topic CNC GCode for BIESSE ROVER J 1530 in HSM Post Processor Forum

CNC GCode for BIESSE ROVER J 1530

Anonymous — Tue, 07 Jun 2016 00:52:40 GMT

Hello Everyone:

I was suggested here to post a program on this section of the forum to start a discussion about the best post-processor to utilize with a BIESSE ROVER J 1530; So I'm attaching a program file and I've used the "rs274.cps - RS - 274 D" post proccessor, that took me 99% there with the exception of two things that I've found so far:

1 - I have to edit every GCODE to remove instruction G94

ORIGINAL = N10 G90 G94

EDITED = N10 G90

Command G94 is not supported by ROVER

2 - When Patterns are created within the program there is an extra Tool change for the wrong tool.

ORIGINALS = N45 T3 (line 16) & N440 T2 (line 101)

EDITED = (N45 T3) & (N440 T2) (added parenthesis to turn instructions into comments)

Any help with this would be greatly appreciated.

Thanks in advance

Paul Kühne

Re: CNC GCode for BIESSE ROVER J 1530

skidsolo — Tue, 07 Jun 2016 17:33:15 GMT

you can remove the G94 by opening the post in a text editor (preferably notepad ++). Find this code in the RS274.CPS file:

 // absolute coordinates and feed per min
  writeBlock(gAbsIncModal.format(90), gFeedModeModal.format(94));
  writeBlock(gPlaneModal.format(17));

Now edit the code to look like this :

  // absolute coordinates and feed per min
  writeBlock(gAbsIncModal.format(90));
  writeBlock(gPlaneModal.format(17));

You can remove the second tool call that apperas by editing this code:

// user-defined properties
properties = {
  writeMachine: true, // write machine
  writeTools: true, // writes the tools
  preloadTool: true, // preloads next tool on tool change if any
  showSequenceNumbers: true, // show sequence numbers
  sequenceNumberStart: 10, // first sequence number
  sequenceNumberIncrement: 5, // increment for sequence numbers
  optionalStop: true, // optional stop
  separateWordsWithSpace: true // specifies that the words should be separated with a white space
};

Change to this :

// user-defined properties
properties = {
  writeMachine: true, // write machine
  writeTools: true, // writes the tools
  preloadTool: false, // preloads next tool on tool change if any
  showSequenceNumbers: true, // show sequence numbers
  sequenceNumberStart: 10, // first sequence number
  sequenceNumberIncrement: 5, // increment for sequence numbers
  optionalStop: true, // optional stop
  separateWordsWithSpace: true // specifies that the words should be separated with a white space
};

I have also attached the file with the changes.

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Wed, 08 Jun 2016 00:08:57 GMT

Can you help me with where to place this post processor. I too have a Biesse Rover 30 I will soon to start programming for. Too, we bought this machine used and I have no manuals for it, if anyone could point me in the right direction it would be greatly appreciated.

Mike Wilkerson

Re: CNC GCode for BIESSE ROVER J 1530

skidsolo — Wed, 08 Jun 2016 16:32:26 GMT

Can you tell me if you are on a Windows PC or a Mac ?

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Wed, 08 Jun 2016 23:13:57 GMT

It's a windows pc windows xp to be exact

Thanks

Mike Wilkerson

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Thu, 09 Jun 2016 14:48:49 GMT

Thank you very much! Will be trying today and posting the results!

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Thu, 09 Jun 2016 15:22:29 GMT

Works Flawlessly !!! Thanks! I renamed the CPS file and copied to

/Users/paulkuhne/Library/Application Support/Autodesk/webdeploy/production/223f6530b321f48634024235f2f8faffc004221d/Libraries/Applications/CAM360/Data/Posts

Is that the right pace?

Re: CNC GCode for BIESSE ROVER J 1530

skidsolo — Thu, 09 Jun 2016 15:41:08 GMT

I believe that post will be overwritten once the software is updated (which is automatic). Its best to open your A360 account from within Fusion, the move the post into your A360 camposts foler drive. These will appear as your personal posts.

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Wed, 22 Jun 2016 11:09:24 GMT

I finally got the post that was offered here in the correct file and it is working. However, I have the rover 30 S2, will this processor work for this router too???

Thanks

Mike

Re: CNC GCode for BIESSE ROVER J 1530

skidsolo — Wed, 22 Jun 2016 14:12:29 GMT

Sorry I dont know that there are so many different types, the only thing I would say is try a small test program and see if it runs

Re: CNC GCode for BIESSE ROVER J 1530

Anonymous — Wed, 22 Jun 2016 23:23:59 GMT

too, can G-code be used on the Biesse routers? I was under the understanding that biesse machines where parametric programming only. This is my first encounter with Biesse anything, so, I really dont know.

Thanks

Mike

Re: CNC GCode for BIESSE ROVER J 1530

skidsolo — Thu, 23 Jun 2016 13:36:32 GMT

Biesse unfortunately seem to use many code formats, I do know that the Biesse Rover uses G&M code