Endmill comes loose during cut (wanders in z-axis)

I’m quite sure that the endmill is moving. What else could be happening? Could the spindle be forced down? The wood is firmly placed on the wasteboard, so that’s not moving around for sure.

no but the piece could be pulled up if workholding is not good enough. I doubt this is the case here, is that a custom workholding jig I see ?

Can you share your cutting parameters ?

It sure is. The jig is working really nicely :slightly_smiling_face:.

Sure. I’m definitely pushing it to the edge… probably over it seems:

I’d be curious to know what your speeds and feeds are, just based on the photo it looks super aggressive. if I were approaching the same job I would assume that I’d have a depth of cut of about 1mm for hardwood.

1 Like

Yeah, 9mm depth per pass at 3mm optimal load is…a lot, I tend to stay in the 1mm optimal load ballpark when cutting deep adaptive like that.

It only comes to mind now, but you should check your zero after this happens, to establish whether you lost Z steps during the job. If you did, chances are it’s that upcut endmill pulling too hard on that poor stock :laughing:

1 Like

You should always have a spare collet onhand anyways, so I would just get a replacement and see if that solves the issue, because it feels like the collet is not gripping the endmill when under strain…

1 Like

This is exactly why you should confirm it. Not being able to think of what else could be happening is a fault in thinking and not an affirmation of reality.

From my experience in manual machining, it’s an indication of chatter.

As mentioned previously, generally too aggressive of a cut. It can also be lack of rigidity, but that is caused by too much tool pressure, or again, too aggressive of a cut.

At least, that’s for metal. I assume the same stands for tree, but may be wrong!


Those scallops could be the result of the toolpath.

I agree that the cut is at least optimistic though.

If there’s enough vibration to move the cutter I’d expect the whole Z assembly to be vibrating too, maybe a video (with sound) of the machine attempting that cut would help?


Isolating fine thanks, new job is keeping me busy and occupied.

I thought those scallops might be the remainder of a roughing toolpath based on the pics posted

But I tried setting up a similar path in Fusion myself and the simulation shows the adaptive leaving relatively smooth walls so, no, it looks like it’s due to substantial deflection.

That’s what makes an experienced machinist experienced :wink:

There are some basic rules we can follow though about minimum feed per tooth to avoid just rubbing and maximum overall cutting loads for the machine. I’ve used Millalyzer to help with this to some success.

There is also @gmack 's excellent feeds and speeds spreadsheet which has a whole load of shapeoko specific knowledge which would be a great first place to check out this cut.

That’s a point I had not considered. I like the idea of having a video clip and sound made during the cutting process. It would certainly assist me to understand what is shown. My expectation is that changing the cutter for a new one of the same type, without out adjusting any settings, would lead to an improvement in the cut seen.

If it was my cut the first thing I’d do would be to either back off the optimal load to 1mm or 1.5mm or drop the max stepdown to 3mm or 4.5mm and see if the machine is happier at that lower load.

As above, well questioned, looking closer at the toolpath, you’re right, it’s not the adaptive, it’s deflection and the sheer size of the deflection suggests machine deflection, in my experience if you bend carbide that much it tends to break and fling high speed shrapnel at you…


You’re absolutely right that a blunted edge on the tool will make any issue with the toolpath worse. A cut with high vibration and chatter will also abuse the cutter and may well blunt it prematurely.

I’ve found in wood that I get a dark buildup when cutting woods with a high resin content such as maple which I can clean off with a tool cleaner or acetone. As for sharpness Julien has some close up pics in the ebook showing the structure of the cutter edge and bevels which are linked in this thread

Since looking at those pics and inspecting some of my cutters under a proper magnifier I’ve learned what a new sharp and old blunt tool feel like to the thumb, at least for wood, still taking baby steps in aluminium.

Have you read gmack’s posts on feeds and speeds?

And yes, hopefully holgersindbaek will soon be finding a way to run that cut without problems, I’ll be interested to see what works.


As always, lots of good information here. Apologies if it’s already been mentioned, but how are you tightening down the collet nut? Using two wrenches, presumably? I find you have to cinch the collet nut down pretty hard, and those wrenches (at least for the Makita router) are short.

I find putting both wrenches in my hand and squeezing my hand shut applies more torque than when I have a wrench in either hand. I’m less likely to wind up pushing sideways on the router. Using the same technique to loosen the collet nut means I have the other hand free to stabilize the tool, and it’s less likely to loosen suddenly, sending my knuckles into something sharp.

I have not investigated or measured a torque spec for this, but it might be worth looking into.


Thanks a lot for the in-depth analysis and sorry for the late reply. I think I’ve come to the conclusion that you’re right and that I’m simply putting too much pressure on my Shapeoko.

