Milling tooth load

I am scratching my head while reading the ME Handbook, page 5.14. TC says that the "tooth load" should be cutter dia/1000 and that feedrate is calculated by TL x RPM x no of teeth.

Using the dia and RPM data for 4 tooth cutters, column C, the calculated feed rate works out to be 1" per min , but the table feed rates are higher for all but the smallest cutter.

Where have I gone wrong?

Btw I want to use a 16 mm cutter in BDMS. Should I use 385 RPM, 80mm / min, which gives a tooth load of more than 3x dia/ 1000

Trying that combo produced blue chips, and the machine "felt" as if it was working hard ( a Taiwanese 8x 30). I am using trefolex cutting oil in a spray can.

i blunted the corner of my hss cutter after about thirty 5mm wide, 1.5 mm deep, 100 long passes. I am making Harold halls t-nuts from wps 35

I'd ignore the data in the book and work out the numbers as follows.

First, I'd cut the other way round, ie, 5mm deep and 1.5mm wide. You're paying for the whole length of the flutes, so you might as well use them. Personally I'd use a smaller cutter, but let's stick to the 16mm cutter for the purposes of the calculations.

For a HSS cutter in low carbon steel we want the surface speed to be on the order of 30m/min. So, for a 16mm cutter that gives about 600rpm. We'll stick to a width of cut of 5mm. If we assume a conservative chip load of 0.05mm (about 2 thou) and four flutes that gives a feedrate of 120mm/min. You could probably up the feedrate because even at a width of cut of 5mm you're going to get chip thinning. In other words the thickness of the chip is rather thinner than the calculated 'chip load' suggests, so you can up the feedrate.

Let's look at some power calculations. A width of cut of 5mm, depth of cut of 1.5mm and a feedrate of 80mm/min is a volume of 600mm^3 per minute. That's 0.037 cubic inches per minute, which is very low. A rule of thumb is that 1hp at the spindle will remove 1 cubic inch per minute.

If we look at the data from the book a tooth load of 16/1000 = 0.016mm is about 0.6 of a thou. That's pretty low; my guess is that your cutter was rubbing rather than cutting, which is why the chips were hot and the cutter got blunted.

If there's one rule for milling it's that very low chip loads are not inherently better, and somehow 'safer'. All that happens is that the cutter rubs instead of cutting.

I hope that gives some food for thought; let us know how you get on.

Regards,

Andrew

Russell,

Been a skilled miller for 40 years and never once used a feed and speed calculator - except for the ONC exam. Once had a stand up row with a design "engineer" who didn't believe I had forgotten the formula.....

Speed of any diameter HSS cutter;

Mild steel; set the rpm by looking at the flutes as it spins, if you can see individual flutes but not follow it round you are there.

Stainless and nickel steels; You should be able to follow a flute with your eye as it rotates.

Feed rates; start slow and work up till the tool squeals then back off.

Waiting to get shot down.......

Trevor

Edited By Trevor Wright on 09/08/2013 12:53:21

Edited By Trevor Wright on 09/08/2013 12:54:44

Thanks guys.

Trevor, I'm glad to see your method of speed calculating. I was shown it many years ago when I was an aprentice, have repeated to many people since and they all laughed. By my thinking it has to do with eye/ brain working, as 24 frames / sec. for movies. Works for other things too, eg lathe work.

The tables in Tubal Caine's book have always puzzled me as well. He gives higher feedrates for 2-flute cutters than for 4-flute which is at variance with the equation he gives. I wonder if the publishers got the two tables transposed?

Russell.

Trevor,

That's brilliant and will not be forgotten.

Neil

Mr Humphries, my instructor had three rules for speeds and feeds

Rule1. Coolant

Rule2. Coolant

Rule.3 Start slowly, Feed slowly,when the swaf or chips start to make a noise like frying beacon and eggs slow down a little

My biggest problem in the home workshop is the lack of a coolant pump and suds tray on my milling machine, stuck with using RTD spray or a soluble oil in a hand spray, can get a bit messy but Mr Humphries words always stay with me even though it was 30 years ago

Look, listen and feel what the cutter is telling you. Its up to you as the operator, speed and feed tables are theoretical values and good starting place.

To my cost I failed to realise the importance of scale too, whilst using my small home milling machine the feed and speed felt about right to me, but after several cuts with a large cutter I burnt out the motor, so now the size and depth of cut (tooth load) is much much less than what the book says !

Thanks again to all.

having bxggered my 16mm cutter, I followed Andrews advice and used a smaller cutter, opting for 10mm which I ran as close as I could to 1000 rpm (925 in my case). Trevor's cine rule worked. Milling was a breeze with a very fast feed rate.

my t-nuts mk1 are now finished. Mk11 will follow, omitting some of the errors committed!

Wouldn't shoot you down on that one Trevor. That's what I was told when an apprentice. Works with all cutting tools. Just lose sight of the individual teeth. Bit slower for stainless etc bit faster for non ferrous. Allways keep a cut on so the teeth do not rub. I always preferred to be on the mills.

With VFD control on my drilling machine, shaper and lathe, I adjust speeds until the swarf comes off in a nice easy spiral.

A wonderful sight to behold compared to pre VFD.

Milling machines to follow, so Trevor's method will be used.

Geoff - Too many bl**dy projects, I really need to get organized!

Edited By OuBallie on 10/08/2013 10:10:01

Whats a speed and feed table ?

It's where you put your drugs and sandwiches

John,

a data table giving RPM and linear feed rate for various diameters, materials and other variables.

Russ

I thought it was a quick lunch. Ian S C

Seriously we must have done it as an apprentice but can't remember.

Since then it's all been seat of the pants and worked out OK.

Personally I can't see how you can make a table up.

OK cold rolled, 1/2" carbide cutter, look in the table and it say 3" deep at 10,000 revs

Hang on, only got an X2.

I have a couple of commercial programs here that have come with CAD/CAM software and neither asks for a rev or horsepower ceiling and it's not settable as well so the figures that are spat out are of no real interest for anyone with less than a 4 tonne machine.

Point here is that when Ketan at ARC was looking to stock some decent inserted tooling for the discerning user, as opposed to us tight arses. Sumatoyo was quoting insane feeds and feeds so out of interest we both popped up the road to the local Aerospace Co.who has some very, very, serious bits of kit and asked if they could run them.

The answer was no, they only had 35 HP on tap at 16,000 revs.

To run at the specified feed rate they would need the next size machine with 50Hp spindle and 40,000 revs.

This is the honest truth and the figures have not been exagerated.