Unwanted taper in my milled pieces

1

Hi; I’ve got some unwanted taper in all of my milled pieces and was wondering what potential things could be going wrong and how to troubleshoot and fix them.

I’m cutting with the 1/8" carbide endmill. Doesn’t matter if I cut plastic or wood. Doing .25-.5" deep cuts that should be vertical walls but the tops of the pieces will be significantly skinnier than the bottom (top of a .2" thick wooden piece that I cut with .01" stepdown was ~.003-.004" thinner on top than at the bottom). Doesn’t matter if I’m cutting with sticky tape or vise.

Could the endmill itself have taper, either from the manufacturer or from seeing more wear at the tip than above? Could I have spindle runout (and is that what runout would do, or would runout make the base thinner than the top?)? Does it matter if I conventional or climb cut?

2

Unless an end mill is labelled as tapered I would not expect the end mill especially from a known quality source. A “carbide endmill” could be many things. Chinese junk, end mill from Carbide3D, uncertain source (carbide end mills ARE NOT created equal) and so forth. Known quality source?

My instinctive reaction would be to check a bunch of things.

A) Feeds and Speeds

Too fast may be able to do this. The end of the end mill can “wobble” - chatter. This has a very
definitive sound. A (jewelers 10X) loupe can help eyeball “waves” in the machining that may help
pinpoint what is going on.

What is your stock (which wood)? What is your feeds and speeds? How many flutes does the end
mill have? Does the end mill have a coating?

B) Collet and collet nut

Is the end mill being inserted into the collect properly? Is the collet and collet nut being installed
properly.

C) Is there a problem with the end mill?

Do a quick test. Use a light to backlight the end mills. Rolling them on a flat surface. Any gaps?
Does it roll straight?

In a production setting one has a “granite”, a multi-ton piece of granite known to be flat to 0.0001"
or better. We can settle for a table top for a first approximation.

How much use has the tool had? What materials have you machined? If you’ve been doing
things as or softer than wood and plastic I would not expect an end mill to be worn unless the
amount of machining you’e done is very extreme (the Nomad hasn’t been out that long!).

In a production shop, each job has new end mills costed in to remove this possibility. The "used"
end mills are used for roughing and tests… they don’t go to waste.

D) Spindle runout

In a new spindle I would not expect this to be such an issue. It's really easy check - if you have
the right tool.

The Nomad spindle has excellent, low runout when it leaves the factory. It takes a great deal of
use to wear a spindle.

E) Mill tramming (adjusted squaring)

My Nomad hasn’t arrived so I can’t speak to this. They are pretty good about tramming at the
factory. I don’t know about tramming procedures in the field for the Nomad. The Nomad is pretty
robust - fixed gantry and all - so I would put this, initially, as a lower chance item.

Climb/conventional milling is unlikely to be the source of this issue; they affect machining speed and fine finish more than anything else.

mark

3

@kjl, this is with the repaired control board (ref. Slight stepping artifacts; any ideas? )?

What kind of geometry are you cutting? Is this on thin protruding walls, or on the “blocky” geometry you showed in that thread? For 2.5D cutting I would not expect any tapering, becuase with vertical walls each waterline cut is the same full-width cut as the one above it. .010" stepdown with a .125" cutter is less than 10% of the diameter so that is very conservative from a cutter deflection standpoint.

With wood, unless it was well kiln-dried, I would expect some movement as you cut through the grain. But plastic is a uniform material and I would not expect movement there, unless your feedrate is too low or RPM too high and you are heating the material by not being agressive enough (i.e. rubbing rather than cutting). The other night I melted some styrene (I could see it soften before it blobbed onto the cutter) by accidentally setting the feedrate too low. But that was really obvious and ruined the workpiece rather than “just” being a few thou off. :smile:
Randy

4

@Randy Hey, I don’t believe it’s a machine bug (stepper board thing).

The shapes I’m cutting vary, but they are all basically rectangular blocks. For example, I’ve made a few soft jaws for the vise that sit in the channel, so they’ll be 28.65mm wide (to fit the channel) and then anywhere from 10mm to 50mm long, by 6-12mm tall. When I cut them out of the raw plastic sheets, the base of the cut out rectangle (the part that was stickytaped to the MDF wasteboard) will be basically cut to perfect size but the top part will be slightly smaller along both axes: so if I want to cut out a 15mm x 28.65mm x 12mm rectangular block, the bottom will measure basically perfectly 15mm x 28.65mm, but the top will measure significantly smaller (14.85mm x 28.50mm), for example. The taper is noticeable by naked eye, and definitely noticeable by fit - it will be quite tight to fit in the vise channel but once slotted in will end up loose. There is no melting at all with this stuff - this plastic is super, super easy to machine I think and I end up with perfect little white plastic comma shapes everywhere.

I also milled a small circular peg out of walnut (which was held quite securely by softjaws in the vise) which was supposed to be .125" diameter and only .2" long. I was milling it so that the axis of the peg went along the grain, and when I was done, the diameter of the base of the circular peg was pretty close to .125" but the diameter of the tip of the peg just .2" above that was as small as .119".

