Are you a Man or a Mouse When Milling?

Now I dont know the first thing about mills or milling but I will be buying a mini mill in the future. I am quite prepared to be shot down in flames but is it right that a cutting tool is glowing red hot, my feeling is thats it not but what do I know..?

I can appreciate the need to want to remove as much material as possible and speed up the job but at what point do you decide that the DOC and WOC and feed is just too much. Andrew you say "so what" to "the smaller machines aren,t that rigid" but surely pushing a machine that hard cant be doing it any good in the long term.

As I mentioned I,m quite prepared to be corrected.

It's a carbide cutter so can be run pretty hot. To be fair it doesn't look red in normal lighting. If you run HSS at that sort of temperature you'll fudge it pretty quickly. Some of the more esoteric coatings on carbide cutters need to be run hot for them to function properly. So running slow ''n' steady can actually decrease cutter life.

In terms of speeds, feeds, DOC and WOC it's a matter of experience. Clearly a benchtop mill isn't going to have the same capabilities as a 8000lb floor mounted mill. But as said earlier I suspect that many users of smaller machines don't run anywhere close to the limits. A rule of thumb is that 1hp will remove 1 cubic inch of material per minute in low carbon steel. So one could assume that the machine would be capable of achieving that. As an industrial machine the Bridgeport does achieve that. I don't know about minimills, although JasonB pushes his mill fairly hard. If the mill isn't capable of utilising the available spindle power then it's a bit of a fundamental design flaw.

Horses for courses really.

Andrew

Thanks Andrew for the explanation.

You will probably have gathered that when I start out with a mini mill I will be in the mouse camp..lol

Ron

I find that if I try 'manly' cuts on my chester delux then as the cutter breaks through the end there's a clunk and chipped teeth on carbide if I haven't remembered to slow feed down enough early enough -- so cheap cutter or main spindle bowing under load? With cheap HSS I just burn them out with blue chips so resigned to modest speeds and depths.

pgk

I think Andrew's demonstration was of potential rather than a recommendation to owners of small milling machines. Andrew shows that a Carbide cutter can be run much harder than most of us would be comfortable with.

A big disadvantage of cutting fast and hot is that the shower of smoking swarf is unpleasant. Making hot swarf on my lathe is particularly uncomfortable because it lands on your hands and arms, ouch. Extra nasty if it gets in your eyes. Slowing down makes the job more civilised.

What limits the speed a machine tool can remove metal is:

• The maximum temperature the cutter and job can take.
• The power of the motor, and the time the motor can deliver power before overheating.
• The rigidity of the machine, ie it's ability to apply power to the work via the cutter without vibration or bending.
• The strength of the machine - gears, belts, spindles, bearings, frame etc. What will break first if you over do it!

Hobby machines are less heavily built than professional machines, and their motors may not be rated for continuous operation. DC motors have brushes that wear quickly if the motor is flogged.

In practice, I:

1. calculate an approximate rpm with 10000 / diameter (mm).
2. increase or decrease the approximate rpm depending on the cutter and material I going to use. (6 to 4x faster with carbide, 20% faster with HSS if flood cooling.) Brass 20% faster than steel.
3. Depth Of Cut - 10 to 20% of cutter diameter, but note the advantage of Andrew's point about using the full length of milling cutters where you can.
4. Adjust the feed-rate for - in steel - straw chips with HSS, blue chips for carbide.
5. MOST IMPORTANT - all of the above is to get into the zone, not a formula for guaranteed success. I listen for signs of stress - chattering, labouring, excessive noise, belts slipping, poor finish - and back-off until the job is cruising. This part has to be learned by trying. I suspect I'm too gentle.

As operator faults go, being over-cautious produces disappointing results especially if tools rub rather than cut. But being over-cautious is unlikely to damage the machine. At the opposite end, some people have gross over-expectations. If you wind the tool up to full power and smack the cutter into the job (causing severe shock loadings), and then force the cutter through the work ignoring signs of stress, then expect blown fuses, worn brushes, damaged electronics, broken sheer pins and stripped gears.

