I’m a little worried that I can’t use my own CAM with the Nomad, despite the advertisement of “If you have a favorite CAM program and work flow The Nomad 883 will work with it. Carbide Motion can read gcode from any CAM program so you’ll never be locked into proprietary software.”
Specifically, has anyone generated g-code for the Nomad 883 from Fusion 360’s CAM workspace?
Shooting in the dark, I’ve tried mach3, grbl, Generic EMC, and haas. None have worked. I receive “Error in line 3: Unsupported G Code.”
Ed Ford mentioned in another post that the Mach3 and LinuxCNC post processors are similar to the Nomad, because they are both based on the NIST RS274/NGC standard.
Unfortunately, I read at CNCzone.com that implementers 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, may not work with Nomad, also based on NIST RS274G, because the extensions are different.
Any corrections to this information? Suggestions? Solutions?
Carbide Motion does not like the following excerpted lines of Mach3 g code generated by Fusion 360 CAM:
G90G94G91.1G40G49G17
M9
G43Z0.25H1
G53
However, when I alter the code to reflect the following, Carbide Motion accepted the g code:
G90G94G91.1G40G49G17 > G90G17
M9 > DELETED
G43Z0.25H1 > DELETED
G53 > DELETED
Unfortunately, when I ran the program, the cutter zoomed off to the left and cut into the tool measuring probe, leaving a nasty scar.
Let this be a warning to anyone considering messing with g code. Though, perhaps the code was not the issue. It should be noted that I’m unsure if the work coordinate system was set up correctly—the machine may have been attempting to go to a zero point I said to be somewhere off to the far left of the probe.
I’ve made the changes to Carbide Motion to take your gcode except for the G28 command. I believe the post process section of Fusion should have a “Use G28” option that can be unselected. If not, I can add it at a later point but it was just a little more code than I wanted to add right now.
If the rest of the testing is good, I’ll post a beta of Carbide Motion 2 on Monday.
What post processor did you use in Fusion to generate that code?
I had unchecked both of those, but still getting problems because of the dropped I/J variables—when the value is zero it seems the post-processor doesn’t write it.
Also, I discovered that I can’t use lead-in/lead-out moves, and that’s what the whole G17/G18/G19 thing was about. If I get rid of the lead-ins and helical ramping, etc. it will take the file, however at the end of the program I get a G53 still, so I had to delete that out, then Carbide would take it.
About to try my tool paths from HSMxpress to see how they go. I’m concerned about the tool-change working correctly b/c of the tool-length sensor/tool-length definitions potentially conflicting.
Well, that was disappointing. It successfully went through the first tool and completed a facing operation, paused, and then came up for tool-change when I clicked resume. Once I changed the tool out it homed, checked tool length then went out over the center, fired up the spindle and started plunging, not in the right location at all, on any axis, and crashed into the spoil-board. Here’s the NC file prepped with the Mach3 settings for you to look at.
Here’s what the tool paths look like in HSMxpress:
And here’s what’s gone on in the machine:
So I’m not sure why it’s off… and not just on the Z axis.
If you’re using HSMworks internally, how are you editing your files to get them to run on the Nomad, if you’re doing that?
I tried outputting just the tool path shown above as it’s own post instead of outputting the whole job (the facing part first), and it complained about an undefined feed, so that’s another example of the post sending an implicitly passed value, and Carbide wanting an explicitly defined value. Also something to put in the hopper with the handling of implied/missing I & J values.
If you guys can get Carbide to handle helical and other lead-in/out moves, that’ll be fantastic.
So would you consider the Nomad 883 compatible with fusion 360 after that release?
I am just curious because I mainly use the fusion 360 SW and am looking to purchase a Nomad 883 (well pre-order), but compatibility with fusion 360 is important to me.
I noticed that Autodesk has many CAM partners, cam.autodesk.com
Does Carbide3D have any intentions of becoming a partner and ensuring software compatibility with the nomad 883 hardware?
