High Speed Milling

I'm doing some relatively fine work (0.25mm holes for example) and so I've built a high speed milling spindle for my mill. By high speed, I mean up to 19,000 rpm. It has an ER11 collet.

So far I've tried to use two types of (carbide) end mills. There's one sort readily available on Amazon which has a 1/8th barrel and quite a long cutting part (so perhaps 1mmx 20mm or so). It's not always clear if these are meant to mill metal, but some seem to be.

The other is a more clearly metal oriented end mill from APT (who very kindly suggest speeds and feeds on their site - a 1mm end mill should run at 20,000 in steel, but I guess 19,000 is close enough). The cutting part in this case is around 5mm.

I've had the joy of breaking a number of the amazon end mills and one of my two APT mills.

I can't quite work out what is the trigger for breaking and end mill. In one test I made a slot in steel 3mm deep, 1mm across and 15mm long with no problems (about 0.3mm DOC). In other tests I am less aggressive (so I think) and 'sping|' away goes the cutter.

Best success so far (relatively speaking) was cutting a 0.4mm deep slot across about 30mm of aluminium (1mm wide) with the APT cutter. This went fine (see later), but right at the end of the slot as it immerged from the metal,'Sping!', the APT one went.

One thing what was disturbing with APT one was a strong signing. If I move the bed slowly it would be intermittent (so contacting the metal, rebounding, contacting and so on). going faster the singing was consistent.

I think that this was mainly due to the stick out of the mill. The barrel is very long and hits the end of the collet internal bore. With my next one I will shorten the barrel.

I'm really looking for general advice on this. Are the cheap cutters really going to work on steel? Should I just buy lots of mills as they will break?

I should say that the mill is substantial (for a hobby - a VM32L, around 240KG) but manual, so my irregular handle turning may be a factor.

Hope this makes some sense.

Iain

So far I've tried to use two types of (carbide) end mills. There's one sort readily available on Amazon which has a 1/8th barrel and quite a long cutting part (so perhaps 1mmx 20mm or so). It's not always clear if these are meant to mill metal, but some seem to be.

The sound like they would fit my wood router.

There was CNC workshop over the road from my final workplace, you could hear the singing clearly in our office.

Armchair suggestions from me I'm afraid!

Looking at a few Amazon adverts gave me no confidence these tiny cutters are for metal, and, though that wouldn't stop me, I'd expect them to be fragile. Any small error will probably break them.

• Is there any wobble? A tiny off-axis error would put enormous stress on a 1mm mill.
• A real CNC machine may be important. People turning lead-screws are clumsy oafs compared with a CNC machine, and manual mills have much more backlash than CNC ball-screws. Backlash on a manual mill spinning a hefty cutter doesn't matter much, but the same movement might be deadly to a weak one. A 19000rpm spindle is a good start, but moving a tiny milling cutter XYZ manually might be too rough for it.

Keep trying. More practice might help. I suspect it's a skill akin to parting off on a small lathe, where a steady hand and spot-on cutting rate are essential.

Dave

Edited By SillyOldDuffer on 21/06/2023 17:58:51

This is a classic symptom of using a 4 flute end mill to cut a slot, instead of a 2 flute slot drill. Due to a weird quirk of the geometry, as the cutter emerges through that last breakout at the end of the slot, forces on the cutting edges are uneven and "Ping" away she goes. WIll even do it on a 12mm diameter cutter if you are not careful.

As teh below sketch from one of GH Thomas's books shows, with a four flute cutter, two cutting edges are in contact with the job at once, the forward one , No 1, is exerting extra side pressure on the cutter, pushing tooth 2 into the job, causing the cutter to break. It gets worse as the cutter breaks through the end of the slot and tooth 1 catches on the sharp edge where metal meets air.

Try using 2 (or maybe 3) flute slot drills instead of 4 flute end mill cutters. Only one cutting edge at a time is then in contact with the job and the above problem eliminated.

It's counterintuitive because a 2 flute slot drill looks spindlier and weaker than a 4 flute end mill, but cutting slots is what slot drills were made for, for this reason.

Also, of course, lock all your slides except the one in use for feed. And push your hand against the end of the table against the direction of feed to help stop the cutter from grabbing the job and pulling it into the cutter as it breaks through the end of the slot.

Edited By Hopper on 22/06/2023 02:16:41

Edited By Hopper on 22/06/2023 02:20:09

The ones with the 20mm flute length with 1/8" shank sound more like PCB cutters than ones specifically for metal.

You don't say if you have different types of cutter from APT for steel (coated) and Aluminium (uncoste) or what the flute count is.

As Hopper mentions for slots you really want 2 or 3 flute not a 4-flute "end mill" due to the cutter flexing to one side.

