Milling cutter damage - what am I doing wrong

I seem to have a natural ability to trash milling cutters, that is, ending up with cutters with chunks out of the end faces of the end mill cutter.

Today, I was cutting a 5mm deep slot 40mm wide across 80mm of mild steel plate, grade 080A15, with a 16mm diameter end mill. Mill revs were 360rpm - the next speed up is 600rpm and the machine said it didn't like that - with a feed of about 1 inch per minute hand fed on the Y axis. Depth of cut 20thou and 40thou. I had put the better of my two 16mm end mills in but it ended up with great chunks out the end. I had been trying to feed the mill in gently until it was cutting across the width of the cut. One cut was 16mm wide across the middle of the slot, the two cuts one each side about 11mm wide, leaving the sides to be trimmed to size.

When cutting on the X axis and with all end mill diameters I have I tend to use a power feed, set quite low, especially now given the damage I seem to be getting, until it is cutting full width. All my end mills are HSS.

I was trying to make todays task a precise fit and not go over hence the shallow cuts but usually I go about 2-3mm deep and D/4 wide.

What am I doing wrong? What improvements to my technique should I adopt?

I don't have a tool grinder set-up yet but it is rapidly climbing the work-list, as the alternative seems to be to corner the market in new end mills!

Chris

Spindle speed of 360rpm is slow for a 16mm cutter in low carbon steel. You don't say what mill you are using, but if it won't deal with a 16mm cutter at 600rpm it might be better to use a smaller cutter at higher speeds and feeds. A feed of 1" per minute is very slow, assuming a four flute cutter, it's about 0.7 thou per tooth. It's quite likely the cutter is rubbing rather than cutting. I'd be feeding at 4"/min or more.

The other big variable is the source of the cutter; some cutters at the cheaper end of the market are poorly ground and will never work properly.

Andrew

It would be helpful if the type/make of mill was stated and the spindle size,A mill with int 40 spindle would take cuts to full depth 5mm easily,a 30 int spindle should take a cut to full depth but if the mild steel is flat plate it can sometimes be stringy so a cut 2.5mm taken ,the centre cut should be no problem but if you try to climb mill the outer cuts then the mill can grab a bigger bite and damage the cutter , mild steel round bar always machines easier than flat drawn bms,black hot rolled is not tough just stringey and difficult to get good finish. Not knowing the machine ,it could be the machine is to light to take a 16mm cutter and the table is jumping about and breaking the teeth.

Andrew, the mill is a Warco 'Economy' round column mill, now discontinued, Axminster and Chester did similar models, for me and my little workshop relatively big and very simple.

It may have been that it was the cutter that didn't like the 600rpm, the mill handled it but the chippings were coming out far too hot and discoloured, so I may have mislead you there. The milling cutter was not perfect when I started by any means, a new one might have gone better but I didn't have one, it was the better of the two I had. In the end I finished the job with the other one as the first one was totally shot.

It is a 4 flute cutter and it just seemed that if I wound the Y axis handle any faster it wouldn't be right as it would be traversing too fast - perhaps that's down to my inexperience, but 4in/min seems awfully fast to a beginner like me!

If I am getting chunks out the 'teeth' would that suggest that this version of HSS is not all that it should be? That doesn't happen with any HSS tool steel I use as lathe tooling. Perhaps I need a better tool?

Chris

Edited By ChrisH on 15/05/2014 20:46:20

Nigel, just been out to the shop and measured it, the spindle that holds the tool is 36mm diameter, the sleeve it sits in is 62mm diameter. The plate was clamped securely either side of the slot being machined, I could see no 'bounce' when machining. All cuts were taken with the cutter rotation opposing the direction of travel, that is Up Milling I hope! The steel is bms not black.

The biggest problem is my inexperience here, hence the cry for help and guidance!

Chris

Chris What are you using for cutting oil ?

Roy

Roy - cutting dry today, but usually use Warco's NeatCut Oil.

Chris

Check for slop in the feedscrews, gib strips etc. and are you milling in the right direction? Sounds like a lack of rigidity somewhere which causes a 'dig in' followed by a 'snap'. I assume the quill is locked and if it's a round column machine, make sure all the clamping bolts are nicely tight. Too slow a cutting speed (rpm) can overload a cutter teeth.

Milling on a lathe I found no different from latheing on a lathe. I only got any good at it after a lot of practice, and quite a few damaged cutters

Chris - everything all tight all round and locked and no slack that I can see. Agree that a slack somewhere can lead to a dig and a snap, but where I don't know. All seems tight to me. Also up milling not down so in the right direction. How does the overloading of a cutter tooth at low speed happen if the cut is light, I am not understanding that?

Ady1 - practice is what I am giving myself but how to do it without damaging cutters is what I am after, so hence the question - how?

Chris

I used to have the larger round column mill/drill, the major was the model I think and that didn't like big cutters unless you were only tickling the work.