I’ve made a new program where I’m putting less pressure on the machine by not making such a deep cut and by cutting parallel along with the wood. I’m making a test cut as I’m writing this. Let’s see if it’ll work :slightly_smiling_face:.

Just out of curiosity, if I wanted to speed up this whole process on my Shapeoko, what could I do? If could probably optimize the program, but that would probably only decrease the time 20% or so. If I upgraded to a spindle, would I be able to decrease the machining time a lot?


Fun as deep adaptive clearing might be (I’m guilty of over-using it), it seems like a few folks have come to the conclusion that shallow depth and large WOC tends to work better on a Shapeoko.
Slotting makes me cringe (compared to the sweet sweet sound of adaptive clearing a channel), but in some cases, it may be more efficient to just run a contour cut blazing fast and at low depth per pass.
What about 30k RPM, 3000mm/min (~120 ipm), and 2mm per pass ? What does Fusion say the cutting time will be then ?


It will be interesting to see how that comes out and whether the adaptive clear leaves a less wobbly wall finish.

I suspect what was happening before was deflection of the machine due to cutting forces, it would be interesting to see & hear the cut.

Well first, do you really need to cut away all that material with the Shapeoko?

Are you creating a flat plate with attached ridge so all that material in the middle really needs to be cut away?

Around the outside it might be faster to run round in a continuous contour cut with stepover as that would be constantly moving not stopping and reversing as the adaptive clear does.

I would probably run an 8-12mm cutter in my spindle and make fast clearing passes at 4-6mm depth depending on how the wood took the cutting and keeping the Shapeoko out of the vibrating wobbly resonant deflection modes, I described how some of these happen a while ago

The upgrade to a spindle is really not about cutting speed though, the Shapeoko is mostly limited by machine rigidity not spindle power.

I would definitely go over the machine and ensure that I had no slack or wobble in the V wheels and that my belt tensions were all in the zone


That’s kind of what I’ve changed it to :slightly_smiling_face:. First I’m doing a contour (with almost the exact settings you’ve just mentioned) and then I’m making a parallel run at 4-5mm depth:

It seems to work well, but it does take some time. I guess there’s no way of getting around a long runtime when you need to clear a lot of material.

1 Like

Be interesting to see where your toolpath time is coming from, the clearing or the finishing passes.

It might be worth trying a few different strategies for the clearing to try to keep the cutter moving -

What you state here isn’t necessarily true. It may be level to the ground, that doesn’t mean it’s equidistant from the axis. The only part that matters is the axis, I think you’ll find that if the wasteboard really is level, the X extrusion isn’t. “level” is a really loaded word. Exactly how the 3.8mm is measured makes a ig difference in what you can glean from that information. The 3.8mm is measured at exactly the same point as where the cut was started, or at the end of the cut? At the home position? Using an electric probe, or best guess using the sheet-of-paper method (which is surprisingly accurate) on a had metal bock, gauge blocks, a machinist 6" ruler, a caliper? Belts were adjusted when you assembled, so the CM DRO is a close match to reality?

  1. You haven’t mentioned the router sliding up in the mount, is it? Can you prove it?
  2. Does the toolpath run continuously from the left to the right? That would prove without a doubt that this isn’t losing steps, nor is the endmill slipping in the collet - if it’s cutting in both directions, it would still be level, but would show gouges such that the last CORNER would be higher than the others.
  3. The slots in the collect are clearly packed with sawdust. Those slots are critical to grip on the endmill. Clean them out. A metal shim works great, or a pick. Can’t have too many pick’s around.
  4. Don’t use the endmill to measure things - take it out of the router. Now use the base of the router (preferably a dial indicator stuck to the mount…but assuming you don’t have one) to measure between the baseboard at the 4 extents with the z-height the same on CM. Obviously, clean the board, find a spot that’s not been cut up, etc. Use a set of metal shims if you don’t have a dial indicator. I suspect you will find that the wasteboard isn’t flat, or isn’t square to the router in one axis. There’s a bit of an art to this measurement, but you’ll get the hang of it. Fine adjustment of the X axis can be messed up by adjusting the tension of the bottom wheels of the Y carriages. ~ .25" or so from left to right (left lower, right higher), which will likely require adjusting the rail where it’s attached to the left and right carriages. You can make the whole machine square in all directions with just a machinist level and machinist square (not a carpenters square or carpenters level unless you have proven both tools are accurate- if you don’t know how to prove those two tools are accurate, it’s not hard, but not necessarily obvious, just don’t do it), but it’s very time consuming and tediously repetitive.

The picture showing the chatter clearly shows there is mechanical free play in the system - carriages, wheels, could be almost anywhere, needs a close going over all the mechanical parts.


Yes, likely chatter, speed is too low , travel is too fast, tool dull or maybe a down cut bit is being used instead of an up cut bit that would clear the chips faster, down cut may be clogging the bits performance.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.