FreeCAD and Nomad 883 CNC machine?

[frankbuss]

I tried creating gcode with FreeCAD, but the proprietary program Carbide Motion for my Nomad 883 CNC machine can't read it. Apparently the machine itself runs GBRL, so I guess this should understand the generated gcode, but Carbide Motion is a very basic program and looks like only reads the output of Carbide Create reliably, again a very basic program.

I don't need Carbide Motion, works in Windows only anyway, and I use Linux as my main system. Is there a program for Linux which can send the gcode to my machine, and which allows to manually and interactively move the drill position?

[chrisb]

Can you upload here the GCode for your machine for such an object:

[frankbuss]

I don't think I can do this in Carbide Create. But here is an example for 2 paths:

test.png (205.89 KiB) Viewed 355 times

Here is the Carbide Create source file and the nc-file (with the gcode) it creates for Carbide Motion:

test.zip

(5.78 KiB) Downloaded 11 times

[chrisb]

The G-code contains only G1 commands, no arcs G2 or G3. This would need a very special post processor which does all the tesselation. I wonder if that's still grbl? Perhaps you can upgrade the firmware of your machine?

[mlampert]

looks like all arcs are discretized, other than that it seems to be straight forward g-code. grbl does process G2 and G3 commands, so this is a bit of a surprise. If there really is a grbl controller at work you should be able to use bCNC. If there is a modified grbl which doesn't support G2 and G3 you might have to write a post processor to discretized them upfront.

Edit: chrisb beat me to it - what he said

[WillAdams]

This object could be drawn in Carbide Create by Boolean unioning a circle and a suitably sized rectangle:

Capture.PNG (168.37 KiB) Viewed 294 times

I would hope that FreeCAD would support making G-Code which Carbide Motion would accept. This post indicates it does: https://forum.shapeoko.com/viewtopic.ph ... 82&p=70299

[dubstar-04]

If the machine is grbl based I'm a bit surprised that the grbl post doesnt work. If required I would be willing to help you make a new post for your machine.

If you gather as much information as possible (supported codes etc) we can work together to make FreeCAD output compatible gcode.

Thanks,

Dan

[chrisb]

I found this page https://mber.dev/rapid-prototyping/cnc- ... 3d-g-codes where G2, G3 are listed.

The following hint may be important: "MeshCam will produce this code only if Enable Arc Fitting is checked. Driver support for the R[radius] arc format is uncertain.".

If it's only the different forms of the circle definitions, then help is not very far, e.g. the philips post processor can create different forms of G2/G3.

[frankbuss]

Looks like it understands the generated gcode, I could mill now my FreeCAD model with bCNC, all in Linux, thanks! There are still some minor problems with the z-coordinate, I want it to be at the top of my stock, but I can adjust this manually in bCNC.

One major problem: FreeCAD generated the command G20, which sets it to inch. So my 5 mm move in the gcode file, which was generated as FreeCAD would think it was mm, was a 5 inch move, which crashed the head into the top limiter. I changed it to G21 in the file, which sets it mm, and now it works.

[chrisb]

Looking at the arguments of grbl post processor by moving the mouse over the "arguments" field, mm should be the default which can be changed to inches. You can try to add G21 to the preamble.