Personally I'd drop back to 10mm cutters and see how you go on with them just to get a yardstick.

We look at something big and heavy and think it's rigid but it's not as rigid as we think.

I feel you're pain.

We should form our own club. ........ With me at the moment it's lathe parting tools that I seem to have a gift for ruining beyond redemption.

The only plus side (if it can be called such) is that I usually know what the cause is.

Nick

Is the endmill cutting on the heel instead of the leading edge? You will see machining marks (half moons) pointing away from the direction of travel if it is. Does it cut better in the opposite direction. If this is the case the head is not vertical.

If you are running a high speed steel cutter at 360 rpm , and it can not take a 1 or 2 mm cut, then your machine does not have enough rigidity.

In smaller machines you would be better off using a smaller 8 or 10mm end mill.

8mm and 10mm tungsten carbide cutters are very affordable now days.

You can run a carbide cutter at higher rpms, The most common cause of cutter damage is by swarf getting trapped between the cutter and work piece, Having a high flow of coolant or even an air fog buster onto the milling cutter will dramatically increase tool life.

Neil

If it's not rigid enough to handle a 16mm cutter I'd advise against using carbide unless you are forced to as the slightest flex with degrade the cutting edge.

I have run jobs on the big CNC on light cuts, 1mm deep 5mm wide in 316 stainless where the edge of a 12mm cutter has degraded to form a radius and not a sharp corner. As I only had two cutters which didn't last long and it being a weekend I had to swap to HSS and one cutter then completed the job.

I had to use 12mm cutter as the jig cut parts on both sides in one pass and the jig had been programmed for a 12mm wide swathe.

Complained to the cutter rep and was told the machine wasn't rigid enough for a light unsupported cut in stainless and I was better off with HSS.

The CNC only weighs 2 1/2 tonnes !!

Just a thought, Chris's mill probably can't go fast enough for a 8 mm carbide cutter. When I got my 2" face mill, 3 indexable carbide cutters, I knew nothing of milling, so I asked about how to take a cut, and the chap that sold me the tool, and the Rexon Milling Machine said "set the speed at 900 rpm, wind on about 1 mm depth of cut, and crank like hell". The Machine is a round pillar type, and I did have to drop the speed to about 800 rpm. With HSS end mills it does not like deep cuts, but you have to keep it up to the cut, or the tool rubs, and the surface finish suffers.

Ian S C

Chris: In the past I have been accused of giving advice that is irrelevant to the modeller, as I base it on the larger machines that I run. However, I still think that 1" per minute is too slow, may be try 2-3" inches per minute? Superficially it seems counter-intuitive, but a lot of milling problems are solved by increasing feedrates, not decreasing them.

I'm a bit confused about the damage you are seeing on the cutter, a picture would be useful. I don't think I've ever taken chunks out a 16mm cutter, and that includes stalling both the Bridgeport and CNC mill. I've certainly damaged edges and blunted cutters, but that doesn't sound like the problem you are seeing?

What is the source of the cutters?

Regards,

Andrew

Chris,

I have a Clarke Mill/drill round column and is about as rigid as a daffodil in a gale. It would not like a 16mm end mill taking a full cut even with a sharp cutter.

The only advice I feel I can give is to set your cutter at 600 rpm and take a 0.010" cut and hand wind the X-axis. If there is little resistance up the speed until you find the resistance increasing. Then try the same with a smaller cutter. After time you will get the "feel" that the experienced modeller (and machinist) learn by just doing it.

If the cutter looks blunt try to polish the front of the cutter tips with a stone, or if you are brave the grinder, although the grinder will ruin the cutter for any future regrinds.

Trevor

I suspect lack of rigidity is the route cause with blunt cutter exasperating this, but why!!, quite often with small mills the cutter gets pulled into the job due to flex, again why, with conventional milling the chip forms from zero thickness and gets gradually thicker (climb milling the opposite happens but that's OT for a manual mill without ballscrews), until the chip eventually becomes unsupported by the parent metal, at this point the chip bends away from the tooth, just before it breaks off, this can cause the damage you are seeing, the chip as it bends overloads the tooth causing cracks which eventually break off, blunt cutter exaggerate this problem.

At first due to it being blunt it cant form the chip and so gets pushed away until the forces overcome this resistance, at which point the cutter digs in and the chip is formed, and so begins a vicious circle, either the cutter overheats because its rubbing and cant push the heat into the chip or bits break off until its completely destroyed, stainless and Inconel are particularly bad for this, I've often machined tough stuff, it can be counter intuitive as to what is actually going on, but lack of rigidity and blunt cutters is never a good starting point.

I have a Warco major, I use it as a drill, I very much doubt it could handle a 16mm endmill.

HTH

Shaun

I found 6 and 8mm cutters more amenable, and the 2-flute ones you can resharpen yourself