2mm endmill help

[old martParticipant @oldmart]

It was harder than I expected to find a source of relatively inexpensive 3mm cutters with a 3mm shank, they commonly have bigger. Cutwel have some on special offer which are coated for steel, but not intended for hardened steel. I hope the link won't get me into trouble.

**LINK**

[Anonymous]

Posted by old mart on 25/06/2020 13:32:14:

A J, your picture shows a 2mm slot drill, but the shank is al least 4mm.

A quick visual comparison with the rule in the picture will show that the shank is 3mm.

My apologies for not reading the thread sufficiently well to realise that an expert had already expounded. At least crawling back into my cave will be some relief from the heat.

Andrew

[old martParticipant @oldmart]

Sorry, Andrew, I thought it was bigger, I blame the heat, 33.8C at the moment. The cutting length on your example would be ideal.

[Andy CarlsonParticipant @andycarlson18141]

I'd be interested in your Z axis setup Dave. Mine is only CNC in X and Y just now and the Z is on the 'to do' list.

My first job is to deal with the thrust bearing. The factory design seems to involve the handwheel dial slowly eroding its way into the moulding at the top of the pillar coupled with (on my example) a heap of backlash. A simple metal washer would probably be an improvement but I'm wondering if I can fit in a roller thrust bearing.

At the moment I'm making a box spanner to get at the Z axis adjuster nut.

A pic of my 'X' axis drive below. I've gone for a very 'low impact' conversion using handwheel cups and I can revert to manual operation in a few minutes per axis. Apart from keeping my options open I also need to take the 'Y' drive off easily in order to fit the MF70 back onto the shelf which it shares with a Cowells lathe and a Unimat SL.

[mickParticipant @mick65121]

I've had my little Seig KX1 for ten years and now wouldn't be without it. I constantly use small diameter solid carbide cutters ranging from 1mm up to 6mm dia. The Mach3 control has excellent conversational programming, where you select the material, tool type and diameter and it calculates speed and chip load (feed) In my experience its the depth of cut that snaps small diameter cutters rather than the feed rate. Write a simple sub routine and vary the cutter depths and see how you get on.

[Dave SParticipant @daves59043]

My conversion was done when I had little money, so its scavenged bits from printers and hacked together mounts. The handles are in the mill box, shoudl I ever be mad enough to want to use it manually – I really like my TOS, even for tiny things.

Overview shot, please excuse last nights swarf and spanners…

The X and Y ends have been replaced with alloy, which have pockets for the bearings to sit in. They are held there only be the lead screw tension. I had to turn a couple of adaptors to fit the inside bearing bore – where the leadscrew is thinner for the handle mount.

For the Z – because the lead screw is just 'hanging' I made a new top from bike crank arm with a pocket for back to back magneto bearings:

The top plate is held on with the original screws, which are a bit long at the front, but at the back they also hold the stepper mount piece – scavenged from an old dot matrix printier IIRC.

IT all looks a bit heath robinson, but the motion part seems to work ok. I built the stepper control box and PSU – this was before simple availability from China.

If you want any more details info just ask.

Dave

[Dave SParticipant @daves59043]

I did some looking at my mills. The 2mm is about 10mm flute length, the real killer I think is the shank length:

Fresh one, last nights snapped one and the proxxon collet. The spindle bore is solid about 1/2 mm from the collet end, so you can see in the next photo how much extra stick out there was because of shank lenght:

Thats about 8mm extra, nearly doubling the stickout.

I also bought 3mm and 1mm, and they also have super long shanks compared to collet length.

Ive chopped a 2mm down (I bought 3 2mm as its the size I'll mostly be snapping using) so I can give that a go with revised tool paths tonight (SWMBO permitting)

Dave

[Andy CarlsonParticipant @andycarlson18141]

Thanks for the pics Dave. Good to see how other people tackle the same question. I admire your upcycling ability. Whenever I look at the things I've kept in case they 'come in useful' I mostly just see a load of old cr*p.

I think my cutters are all 40mm long. I must see about getting something that can shorten one. At the moment I'm pretty sure that I don't have anything that will touch carbide.

[Anonymous]

Posted by old mart on 25/06/2020 14:47:38:

………I blame the heat, 33.8C at the moment.

Man, that's hot. Higher than Heathrow reported today I think. One normally expects airports to be slightly hotter than the surrounding areas due to all the engines pumping out hot gases. But not at the moment. I went down to Stansted yesterday to renew my Civil Aviation Authority medical. Never seen it so quiet. Very few cars and no buses around the terminal building and the long term car park was empty.

Andrew

[old martParticipant @oldmart]

The cheap mini diamond files in wallets will score carbide easily, get the cheapest out there. The ideal length would be about 1mm of plain shank projecting when the collet is tightened.

The temperature has gone down now (21:10) to a mere 27.7C.

[Dave SParticipant @daves59043]

Sad news, another 2mm endmill has been sacrificed to the cause of getting my CNC to work.