IMG_7794.JPG1632×1224 525 KB

@mbellon: It’s a flat carbide .125" 2 flute endmill from Carbide3D. Actually still the one that shipped with the machine. But I haven’t actually used it that much, and only on plastic mostly and a little bit on renshape and wood. A far amount of plywood as well.

A) Stock is Walnut. Or plastic. Feeds and speeds right now are ~.004 IPT, 7500 spindle speed, ~60 IPM, and I’m being quite conservative in stepdown (.01", sometimes I bump up to .04", but doesn’t seem to matter).

B) Yeah, pretty sure collet is all fine. It kind of doesn’t make any sense anyway - collet or endmill placement mistake, or spindle runout - both of those wouldn’t result in a taper with a thin top, right?

C) I’ll see if I can check the endmill - I don’t have a good way to really inspect them, but they haven’t had that much use- some wood and plastic only, and honestly not that much (too busy with my full time work to play with the Nomad too much).

D)

E) If I had bad squaring I’d assume taper only on one side and not the other, right? Like I’d have taper on just the -X wall but not the +X wall, or vice versa?

Anyway, it’s all very confusing to me. Maybe I should slow down my feed/speed and see if that helps…

5

My suspicion there is the wood is flexing and getting pulled into the cut — try a Downcut bit?

6

Any out of tram would show all of the time… a bias in all cuts. Like I said, not likely.

Any runout is unlikely due to the newness of the spindle.

Collet OK. Check.

Feed and speed reasonable for the material. Check.

Good end mill. Check.

Randy and others are pointing out something important. Machining is not unlike hitting the surface one is cutting with a hammer and chisel - REALLY FAST. Even if the material is held tightly from moving in the bulk, it can still move due to the pressures of the machining - the material rebounds! Think of an eraser in a vise that you hit with a hammer… at the near microscopic level.

Those look like really small parts. The materials you’re using are softish (compared to metal) and things can be moving around.

Can you machine a square pillar, in plastic, that is about 1" square and 0.25" deep and tell us what the edge looks like? Let’s be sure we’re out of any “edge case”.

mark

7

Yeah, those parts are small - I’m proud of how good I got them :slight_smile:

OK, I think you might be right. I had previously cut some HDPE rectangular blocks, and they are also slightly tapered, though it seems the larger the size of the block the less taper there is. So I have a 11 mm x 28.65 mm x 11 mm plastic block, and the taper is there for both X and Y dimensions there as well, but not as much as they were for my itty bitty wooden pegs (only ~.0015" to .002" taper), and then I had a larger block (28.65mm x 50mm x 11mm- this is pretty close to the 1" square x .25" deep you recommend I cut) where the taper is still there, but just barely, only about .001", or right at the tolerance level of the machine.

OK, so I suppose I can live with that. I did some reading and it sounds like there is some difference between climb and conventional cutting, where climb cutting is supposed to create less force between the endmill and the workpiece, but the force is pulling the workpiece towards the endmill, whereas conventional cutting is supposed to create more force, but (more) parallel to the direction of the cut. So I am going to try conventional cuts and see if that helps.

In any case, the finish (on the plastic, anyway) is superior with conventional cutting, which I think is backwards from the way it’s supposed to be.

So: if my taper is a result of my workpiece pulling towards the endmill, aside from trying a conventional cutting direction, is there anything else you’d recommend I’d try to limit that effect? Even more conservative stepover/stepdown? Slower feed speed?

I really appreciate the time you’re taking to troubleshoot this, by the way - thanks!

8

Conventional cutting is called that because it works most of the time for most things. It’s certainly worth a try.

I’ve seen advanced CAM software do what I’m about to describe. I can’t think of a way to do this with MeshCAM at the moment. Randy and others may suggest other approaches.

The lead in enters away from the part with the end mill moving parallel to one of the surfaces. For a round part this would be a tangent. No roughing passes other than removing big stuff out of the way.

Moving along until we touch where we need to machine. Pencil finish around and when one returns to the entry point follow the parallel line (tangent) to depart some distance from the part. Rinse, repeat. Bite a little bit each pass until part reaches the desired size. Very gentle.

My immediate hunch is to increase the RPMs (some feed adjustment too), use a 4 flute coated (ALTiN) end mill (“slipperier”) and waterline it with very small step down. No roughing.

I’m going to sleep on this. Honestly, machining really tiny parts in wood isn’t something I’ve done!

mark

9

I use Fusion360 and it has leadins and leadouts and ramps and all sorts of niceties like that (and they’re on by default) so perhaps all I need to do is leave quite a lot of material on the roughing pass, and then go super, super conservative in terms of stepover and stepdown for the finishing.

Yeah, the tiny wood parts were fun, esp as a total cnc newbie. I had to learn how to make little softjaws and invent (I’m sure reinventing the wheel) a procedure for cutting out little tiny blanks and then whittling them down in a few passes to get them just right. So satisfying!