Does anyone know where I can get a post processor for MeshCam for the X-carve? I’ve been using the Shapeoko post processor but that doesn’t start or stop the spindle or do a few other little things for the X-Carve
I finally decided to futz a bit with mesh cam to see if I might prefer it for 3d workbefore I pull the trigger on a vcarve pro upgrade to v 8.0 from 7.5.
Vcarve would be a bit less expensive (a plus) and I am more familiar with the user interface of 7.5 .
That being said, I have the trial version of meshcam loaded and have set up a file using thev silhouette of a rose for practice. All well and good. but when saving the g code, what post processor do I use? I tried basic gcode *.nc but the machine raised the bit above the work and started an air carve and was travelling so slow I will be drawing social security before it finishes.
I checked the forums for meshcam and although there was an entry regarding the shapeoko, nothing was found for the XC.
For the Vcarve 8 users, will V.8 let me take a random 2d clipart (say .jpg?) and generate a simple 3d file from it?
Use the Shapeoko-grbl processor.
I looked again, and no shapeoko pp was listed. Hmm, vcarve 8 is starting to look even better. If it works dont fix it?
That’s odd mine have them, anyway here they are. Put them in your Posts folder
Thanks again Brian,
got it into the Posts folder and managed to get a file across. Didn’t come out the way I was expecting but that wasn’t the point. Now I can seriously play with it and decide which way I want to go.
I did notice that at the end of the run (file) the program came to a complete end. Not the usual, “pause/resume” routine to get the “job ended” message when I work in vcarve.
As a workaround, you could create a template, like this one:
G1 Z3.810 F228.6
(rest of G-Code goes here)
G0 X0.000 Y0.000
Which has the “raise bit, turn on spindle” and “turn off spindle and go to 0,0” commands in it and you copy/paste your G-Code into it.
It’s surely possible. By someone more ambitious and skilled than I.
Did you use MM or Inch, I think I change Inch to finish correctly. I don’t scale in mm so never changed it, but will if you’re using it.
I was running in inch since, like you, I dont operate in mm.
open the inch file in a text editor like notebook or something it should look exactly like this.
; MeshCAM config
; This config is the basis for the minimum
; gcode output. If you’re looking for
; the shortest output file then this is the config
; to start with. Also show how to integrate CutViewer config into
; the output.
; 2/29/04 Changed comments to be enclosed by () rather than start with ;
; Added CutViewer config output
; 5/13/04 Added toolchange gcode
; 2/12/05 Changed name and added units
; 3/17/05 Changed stock definition to use CUTVIEWERSTOCK variable
; 5/19/05 Removed feedrate command for rapid moves
; 5/25/05 Added dummy tool for CutViewer
; 6/27/05 Changed the formats to 1.4 to get 4 decimal places of accuracy
; 5/21/14 Changed to Shapeoko, removed %
; 12/5/14 Changed precision and removed Cutviewer info
DESCRIPTION = “Shapeoko GRBL-Inch(*.nc)”
FILE_EXTENSION = “nc”
UNITS = Inch
FORMAT = [F|#|F|1.1]
FORMAT = [X|#|X|1.3]
FORMAT = [Y|#|Y|1.3]
FORMAT = [Z|#|Z|1.3]
;START = “(FILENAME: [FILENAME])”
; The following is a dummy tool to keep CutViewer from generating an error when G20 is called without a tool
;START = “(TOOL/MILL,0.1,0.05,0.000,0)”
START = “G20”
START = “G90”
START = “G1 Z0.15000 F9.0”
START = “M3 S18000”
START = “G1 Z0.15000 F9.0”
;START = “([CUTVIEWERSTOCK])”
;TOOLCHANGE = “([CUTVIEWERTOOL])”
TOOLCHANGE = “M6 [T]”
RAPID_RATE_MOVE = “G0[X][Y][Z]”
FIRST_FEED_RATE_MOVE = “G1[X][Y][Z][F]”
FEED_RATE_MOVE = “[X][Y][Z]”
END = “G1 Z0.15000 F9.0”
END = “M5”
END = “G0 X0.00000 Y0.00000”
END = “(END)”
END = “(OF PROGRAM)”
The end is basically moving it up to a safety level “G1 Z0.15000 F9.0”, Shutting off the spindle if you’re hooked up PWM “M5”, Then returning to your Zero or starting position " G0 X0.00000 Y0.00000"
Works fine on mine, can’t imagine why it would be different on yours.
That’s pretty cool! In case you need to tweak any of those numbers, here’s what they mean:
G90 = absolute distance mode
This tells the machine to work with coordinates instead of increments. So if the machine is at X2 Y2 and you tell it to go to X5 Y5 it will go to 5 units by 5 units from 0,0, not 5 units by 5 units from 2,2.
G1 = “straight feed” (as opposed to a helical feed mode, which grbl doesn’t support)
Z#.### = initial height of the Z axis when starting. If you do a global search and replace for whatever # this is, you can also use it as the safety height.
F#### = Feed rate for the Z move preceding it.
M3 = Start Spindle
- S##### Spindle speed *note that the number is not an actual RPM, it’s a scale where 12k is Max and 1 is Min.
M5 = Stop Spindle
G0 = Rapid move
- X0.000 Y0.000 = origin point of the job, leaving the spindle at the specified safety height.
On Inventible’s Easel software it says to use Shapeoko-grbl for x-carve