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

Yes, thanks Sam. I had guessed as much. I was trying to understand the cyclical nature of the fault and thought that a feed rate that was too high when combined with a high percentage of tool engagement (9mm on the face in contact with the workpiece) and the addition of conventional milling, would lead to some type of chatter.

The appearance of the fault looks as if the tool was constantly being deflected from and returned to its expected position at the workpiece. The speed of the feed rate was probably responsible for the repetitive phenomenon seen.

The deflection of the tool was likely the result of a high feed rate and high tool engagement percentage at the interface between the cutter and the workpiece. A blunt tool would not have helped this situation either and the torn rather than cut wood would suggest that the tool was due a replacement.

The tool rigidity initially did not strike me as an issue because wood and a 1/4 inch diameter 3 flute endmill (I believe that is what the #201 tool is) ought to be good together. The tool engagement with a large DOC of at least 3½ times the tool diameter with constant engagement of the cutting face, would easily be enough to induce deflection at the high feed rate used.

The collet on the Makita/Carbide router is tiny in relation to the job it is being asked to do here. The endmill loosening suggests that several factors need correcting before a satisfactory cut is obtained. I would clean the collet, nut and spindle taper after every job on my own machine. I don’t think that was being done here. The stickout may be too little if the endmill is butting up against the router spindle and potentially may cause deflections in the tool. it may be too much stickout if insufficient tool metal is held in the collet.

118 inches per minute is a high feed rate and I would use half that for my own softwood projects. I would not use a 9m stepdown on soft woods and the most I might get to is 1mm with a .5mm stepdown. The tool is suffering when you look at the wood, even assuming all was fine with the feeds and speeds, the cut edge of the wood looks to be torn rather than cut. I have not done any adaptive clearing in wood and I am only just learning about it. My understanding is that adaptive toolpaths save wear on the tool as well as time and expense and there is less tool breakage.

Perhaps all we are seeing is too fast a cut with a tool that was blunt. If the toolpath was appropriately calculated by the software, I am in no position to gainsay that.


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?


Hi Liam, I hope that all is well with you during these mad days.
Are you suggesting that the toolpath chosen by the software had induced the scallops by creating a toolpath that was based upon the numbers fed into it?

It gives me the impression that tool speeds and feeds is an arcane art rather than a science. :grin:

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.


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…


Thanks for helping me to understand what is going on. I guess simple things are simple. It is quite difficult to appreciate but as close an inspection of the tool that one can get from an internet image potentially indicates a hard driven tool. The wooden cut edge I had enlarged does not appear to be burnt or scuffed from a tool staying too long in one location.

I enlarged both images of the tool as much as I dare and still have something to show. The impetus to this was that the first view showed a tool that looked a little tired. (I cannot explain what made me feel that but it did not look its best)

The picture shows inside the fine red highlighted area a discoloured portion of the flute tip which suggests that it has been too hot. Metal on wood it is probably less important than metal on metal but excessive heat may well adjust the temper of the tool. I would expect that the end of the service life of the tool would be a chipped flute tip. I offer this image as corroboration for a tool being driven too hard.

The second image shows the tool to be nice and bright and displaying intact cutting edges. I have to assume that the dull grey of the first image (which had first attracted me to look at the tool more closely) was just a matter of inadequate lighting. This image has a fine red highlight around an area of discolouration which was possibly heat induced.

Interesting stuff. I hope it has been useful for @holgersindbaek to see his work analysed in this manner.


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?


Great information! I have some hardwoods on order including Cherry, Maple, Poplar, Oak and Walnut so I need to brush up on what their machining characteristics are likely to be.

I have read that excellent work by @gmack. I have also purchased the static version of Millalyzer which I have yet to learn how to drive. Everything is baby steps for me right now but I am enjoying the journey. :smile:

1 Like

Yes, I do this too. It seems easier and a more natural movement and you can stop the bits from falling out of the chuck or slipping when tightening them.

I hope that there will be an improvement in finish and machinability.

Interesting question: I cannot answer the second part about a spindle. Machining time has to fit into a well understood set of parameters. viz.

It is crucial to visualise the endpoint because that will inform all of your choices. Ask yourself whether the desired endpoint is achievable with the tooling and machinery that you are intending to use. Along with that question you will need to question whether what you are trying to achieve is desirable. e.g. If it will take 7 months of running your machine continuously 24 hours per day to achieve what you want, then clearly that would not be a desirable outcome and you may as well outsource the work to a machine shop that can do the job in hours. In other words, there is no point in re-inventing the wheel.

Amongst other questions you need to ask yourself are what tolerances will you accept and work to for the particular job in question. Hobby class machinery driven hard will never produce work to fine tolerances, even though it is capable of doing so at reasonable speeds. How important is similarity between workpieces going to be if you are producing more than one item that is supposed to match. Once again, hard driven machinery of the domestic/hobbyist variety is never going to be as accurate as when it is driven at reasonable speeds to take account of all of the factors that can affect similarity. This also applies to using sharp and appropriate tools. I would probably opt for a straight two fluted cutter if roughing was the bulk of the work.

I always ask myself what do I need to do to provide the conditions that will give me the best opportunity to achieve what I want. Waiting for the machine to finish can be irritating when one would rather get on with the planned work. However, the amount of stress that one can place on the workpiece, machinery and tooling is finite. Each component in the chain from blank canvass to finished workpiece has a known limitation and working within all of those limits will be less of a frustration than replacing tools, redoing the work and wondering what has vibrated loose.

1 Like

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

Everything takes time, Holger. Expectations of how long things should take may be awry. Practical considerations are likely to change our expected timings and the closer that our own expectations move towards every day reality, the less time things will appear to take.

The suggested timings in software are often inaccurate, not because the software developers don’t know anything or don’t care how we use their products but the algorithms used are only best guesses. Humans tend to view digital information on a screen as immutable, when the reality is that it is often wrong.

It can be helpful to see many other projects being carried out to get a better sense of the capabilities of the Shapeoko machinery. I like to break projects into sections so that I am not undertaking just one repetitive process ad nauseam. I may decide to do some hand sanding, assembly or painting work, while I have a piece being machined on the Shapeoko.

Here is a great project: See how long it occupied.

@wmoy has produced some great video presentations. Look at the processes used - they all take time.

While time is always a factor to be considered, I would like to think that what is produced assumes more importance than how long it took to produce. YMMV.


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.


Hi Tom; @holgersindbaek was running the router at 30,000 rpm so that would appear to be fast enough. What I see (as a complete newbie) from the patterning of the edge left, after the pass, is a mismatch between cutter choice, cutter condition, DOC, speed of cut and material. There are likely to be multiple causes for such patterns and one all encompassing solution does not readily present itself to my mind. I would be making many test cuts with minor adjustments to one parameter at a time to discover which adjustments had the most desirable effect.

Hopefully we will see the results of @holgersindbaek’s test cuts soon. That should bring us a little nearer to understanding how the patterning had arisen. It is a separate issue for me from getting the job done, although it is clearly integral to making the SO3 work at its most effective efficiency level. I don’t mean to sound dismissive at this early stage in my hobby machinist life, I am looking for good general principles that can be applied across the board to all work I undertake.

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