Milling Feed Speeds.

I have just acquired a new 10mm two flute slot mill for cutting aluminium.

Looking at the vendors (APT Tools) website they quote speeds for slot and side milling of 5000 rpm and Feed rate of 1200mm/min (slot) 1500mm/min for side milling at doc of 5mm (slot) 10mm(side).

The mill (SX1LP) will do 5000rpm, but I don't think there is any way I can crank the handwheels (2mm/rev) at 600/750 rpm. Am I misreading the data, or are these really the sort of speeds production grade machines achieve?

What are the implications of going far slowly on the feed (I would guess 100rpm 200mm/min is about as fast as I could crank). Should I reduce the rpm to match and to keep the tooth loading fairly constant, or just go for it?

Edited By Peter Cook 6 on 27/04/2021 14:25:18

Hi Peter,

Seems to me that the cutting data you quote are for industrial size milling machines, not a small SX1. My milling machine will not do 5000RPM, only about half of that and I still get a good surface with slower feed rates. Don't let the cutter rub, I would say go ahead and try on a piece of scrap aluminium and get some experience.

Thor

First question before you even try to crank that fast: Would your mill motor drive at that material removal rate? Somehow, I think you would stall the motor and likely break the cutter. Your reading skills are likely accurate - it’s just the understanding/interpretation parts that you have not thought through.

Those are fairly conservative numbers for aluminium in industry. The feedrate for slotting works out at 0.24mm per rev, ie, a chip load of 0.12mm. The feedrate for side milling is higher because the width of cut will be smaller, usually 0.1D in examples, and chip thinning will apply.

Running at a slower rpm and with a proportional feedrate will be fine. At high speeds and feeds the biggest problem will be getting rid of the swarf and stopping it sticking to the cutter.

Andrew

What I do is set the rpm to recommended speed and the depth of cut (DOC) to about 10% of tool diameter. Then I feed as fast as seems reasonable by ear. I listen to the motor and cutter for sounds of trouble. I like to hear the motor loaded but not labouring, the machine cutting rather than forcing it's way through the metal and definitely not rubbing because that blunts tools outrageously quickly. I don't like to stress my hobby mill by pushing it very hard even if the motor sounds OK: hobby mills are a bit bendy, and their innards may not take kindly to a gorilla at the controls! With carbide, I avoid red-hot chips even though this indicates good cutting because flaming metal is anti-social. Red-hot swarf coming off an HSS cutter is too hot; slow down.

Experiment if the cutter chatters or finish is poor. Often reducing RPM and increasing feed gets rid of chatter, but much depends on the set up, the material, and the cutter. Although there's usually a combination of rpm, doc, and feed that delivers don't be surprised if it doesn't match what the book says. In particular, hobby machines don't have the power and rigidity needed to deliver industrial work rates, nor do they need to.

My rule of thumb RPM = 10000 / diameter in mm, which is roughly right for mild-steel and HSS. Slower for Silver Steel and Stainless, bit faster for Brass, much faster for Aluminium. However, cutting speeds aren't all that critical provided the alloy is machinable.

Take account of the material. Machinable Mild steel like EN1A is markedly more tolerant than ordinary mild-steel, which cuts OK but tends to smear - poor finish. Certain metals, like some Stainless Steels, need to be close to target, usually because if not treated correctly they work-harden and damage the cutter. In my opinion unknown scrap is best avoided by beginners because so many metals don't machine well at all - some are truly horrible causing massive trainee confusion, especially if self-taught. You can guess how I know scrap can be uncooperative, but not that it took me months to realise my collection of cheapskate metal was total carp. All of it! Problem fixed by buying the right thing.

Dave

I doubt the small mill will like a 0.12mm chip load, more likely it will be happier with 0.02mm or even less depending on DOC so that 1200mm/min soon comes down to 200mm per min.

On my KX3 I tend to run a 10mm Ali 2-flute at 4000rpm and feed of 300mm/min and it will happily run like that, bit less if slotting..

Thanks. I was a bit put off by the implied speeds. But I have clearly been being far too tentative - even on my little mill.

I just experimented with a piece of aluminium ( to make HH's square tool holder for the grinding rest). New two flute cutter, WD40 lube, 2.5mm doc, 4000 rpm and crank as fast as I reasonably could. Probably 60-100mm/minute feed rate.

Hot knife and butter came to mind and the surface finish is way better than I have been getting with my tentative approach.

More learning undertaken!! Isn't this hobby fun.