Your biggest cause of cutters breaking will be hand feeding and backlash and keeping the cut free from swarf

For the very small the chip loads are also very small so feeds need to be correct and constant Note that APT give speeds of the 3 & 4 flute cutters for side milling, when cutting a slot you need to reduce by upto 70%  so even with your high speed spindle you may only want 50mm feed on a 3-flute cutter which is quite hard to keep constant. Any runout in the setup will also have far more effect as the smaller chip load could exceed the run out very easily so you are only using one flute, as chip load increases runout will play less of a part. Other makers give even less DOC for their cutters of this size, YG-! for example suggest0.15 x D which half of what you are using 

Your snap on exit could well be due to backlash with the tool catching as it broke out.

Swarf in the cut will not only blunt the tool as it is recut but can deflect it so good air blast or liquid flow to was it out. Don't be fooled by those that say it's acceptable to machine under a pile of swarf that is due to other restrictions such as noise they impose on themselves.

Cutter type, it is better to use an aluminium/nonferrous specific cutter for aluminium as they have a polished and uncoated surface which is less likely to form a build up of metal, some lubrication should be used if you don't have full flood coolant such as paraffin or WD40 applied by brush or with a fogbuster type setup. The non ferrous cutters also have a different helix angle which helps get the greater amount of swarf out of teh slot.

Edited By JasonB on 22/06/2023 07:19:58

Cutting parameters are over-ambitious. I use YG cutters from Cutwel and they recommend 14750rpm for a 1mm cutter in low carbon steel with a feedrate of 75mm/min and maximum DOC of 0.2mm for slotting.

By far and away the biggest problem will be maintaining a smooth, and constant, feedrate. With small cutters chip loads are a few tenths at most and it is only too easy to exceed that. It only needs to be exceeded for a fraction of a turn of the cutter to break said cutter. I hate using small cutters (<3mm) on my manual mill and do my best to avoid it. Spindle runout needs to be less than the typical chip loads.

When I made this "nameplate" in steel on the CNC mill, with a 0.5mm diameter cutter I started with cutters from Drill Service. Even so they both broke part way through:

I swapped to YG cutters from Cutwel and one cutter did both parts without breaking. I have just used the same cutter to make two nameplates in engraving brass, running at 24000rpm, again without a problem.There is no substitute for quality cutters.

I use flood coolant on the CNC mill, primarily to wash away the swarf.

Andrew

Ian

I think you were doing well to hand feed such small high speed cutters at all on an ordinary mill of that size. Hand feeding is a right pain even on something designed for that sot of thing such as a BCA.

Possibly the worst issue is having no feedback at all from the cutter. You are always working against the inherent drag of the slides which is never exactly constant so its incredibly difficult to keep the feed truly even,

Best bet would be to arrange some sort of power feed. Wouldn't need to be terribly sophisticated. Simple belt drive to a pulley from some sort of variable speed motor.

I'd be looking at cannibalising an older two speed battery operated drill being disposed of because the batteries are kaput and new ones either un-obtainium or way too expensive. Cheap DC power supply off E-Bay or whatever will run it just fine. OK the durability of a drill motor isn't going to be up to what we consider machine tool standards but it should last a useful time and the supply is more than ample.

I'm sure I've seen "look what I made" pictures of such on the internet, maybe even a how to article.

Clive

I use Proxxon carbide milling cutters in a Proxxon MF70 (max speed 20 000rpm).

PROXXON 3 Piece Tungsten Milling Cutter Set | Axminster Tools

These work well on brass, aluminium and steel. I have cut keyways in moderate carbon steel (ST50) and milled rockers from keysteel (C45k).

There are some pictures in my album MF70.

Firstly, many thanks for the various answers, which were helpful.

My main take-aways were to lower the speed and DOC a bit and to avoid slot milling!

I set to and did my first attempt at what I'm (ultimately) trying to make. that being watch hands. the image below is the result.,

I ended up using a 2mm cutter for this item. The first step was to thin it down from 1mm to about 0.25 except around the boss you can see. Then to finish the rough square on the rotary table down to 2.5mm and drill the centre to 1.9mm.

Although the thickness is ended up at about 0.3mm, I@m more than happy for this as a first attempt. I had expected to use the smaller cutter to actual carve out the hand shape (which is essentially a rectangle with arcs where the boss is) but I realised I'd not got all the measurements I need on my drawing. Plus, I definitely felt that I should quite whilst I was ahead.

For those interested, I started by squaring (well two faces) some 6mm ally on the mill, then bolted it to the rotary table more or less in the middle. Then mill the centre to ensure that it was still square.

Next to make some slots to absorb any excess superglue (initially with the 1mm slot drills, but that turned out not work so well - see earlier posts!).

