MultiCam 3000 and Fusion 360 Post Processing

[Anonymous]

We are relatively new to Fusion, but have been using it to create models and specification drawings of our products for small scale manufacturing. 

We are looking to do more prototyping in the shop and have access to a MultiCam 3000 CNC router. We've been attempting to start out with cutting a simple leg profile by using the MultiCAM ISO and HPGL post processors.

Unfortunately, even when changing the file type to a .nc or .cnc after post processing , the router is not recognizing the G-code created from Fusion.

I've attached a STEP file of the leg profile and an image for reference. 

Any help would be greatly appreciated. 

[bob.schultz]

Hello,

In order to assist you in getting the NC file that you require I will need sample output that runs on the machine and the Fusion program you are trying to post.  If you have a programming manual on the controller this would help also.

Thanks.

[Anonymous]

Thank you for your response, appreciate your help! 

I've attached a .anc file for a simple square profile that runs efficiently on the CNC. 

The second attachment is the Leg profile we're attempting to cut. I exported it using the Fusion ISO Multicam processor and added the .nc extension so our machine would recognize the file. 

Still working on the controller manual but will reply when I can locate it. 

[bob.schultz]

Did you try to run the Leg profile on the machine?  If not, do you know why it doesn't run?  It is a small file and could be hand modified to get it to run on the machine.  This would give me a starting point on the modifications required in the post for your machine.  Please furnish the following files/information.

1.  The Fusion 360 part that you are posting against (Folk Leg File.f3d).

2.  Modified Fold Leg File.nc that will run on your machine.

3.  Comments on the changes you made to get Folk Leg File.nc to run on your machine.

4.  How did you generate the .anc file that runs on your machine?

If you can provide all of this information, I don't know if I'll require the controller manual.

[Anonymous]

1.  The Fusion 360 part that you are posting against (Folk Leg File.f3d).

2.  Modified Fold Leg File.nc that will run on your machine.

3.  Comments on the changes you made to get Folk Leg File.nc to run on your machine.

4.  How did you generate the .anc file that runs on your machine?

1. I've attached the Fusion File and the .nc file.

2. As of yet we haven't been able to get a code from Fusion that will actually run but simply adding a '.nc' or '.cnc' file extension to the closed file name allows for the file to at least be recognized by the controller -- it attempts to load the file but the machine does not react to the G-code as written.

3. The only other change I made is changing the T13 tool to a T5 as our 3/8" flat is Tool 5 on our machine.

4. The .anc file was generated by the other company that shares the machine using a program called Cabinet Vision. 

Hope this makes for a clearer picture,

Thanks again for looking into it.

[bob.schultz]

Thanks for providing the information.  I am unavailable to work on it this week, but will hopefully get something to you next week.

[skidsolo]

Here is a Multicam post for a customer in Australia, seems like they have a different version of software but this post is worth a try?

[Anonymous]

Thank you for your reply, 

I've created a new G-Code using the Australian .cps -- I'll do a test run on our machine this week and see how it goes!

[killerjohn64]

Hey @Anonymous, how the test run go with the that postprocessor? I'm having the same problem on my clients machine, where is doesn't recognize the nc file, made for multicam postprocessor

[Anonymous]

Im having an issue with my multicam posts also involving the m12 and m22 codes. these are modal codes that are set for "cut shape" and "not cutting shape" in theory its just a redundancy for g01 and g00 but you have to use an m12 command before every first g01 in a sequence, and a m22 before the g00 at the end of every sequence. As it sits now I have to post, and then manually go back and include the m12 and m22 in the appropriate places or the machine will rapid through the entire program.

[bob.schultz]

Hello @Anonymous,

You can change the behavior of when the M12 and M22 codes are output in the post using the following modifications.

First create a modal to output the M12/M22 codes so they are only output when they are changed.

var gMotionModal = createModal({force:true}, gFormat); // modal group 1 // G0-G3, ...
var mMotionModal = createModal({}, mFormat); // M12/M22 <<< ADD THIS LINE

Now output the codes whenever G0/G1 are output by placing the following lines prior to ALL writeBlock statements that output G0 or G1, for example in the onRapid and onLinear functions (you may have to add the M12 output prior to G2/G3 output in onCircular also).

    writeBlock(mMotionModal.format(22)); // ADD THIS LINE PRIOR TO gMotionModal.format(0) output
    writeBlock(gMotionModal.format(0), x, y, z);
...
...
      writeBlock(mMotionModal.format(12)); // ADD THIS LINE PRIOR TO gMotionModal.format(1) output
      writeBlock(gMotionModal.format(1), x, y, z, f);

Now you will want to remove the existing output of the M12/M22 codes.

  // writeBlock(mFormat.format(12)); // COMMENT OUT THIS LINE IN onOpen
...
  // writeBlock(mFormat.format(22)); // COMMENT OUT THIS LINE IN onSectionEnd

[Anonymous]

thank you so much Bob. this was a huge help. I have been struggling trying to figure out a fix to this issue, other than just manually writing code for these programs. I just slowly realized it was slightly over my head for a permanent fix. This fixed me up immediately. Thank you.