So, this is interesting. I’m trying my first whack at pushing an STL file through MeshCAM, instead of simply downloading a tutorial NC file. And the project seems to load and run okay in CarbideMotion, except that the spindle never starts turning.
I went back and did the “Face” Tutorial (which I admit, I skipped after doing the Wrench), and the resultant NC file does the same thing. It’s like the G-Code doesn’t have the spindle-on command in it. I dug out my NC file from the Wrench Tutorial, and it works.
So, when I generate GCode from my MeshCAM (v5 b45, 64bit), it doesn’t seem to include the correct command to start the spindle. I’ll also note that my MC doesn’t have the Nomad-specific toolpath generation under the “Tools” menu – only the “Run Script.” Which lead me to a forum exchange where someone suggested that downloading the V6 Beta would resolve that issue. It did, but now when I load that same STL file, nothing gets displayed in model window.
Still, V6 did generate a toolpath for the STL file, and an air test showed that it did spin the spindle, so there’s that. But it leads me to wonder, is there a GCode guide for the Nomad? I assume it adheres mostly to “standard” GCode, but like RS232, that “standard” often isn’t, entirely.
That means start to spindle at 8000 rpm, and at the end
M5
M30
That means stop of spindle and finish the program.
I’ve not run it yet but at least now spins. It’s too late to run it now where I live, I will run it tomorrow. Otherwise I’m downloading the beta version to test how it does the .nc file.
Skyefire, the last V5 MeshCAM release was in November 2013, which predates the Nomad machine. The Carbide3D post which comes with MeshCAM V6 does include the M3 (on) and M5 (off) spindle commands.
; MeshCAM config
; This config is the Carbide 3D Nomad 883
; http://www.carbide3d.com
;
;
DESCRIPTION = “Carbide3D-Inch(*.nc)”
FILE_EXTENSION = “nc”
UNITS=INCH
;Feeds
FORMAT = [F|#|F|1.1]
;Moves
;FORMAT = [I|@|I|1.4]
;FORMAT = [J|@|J|1.4]
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
FORMAT = [R|#|A|1.4]
;
;
COMMENT_START = “(”
COMMENT_END = “)”
;
START = “%”
START = “(FILENAME: [FILENAME])”
;;the following sets the stock for CutViewer
START = “([CUTVIEWERSTOCK])”
START = “G20”
START = “G90”
;
TOOLCHANGE = “([CUTVIEWERTOOL])”
TOOLCHANGE = “M6 [T]”
TOOLCHANGE = “M3 [S]”
;
RAPID_RATE_MOVE = “G0[Y][Z]”
;
FIRST_FEED_RATE_MOVE = “G1[R][Y][Z][F]”
FEED_RATE_MOVE = “[R][Y][Z]”
;
;FIRST_CW_ARC_MOVE = “G2[Y][I][J][F]”
;CW_ARC_MOVE = “G2[Y][I][J]”
;
;FIRST_CCW_ARC_MOVE = “G3[Y][I][J][F]”
;CCW_ARC_MOVE = “G3[Y][I][J]”
;
;
END = “M5”
END = “M30”
END = “(END)”
END = “(OF PROGRAM)”
Quite a few V5 posts did include the spindle commands, so it would depend on which post you chose.
On MeshCAM V5, choose “Mach3-inch” or “Mach3-mm” depending on your units. They have the arcs and the M3/M5 commands and are basically identical to the Carbide posts in V6.
I just received my Nomad this week and spent a good chunk of today wrestling with the same issue.
“Why isnt the Spindle Speed being written in the G Code?”
It is pretty hard to just guess what post processor file type to choose for which machine especially with the practically non existent direction on this subject without searching through a thousand forum threads.
I was choosing the Simple G Code. NC file type thinking that this would be a default but it didnt matter how many times I did it and what I changed it still wasnt writing it.
So, in the end I discovered that I needed to save the file I was using as a MACH 3 Inch.NC file in MeshCam.
After I knew that the Spindle Speed was written into the code every time.
If there is one thing I can say about this package is that it would be really nice to not have to do hours of searching on line for something so simple.
More tutorials on the Carbide 3D site, maybe a small instruction manual, something.more than just having to guess.
Ive run a Thermwood 3 Axis router full time for 5 years and I had a hard time getting this little guy to work.
Totally Unexpected.
