End Mills

Hope this don't sound daft, but I bought some end mills yes they were made in china and they don't seem to last very long I have broken two with very little use. I would appreciate advice on better mills with out paying an arm and a leg and not made in China. I know its difficult and you get what you pay for but I am sure some one will point me in the right direction. Thank You

ARC euro or tracy tools, reasonable quality and excellent delivery, ask any one on here ! Noel.

ARC's Premium range, APT or NC via Cutwel, all from China but all of a reasonable quality without breaking the bank. YG-1 also from Cutwel if you don't want them from China

Edited By JasonB on 04/04/2022 20:49:54

Can I ask what you were doing when they broke ?

Roy

Hi John,

I have end mills from both Tracy Tools and the ARC ones mentioned by Jason and they work well. I also have some unbranded Chinese ones and have broken one cutting edge on one of these end mills, and the cutting edge needs grinding more often than the branded ones.

Thor

It would certainly be interesting to know what cause the breakage so an idea of setup, feeds and speeds and also direction of cut may help. Of the few I have broken over the years I would say I can put them all down to my user errors not the cutters, how well they cut and for how long is the usual sign of how good they are not resistance to breakage.

All cutters have a Goldilocks zone, they need to work but not too little and not too much. Letting them rub heats them, blunts them off and can lead to premature breaking, too high a feed or speed can put too much load on them causing breaking.

You posted in December that you were new to milling. The chances are you are not working the cutters correctly, there is a tendency for new operators to overspeed and under feed. This need for suitable speeds and feeds has been covered a number of times in the forum. In order to know if this is the problem some information would be useful before we start blaming the cutters.

What material?

What RPM?

What type of cutter (number of flutes, material it is made from, diameter, coated/uncoated)?

Depth of cut?

Step over?

Dry, flood coolant or cutting fluid?

Power feed or manual feed?

If you have not been considering all of these factors and setting things up to suit then that could be the source of the problem.

It should be noted that if you have manual feed then the rate of wheel spinning for the correct chip load can be surprisingly high.

Martin C

I've used my Warco mill for many years, mainly with HSS cutters and I dont think I have ever had one break. These have come from all manner of sources.

In fact, I'm not blowing my own trumpet as a user - In fact I feel that I have never quite ever got technique fully correct. Martin's list of all the factors for correct use is perfectly valid. and as he says, feed & speed are vital to get optimum cuts and I feel that personally I cautiously underfeed always thinking the cutter will flex or break and I often get poor results.

While the key factors are easy to consider - material, depth of cut, cutter type and speed is normally easy to get right with rpm counters on many modern machines. Feed rate is less obvious - although there is plenty of info around on rates for this or that material etc. how exactly is that supposed to be transferred to actual handwheel turning? (obviously I'm talking manual ops here) Ok with a stopwatch and appropriate length of cut you could time it but normally my eyes are focussing on the job itself and a several other things at the same time. I've never read anything that gives an explanation of a practical technique to get feed rate right - only many comments on how important it is.

So, is there some time honoured trick to getting this right - or as near as practical - I would dearly love to know, as I'm sure the OP would also!

All the bst Mike

The two most likely causes of breakage are likely to be feed direction and work holding. If you climb without knowing particularly into work that may flex or move you are asking for trouble.

As to feed rate it is affacted by many variables, The machine will be one of them as a lightweight low powered minimill simply won't have the grunt to remove large amounts with each pass of the flute. Type of cut also comes into it as using the side of a cutter will often allow a faster feed than if using the end due to factors like chip thinning and tool/machine flex.

I suppose a simple rule of thumb on a benchtop hobby machine to use as a starting point would be in the region of 0.02mm t 0.05mm or 0.001" to 0.002" chip load and ignore chip thinning.

So lets take a 6mm dia HSS cutter with 3 flutes cutting steel at a surface speed of 25m/min

First work out how many revs the cutter needs to be turning at. 25 / (0.006 x 3.142) = 1326rpm

Now for the feed which is No of flutes x rpm x chip load

3 x 1326 x 0.02 = 80mm/min to 3 x 1326 x 0.05 = 199mm/min

In physical terms depending on the mills leadscrew pitch that would be 40-100 turns per min if it has a 2mm pitch or 25-60 turns if it has a 3mm pitch

If you run carbide and can get the speed required you would need to be cranking at 3 times that as you would for HSS cutting aluminium.

If you are breaking end mills, obviously something is wrong.

Carbide can be run at higher surface speeds than HSS, but is much less tolerant of any form of abuse

CARELESS, like me, banging the cutter into the work?

