Help with my tool change process

Looking for some help with my tool change process. My biggest issues are currently 1. Returning the spindle to a location where I am able to easily access it. 2. Being able to re-zero the Z axis after the tool change.

Below is what I am planning for my tool change. Thank You for the feedback

G0 X10

G0 Y10

G0 Z0



M00 ;Change tool:



The easiest way to get started is to post the toolpaths seperately, I think. That way, if something happens you don’t have to kill a program.

You also want to make sure you’re using a consistent z, so don’t take your initial offset from a piece of the stock that is going to be milled away (like the center). I like to take all my zeroes from the spoilboard, somewhere next to the project.

So, you can home your machine, set the xy work zero, then pick a good spot and touch off for the z zero. When your first tool is finished, change the tool, go back to the good spot, touch off again, and run the second path. Repeat until all tools are run.

Does that help?

It is somewhat helpful.

Generally the projects that I am changing tools on, are full sheet projects, where in the first pass I am drilling holes, and in the second pass I am cutting the perimeter.

Similar to your suggestion I will put a mark off to the side of the sheet where I know is away from any milling. My goal was to not have to create separate gcode files, where I would need to re-zero after each process.

I don’t have a Lowrider, so there may be some specific issues with using that machine that I don’t have. On the Primo, I author separate files for each tool, BUT, I don’t turn the electronics off as I switch tools. By not turning off the electronics, and by moving the router electronically, the X and Y origin of the job is preserved. After changing the bit, all I have to do is execute a G0 or G1 to move the router back to the origin.

If you want to go down the rabbit hole a bit, there is a more sophisticated way of approaching the problem. Marlin has workspaces. Using them allows you preserve both a machine coordinate system and coordinate system local to the stock. Using something like this would allow you to have the router go to a specific place for a bit change, and even have a bit-setter-like switch to reestablish the Z height. I’ve only seen a couple of people on the forum use workspaces given their added complexity, but down the road when you could consider them.

If you’re trying NOT to rezero after changing tools, well, that’s unusual.

You could remove the old tool, place the new one loosely, and drive to z0 at your reference location, then tighten the tool. I’ve done this, but the accuracy is only so-so. The collet tends to grab the tool before it’s tight, so the final turn or so lifts the tool up.

I suppose you could jog it back down and rezeroing, but then you’re basically using the first method without the benefit of a z plate.

What’s the constraint that keeps you from wanting to use the first method?

It’s not that I am trying NOT to zero.

My thought process is this.

Bit 1 is a 12mm straight cut end mill which I use to drill holes. It has a length of 68mm
Bit 2 is a 3.18mm 2 flute endmill which I use to cut the perimeter of the project. It has a bit length of 45mm

Step 1. Install 12mm endmill and when installing the bit set the bit depth, along with the router collar (dewalt dwp611) When I get to the next cutting step I have room to adjust the router down so the cutting head is at zero.
Step 2. Zero/Home machine.
Step 3. Start Milling Process
Step 4. Return cutting head to specific location.
Step 6. Change tools
Step 7. Adjust router/tool height to material height.
Step 8. Start second milling.

Since ALL of my milling projects are going fully through the material I don’t see a downside to this process. But that is why I am posting it here. I am also asking to make sure that the Gcode which I posted will actually do as I am asking.

Perfectly reasonable steps, and one I’m sure most on this forum have followed same or similar. I have a guideline for my jobs. If the job is entirely cuts through the material, then I use the spoil board as my Z=0 reference rather than the top of the stock. Given that, for many materials, stock height varies somewhat across top surface, using the spoil board as a reference assures that I will cut through the stock, but not score up the spoil board too badly. I will also author my CAD/CAM so that the stock is slightly thicker than my real stock measurements. This assures that my (0,0) point will be above the stock even if that point turns out to be one of the high points of the stock. Of course, this assumes that your spoil board is flat.

Robert - Thanks for the reply and the vote of confidence here. However your process walkthrough is giving me more questions.

