Create 2nd Setup using remaining geometry in RhinoCAM? Or pause?


I’m new to RhinoCAM, and I am using a Laguna Swift CNC router.

The Laguna controller is really built for single-tool operations, but I’ve found workarounds using Fusion360 to pause an operation between tools to do a manual tool change.

However, I can’t find a way to do this in RhinoCAM.

Ideally, I would simply create a 2nd setup using the remaining stock from the roughing operation. If there is a way to do this, I would love to hear it.

Alternatively, if there is a way to add in a manual pause in between operations, that would be great too. That is what I’ve done in Fusion, by editing the Gcode after posting. I tried the same thing with the RhinoCAM Gcode, however, but the machine just skipped right over the pause and dove into my finishing pass using the roughing tool (ACK!).

If anyone has any solutions, I’m all ears.
Thanks so much!

Hi Benjamin -

Just to be sure, for RhinoCAM support, please visit

Thanks Wim!
I forgot you can just email them a support request.
For some reason I find their forum a pain in the neck.
I’ll see what they say.
Thanks again!

1 Like

Hi Benjamin,

To place an M0 (or whatever your particular M code is) for a stop, use the Machine Controls. Set it up in the post generator. Something like this:

Then in the Mops, just place the machine control where you want the machine to stop. You find those here:


Once it shows up in the Mop, you can place it where you want and even rename it for clarity:

Then simply include it when you post.

But if you want to have a stop between every tool, then I would place the appropriate code in the tool change section of the post generator.

The top section defines the code for the first tool load, so if you don’t have an ATC you might want to put your M0 (or whatever) here.

I agree that the MecSoft forum is underwhelming. I always e-mail directly to Don. I think the excellent e-mail and phone support is why the forum is pretty dead. It’s not really necessary, IMHO.

Hope some of this helps,


You can in most cases edit the post for your machine and insert an M0 (stop but not rewind) before the tool change. Some machines won’t respond to this though, depends on the age and the CNC control language.

I reached out to MecSoft as Wim suggested, and below is what Don over there sent(posting for anyone else looking for this info).

First, important to note that I’m using the Professional configuration of RhinoCAM, which may work differently than others. Here are the steps from Don at MecSoft:

  1. Create one setup.
  2. Add the 3 axis Horizontal Roughing operation using the larger tool.
  3. Add a second 3 Axis Horizontal Re-Roughing operation using the smaller tool.
  4. Then right-click on the 3 Axis Horizontal Roughing operation and select Post to post out only that operation.
  5. Then right-click on the 3 Axis Horizontal Re-Roughing operation and select Post to post out only that operation using a different output file name.
  6. Then on the machine, setup the stock and run the first gcode file.
  7. Then change tools manually and run the second g-code file.

Thanks so much for this! I will try to get this working. It makes me a bit nervous to get into the deeper parts of RhinoCAM, but hopefully I’ll get a better understanding of how the whole process works.

Thanks again!

I’ll add one thing. If you are using a work zero with a fixture offset (G54, G55, etc.) make sure you include that when you post your individual toolpaths.