Attitudes to machines vary as well. If I owned a fine watchmakers lathe I would treat it with respect. I see my Chinese kit as consumable. If my lathe lasts 5 years, it only cost £1 per day. If I wear it out or expensively break it, I'll replace it. Going well so far, light to moderate use, kept clean and oiled, no sign of wear after 4 years.

Dave

Edited By SillyOldDuffer on 07/08/2018 11:39:49

During my working life I worked in many sub contract shops and if swarf was not coming off blue you were not making time on the job and not making bonus. Consequently machines and cutters were pushed to the limit, two or three cutters per day were blunted and were thrown in the regrind box and a cutter grinder was employed full time to sharpen them. The machines were mostly Bridgeport’s, the heads had to be re clocked almost daily because they moved no matter how tight the bolts were done up.

In my own workshop I have to buy my own machines and tooling and so they are treated with respect. Swarf is never blue and much smaller cuts are taken both on mill and lathe and I can actually enjoy the machining operations, where does that put me on man or mouse scale?

I think one of the differences between the power of a modern hobby mill and the power of a Bridgeport is that one adjusts it's speed buy electronically and the other mechanically so unless the hobby machine is being run at the motors max speed you will get a reduced wattage or HP. So that 750w brushless soon becomes 375w when run at the mid speed of the machine. I suppose it depends on the design brief whether it is a flaw or not if the brief was to make a machine below a certain price and an electronic speed control works out cheaper than gears then it has met that brief.

Yes motor starts to get a bit loud as you get up to the mills max but still quieter than my X3(gears), motor is at 7000rpm when mill spindle at 2000rpm

The hot swarf can be reduced by thinking about the direction of cut on the mill and if a carbide insert is working well on the lathe will throw the swarf away from the cut face which is usually out of harms way

Hah!

Eat your hearts out, yer rufti-tufti metal-rippers!

My chips come off yellow...

https://www.youtube.com/watch?v=CO8gPLiHlfw

...only not from heat

Edited By Mick B1 on 07/08/2018 19:20:32

Anyone seen the cheese?

I have a myford mill which is heavy and well built but I am somewhere in the middle and leaning towards mouse.

Looking at Andrews photo maybe I should be a bit more adventurous.

Yep, I did the cuts wearing a short sleeve T-shirt. Not too much problem with hot swarf. I also wore goggles all the time. Swarf on the arm only causes some blue language, one in the eye will ruin your whole day and every day after.

Andrew

I have another video but a client with a leaky pipe means it will have to wait until tomorrow. Why will some builders bury bare copper pipes straight in the screed

Cheap cutter? I don't recall ever chipping a carbide cutter during normal cutting. I did get fed up chipping teeth when touching off to set tool heights using a fag paper on the CNC mill. Just a bit too far and the end of the tooth goes ping. That's why I bought an electronic tool setter.

The only time I've taken the teeth off a carbide cutter was milling the spokes for the traction engine rear wheels. After several spokes had gone through I could hear the mill struggling. Turns out the endmill had been converted to a ballnose mill by losing its teeth. After changing the cutter, and a new workpiece, I proceeded to machine the remaining 40 odd spokes without a problem. The last thing I did was go back to the spoke that had caused the problem. Exactly the same thing a bit further along. All I can think of is that there was some sort of hard spot or crap embedded in the material.

Cheap cutters are cheap for a reason. Carbide cutters, and inserts, are not homogenous materials. They consist of tiny tungsten carbide particles embedded in a metal (often cobalt) matrix. Tungsten carbide is expensive, so cheap cutters reduce the amount and add more cobalt. Outside of a production environment it is quite possible that the reduction in lifetime will not be noticed. But there may well be other deleterious effects, like chipped edges.

Andrew

I thought I would try the same 2-flute carbide cutter at a more sedate 760rpm. the frequency of the vibration was lower so there was little or no squealing but the actual vibration was a lot easier to see. Chips were a more pleasing shape but just bright steel colour.

As I was running at the lower speed I then thought I may as well try a 3-flute HSS cutter, that actually vibrated even more so decided not to continue the cut incase something got damaged.

Finally a budget 4-flute cutter, far less vibration, reasonable chips but not as cleanly cut as the carbide and even started to get a bit of a straw colour on some.