Deburr, clean and then stick a piece of 1mm thick 5x10 carbon steel in roughly the centre. You can see that I was quite a bit out!. Add some weights and leave till the next day.

Trim round the central boss .02mm or so oversize and down to 0.25 mm (target is 0.22, but will need polishing etc), then turn round the boss using the rotary table and finally centre and drill the boss to 1.9mm.

Given that the mill end diameter is 2mm you can see how small this is!

All in all this has gone much better than I expected. Probably next step is cut out and file to shape (with VERY fine blades) and if it's not broken by then, polish and heat treat. I suspect, however that this will not end up being the final hand - I have so MANY mistakes to make yet!

Iain

Am I missing something as I can't see why a small cutter would be needed to thin the material, trim to o/a size and form the round boss?

A couple of reasons. One is that a larger cutter has more force and is likely to take the piece off the superglue chuck fixture. At least it has for me in the past.

Second, the intent was (and perhaps is) to take the remainder of the metal away leaving the hand in place. Shaping this will require a finer cut than a bigger mill will do (the hand is narrower than the boss). As per the above, I've not got to that part yet

However, at least the thinning is tedious and it would be worth experimenting with a larger cutter, though previous attempts have not gone well.

Iain

Anyway, it's nice to have a new toy to play with.

Iain

Iain, it very much comes down to chip loading and DOC as to how much force is being created. Similar depths of cut and stepover could still have been used with a larger cutter and you could even have used the same chip loading. Small parts with a hole in them suit having the hole done first so you can then drill and tap the subplate to take a screw which will add a lot of security to the part.

As for external profiling or pockets of any part the only thing that really influences the diameter of the cutter is any internal corners as a tighter corner needs a smaller cutter so you don't end up with a large fillet. Even then roughing can be done with a larger cutter and then you can go back in with the smaller one to clean out the corners and do the final profile

Ian, I have to makes some clock hands soon and was thinking of a similar approach. What steel are you using please?

I have successfully milled 10t pinions into the end of a FC steel bar running a carbide 1mm slot drill at 5000rpm, taking it slow, so high speeds are not necessarily needed. Have you considered adding holding tabs and linking the hand shape to a larger surrounding area to reduce the risk of the superglue bond breaking? Obviously you have to file the tabs off at the end but a bit of added security.

HI, John.

I'm using Carbon steel from Cousins. It's available in sizes from 0.8mm and up. Carbon steel of course so it can be hardened and blues.

The actual hand is around 2mm across and 13 or so mm long. the piece I milled was about 10x20 mm for exactly that reason.

Not entirely sure how you are milling pinions with a slot drill - would that not be an incorrect profile?

Cheers!

Iain

Back in my working life I occasionally hand carved odd tools or items using my high speed dental handpiece. Those run at 300,000 rpm upwards and water cooled. If you were to be doing a lot of shallow narrow cuts as you describe then cobbling something like that together is worthy of consideration. Cheap handpieces aren't pricey and would run off a compressor and water reservoir hung from the ceiling. And dental drills are cheap enough.

Pgk

When doing gears on as 3 axis CNC you do it with the blank laid flat and the small cutter runs around the outside forming each tooth. As I mentioned above the limiting factor is again the root at the bottom of the tooth, this is why it suits the relatively thin gears of a clock rather than thicker ones where you run out of flute length on the small dia cutters

Thanks for the info Iain.

As Jason says...

Basically profiling into the end of a bar, then parting off. Under power of course...

Dunno if this is helpful....

but in my limited experience of manual machining, smoothly turning handles makes for a happy operator & a better finish.

Any work done to your machine that makes your handles turn more smoothly is time well spent IMO.

Hi Iain, a very interesting post, and answers from everyone.In the past I have done a few thin piece milling as you mention, but found super glue too fail.Even if the metal is clean and surface prepared. This might not help but soft solder is a much preferred, as the attachment medium to the workblock.If you tin each surface first ,after cleaning, with a thin layer then sweat the two, finally pushing down with a flat block to seat it. A bit of practice... then when the job is done separate with heat. Ok the drawback is solder, but it is only a thin layer. That way bigger profile cutters could be used to rough out., Much stronger than super glue.. old hands used melting shellac which work much the same...which has been in me or mew which I could find if you need it. The cutter flute length could be a factor for slotting as well, my small 2 flute are very short , rather than the long carbide ones you mention.

. Chemical milling was used for small parts, and I think the profile and size would be a perfect candidate, but mainly brass for clock hands. I have seen small CNC doing this work, running 25,000 revs but it is axis feed control, even they broke cutters at times. So your steady hand feed is well controlled!.good luck!

Vic