Can Vcarve files still be cut via Carbide Motion?
(I can get a preview, but getting bounds limit, etc errors)
If so, does anyone have an A-Z method for:
setting up Vectric file , selecting the right PP, and loading it into CM for a Shapeoko Pro 5?
TY
Do you mean “Vcarve” as in the Vectric software product, or “vcarve” meaning the engraving style with a V-bit? I think you mean the former, but just wanted to clarify before opining.
I edited for clarity sorry: a Vectric file. The software is called “Vcarve Pro”.
I dont use vectric but I think you can save your file in vectric as .nc and run that .nc file in Carbide motion
I use Aspire but process is same for Vcarve or Cut2D. User @Allen44 created a series of Post Processors for Vectric and you can find them here. The post where he talks about the differences among the versions is here. I have a spindle and use (I think) version 7g. I read recently on these forums that the metric PP imports best into Carbide Motion, even if your Vectric file is set up in inches. Save from Vectric, Load into CM and it cuts fine.
You know that may be a clue- the error mssg said it was ___ mms out of bounds, even though I sent it in English units…
Will look into thanks!.
This is a warning as noted at:
https://carbide3d.com/blog/carbide-motion-bounds-checking/
Usually it is caused by a mismatch between job setup (presumably Vectric has an equivalent to: Job Setup | Carbide 3D Guides) and how origin is set relative to the stock:
I find that opening the source file up and drawing a box which matches the specified dimensions (draw up the cut in profile if need be) or moving the machine to the origin and then using a tape measure to measure out the dimension(s) in question will make clear where things aren’t lining up.
The bounds checker presumes that you have set your Zero BEFORE loading the toolpath.
It compares the toolpath min/max envelope, the machine envelope, and the current Zero point to determine if the path is completely within the machine envelope.
I’m going to add that I’ve used VCarve Pro with CM with both set to imperial/inches for as long as I’ve had the 5/5.1 without issue. About a year now. VCarve includes a simple “Carbide Motion ATC” PP which will work. The Allen PP’s are much more detailed with status messages.
Expanding on a couple of points above.
The native unit system of CM (and GRBL) is metric. Error messages, logs, certain macros, etc will always be in metric even when the install is set to inches. It can be confusing when troubleshooting, but it isn’t noticed during normal operation.
Bounds error means a file is loaded which is attempting to move to a coordinate outside the machine’s travel limits based on where X, Y, and Z zero are currently set.
For an extreme example of the bounds limit error, if the VCarve job has XY0 set in the SW corner, and zero is accidentally at the machine at the opposite SE corner.
On my 2x4 machine I’ve surfaced full sized 2 x 4 sheets right up to the boundary with XY0 set properly in the job and at the machine.
Am I right in that you posted recently something about using the metric PP for best results, even when the CAD file is in inches? I think you did, but maybe I’m making that up.
Correct.
If a G-code file is set to use millimeters it is less likely to have arc errors than if set to the larger Imperial units.
Very helpful thanks!
So “Carbide Motion ATC” PP is the one that works?
So I just looked at the stock PP’s again I hadn’t I a while.
There were two pairs of PPs included with my VCarve Pro software that will work with CM. One called “Carbide Motion ATC” one called “Shapeoko”. I believe the difference is “Shapeoko” supports arcs directly while “Carbide Motion ATC” converts them to a hundred tiny lines in the gcode. The latter is harder for the controller to process.
I don’t use either of them anymore. Both have limitations with tool changes prompts. It shows only the number not the name. This is one of the things fixed in Allen’s PP.
Try contacting VCarve support and see what they recommend? They’re pretty good about answering within UK working hours
The ATC PP works thanks!(Customer service recommended it)…
Next mystery is why it’s cutting way too high on the test piece…
Usually, that is a disconnect between Job Setup and where the zero is set relative to the stock.
A common way this can happen is if the VCarve job is setup for Z Zero Point Machine Bed, but before starting the file you set Z0 off the top of material. If the material is 1" then all cuts will be 1" too high. Depending on the depth of cut relative to material thickness, it would cause shallow cuts or complete aircutting.