Will it take larger sizes? 3 and 4mm are much stronger and well able to use the speed of your machine.

Hi Dave I've got a Sieg KX1 CNC and tend to cut steel like it's made of kryptonite! So I usually take it easy and slow until I am confident with the progress. For a 2mm cutter I would start out like you, but at 20% or less of 100mm / min at about 3000 rpm, tweaking the feed rate and rpm as the job progresses. Depth of cut sounds about right. The KX1 max speed is 7000 rpm which I very rarely use, 10-15,000 revs seems a bit too high, could be causing vibration.

Having said all the above I find recommended feeds and speeds to be totally irrelevant and meaningless, and i ignore them, because in the home workshop it all depends on the machine, rigidity, quality of tooling and material. Just go with what feels and sounds right for you. If it's wrong the machine will quickly tell you!

IanJ

Dave, I've owned a bog standard MF-70 for around fifteen years.

Although your spindle speed sounds about right for mild steel [I'm assuming that's what you're cutting], a 0.5mm DoC at 50mm/min strikes me as a little ambitious, chiefly because the motor has so little power and the machine lacks the mass that helps create the stability/rigidity that carbide calls for. There's a fine line between snapping and rubbing cutters with this machine, I'm afraid.

Your setup is very similar to mine Dave except I use Marlin firmware. I've snapped several 1mm cutters (I use this size more often and it's inherently weaker) but so far (touch wood) the 2mm and 3mm Proxxon cutters have survived OK including several jobs with 3m on steel.

As far as the theory of what should work and what should not I have no idea but right now I'm cutting brass at 40mm/min with 0.2mm DOC on a 2mm Proxxon cutter. 0.25 DOC is probably about as far as I've gone with steel and this was before I did CNC but the feed was probably around 40 or 50 mm/min.

I have also tried some cheap chinese 3mm cutters. They did OK while I was practicing on Aluminium but the difference between them and the Proxxon ones on steel was like chalk and cheese.

For those unfamiliar with the MF70 the collets only go up to 3.2mm and the speed dial covers 5-20K RPM. It is a very small machine and I'm sure would attract scorn from many on here but it fits on a shelf indoors and is fine for what I bought it for (scratchbuilding 2mm scale locos). When I was looking to buy it I really couldn't find anything else at this size and price.

Friends have fitted a spindle conversion that allows an ER11 collet holder (from Usovo I think) to their machines. Same friends have also reported broken MF70s on occasions which may be unrelated but I'm not tempted to do this myself. One friend is also in the process of remotoring her MF70 to allow slower speeds – I certainly find the speeds too high when using 2 or 3mm drills.

Here's the calculation for your chip load (advance of the tool per pass of the cutter tooth).

Chip load is travel speed/flutes x rpm. Taking the possible top speed of 15000rpm and travel speed of 50mm/minute and assuming a 3 flute cutter that gives 50/(3 x 15000) = 0.00125mm per tooth per pass. That is definitely rubbing territory. Let's go for 10000rpm and 2 flutes and you get 0.0025mm per tooth per pass. Still in rubbing territory.

So babying the feed but too aggressive on the depth of cut seems like the summary from previous posts and this calculation.

Does the supplier or manufacturer of the cutter have data for it? It would help avoid breakages. If not then the Little Machine Shop feeds and speeds calculator would be worth checking out.

Martin C

Little Machine Shop calculator

Link added

Edited By Martin Connelly on 25/06/2020 09:08:29

Hi Dave,

I regularly cut brass and steel on my 3040 CNC router with 1 and 1.5mm end mills.

I hope you don't mind me making some observations:

1) your end mills seem to have really long flute sections and stick out from the chuck a fair way. This will increase chatter and increase the risk of them breaking. Unless you need the increased flute length, I'd suggest something with shorter flutes and a thicker shank. I've had good luck with these

2) You seem to be taking full width cuts. If I do this with small end mills, it tends to be because I am cutting out something like a clock wheel and want to use the CNC as a kind of scroll saw. In this case I find that a depth of cut of 0.2mm is all I can handle before tool breakage.

For facing and adaptive clearing operations I tend to run with a width of cut at just under 1/2 the diameter of the end mill I'm using.The setting for this is under the "passes" tab in the toolpath in fusion 360 and will be called "stepover" or "optimal load" depending on which type of operation you are doing.

3) assuming you are running a 2mm, 2 flute end mill at 0.9mm stepover and 15k rpm the minimum feed rate you should use (according to g-wizard) is 107mm/min. Any less than that may give rubbing. for a 3 flute this goes up to 161mm/min. Personally I'd be tempted to back the speed down to 10k rpm and use 70mm/min for 2 flutes and 107mm/min for 3 flute.

once you have settings that work, you can then play with increasing feeds and rpms!

good luck

ro

Edited By Ro on 25/06/2020 09:19:17

The late great Sir John made "Carriers" to allow the minimal amount of cutting length to be presented to the material to be cut. Even with super sharp cutters, long wobbly flutes bode for tears before bedtime.

Regards Ian.

You can always cut the end off the shank with something like a Dremel cut off tool so you can just have the flutes exposed. I'd also go for a short or standard series cutter so you should be able to get a 5-6mm flute length no problem.

I think F360 defaults to 90% cutter width, I tend to use 60-65% on a surfacing cut but on your test piece would more likely go full height but 10% of cutter width on a small cutter like that.

Definately would not be wanting burrs like that which usually indicates a cutter that has become blunt or is otherwise not cutting as iy should.

F360 allows the file to be shared, if you post a like I'll set it as if I were cutting than you can look at that to compare. If you go to top left Icon, select "Share" and then "public link"

I've definitely found that DOC makes the difference between horrid burrs and virtually no burrs so hopefully that will be true for you too.

I'll be interested to know your plans regarding backlash compensation. This was the reason I switched from GRBL to Marlin. Marlin is in many ways an odd choice for milling but it did allow me to do backlash compensation and stay with the Arduino CNC shield that I already had.

FWIW the Marlin backlash compensation setup for my MF70 that I reached after experimentation is…

M425 X0.094 M425 Y0.085 (backlash comp)
M425 F1 (backlash comp ON)

I also compensate by using a fudged cutter diameter (typically 0.1mm higher give or take a bit) when generating the G code – the cutter seems to cut slightly bigger than its nominal diameter. This is unrelated to backlash – my best theory is that it is down to flexing.

3.2mm max shank size in the standard Proxxon collet.

Go for stub length 3.2mm (1/18&quot solid carbide cutters, if the shanks are too long, then score right round the shank with a diamond file and snap them off. If you put the cutter flute end down in a vise with soft aluminium jaw protectors and put a tube over the unwanted end, they will normally snap off very well.

As said I'd use more of the side of the tool cutting 0.1 x D on the climb and 0.05D on the conventional using both way clearing then a wider pass to take the axial clearance off which will leave less tool marks on the bottom. I also increased the size/number of shapes as not much point in machining away lots of metal just for a test. You will see that my cutting speed has gone up as side cutting like this will allow you to run almost twice as fast

Try it here

A 3mm cutter could have been used on that part which would be stronger and would be my preference.