feeds and speeds

I'm coming to learn that using end mills (mainly hss) has a lot to do with feel and hearing . I've looked up feeds and speed also sfm and it just confuses me to be honest ,I'm a rpm guy lol . Surely feeds and speeds are for machines with the power feeds rather than my little ol Centec2 with all manual feeds on the thae table . One thing I have learned ,after burning the the end of one of my end mills (cheapo) is I think I've been running too fast . 12mm hss 4 flute 1200rpm on steel ,or is it down to the fact they are crappy end mills ( europa tool ) .

Sean

I use the simple approximation rpm = 10000 / tool diameter in mm. (It assumes a recommended cutting rate of about 30 m/min, which is middle of the range, OK for many steels, but slow for Brass and Aluminum. Too slow is safer than too fast.)

In your example, 10000/12 = 833 rpm. In other words 1200 rpm is too fast, very fast for HSS without flood cooling.

Overheating HSS destroys the edge, once it's gone the blunt tool will get even hotter, perhaps burning it such that a lot of grinding is needed to get back to good steel.

Dave

Thanks for that 😊

Sean

Not at all, the endmill doesn't know if you have power feed or not.

Looking at the Europa Tools website they seem to be selling professional grade endmills, although I have no personal experience of them.

Speeds and feeds are simple. There are tables for surface speeds for milling different materials in Machinery's Handbook as well on the net. A rule of thumb for low carbon steel with HSS is 100fpm. Let's call the endmill ½" diameter. The circumference is pi times the diameter, call pi 3 so we have 1.5". In a foot we have 8 times the circumference so that's 8 revolutions per foot. For 100fpm that's 800rpm. That agrees with SoD, except that he's calculated it properly, rather than winging it like me. I agree that 1200rpm is a bit fast.

Now we need to look at feeds. The important parameter is how much does each tooth remove per revolution. Too much and the cutter may go ping. Too little and the tool will rub and cut, and rub and cut, rather than cut properly. That'll sound awful, and destroy the cutting edges in short order. For the cutter in question let's be conservative and say 2½ thou per tooth. For 4 teeth that's 10 thou per revolution. At 800rpm that's a feed of 8000 thou per minute, or 8" per minute. So you don't have power feed? Looking at the "lathes" website it states that the Centec feedscrews are 0.1" pitch. So 8" is 80 turns. To get 8" per minute you need to be turning the handle rather faster than 1 second per turn. That's pretty fast; handle w*nking! None of these values are particularly critical, but it helps to do the calculations in ones head and to be at least about correct.

I learnt early on that counter-intuititively the solution to a horrid sounding cut is often to increase the feedrate.

Another snippet from the "lathes" website is that the Centec feedscrews have square threads. I'm curious to know if that is so?

Andrew

NB: No calculators were used, or harmed, in the production of this waffle

Andrew's excellent dissertation leads to the conclusion that for the same tooth load a small cutter should be fed faster than a big one. This is counter-intuitive, but I can confirm that feeding too slowly blunts cutters, been there, done that! I'm about to embark on making my powered table feed go faster, as at the moment I have to run cutters slowly to get an adequate rate of feed. Just one query, I seem to remember Arnold Throp's book Milling in the home workshop gives much slower fpm than Andrew, but Andrew agrees with Tubal Cain.
​And yes, Centec feed screws are square threads

This is the Y axis lead screw ,which to me looks like and feel like it's brand new with zero backlash . ,The X axis screw is more like a traditional acme.

Hi Sean,

I agree with Dave and Andrew, 1200 rpm might be a bit fast. You can find a calculator here, that you can use to calculate how fast ( in rpm) to run, both for turning, milling and drilling.

Thor

The other factor to bear in mind is depth of cut, it may be possible to feed your 1/2" cutter at 8" per min doing 800rpm if taking say a 1mm deep cut. Now try that at 4mm deep and a lot of the smaller machines will start to complain which is where feel and sound come into the equasion.

Having used a mill without knowing what speed it is doing for about 11yrs I tend to go by the sound of the machine and how the handwheel feels this becomes more of an issue with the variable speed machines as when the speed comes down you can start to loose torque, not such an issue with an old belted machine.

I would say use the calculations to get into the right sort of ball park speed and then adjust to suit the machine and job in hand.

J

I somehow doubt that machines with half nuts have square threaded lead screws. No bother with square threads where no half nuts are involved - stronger but maybe s lityle more power to operate? One needs to remember that industrial feed speeds are sorted out for machines capable of climb milling. There will be a difference, with cutter wear, for hobby machines used mainly in the other feed direction.

Very much agree. rpm = 10000 / tool diameter (mm) has a bunch of assumptions behind it and the operator should always be prepared to adjust. Some of the assumptions are:

• No coolant
• Tool life 1 hour
• Medium feed rate taking a continuous cut
• A recommended cutting rate of 30 metres per minute. (OK for most metals, but too fast for 'tough' steel and 5 times too slow for Aluminium or Brass )
• pi (3.141) is assumed to be 3
• Your machine is man enough
• Depth of cut and feed rate are also 'reasonable'

On the up side, with flood cooling you can probably double the formula rpm safely. On the down side, the approximation is for industrial use. A hobbyist should get results by slowing down, which is essential if the machine complains. It also pays, I find, to crank the speed well above calculated rpm to do light finishing cuts.

