N28 G0 Z.1
N29 X6.7
N30 G1 Z-.1745
N31 X-1.7
N32 G0 Z.1
N33 X6.7
N34 G1 Z-.2036
N35 X-1.7
N36 G0 Z.1
N37 X6.7
N38 G1 Z-.2327
N39 X-1.7
N40 G0 Z.1
N41 X6.7
N42 G1 Z-.2618
N43 X-1.7
N44 G0 Z.1
N45 X6.7
N46 G1 Z-.2909
N47 X-1.7
N48 G0 Z.1
N49 X6.7
N50 G1 Z-.32
N51 X-1.7
N52 G0 Z.1
N53 X6.7
N54 G1 Z-.33
N55 X-1.7
N56 G0 Z.1
N57 M9
N58 M5
N59 M998
N60 M30
%
(edited)
%
O9999(ROUGH THICKNESS)
( T10 | 3" FACE MILL | H10 | D10 | WEAR COMP | TOOL DIA. - 2.25 | XY STOCK TO LEAVE - -.02 | Z STOCK TO LEAVE - 0. )
N1 G90 G54 G64 G50 G17 G40 G80 G49
N2 G20
N3 G54
N4 M8
N5 M998
N6 T10 G43 H10 M6
N7 S4000 M3
N8 G0 G94
N9 X6.7 Y-1.005
N10 G94 Z.1-----edited
N11 G1 Z-.0291 F40.
N12 X-1.7
N13 G0 Z.1
N14 X6.7
N15 G1 Z-.0582
N16 X-1.7
N17 G0 Z.1
N18 X6.7
N19 G1 Z-.0873
N20 X-1.7
N21 G0 Z.1
N22 X6.7
N23 G1 Z-.1164
N24 X-1.7
N25 G0 Z.1
N26 X6.7
N27 G1 Z-.1455
N28 X-1.7
N29 G0 Z.1
N30 X6.7
N31 G1 Z-.1745
N32 X-1.7
N33 G0 Z.1
N34 X6.7
N35 G1 Z-.2036
N36 X-1.7
N37 G0 Z.1
N38 X6.7
N39 G1 Z-.2327
N40 X-1.7
N41 G0 Z.1
N42 X6.7
N43 G1 Z-.2618
N44 X-1.7
N45 G0 Z.1
N46 X6.7
N47 G1 Z-.2909
N48 X-1.7
N49 G0 Z.1
N50 X6.7
N51 G1 Z-.32
N52 X-1.7
N53 G0 Z.1
N54 X6.7
N55 G1 Z-.33
N56 X-1.7
N57 G0 Z.1
N58 M9
N59 M5
N60 M998
N61 M30
%
Re: Modifying Mastercam post processor.
Copy the original post to a different location..... if you stuff up any editing, then copy back overwriting the original
open the original post & search for nobrk$....it should be in the early lines of the post
it should be
Quote:
# --------------------------------------------------------------------------
# Additional General Output Settings
# --------------------------------------------------------------------------
nobrk$ : no$ #Omit breakup of x, y & z rapid moves
no means..... the Z will not appear on the same rapid line as a X &/or a Y
Re: Modifying Mastercam post processor.
Superman here is what the general outputs currently are.no$ was already set. What am I missing?
# General Output Settings
# --------------------------------------------------------------------------
sub_level$ : 1 #CD_VAR Enable automatic subprogram support
breakarcs$ : 2 #CD_VAR Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs
arctype$ : 2 #CD_VAR Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.,
#5 = R no sign, 6 = R signed neg. over 180
do_full_arc$ : 0 #CD_VAR Allow full circle output? 0=no, 1=yes
helix_arc$ : 2 #CD_VAR Support helix arc output, 0=no, 1=all planes, 2=XY plane only
arccheck$ : 1 #CD_VAR Check for small arcs, convert to linear
atol$ : 0.01 #CD_VAR Angularity tolerance for arccheck
ltol$ : 0.002 #CD_VAR Length tolerance for arccheck
vtol$ : 0.0001#System tolerance
maxfeedpm : 500 #SET_BY_MD Limit for feed in inch/min
ltol_m : 0.05 #Length tolerance for arccheck, metric
vtol_m : 0.0025#System tolerance, metric
maxfeedpm_m : 10000 #SET_BY_MD Limit for feed in mm/min
force_wcs : yes$ #Force WCS output at every toolchange?
spaces$ : 1 #CD_VAR Number of spaces to add between fields
omitseq$ : yes$ #CD_VAR Omit sequence numbers?
seqmax$ : 9999 #CD_VAR Max. sequence number
stagetool : 0 #SET_BY_CD 0 = Do not pre-stage tools, 1 = Stage tools
stagetltype : 1 #0 = Do not stage 1st tool
#1 = Stage 1st tool at last tool change
#2 = Stage 1st tool at end of file (peof)
use_gear : 0 #Output gear selection code, 0=no, 1=yes
min_speed : 50 #SET_BY_MD Minimum spindle speed
nobrk$ : no$ #CD_VAR Omit breakup of x, y & z rapid moves
progname$ : 1 #Use uppercase for program name (sprogname)
prog_stop : 1 #Program stop at toolchange: 0=None, 1=M01, 2 = M00
tool_info : 3 #Output tooltable information?
