G-Code Output to Nomad 883

[NickMathis]

Does anyone know which Code machine to choose to output to Carbide 3D's machine Nomad 883?

http://carbide3d.com

Shooting in the dark, I've tried mach3, grbl, Generic EMC, and haas.  None have worked.

Mach3 was recommended on the Nomad forum as being similar to the Nomad 883, as it is based on the NIST RS274/NGC standard.

Unfortunately, I read that implementors of the NIST RS274G standard often want their own extensions and those extensions make the code incompatible across other machines.  For example, Mach3, while based on NIST RS274G, will not work with Nomad, also based on NIST RS274G, because the extensions are different.

Any solutions?  Suggestions?

[fonsecr]

I did a quick search but could not find any explicit information. If you got any manual with the machine it might say something about this. But I would assume the EMC or Mach3 posts to be very close to what is required. It would be unusual if it isnt just a minor thing.

However, "not working" can mean anything really. Could be that the machine just needs a different file extension or specific G-code/M-code are no supported. So you would need to look into this more and provide info for us to comment on. Best is the get a G-code/M-code list so we can see what is supported on this machine.

You might get an indication of the line failing if you can start running the program. You could also try to remove codes like G28 (if enabled). G41/G42 are commonly not supported but these would only be output when explicitly enabled in Fusion.

[NickMathis]

Thanks for your quick reply!

Here's what I know:

Carbide 3D's CNC machine, the Nomad 883, is run by their proprietary motion control software called Carbide Motion.   This software prefers g code produced by MeshCam (software also designed by one of the company's founders).

After producing Mach3 g code through Fusion 360's CAM workspace, Carbide Motion gives me an error that reads, "Error line 3: Unsupported G Code."

Attached are the Mach 3 g code produced through Fusion 360's CAM workspace and the g code produced by MeshCam.

[fonsecr]

Yep, that would be this line G90 G94 G91.1 G40 G49 G17 indicating that they only support a subset of mach3.

Replace line 3 with "G90 G17" and see if that is enough to make it run. There could be other G-code that need to be removed or changed, though.

One thing more. You might need to turn off "useG28" in the property list when posting.

We are working with a lot of CNC vendors so I'll ask our team to get in tough with Carbide3D also if they arent already. That way we ensure we have dedicated posts available when it makes sense.

[NickMathis]

I tried your suggestions, but no luck.

Turned off G28 (which, I believe, is Return to Reference Point)

Turned off M6 (which, I believe, is a tool change operation that Nomad is not equipped to do)

Deleted all instances of M9 (which I believe is coolant control, which Nomad is also not equipped to do)

This is all above my head, so I will have to pause for now.

I very much appreciate you checking to see if Fusion 360 is looking into working with Carbide 3D to incorporate a dedicated post process for the Nomad 883.

Thanks for the help!

[hudriwudri]

As far as I know, the Carbide motion controller is just a clone of Arduino + gshield, running the GRBL firmware. You should be able to use the grbl post processor, but you may have to remove the G28 lines (see http://www.shapeoko.com/forum/viewtopic.php?f=10&t=5303#p39062 )

[fonsecr]

---

@hudriwudri wrote:

As far as I know, the Carbide motion controller is just a clone of Arduino + gshield, running the GRBL firmware. You should be able to use the grbl post processor, but you may have to remove the G28 lines (see http://www.shapeoko.com/forum/viewtopic.php?f=10&t=5303#p39062 )

---

You are right. I see this listed in other places too. Please use the included generic GRBL post instead. Their CNC might still use a subset of GRBL so you can still get failures until verified/confirmed.

[NickMathis]

Sounds like we're on the right track.

However, when I post processed my project using F360's Generic Grbl, Carbide Motion gave me the error, "Error in line 4: Unsupported G Code."

Line 4 of this code is:  G90 G94

Does this mean anything to you all?

As per an earlier recommendation, I've gone ahead and asked Carbide 3D for a G-code/M-code list so we can see what is supported by Carbide Motion.

[fonsecr]

---

@NickMathis wrote:

Sounds like we're on the right track.

However, when I post processed my project using F360's Generic Grbl, Carbide Motion gave me the error, "Error in line 4: Unsupported G Code."

Line 4 of this code is:  G90 G94

Does this mean anything to you all?

As per an earlier recommendation, I've gone ahead and asked Carbide 3D for a G-code/M-code list so we can see what is supported by Carbide Motion.

---

Likely G94 is not supported then.

If you get a G-code/M-code list you can attach it here so we can have a look.

[Anonymous]

I also have a Nomad 883, so I have a vested interest in this thread.  I haven't tried Fusion 360 with it yet, only the suppled MeshCAM software.  A list of the supported G-codes is on Carbide 3D's website:

http://www.carbide3d.com/docs/list-of-supported-gcodes/

[fonsecr]

Thanks for the follow up.

Here is an updated post for Carbide 3D that you can try out. Let us know if you find new issues. Thanks.

Test carefully 🙂

René

[gscotti]

I'm using your file, but I'm getting error on line 21: Bad  Arc Format, No I/K, although:

G18 G3 X33.746 Z-0.738 I-0.318

Any suggestion?

[fonsecr]

Try the attached post instead. Now IJK are forced for G2/G3s.

René

[gscotti]

It worked! Thank you.