When it comes to actual cutting I'm still very much a learner. The formula helps a lot but it's not the end of the story by a long shot. The give-away in my case that is that I'm inconsistent. Sometimes I get a first-class finish, other times not. The main reason I think is I'm not quite experienced or talented enough to know when I'm on the nose. Sometimes I cut too shallow or not fast enough for the tool and material I'm working with, and I don't recognise issues fast enough. Theory is a great help but only experience develops skills.

Finally, a crude approximation for cutting with carbide is 5 times HSS speed. Unlike HSS where slowing down is a good strategy, carbide much prefers to be driven hard and fast. Carbide requires a rather different technique, which is why I think some people don't like it.

Dave

Excellent advice. You ears and fingers tell you what's actually happening, tables in a book don't know how sharp your cutter is, how rigid your setup is or how steadily you can turn a handle.

Neil

Thanks for the picture of the leadscrew; definitely a square thread. I wonder what on earth made them use a square thread. It's much more difficult to fit, as there are three independent interferences that can stop the threads engaging. Of course it might have been willy waving in the toolroom, as in "We can make accurate square threads, we don't need no stinkin' Acme threads here".

Of course the ultimate test is how the cutting process sounds and feels. But rough calculations, along with an understanding of the cutting process, at least get one in the right ballpark. Otherwise you may well end up "optimising" the cut in small area, ignoring the bigger picture. If one can hear and feel the cut then it's probably wrong. When cutting with endmills there should be very little noise or vibration.

The Centec looks a nice solid machine, so I expect it can be pushed much harder than many people would consider normal.

I would disagree to some extent with SoD on carbide cutters. What I would agree with is that carbide inserts for lathes often, but not always, need to be driven hard and are not so good at taking shallow cuts. However, much of that does not apply to carbide milling cutters. Of course they can be run much faster, but it's not a necessity. If you do push hard then the cutter will still perform while glowing a dull red, at least in the subdued lighting in my workshop. Carbide cutters can also take shallow cuts; in one respect they're better than HSS as they're much stiffer and hence will deflect less. A caveat is that coated cutters, particularly TiAlN, need to run hot (>800°C) in order for the coating to function properly.

A point to note is that carbide cutters are formed by sintering, rather than being a homogeneous alloy. So how sharp the cutting edges are depends upon the size of particles before sintering. Some manufacturers advertise now sub-micron particle size, so the cutters are pretty darn sharp. At least the equal of HSS, based on how badly I cut my finger when opening the packaging.

Andrew

Conversely (following on from Andrews comment on upper speed) on a non power feed mill, my impression is that you can also run cutters to slow to the extent that the feedrate has to be reduced to such and extent that variations in turning the handle cause rubbing or at least tiny cuts.

Up the spindle speed a little and you get to turn the handle faster which results in proportionately smoother feed.

Certainly when I started I think I tended to underrun spindle sppeed wise.

regards Martin

Depends how flexible your machine is. If things are dancing around and jumping up and down, drop the rpm. And the feed rate to match. YOu can run cutters slower than then recommended speed as long as you don't jam too much feed into each tooth. Number of flutes makes no great difference to rpm. That is dependent on diameter mostly. But the fewer flutes, the thicker the chip bitten off by each cutting edge, so feed may need to be a bit slower.

The feed per tooth is the critical parameter, as the speed slows then the feedrate should slow in proportion, but the feed per tooth should stay the same.

When I first started using my horizontal mill I had the whole machine shaking; not bad for a machine that weighs nearly two tons. An instant cure was achieved by doubling the feedrate, while leaving the rpm alone.

Andrew

Thanks everyone ,most helpful information given . Just need to get going with this vertical head I'm in the middle of making . Dovetails cut today so some headway made .

Sean

Now all the knowledgeable people have finished I would like one small rant...

Cutting speeds in ft/minute are all well and good until you do the sums and discover that you need a budzillion rpm while your poor old mill is flat out at 2000 and doesn't sound good much above 1500.

Also those monster feed rates suggested for tiny tooling, a person has to wonder how many Watts the tool shank can actually carry to the tip before catastrophic failure is inevitable. If you reduce the cut depth the tip goes blunt before you know it.

Do I really want to buy a 3kW water cooled 24,000 rpm "milling" spindle c/w a hopeful can of WD40 to lube it while it chews it's reluctant way though great billets of aluminium alloy? I think not.

Oops! Have to go, apparently the cat's bowl is empty

Application of cutting speeds does require some intelligence in it's application to a particular mill.

I wouldn't say a 12mm cutter is tiny, cutters 1mm and less are small. Nor are the feedrates discussed large, especially for aluminium. It is very difficult to use small cutters on manual mills. Since spindle speeds are often low the feedrate needs to be correspondingly low. Chip loads are a few tenths per tooth. I've found it darn near impossible to rotate the table handle at a consistent feed, slightly too fast and ping, bye-bye cutter.

Any half decent cutter will take more torque than many model engineering milling machines can provide. I've stalled my Bridgeport with a ½" HSS cutter, and it didn't break the cutter. The Bridgeport is rated at 1.5hp.

A 24000rpm spindle is very useful for small cutters, less than 1mm, although 3kW may be overkill. I find a 350W air cooled spindle is fine.

Andrew