I was milling some gauge plate/ground flat stock (take your pick on description) yesterday using a Ø16 insert milling tool. I have had this tool for some time and use it a lot and have yet to rotate or replace the inserts. The feeds and speeds calculator suggested that for a feed per tooth of 0.05mm I should have the rpm at 1300 and the feed rate at 130mm/min. Sure enough running using these figures gives blue chips. These chips are then thrown about with some force and when they hit paint they can stick and embed themselves in it. Landing on any material made from man made fibres has a similar result so keep to the cotton overalls. Having tried these recommended values I reduced the speed and rpm to 650 rpm and 65mm/min. The result is of course that it takes twice as long and the chips come off silver with a hint of straw. The other result is that the distance the chips are thrown is far shorter and they do not embed themselves in any paintwork they hit. In the approximately 3 hours I was working the actual time spent cutting metal by milling was only about 20 minutes. If I had gone at the recommended rates I would have saved maybe 10 minutes of machining time but lost more time clearing up the scattered chips.

One other observation is that the gauge plate chips that are blue are a lot harder than the silver ones. This is important if you don't have flood coolant and there is some recutting of chips taking place if they remain in the area of the cutting action. Recutting is going to reduce the wear and tear on any cutting tool as well as affecting the finish and is something that needs consideration if you can't clear them as they are produced.

Martin C

For most of us machining metal is the end, as much as a means to an end.

That means for many folks, taking it easy and getting a quieter, less rushed and probably less stressful result is a preferred option, especially when working by hand and (as is often the case) less than pristine cutters.

Having much increased the rigidity of my old-style X2 it can take hefty cuts and climb mill, but my machining 'style' depends a lot on what I am doing and why..

Also power isn't just about metal removal, its about ensuring speed is kept up when a cut starts and avoiding stalling when using low speeds.

The original question forgets the all important fact that there are NO right answers as everyone's situation is different.

Neil

Just for the record the original picture was taken while feeding by hand and using a definitely less than pristine cutter. If people don't have the curiosity to want to explore the capabilities of their machines that's up to them. Hats off to JasonB for trying things out and getting some interesting results.

If it's true that there is no right answer because everyone's situation is different then there is no point in anyone on the forum offering advice because, by that definition, it will be wrong. Of course there are shades of grey, but there are definitely right and wrong answers irrespective of circumstance.

Andrew

Edit: Spell errors only show up after posting

Edited By Andrew Johnston on 09/08/2018 19:31:34

It just means advice has to be tailored to suit someone's situation - as this forum regularly demonstrates. Someone asks a question and the first responses are usually asking for more information!

Neil

Whilst we mention HSS and different coated carbides there is also a difference in the quality of carbide. I have some UK manufactured carbide cutters from my design days. There is a noticeable difference in the density of the carbide. When using these they outperform hobby carbide cutters by some degree. I wouldn’t go out and buy these cutters as the prices are beyond what I want to pay, but I have bought cutters from surplus tool outlets which are more affordable. So I would just say it is worth trying different sources for cutters.

I don't own any carbide cutters, the few cutters I do own are mostly the non coated HSS (black) ones from Arceurotrade. Today I had cause to cut 6mm wide slots in some 12mm bright mild stee. I am quite conservative with how much depth I wind on, mostly because I don't have a large stock of spare cutters and don't want to be stopped by ruining a cutter half way through a job. Today howeve I decided to live dangerously. Instead of the usual 0.5mm DOC I have been using I wound on 1mm and then 2mm cuts. This was with a 3 flute cutter at about 1100 rpm and it didn't seem to mind a bit. I did try a cut the full depth, 12mm, of the slot but I was getting steel powder instead of chips and it seemed obvious by the noise, vibration and heat that it was too much for the SX2.7 and I stopped that particular experiment.

A common guideline for HSS cutters is half the diameter in width of cut and the full diameter in depth of cut or the full diameter in width of cut with half the diameter as depth of cut.

Generally speaking, the more depth you can use, the longer the life of the tool befire resharpening, since the corners tend to blow out first.

YMMV

Edited By Mark Rand on 10/08/2018 22:55:50