Spindel Stalls at very end of job

I am cutting some happy faces from a piece of 5.2mm wood using the Nomad and a 0.063 cutter (Carbide3D #112)

The toolpath parameters and the simulation of the cut path are shown in the two screen shots below.

Near the very end of the job the cutter seems to take a very deep bite and it stalls out. Literally stops spinning for a couple of seconds until it moves slightly. I do not know what causes this so I stopped the job and finished the last fraction of a mm of the cut with a knife.

What would cause the spindle to stop and bind up at the end of the job? What should I check or look for?

Will the spindle stopping like this hurt the machine?

I have had the spindle stall when using the 0.0625 cutter too (I am relying on my mislabeled 0.0625" end mills until larger cutters arrive).

If you notice the cutting flute of the 0.0625" cutter is significantly narrower than the 0.125" shaft. And the flute itself isn’t terribly deep. If you attempt to cut deeper than the length of the flute then the shaft grows wider and will rub and eventually stall against the side of the workpiece.

I had thought that MeshCAM was supposed to model this attribute of the cutter and flag this condition. Maybe it does and I haven’t looked it the right place (I am still very much a newbie).

While I haven’t been able to try it myself, using a longer cutter like the 0.125" for roughing should allow the finer 0.0625" to reach in. Hopefully meshCAM won’t try to apply the 0.0625 closer to the wall than the shaft will allow.

You may also be able to adapt your model to slope the surrounding wall away to allow the 0.0625" and its wider shaft to fit.


I had a similar problem. I had a value in the machining margin like you did and for some reason meshcam wanted to do a pencil line finish around the profile of my cut In areas that hadn’t been machined yet. So it plunged to the max depth which was the thickness of my material.

Try unchecking the pencil line finish and run the program again. I don’t think you need it with a 2d cut anyways. Or you can try setting the machining margin to zero. I believe you can also click on “machine geometry only” which may do the same thing.

@keng brings up a good point about the tool definition. MeshCAM assumes that the diameter of the cutter increases from the flute diameter directly to the shaft diameter at the end of the flutes without taper. It interprets this definition


MeshCAM will avoid the shank on 3D parts where the surface is sloped, by offsetting the toolpath outwards from the part. I have not checked its behavior on 2.5D parts (where all sidewalls are vertical) but will do so.

@3dsteve, your toolpaths look fine from the screenshots. You used a reasonable stepdown for the waterline, and from the toolpath shot there wasn’t a big jump down to the pencil pass at the bottom of the material.

Since you didn’t add supports to tab the workpieces into the rawstock, another possibility could be that the pieces shifted as you began to cut through and pinched the cutter.

@Darren, it is always good to use a pencil finish on 2.5D machining. Waterline isn’t guaranteed to cut to the bottom of the material, even when the stepdown is an even divisor of the material thickness. Due to internal calculation roundoffs, MeshCAM will usually not take the bottom possible waterline cut, and that holds true also for roughing cuts. MeshCAM might not take the bottom possible roughing cut, so always assume that the finishing cuts might encounter a material depth equal to a roughing stepdown. My rule of thumb is never make the roughing stepdown deeper than I am willing to let the finishing cutter bite.

It is always a good idea to use the same cutter for finishing as pencil in 2.5D machining. On 3D parts where you are just tighening up corners is the place where smaller-diameter pencil cutters are usable. But flute length is always important to keep track of there too.

1 Like

As promised, I did the experiment I mentioned above. I defined a cutter with .125" diameter flutes, .375" long, and a .250" diameter shank. I made a 1.000" square workpiece, .500" thick and told MC to do a waterline+pencil toolpath to cut it out of the .500" thick stock. Even though the max depth is at the bottom of the stock (shown by red outline to the stock outline), MC limited the toolpath depth to the .375" flute length.

So if you define your larger-shank cutters with the actual flute length, MC will not try to wedge them into a too-deep cut. I pretty much expected this from observing the 3D cutting behavior, but it is good to know for sure.

For same-size-shank cutters, it is convenient to define a long flute length. On deeper cuts, the shank might rub against the sides of the kerf, but it will still be cutting “down below” as long as the stepdown isn’t larger than the actual flute length.

1 Like

That’s a great observation Randy as to the flute setup.

I’m going to go check a few cutter definitions to account for the right depth-of-cut for some smaller tools I have! I have some long-reach tools that I’d put in the flute length as the actual flute length, not the length to the transition where the shank widens out to the full .125" for the collet.

I hadn’t run into it cutting to shallowly yet, but I’m betting I would have soon enough.