2mm endmill help

I sort of expected to break a few things on the learning path, but I was hoping it wouldn't all be at the start....

I clocked the runout on the shank of a cutter held in the collet where it exits the spindle. As I did this with 2 different sized collets I assumed it was the spindle, but maybe all my collets are a bit 'wonky'

Ill clock the actual nose tonight.

Does your spindle feel 'steppy' when turned by had - way stiffer than it fells like it should be? I assume this is cogging on the spindle motor, so if another one does then Ill ignore that.

Might also try a different lump of steel. My other mill has not trouble with this stuff, but then is full sized industrial and I rarely use less than 6mm dia cutters on it - its top speed is about 4500 RPM.

Dave

For Clarity Dave's original cuts were going 0.5mm deep with the initial cut at full 2.0mm width and subsequent ones at 90% stepover of 1.9mm so taking the later 0.95mm2 area of metal being removed and high cutter engagement particularly the first cut and at ends of the path

The path I suggested was 0.2mm stepover (sideways DOC) and 1.4mm hight of cut (Vertical DOC) so only 0.28mm2 removed per pass which is 30% of Dave's original load and makes better use of the available cutting edges rather than just blunt the end..

I'm inclined to put it down to the machine and tool, tool even when gripped right down to the flutes has long stickout and the reported runout may be even worse at the cutting end. Add to that some backlash in this basic screws/nuts and low rigidity of a very small machine. I'm just uploading a video of something cut with a 2mm cutter this morning and that would seem to confirm this.

I had something to cut with a 2mm cutter so took a video.

Cut is very much like Dave's original being full width and in this case 0.6mm deep as that was the thickness of the steel. Cutter is a HSS 3-flute FC-3 "throw away" type by Hertel running at 5000rpm which is my max. I started with a modest 60mm/min feed doing the central bore which showed I could go faster so the video does half at 72mm/min and then I override more to 96mm/min which it was still happy with.

Path ramps down at a shallow 1deg and then follows around the job leaving 0.25mm, some burrs thrown up on this cut but it is a well used cutter, it then goes round again with a 0.25mm finishing cut which you can see removes the previous burr and leaves a good finish. My tabs were a bit thin as you will see but I was able to remachine with a screw in the middle. Finished item has just had a quick rub on some 150g Emery. Nice chips can be seen at 1.40 onwards

Thin tabs

Edited By JasonB on 26/06/2020 14:27:22

The cutter is way too far out of the collet. The collets look like pin chuck collets and would allow sideways movement. Can you fit a small ER collet to the spindle, you might have better results.

@Dave. Yes it does feel steppy. I'm pretty sure it's just the motor poles. I would not describe it as stiff though.

@Jason. Yes I understand. I'm not trying to argue with your suggestions... just saying what has worked for me.

Looking at your numbers it does look like the stress on the cutter should not be any higher than with my setup so it's puzzling why the cutter broke again.

The vast majority of my milling has been cutting around a profile... basically ploughing a furrow with the leading edges of the cutter, then move down by the DoC and repeat the same path. Dave's test job looks like it could be done with this style of milling with some additional 'colouring in' between the outlines.

My profiling goes 0.2mm deep and I have been using the full width of the cutter, so I suppose that adds up to more load than your numbers. My cuts with the 2mm cutter were all in brass though.

Having said that 40mm/min and 0.2mm DOC is also the setting I use with the 1mm cutter on brass... which mostly doesn't break. I think the last 1mm cutter that broke without additional assistance from silly mistakes was shortly after using it for profiling some phosphor bronze sheet at 40mm/min. I have resolved to reduce to 30mm/min for PB in future.

I do think these things have a 'stress life'. A couple of times mine have broken under light orin one case no load at all but after some considerable 'mileage'.

I can't offer so much concrete info from past experience using the side of the cutter more heavily but I have done a small amount of work using the 3mm cutter on steel in manual mode.

My memory is hazy on the depth of sideways cut I'm afraid, but would probably be no less than 0.1mm. The cut had about 5mm of height. The 3mm cutter will of course be a lot stronger than the 2mm one... it has more than double the cross sectional area.

Andy, not aimng my comments on you but someone said 2mm DOC was being used but did not look like it to me.

Yes your 0.2mm deep by 2mm wide would be a similar loading to my suggested option and again about 40% of Dave's. His path was very much like you describe cutting a slot and then removing material from each side, I'll see if I can do a screen cast of the two paths for those that did not open the F360 links.

This shows Dave's one first where the metal is removed in three 0.5mm layers using all or most of the width of the tool and a cleanup around the vertical faces. Followed by my alternative where almost full depth is removed in one go but with much less stepover then a final pass to clean up.

I have no idea how to drive a CNC, the little I did was many years ago. So I guessed a tool path, based on the few things I remembered being a typical clearing path as was.
I’ve never “run the numbers” as such on my manual mill, it’s built like a brick outhouse and being manual you can “feel” how the cut is going. It’s a while since I snapped a mill, iirc the last one was a 12mm rougher that I took an overly optimistic DOC into 316.

Im having a “family night” but hopefully some garage time at the weekend will allow me to try some more.

Ive already learnt loads and the video of a successful 2mm cut is encouragement.

If I’m being overly optimistic on my machines capacity maybe I need to rethink my longer term plan, but for now it’s the only CNC I’ve got.