#0 = Off - Do not output any tool comments or toolpable
#1 = Tool comments only
#2 = Tooltable in header - no tool comments at T/C
#3 = Tooltable in header - with tool comments at T/C
tlchg_home : no$ #Zero return X and Y axis prior to tool change?
Quote:
Originally Posted by
Superman
Copy the original post to a different location..... if you stuff up any editing, then copy back overwriting the original
open the original post & search for nobrk$....it should be in the early lines of the post
it should be
no means..... the Z will not appear on the same rapid line as a X &/or a Y
Re: Modifying Mastercam post processor.
I usually try and find the part of the post file that outputs what you want and you can add a line in below or something. Can you upload your post processor file?
1 Attachment(s)
Re: Modifying Mastercam post processor.
Quote:
Originally Posted by
mmurray70
I usually try and find the part of the post file that outputs what you want and you can add a line in below or something. Can you upload your post processor file?
Here is my post from work. I will not go through from work as the firewall blocked it. Also zip and rar are blocked.
Please take a look. AS i told Superman the nobrk$ was already set to no$. I am stumped.
1 Attachment(s)
Re: Modifying Mastercam post processor.
Try this file now. I removed the Z value from line 689 and moved it to another line, hopefully it will post out this way too. Im not an expert, might not work at all but worth a shot. I've managed a few mods like this with mastercam posts before.
This will hopefully post it with Z on the following line, but it will not add another G94 as you dont need it twice anyway. As long as X/Y are on one line and Z on the next it wont move 3 axis at once. It should come out like this:
%
O9999(ROUGH THICKNESS)
( T10 | 3" FACE MILL | H10 | D10 | WEAR COMP | TOOL DIA. - 2.25 | XY STOCK TO LEAVE - -.02 | Z STOCK TO LEAVE - 0. )
N1 G90 G54 G64 G50 G17 G40 G80 G49
N2 G20
N3 G54
N4 M8
N5 M998
N6 T10 G43 H10 M6
N7 S4000 M3
N8 G0 G94
N9 X6.7 Y-1.005
N10 Z.1
N11 G1 Z-.0291 F40.
N12 X-1.7
N13 G0 Z.1
N14 X6.7
N15 G1 Z-.0582
N16 X-1.7
N17 G0 Z.1
Re: Modifying Mastercam post processor.
mmurray it worked for the first tool change but subsequent ones remain the same. Any idea what may not be allowing it to populate all other tool changes?
This will hopefully post it with Z on the following line, but it will not add another G94 as you dont need it twice anyway. As long as X/Y are on one line and Z on the next it wont move 3 axis at once. It should come out like this:
%
O9999(ROUGH THICKNESS)
( T10 | 3" FACE MILL | H10 | D10 | WEAR COMP | TOOL DIA. - 2.25 | XY STOCK TO LEAVE - -.02 | Z STOCK TO LEAVE - 0. )
N1 G90 G54 G64 G50 G17 G40 G80 G49
N2 G20
N3 G54
N4 M8
N5 M998
N6 T10 G43 H10 M6
N7 S4000 M3
N8 G0 G94
N9 X6.7 Y-1.005
N10 Z.1
N11 G1 Z-.0291 F40.
N12 X-1.7
N13 G0 Z.1
N14 X6.7
N15 G1 Z-.0582
N16 X-1.7
N17 G0 Z.1[/QUOTE]
1 Attachment(s)
Re: Modifying Mastercam post processor.
Try this, looks like the same change had to be made in another place too.
I did the mod from my phone this time. If it something doesnt work right ill do it again tomorrow when im on my computer.
Re: Modifying Mastercam post processor.
Thanks a bunch man. I have to drive out to the shop tomorrow and try it I have something I was hoping to do some cutting this weekend. I will let you know how it goes. Thanks again.
Re: Modifying Mastercam post processor.
Everything looks good now. I am using this as a back up from work. I am currently using and learning fusion the part design is (similar) to MC and so is the toolpath creation, just a lot weaker. But it's free and whats not to like about that. If you haven't looked at it is not a bad software package. This mill has a pretty good and easy to learn conversational control. Thanks again.
Re: Modifying Mastercam post processor.
Good to hear it worked out. Glad i could help. Thanks.
2 Attachment(s)
Re: Modifying Mastercam post processor.
Quote:
Originally Posted by
ranchero60
Here is my post from work. I will not go through from work as the firewall blocked it. Also zip and rar are blocked.
Please take a look. AS i told Superman the nobrk$ was already set to no$. I am stumped.
your post doesn't look like the machine code.
Re: Modifying Mastercam post processor.
Hello OkumaHero,
Have you D-disk software for osp5000?
Please hlep me.
My email : [email protected]
Thank you very much
Re: Modifying Mastercam post processor.
That was an old shop, with a dumb boss, with old crap machines.
Why bust your ass for an owner that doesn't even care about his own shop?
There are many shops like that.
