What endmills for delrin/acetal?

How To
1

So I’m eagerly awaiting my Nomad. But since I don’t live in the states the first thing I’m doing is buying new collets and switching to metric. Using imperial bits is just going to result in confusion and way to long delivery times when I need a new one.

Mostly going to cut Delrin/acetal/pom. (with a focus on gears and other mechanical parts)

Anyway, is four steps from .0312 to .25in cutters a good number? or do I need more? (and how many am I likely to break in the beginning? :slight_smile: )

Was planing on buying those carbide endmills for alu/plastic?

Is it 2 flutes or should I be looking at 3 and 1 as well?

Thanks in advance!

2

I own a shapeoko not a nomad. Whats the rpm range on the spindle?

3

The official Carbide 3D speeds for the Nomad range from 3600–9200

4

The community has some recommendations at: https://www.shapeoko.com/wiki/index.php/Endmills#Specific_Bit_and_Brand_Recommendations

I was able to use Harvey Manufacturing’s “Locate a dealer” page to find a local shop which will let me drop in, pay for an order w/ a check, and then pick it up after their next delivery which is pretty convenient — machine shops are more common than one would think, so perhaps you can find such a shop?

Entering 3.175mm and 6.35mm and so forth isn’t that bad.

5

He may be referring to availability of metric vs imperial, rather than preference?

1 Like
6

There;s been a lot of discussion, and there is some dependence on the geometry you are cutting and the desired finish, but I would say that four sizes from 6mmm down to 0.75mm (6, 3, .5, 0.75 or 0.8, as available) will do a lot. Fast removal with the larger tools, cleanup with the smaller, if needed. Flat end (square end), vee, and ball end are a decision based on what you are doing. Pocketing boxes is likely to be flat end. Sloped and figured surfaces are likely to be ball end for finishing. Engraving and tracing, vee. Note that smaller tools are going to be shorter and less stiff.

Number of flutes matters less than some manufacturers would have you think, but does matter. I do a variety of materials, so I pretty much only use 2 flute, TiCN (grey/purple coating) for everything. Not always ideal, but generally good. For most plastics, the advantage to fewer flutes is clip clearing. You need a sufficient thickness chip to prevent rubbing due to material deflection, and this is easier to do with fewer flutes.

You would be surprised how rarely you need the smaller tools for most jobs. The larger ones give a better finish, since they can be run nearer the optimal surface speeds, are more rigid, and present a larger radius (better approximation of flat, easier to get a smooth surface with a ball-end). Not to say that the smaller tools don’t get use, but 95% of the machine time (or more) is with the largest, for me.

2 Likes
7

Both, there are some perfectly good Swedish webshops that I’ve used before to buy endmills (that doesn’t have imperial stuff). And I was also thinking that since I have to buy a collet set (how many comes with the nomad pro?) for metric drills anyway I might as well use them for the endmills.

It seems like its single flute since we cant run as low rpms that we probably should.

Yhea I don’t see myself using anything smaller than 1mm, anything smaller and they’ll be to short anyway.

Thanks for the advice!

1 Like
8

The 1/8" ER collet (3.2mm) that comes with the machine is actually a pretty good choice for a lot of things. ER collets have a pretty good range (ER11 is 0.5mm, give or take a bit depending on manufacturer) and are sized by the largest size they hold, so the 1/8" will go from 3.2mm down to about 2.7mm.

You might want a larger collet, like a 1/4" (6.4mm) as well. If you get more collets, invest in at least one extra nut. Leave a nut on the collet(s) you most use. Removing the nut from a collet can be less than easy.

Milling tools smaller than 1/8" (3.2mm) generally should have an oversize shank for ease of handling and good grip in the collet. The supplier I use doesn’t even stock any endmills with shank smaller than 3mm (they have both 3mm and 1/8").