Sod, interesting. Your depth of cut seems a bit shy, but the rpm=. 10000/ cutter dia gives 1666 rpm, the presto data for slot drills gives 1592 rpm - very close. - with a feed of 0.023 mm per rev but only 73 mm/min . So your figures give a very good speed basis
for a 10 mm cutter, yours, = 1000 rpm, presto 955 Feed 92mm/min So your easy calculation is sound, but gives a speed just a bit too high

the recommended depth of cut is 1/2 diameter (slot drill diameter for end mill) but that of course depends on your machine. No probs in my Bridgeport, but too much for my Sieg sx2+ cnc conversion

my numbers refer to an HSS cutter, for carbide, the numbers would be  3988 rpm   With 0.038 cut per tooth  = 285  mm/min.   So it seems the op quoted numbers are a quite a bit on the high side! As I also have seen from the vendor

Edited By Zan on 27/04/2021 19:26:29

Edited By Zan on 27/04/2021 19:30:32

Little Machine Shop has a nice feed/speed calculator:

**LINK**

That's a valuable lesson. One doesn't need to run at industrial speeds and feeds but it is surprising what can be done. Being too cautious can be worse than being gung-ho as the tool rubs, and that's a surefire way to damage a cutter. Of course some people (no names. no pack drill) will say my advice is irrelevant since my manual vertical mill is a Bridgeport. But consider this - it's only 1.5hp, or 1100W. That's on a par with many of the mid-size hobby mills. Another important lesson is that cutters are consumables. Pussyfooting them to extend life often has the opposite effect.

On another matter when quoting speeds and feeds for slotting in softer materials such as cast iron and aluminium and copper alloys manufacturers often use a depth of cut of D, reducing the depth to 0.5D for harder materials such as steels.

Andrew

My first mill was a Victoria U0 universal horizontal with a vertical head driven from the horizontal arbor point, the VH doubled the speed from the arbor drive but then it was only 1000rpm.

Advice I was given at the time was for 1/2" HSS 4 flute milling cutter was DOC = Diameter, stepover 1/4xD.
Spindle speed was max spindle speed in ally and around 600 for mild steel.

There were a good range of X axis feeds and selected those that worked after trialling.
Still work with DOC=cutter diameter and stepover = 1/4 cutter diameter.

Emgee

rpm = 10000 / cutter dia(mm) is more scientific than it looks. The approximation works thus:

Cutting speed = Circumference x rpm

∴ Cutting speed = π x diameter x rpm

∴ RPM = Cutting Speed / π x diameter

The magic! It happens that a sensible a sensible cutting speed for for mild steel is about 30 metres per minute, so in millimetres:

RPM = 30 * 1000 / π x diameter

∴ RPM = 30000 / 3.14 x diameter

By making π = 3, the sum simplifies via

RPM = 30000 / 3 x diameter

to:

RPM = 10000 / diameter

This is 'good enough' for most purposes.

Next stage is to notice from the graph mentioned above that Aluminium cuts about 4x faster than mild-steel, Brass about 2x faster, Cast Iron, Medium Carbon Steel & Bronze about 20% slower, and harder steels cut at about 1/3rd the speed of mild-steel. Again, applying the correction for other metals as a multiplier produces an RPM reasonably close to the book answer.

Much easier to remember than to look up surface feet per minute and plough through the maths properly especially as practical cutting speeds depend so much on the machine and it's condition. As the working range of cutting speeds is bigger than the mathematical error caused by the approximation, 10000/dia is a quick off the cuff way of getting close without a lot of faff.

Dave plowing throu

Edited By SillyOldDuffer on 28/04/2021 11:48:17

Pure aluminium is for extruding into coke cans and not for cutting. You get ghastly burrs around the cut edge.

High helix cutters, extremely rigid machinery and flood coolant help a bit.

Such fun. But let's hope your "aluminium" is a more cut-able alloy with things like copper, manganese and magnesium added. Extruded bar cuts a treat.

If you are planning to cut any distance at one particular depth remember that the aluminium oxide surface layer is grinding paste which will cut a groove in the edge of your tool if you localise it.

I just bought some cheap "aluminium" plate off e-Bay to make a belt guard. Thought I would cut front and back from sheet, 3D print the sides. Hopefully not pure Al but I am sorting through my fancy cutter box just in case...

The bar I was using was sold to me as 6082 alloy, and it does appear to machine well - now that I have got a bit more aggressive with it!

The tip about the surface layer is something that I had not realised - again thank you, and all the rest of the helpful people on this forum.

It was just the concept of hand cranking at 750rpm that initially blew me away!

Edited By Peter Cook 6 on 28/04/2021 14:24:55