Post Processor Editing
I have read on the fourms that some of you edit the post processors. Is there any kind of documention on how to do it? I have not found anything in the help files about it.
Similar Threads:
What CAM software are you using? I use SmartCAM and BobCAD, and for both of those you can download literature from their websites on editing post processors. With BobCAD, they have a pretty extensive .pdf on it.
My suggestion is check with whoever makes your software.
I just upgraded to BoBcad V22
Thanks for the links!
Only bad thing is that I get and error when I try to lunch the MillEditPost.exe
"MillEditPost MFC Application has encountered a problem and needs to close. We are sorry for the inconvenience."
Ouch! I am running WindowsXP at the shop and Vista at home. They both run ok on my OS's. Not sure I can help ya out there
post editor
You need to go to the bobcad website and redownload the millpostedit file. Click here http://s229444871.onlinehome.us/bobc...dsupport/posts
Then read the instructions for downloading and installing the file. This should get you up and running again.
Dave
Thanks for the info. It now works!
Great to hear it!
Ok, I got the post editor to work now I have one small problem with the cose I am generating. The Haas mills allow the use of the M97 subroutines instead of the using the M98 sub program call (M97 will put the subroutine right after the main program in the same file, while M98 creates an entire new program to call). I perfer using the M97 as I like seeing the entire thing in the same program. I changed the subprogram call to M97, but I need to have the prgram of the subrotuine be N1000 (SUBPROGRAM OF O173) instead of the O1000 (SUBPROGRAM OF O173) that it is creating. Is this possible to do?
Below is the program I created...
%
O173 ( PROGRAM NUMBER )
( PROGRAM NAME: B010862.NC)
( POST: HAAS TM)
( DATE: MON. 02/25/2008 , TIME: 09:49AM)
( T1 CENTER DRILL , DIAMETER = .25 , LENGTH = 5.)
( T2 DRILL , DIAMETER = .1875 , LENGTH = 5.)
N10 G20
N20 G00 G90 G17 G49 G80 G99
N30 G91 G28 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(TOOL #1 0.2500 CENTER DRILL)
N40 T1 M06
N50 S1497 M03
N60 G90 G54 X.25 Y-.235
N70 G43 H1 Z.1
N80 M08
N90 G81 G98 X.25 Y-.235 Z-.08 R.07 F5.9893
N100 M97 P1000 ( SUBPROGRAM CALL )
N110 G80
N120 G00 Z.1
N130 M05
N140 M09
N150 G49
N160 G91 G28 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(TOOL #2 0.1875 DRILL)
N170 T2 M06
N180 S3340 M03
N190 G90 G54 X.25 Y-.235
N200 G43 H2 Z.1
N210 M08
N220 G81 G98 X.25 Y-.235 Z-.4683 R.07 F26.7278
N230 M97 P1000 ( SUBPROGRAM CALL )
N240 G80
N250 M09
N260 G00 G91 G28 Z0.
N270 M05
N280 T1 M06
N290 G90 X0. Y0.
N300 M30
%
O1000 (SUBPROGRAM OF O173)
X.5 Z-.08 F5.9893
X.75
X1.
X1.25
M99 ( SUBPROGRAM RETURN )
this is what I need
Below is the program I created...
%
O173 ( PROGRAM NUMBER )
( PROGRAM NAME: B010862.NC)
( POST: HAAS TM)
( DATE: MON. 02/25/2008 , TIME: 09:49AM)
( T1 CENTER DRILL , DIAMETER = .25 , LENGTH = 5.)
( T2 DRILL , DIAMETER = .1875 , LENGTH = 5.)
N10 G20
N20 G00 G90 G17 G49 G80 G99
N30 G91 G28 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(TOOL #1 0.2500 CENTER DRILL)
N40 T1 M06
N50 S1497 M03
N60 G90 G54 X.25 Y-.235
N70 G43 H1 Z.1
N80 M08
N90 G81 G98 X.25 Y-.235 Z-.08 R.07 F5.9893
N100 M97 P1000 ( SUBPROGRAM CALL )
N110 G80
N120 G00 Z.1
N130 M05
N140 M09
N150 G49
N160 G91 G28 Z0.
(JOB 1 HOLE RANDOM POINT PATTERN)
(TOOL #2 0.1875 DRILL)
N170 T2 M06
N180 S3340 M03
N190 G90 G54 X.25 Y-.235
N200 G43 H2 Z.1
N210 M08
N220 G81 G98 X.25 Y-.235 Z-.4683 R.07 F26.7278
N230 M97 P1000 ( SUBPROGRAM CALL )
N240 G80
N250 M09
N260 G00 G91 G28 Z0.
N270 M05
N280 T1 M06
N290 G90 X0. Y0.
N300 M30
N1000 (SUBPROGRAM OF O173)
X.5 Z-.08 F5.9893
X.75
X1.
X1.25
M99 ( SUBPROGRAM RETURN )
%
It also has to put the % sign after the subprogram.
I also have to do some tinkering with some of my programs after they are posted. I find it easiest just to go into the program at the editor and change what I need to change before sending it to the machine.
I am trying to make this out. So there is not really a sub program number but a line number instead? Wierd from what I have seen on other controllers. I see how it works...just never saw that done before.
I am not sure without some toying around in the post how to make this work (if at all). This may also require a special post from Bobcad.
Did you know that you have more options in the post than the post editor program shows you? You can go into the post directory and edit the post using notepad. Then you may see something that could help.
Its in the post
It was simple to find.
Look in the Last tab (Prefixes) on the post editor.
There you see the prefix for Subprograms. Change the O to a N and you should have it.
I like the M97 command better then the M98 becasue it keeps the subprogram in the same file as the main program. It's kind of like the old GOTO commands in basic. when the controller reaches the M97 it skips ahead to the end of the program and finds the subprograms after the M30 of the main program. After it reaches the M99 in the subprogram it goes back and picks up where it left off in the mian program.
I actually got the % sign to go to the end by moving it from the End of Program section to the Program Trailer section. This places it at the end no matter what.
I got the "N" to post as the subprogram prefix by changing the line in the post using notepad.
645. Subprogram prefix? "O"
I change the "O" to "N" and it works fine now. This value didn't show up in the post editor so I had to do it manually in notepad.
If it did not show up in the post editor then it sounds like we have different editors.
Also if you wish to add the text to the sub call you can go to the 'Edit Code blocks' tab of the post editor then select 'Subprograms>Subprogram definitions'
change the line like this.
Code:" " sub_num_with_prefix" (SUBPROGRAM OF O", prog_n,")"
Cool, I see it now. Did not relize that that was what those were for.Originally Posted by tjones
I like this method of subprograms as long as your not using the same subprogram in other main programs. It's much easier to see what your doing and to edit if you have to.
The post editor is Bobcad's little known tool that most people are afraid of using.
What I did was make a copy of my original post and then edit that one (just in case I got it really screwed up. You can not mess up a copy because you can simply delete it.
SUsing the post editor you can also play with the code to determine if you messed up a internal procedure call. The editor changes valid commands to a blue color. If the text is black then it is not a valid command (variable).
Where is the post editor for v20?
Thanks,
Randy
Never mind...I'm new to Bobcad and didn't realize that there was no post configuration file (like the SheetCam and MeshCAM I'm used to) but a whole lot of little menu things to change... [sheesh--newbies]
Randy
I have another question for everyone (I think it's along the same lines as my orginal post so I put it here).
Anyways, one of the things I always did was list the tools needed for the program at the top of the program so the operator can know what to put in what tool slots. Is there a way to make the post processor do this? It already puts it in the line when it is switching from one operation to another.
Reply with Quote