CLIMB MILLING Not advisable on machines without backlash prevention. The work travels in the same direction as the teeth of the cutter. There will be a tendency for the cutter to grab and pull itself into the work. This can damage both cutter and work.

The cutter tooth and the work should always approach each other head on.

LACK OF RIGIDITY IN WORKHOLDING If the work and cutter are not rigidly held, there is the risk of the cutter grabbing, and damaging both.

If the cutter is not held securely, the helix on the flutes can pull the cutter out of the collet (NEVER use a drill chuck, they are not designed for the side loads imposed by mill, and do hold mas securely as a correctly sized collet ) This will result in an increasing depth of cut as the job progresses, and risk of damage..

EXCESSIVE FEED RATE. All Milling Cutters should be fed on the basis of Cut per Tooth. For an End Mill this should not exceed 0.002" / tooth (0.050 mm per tooth ) So, as an example a 4 flute HSS end mill running at 400 rpm should be fed at a rate not exceeding 3.3" per minute (81 .28 mm per minute )

Having said that do not allow the cutter to "Idle" over the work. A rotating cutter, on stationary work is liable to rub, producing heat which will ultimately soften the cutter.

EXCESS DEPTH OF CUT The general rule is a maximum of one quarter of the diameter of the End Mill .

EXCESS CUTTING SPEED If the cutting speed (Surface speed of the cutter) is excessive the cutter can be softened by the extra heat generated.

The cutting speed is related to the material being cut. Brass can be cut at higher surface speeds than steel. Aluminium, ditto, but can weld itself to the cutter lips. A suitable lubricant, such as Paraffin, (Kerosene ) can help.

The harder the material, the lower the surface speed, but carbide was developed to run at high speeds (So that the work is heated and softened locally ) so that blue or brown chips can be tolerated.

Intermittent cooling of carbide can result in cracking and breakage, so it is better to cut either dry, or with flood coolant.

HTH

Howard.

I've broken a few cheap taps in circumstances where brittle carbon-steel was probably at fault, but never an end-mill.

The few end-mills I have bust were all small diameter, and the error was mine - either careless bumping or feeding too fast or deep. Howard's quarter of the mill's diameter is a little brave for me, I keep under 20%.

Was the material the dreaded work-hardening Stainless Steel? A sharp cutter moves quickly at first through this horrible alloy until the steel work-hardens and blunts the cutter. If the operator doesn't realise the cutter is going blunt, he gradually increases the cutting pressure to keep the cut rate constant, and eventually snaps the blunt cutter. A well-made end-mill should stay sharper longer than a cheap one, but I find it best to avoid work-hardening stainless altogether! It can be machined, but the nasty stuff stretches my skills to the limit.

Dave

Using carbide cutters for full width slotting I use a depth up to 50% of cutter diameter for 6mm and above, Below 6mm I use 25% of cutter diameter. For less than full width I'll use a DOC up to the full length of the flutes. I use these rules for any metal up to and including low carbon steel. For tougher materials I back off a bit.

This morning I needed to tweak the crankshaft bearing holder caps, as for some reason I didn't machine the oil reservoir cutouts to the drawing. Using a 3-flute 6mm carbide, cutter depth of cut was 0.25" and width of cut up to 6mm.

Andrew

Thank you all for your kind replys, I use a waco major the old solid type, one broke cutting side on and the other cutting down like a drill both my fault as I am new to milling.

In the case of the downward cut if it was a traditional end mill then they are not suitable for that as the end flutes do not go all the way to the middle. You can get centre cutting ones but even they can find it difficult particularly as the dia goes up so drill slightly smaller first or work up to size in stages starting with a smaller cutter

No shame in that! When new to anything don't rush to blame the tool. Probably better to learn by breaking cheaper end-mills than expensive ones! It's why I often use a cheapo digital caliper rather than the superior model kept in a box for special occasions. Didn't upset me when I dropped a Lidl on a concrete floor and then stood on it. I'd have needed counselling if I'd done the same to a new top-of-the-range MItutoyo.

Most of the trouble in my workshop is caused by me and I'm pretty sure spending a few millions on a Stradivarius won't help me learn the violin!

Dave

I have bought used carbide milling cutters on ebay, a batch of 6mm cost me less than 50p each, and when they arrived, I quickly bought the rest that they were selling. They are plenty sharp enough for my use, probably discarded cnc mill ones which are changed before they cause trouble. They are my go to for jobs which are too risky for higher priced ones and still I haven't broken one.

The problem with plunge cutting with a centre cutting endmill is that theoretically the centre isn't cutting, as the surface speed is zero. If absolutely necessary to plunge I reduce feedrates by half to two thirds. On the CNC mill I use a ramp or helix path to depth.

Andrew