I used Jason's suggested toolpath – although I did re-generate it first as I moved the work coordinates.
However the basics were as he suggested: 0.2mm engagement, much greater DoC.

It all started promisingly:

And it made a couple of the passes all round to the back side before I was called to eat:

During the meal I was keeping a ear out, and when it all went silent I returned, mid meal(!) to discover an ex-endmill

So I paused the machine, and went and finished my steak and had a beer.
Seem the most productive thing to do at that point…

On the plus side the swarf looks more 'swarfy' than last time:

I put the part under the microscope, this is where it snapped from the side:

You can see the not quite left the metal cut that was in progress.
From the top there is no obvious extra width of cut:

I managed to find the end of the endmill from where it had been thrown behind the lathe.
It shows a single tooth has more wear that the other 2, and one of the other 2 appears to be poorly formed in the first place, or possibly chipped – its very hard to tell.

For comparison here is the last unused 2mm, not snapped one:

The edges on that however look distinctly rubbish compared to the 1mm Kyocera mill

After a serious dose of thinking about it I measured the runout on the tool – using the as yet unsnapped 2mm which has a long shank – ideal for an indicator to run on. approx 0.076 mm (a little over 3 thou). With a toolpath supposed to take a side cut of 0.2mm this is quite a significant change in cut load per rev I think.

I also checked with a 3mm tool, in case it was the collet – same result, so I guess that's the natural spindle runout.
I think I need less runout than that to successfully use tiny mills – certainly if I put in a 1mm end mill and the runout is nearly 10% diameter that sounds bad.

Should I formulate a new spindle plan at this point?

Dave

[Tony Pratt 1Participant @tonypratt1]

Your cutter is a long way out.

Tony

[Martin ConnellyParticipant @martinconnelly55370]

The recommended depth of cut was 0.2mm not 2.0mm. Lots of small passes with the correct speeds and feeds and overlap of about 1mm (50%) as a starting point. Make the tool last to the end of the job.

Martin C

Edited By Martin Connelly on 26/06/2020 12:34:04

[JasonBModerator @jasonb]

Looks like it was cutting as I suggested 0.2mm stepover eg 0.1 X D and height was 1.4mm (0.1mm axial stock left for cleanup) height of features is 1.5mm

[Dave SParticipant @daves59043]

Yes, as suggested by Jason – engaging more of the flute length in the cut, but with shallowed stepover. It felt like that was a sensible thing to try – it spreads the wear over more of the cutter – rather than relying on just the tips.

Sort of like vertical slab milling (if you squint a bit)

Dave

[Andy CarlsonParticipant @andycarlson18141]

Hi Dave,

Sorry to hear that another cutter has bitten the dust.

I checked the runout on a cutter in my spindle. I got 2.4 thou. Not great I realise… but the thing is you are breaking cutters for passtime (as my gran used to say) and I've just cut a 10mm hex (in stages) about 6mm deep in a lump of brass.

Your post doesn't say what DoC you used but in the short term I can only suggest a smaller DoC – I used 0.2mm for my most recent job but I think I've used 0.25mm with steel in the past.

I did some more measurements on my MF70…

I clocked the top of the collet holder 'nut' and got around 2.4 thou again. I'm not sure how meaningful that is though – the outside of my ER16 nut on the Unimat runs out appallingly but things held in the collet have sub 0.5 thou TIR.

The spindle has almost no room to put the DTI probe on but I tried anyway right at the top of the threads and got about 0.5 thou.

I checked inside the taper of the collet holder and got 0.7 thou.

I borrowed a 3mm collet from another Proxxon set. That made no difference.

I looked at borrowing another nut but none of the others have the flats for tightening in the miller.

Finally (should have done this earlier) I did some more paranoid than usual cleaning of the holder and nut with half a cotton bud. I did find some swarf hiding inside the nut but the runout was not improved by cleaning.

So it looks like (on my MF70) the spindle is contributing some runout and the collet nut and/or collet is adding a good deal more.

All of which explains why my 2mm cutter is effectively cutting a diameter of 2.1mm.

This does make me think a bit more about an ER11 spindle conversion but at the moment my MF70 is doing the job for me and my 'to do' list is already long and distinguished.

Regards, Andy

[Dave SParticipant @daves59043]

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

[JasonBModerator @jasonb]

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.

[JasonBModerator @jasonb]

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

 

This shows that the depth and width can be cut but the machine/tool is more likely where the problem is

 

Couple of extra photos – straight after cutting

 

 

Thin tabs

 

 

 

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

[mickParticipant @mick65121]

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.

[Andy CarlsonParticipant @andycarlson18141]

@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.

[JasonBModerator @jasonb]

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.

[JasonBModerator @jasonb]

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.

[Dave SParticipant @daves59043]

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

[Andy CarlsonParticipant @andycarlson18141]

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

[Author]

Posts