Dave

Dave,

I think it depends on what you want to make on your mill.

Just in case you were having doubts whether useful work can be done on an MF70...

I bought mine to mill 2mm scale locomotive chassis. The biggest locomoties in our scale are about 6 inches long which fits the MF70's X axis travel. Several 2mm scale modellers use MF70s and a fair few locomotives have been turned out this way. Most of the bits in the photo below were cut out on the MF70. For scale the frames are 55mm long. They are 20 thou phosphor bronze and were sweated together and cut out as a pair with a 1mm cutter. The front frame spacer is brass, about 6mm thick and used a 2mm cutter. My notes say I used a 40mm/min, 6000 RPM and 0.5mm DoC for this part.

The tufnol rear spacer was done outdoors because of the nasty dust. I remember it well. It was the middle of winter, dark and cold.

Other folks have milled whole chassis from solid brass rather than using a spacer based design.

The main (flat) body panels were also cut from 10 thou brass on the MF70...

Sorry, no videos of actual milling from me though.

Edited By Andy Carlson on 26/06/2020 23:27:00

There seem to be three fundamental issues. Roughly in order of importance:

The new cutter shown seems to be poorly ground. The used cutter shown is badly worn with the cutting edges rounded. It would seem that these cutters are simply not up to machining steel.

Runout on the collets - it's way bigger than the chip load. So one tooth may not be cutting while the next will be taking double or more the expected cut. So the loads on the cutter are much higher than expected from simply looking at the rpm and feedrate. Varying chip load is also a recipe for vibration and chatter.

There is still quite a lot of cutter stick out. even with the shank cut down.

One and three could be ameliorated by buying quality cutters intended for cutting steel. Two is more difficult, short of acquiring a different mill. A good clean and check for any small burrs may help. Reducing the stick out of the cutter would also help.

Andrew

Trawling around the net yesterday I found a couple of other places where people reported similar runout figures from the MF70. The Usovo ER11 spindle conversion is an option. Their site (naturally!) claims very good precision but I have no experience of this conversion myself.

I will drop a line to the two folks who have done the conversion and see whether they have done any runout measurements. They may not - not everyone owns a DTI.

Cutter-wise, when I bought my MF70 I asked one of the folks who had milled several chassis which cutters he used and he told me that he had always stuck to the Proxxon ones. All of my 2mm and 3mm cutting has been with Proxxon cutters. That's not to say that other good cutters can't be had of course.

I've cast the net wider for 1mm cutters and have used Cobra Carbide since breaking my first Proxxon one. These are now unavailable from the UK eBay seller so that advice is not much use now.

.

It is interesting ... [‘though probably futile] to compare your excellent analysis with Proxxon’s product descriptions:

**LINK**

https://www.proxxon.com/en/micromot/27110.php

**LINK**

https://www.proxxon.com/en/micromot/28940.php

MichaelG.

Looking at those Proxxon cutters I would say by the angle of the helix that they are designed for non ferrous and plastics as they look to have about a 45deg helix and could very well have deeper gullets to clear swarf making them weaker.

How close is the fit between the parallel part of the collet and the bore it locates into in the spindle?

I found with my Dremel type hand tool that there was quite a bit of clearance here which caused significant runout of the cutter. I made new collets that fitted the bore closely and it helped tremendously in reducing runout. I used a drill shank to 'measure' the bore size.

Martin.

I had a bit of a look around for the shortest cutters and it turns out our friends at ARC have a couple of cutters that look like they would be upto the job.

Their Standard length Premium carbide3-flute at 2mm dia has a 6mm flute length and their stub length 2-flute an even better 3mm flute length, both have 3mm shanks. They are a bit more expensive than the Hertel but not far off the cost of Proxxon. May be worth a try though doing so after chasing down the runout may be a better bet for the wallet.

I managed to pull Ketan away from something far more important long enough to get a couple of photos.

@blowlamp: Interesting thought. Thanks. The collet mikes at 186.4 thou which seems suspiciously close to 3/16 for such a metric machine. My 3/16 brass bar mikes at 187 and is a fairly loose fit in the collet holder. I thought 5mm... My 5mm drill shank mikes at 194.4 thou (4.93mm) and won't go in. That's about exhausted my stock of things in this sze range. I might have a try making a new collet but my only slitting saws are too thick for that job so it won't be any time soon.

@Jason: I have just bought a 1mm stub cutter from Arc Euro but so far it has not been on the machine so I'm not able to say anything much about it. Any thoughts on how the geometry compares to the Proxxon ones?

If you can get some good dimensions of your collet, I could CNC one up for you to try if you think yours is slack.

Just let me know if you want one doing.

Martin.

If you look at the photo on ARC's site for the stub and standard length ones you can see that these cutters have the more traditional 30deg helix, compare this to one of their 45deg helix cutters for aluminium (& Non ferrous / plastic) and that looks far more like the geometry on the Proxxon ones suggesting they are more suitable for easier cutting materials.

Thanks but I think I will need to turn some bar on the lathe myself to find out what the internal size of the holder is. I tried wrapping some 2 thou shim around the collet. That wouldn't go in but that still leaves a big band of uncertainty.

Must say: I was astonished by the modest price of the Proxxon collet set.

MichaelG.