  1. In your process walk though. You mentioned that you Z=0 to your spoil board for through cuts, which is confusing me. The material I am cutting is pretty consistent as far as thickness is concerned. (10mm
    thick Coroplast). However My concern with what you mentioned if you zero to the spoil board, then wouldn’t your spindle plunge past the thickness of your project material, and plunge the Z-depth into the spoil board?
  2. I also found needing to set my material thickness to 1-2mm thicker than the material. I feel that this allows for slight table variances.

This is more just looking for ideas or alternative solutions
Attaching material to the table. As I mentioned previously 99% of my projects are full sheet, and through hole/cut designs. My material is full sheet (4x8), and as is my table. Currently my process is to screw down the material in the 4 corners, and if necessary when I am authoring my CAD/CAM I will plan for additional hold down screws, and plunge these locations as my first process and add in a tool change just so I can add the necessary screws.
3. Are there better methods for holding down the full sheet material. I have thought about 2 sided tape, but have yet to try it. What is most concerning is that the material I am working with is very light weight an entire 4x8 sheet is less than 5lbs if I had to guess.

Thanks for the help

I don’t know what tools you are using. In Fusion 360, I can pick a stock point on the bottom of my stock as a reference. If you cannot do this in your CAM software, you can:

  • Zero against the spoil board
  • Raise the router your material thickness as defined in your CAM
  • Run a G92 Z0

needing to set my material thickness to 1-2mm thicker than the material

If everything is well calibrated and you’ve surfaced your spoil board, and you use that surface as your reference, you should be able to avoid most of this extra depth of cutting, saving your spoil board somewhat. Or maybe just not worry about it. I have a Primo, not a Lowrider. My spoil board has an array of threaded inserts, so replacing the spoil board is time consuming job, so I like to give it as much life as I can. If all you have is a sheet of MDF, maybe don’t worry about cutting up the spoil board as much.

Are there better methods for holding down the full sheet material?

I have a Primo, not a Lowrider. I expect the hold-down strategies for full sheet goods to be different than smaller stock. I suggest you ask this as its own Forum topic/question to see what other Lowrider owners are doing.

Rather than double-sided tape, you could use the masking tape trick. You apply matching masking tape to the spoil board and the stock, put CA glue on one side and activator on the other and push the two together. I’ve seen this done with shelf liner rather than masking tape for covering larger areas cheaper. The problem with this idea is that, with a full sheet, matching the tape on both surfaces could be difficult. It would be easy along the edges, but you have to do some planning out in the middle, or make the tape on the stock larger to compensate for errors.

If you plan on doing a lot of full-sheet cutting (like this is a business), you might consider making your spoil board into a vacuum table. I’ve seen DIY solutions that pull the air directly through the MDF, and I’ve seen DIY vacuum tables using shop vacs.

Coroplast is very flexible, but if you’re cutting through movement in z fine as long as it stays pinned in xy (just keep z safe higher to compensate for the warpage). From experience double sided tape (ie carpet tape) works well for stiff material like thicker woods etc, but it can be too sticky for something like coroplast. There’s a good chance the parts will get kinked/damaged during the removal process. You could get by with tuning the size and placement of 2-sided tape strips where removal results in no damage, but long term you would probably be much happier using a vacuum table.


Thank you again for the details this has been very helpful.

I am currently using Estlcam for my authoring. But would like to get into Fusion 360 a bit more. Are there any good tutorials that you can recommend for setting up Fusion 360 for our machines?

There is a fairly steep learning curve with Fusion 360. I was already using F360 for my 3D printing, so it was a natural transition for me when I built my MPCNC. A lot of people are happy with, and do amazing things with, Estlcam. As for F360 CAM, the only thing MPCNC specific about it is the post processor. You can find a link to download it in this topic.

If you are looking for F360 CAM tutorials, I don’t know of a current author making beginning tutorials. I can point you towards some YouTube channels where I picked up my CAM (directly and indirectly), but their content might be a bit dated. The concepts still apply, but the F360 interface continues to change/evolve.

1 Like