Multi tool work flow for VCarve -> XCarve. HOW?

Hey all,

Happy to join the community with my purchase of an XCarve. I can tell already in my experimentation with Easel that it will not meet my needs. VCarve however seem to be what I am after.

My trouble is understanding a multi tool process, let’s say a V-Groove engrave cut and a Full shape cut with a different bit (So one tool change for simplicities sake). I have several questions:

  • For those that do multi tool jobs with V-Carve, do you prefer UGS for a sender or Easel? Why?

  • Does the Gcode from VCarve have all information for both tools in a single output of the code? If so does Vcarve’s Gcode include some sort of pause function for the tool change?

  • When I do a tool change what does that process look like? Id imagine I’d need to physically move the spindle which would lead to an X-Y-Z- change. Does the Gcode somehow know where to return? I bought the z axis home plate kit. How does that fit into the process?

  • What is the point of the x y and z limit switches on the machine? Do these act as an estop in the event of a crash, or do they merely assist during some sort of homing routine?

Thanks for the help. Hope to get some of this stuff figured out so I can contribute in the future.


-First, think of the limit switches as “homing” not “limit” switches. You can then repeatedly home your machine to a known machine XYZ Zero location. The machine will throw an error and stop if you try to move past those switches, but if you’re moving at speed, it may still overshoot… There will also be soft limits (based on machine travel) for the opposite points where the machine will error as a “Soft Limit” alarm and stop. (If set correctly, this will happen before your carriage slams into something hard.)
-I personally prefer UGS over Easel as a sender. I use the nightly build (2.x instead of the older 1.9 stable version). The jog controls and command line are right there, as well as a display of machine position coordinates.
-V-Carve will let you do multiple tool paths as you’ve probably already figured out. It will not let you save tool paths that use different bits to the same g-code file.
-My general process for multiple tool cuts is:
– Save tool path for whatever function I want to do first (V-Carve, pockets, details, whatever) with the bit and note the bit in my filename. ex: “Lettering Detail 90V_55IPM” or “Final outline_25_125doc_60IPM”
– Home the machine. Then find my workpiece X,Y,Z Zero location. store it as machine Zero location.
– Send tool path(s) with the first bit. Machine will return to X,Y Zero.
– Change bits with spindle off and machine still ON and running. Motors should hold your coordinates just fine for a tool change.
– Set new Z Zero for Bit #2.
– Return to new XYZ Zero to verify it’s where it should be.
– Run tool path(s) for that bit.

** Should you not feel confident your spindle is in the right X,Y Zero spot after a bit change, rehome your machine. Then move to your stored XY Zero. That’s what the homing switches are for after all.



Thank you for the input!

When you say your work piece zero location I am guessing that would be the same 0,0,0 location that you use in VCarve? How do you “find” this location? Do you know the lower left corner in VCarve is 0,0,0 so you just jog to that and then tell UGS to zero?

You say motors should hold coordinates? So after the cut can I just jog to a good position make my tool change and then when I hit go the first bit of Gcode tells the spindle to return to 0,0,0 before cutting? Or do you jog back to 0,0,0 and just visually verify its correct?

Finally for your last bit I’m not sure I follow. If the machine loses position (let’s say x is now +1" but machine thinks its 0) and I re-home, does it work out that now going back to previously saved 0,0,0 will be correct?

Again, I really appreciate the help. :slight_smile:

Just to be a voice for the Easel webapp; I use it for 100% of the carving I do.
I have played with F-Engrave and used Chilipepper as a g-code sender. But, I don’t consider myself to be an advanced user compared with others on the forums here.

Easel supports multi tool carving. And with a new feature; Workpieces, that allows different carves to be saved as seperate pages within the same project, it’s easy to setup detail cuts and then switch bits and do a cutout.

My two cents.


0,0,0 can be anywhere you choose, but is commonly the lower left corner in VCarve. (Also in Easel by default). I call that workpiece Zero.

The motors should hold. Make sure you have idle current reduction turned off or they won’t. (Search on the forum if you need details on that).
You need to re zero the Z axis after every bit change. Your bits will have different amounts of ‘stick-out’ from the collet.
I use G0 X0 Y0; to return to my XY zero point to make sure it is where I think it’s supposed to be. Then I jog and zero my Z. After setting my Z, I lift up so not to scrape the bit along the material, then return to X0,Y0. Then go to Z0 to see if I did it right.
Rarely do I ever tell my machine to go to 0,0,0 at once. Usually I do XY, then Z.

If you have set your 0,0,0 point then after a homing cycle, you should be able to return to that same point.

UGS also lets you create Macros of commmands, like move to X0 Y0, or z-probe, or go to Z0. The macros become button clicks instead of having to type the command out.

1 Like

This is a good thread to explain Machine Zero & Work Zero and the G28/G30 commands:


Thank you for the input

1 Like

Nice! That was the info I needed. Thanks!