For drills, I use 1/8" or 3mm shank bits, again both due to the good holding and ease of handling. They are readily available, and if you are using carbide bits (rather than steel), these are pretty much your only option for small sizes in the US. I don’t know about Europe, but would imagine it is similar. The smallest I use with the Nomad is 0.25mm (0.010"), mostly for circuit board work. At that size, drilling is pecks of about the drill diameter with full retraction each peck for clearing. In the US, these are referred to as quick change, circuit board, or oversize shank, among other names, and are almost invariably 1/8" shank for sizes less than 1/8"(3.2mm).

I wouldn’t expect the Nomad to drill any larger than 1/8"(3mm). The torque isn’t there. Larger holes are actually as fast or faster boring (with or without pilot hole… there are a number of variables), and in practice, I tend to bore any shallow holes (less than 5mm deep) larger than about 2mm diameter (using a 1.5mm flat endmill).

1 Like
9

Not even in something that machines as nicely as delrin? if I do pilotholes with the 3mm you don’t think it will go as high as 5mm?

Guess I’ll have to do pilot holes and the rest on the drillpress at work… 3.3 and 5mm is sort of essential for M4 and M6 treading (that I use for everything).

And yes but collets just tend to get annoyingly tight if you use them for stuff that is smaller than their max size after a while, at least the larger ones I’ve used.

10

Delrin machines very nicely, but I suspect the torque limit will get you much above 3mm. I have drilled 3.3mm in acrylic for 4mm taps and it is satisfactory, but generally just mill them, if I can, to avoid the tool change. I wouldn’t try any larger in acrylic. Delrin is less gooey than acrylic, but it still takes a fair bit of torque to drill. Note that the torque required is approximately proportional to the square of the diameter of the drill.

For 5mm and 6.75mm, I mill the hole using a 1/8" endmill, and, if I can’t go deep enough (25mm is about the limit with tools I keep on hand, but, then again, I would be hard pressed to get much more with a drill bit on the Nomad), follow up on the drill press or using a handheld drill using the milled hole as a guide.

That said, I have not tried a drill as large as 5mm on delrin in this machine. I discovered early on that much over 1/8" were impractical on the materials I most work with, and that milling holes generally saves my time anyway, so I stopped exploring the limits for every material. I can say with confidence that it is not practical to drill a 5mm hole in aluminum, nor a 5mm hole of significant depth in acrylic (actual size was 0.166 for a #10-32 machine screw, so actually about 4.2mm. Coolant would have helped, but it is easier to just mill the hole dry at that point).

When you drill, watch the machine carefully until you get your settings, especially with larger bits. You can and likely will stall the motor at some point. If you find you can drill 5mm, that would be very nice, but my suspicion is that the machine will bog.

As for collets getting tight, I haven’t had that problem, but I typically only bring a 1/8 (3.2mm) collet down to 3.0mm. It is so much easier, and more efficient, to just get as much tooling as I can with standard shank sizes, which, for me, on the Nomad, is 1/8" and 3mm, with some 1/4" (6.35mm) shank. I use a different flavour of collet on the lathe.

1 Like
11

What about “roughing end mills”? I’ve used them on aluminium with a manual mill and there they allowed for much deeper cuts and less vibration. But since we are talking plastics and single flutes and they only come in 4 flutes I’m guessing I shouldn’t bother?
Is a setup with compressed air blowing is more important than a vacuum solution for chip clearing?

Btw what type of er11 nut is it? or do they all have the same thread just different exteriors?

12

AFAIK, the thread is standard, the only difference being the dive of the nut. My Nomad came with a hex nut for a conventional wrench, and I think that is what they still ship. The other common style uses a spanner (US usage of spanner-- often a hook type or a two pin face type-- not British usage).

I have never tried a roughing endmill with plastic (except polycarbonate on a 4KW (5HP) Lagun), not have I used one in the Nomad. I would not expect great results, but that is a gut feeling rather than based on actual experience or hard data.

1 Like