Slot milling speeds

I am trying to mill a series of 6.5 mm slots about 70mm long in a piece of 4.8 mm thick BMS bar and have already blunted two slot drills on the first ho;e.

I started at 1600 rpm with neat cutting oil but after blunting the first drill I reduced the speed a little.

What am I doing wrong?

1600 rpm sounds high to me. I would go for about half that. What depth of cut are you taking? On my Hobbymat full depth would be too much. I would probaly take three passes with a 2mm or less cut.

Roger Woollett

I agree with Roger about the speed. You do not say how deep the slots are or what cut you are taking but I would limit the depth of cut and take several passes for each slot. perhaps even more conservatively I would only take around 0.5 t0 1mm at a time.

I took the speed from Tubal Cains Model Engineers Handbook. The table on page 5.14 recommends 1600 rpm for a 1/4" slot drill in BDMS.

Each cut was about 1mm deep.

I should have added that I was advancing the table quite slowly - about 40mm/min - as the walls of the slot are only 1.3mm thick and I wanted to avoid any distortion. ( I am trying to make the parallel motion hanger straps for a Vulcan beam engine).

I'd second that Terry, perhaps suggesting about 480 rpm that I use, I think when I taught myself I started at the opposite end of the speed range than a number of beginners on here, I started using my bottom speed of 90 rpm, and worked up from there. Ian S C

I think Peter has not read the table in Tubal Cain's book quite rightly. The machinabilty column C is for FC (freecutting) steel which has much better machining properties ths bright drawn steel. Due to the way BDMS is made i.e. cold or hot drawn its properties change making it tougher particularly in thin sections whereas free cutting steel has additives to make it machine very easily.

I suggest,like others above, that you reduce the speed to a maximum of 600rpm or less according to the way the cutting progresses. All speeds quoted in any literature are guides only and cannot take full account of the actual conditions of use. I always use 5% cobalt 3 flute cutters.

I agree.

300-400 rpm.

And use a 2 flute cutter which you can resharpen on a grinding wheel.

You'll see the difference once the cutter is happy, never force it

I would question the grade of mild steel as Eric says, there are too many grades of mild steel which will affect the cutting speed. That said, 1600 rpm isn't necessarily wrong! Depth of cut and rigidity of the tool and work holding can cause excessive cutter wear or breakage. Explore all avenues but try to find the type and quality of the material you are cutting.

Just to add to the 3 or 2 flute cutters thing, yes 2 flutes are easier to regrind, they also have more clearance for swarf removal, they are also weaker than 3 fluted cutters. Buy the best quality you can or source from production engineering friends if possible, they will not use rubbish (I hope!!!!). I could recommend some manufacturers but don't want to be biased towards any one of them.

I hope you find your solution to your issues.

Generally recommended cutting speed for low carbon steel with HSS tooling is about 100fpm. For a 1/4" cutter that works out at 1528rpm, so not too far out. Being cautious you may want to reduce that by a third to a half. I think the real problem is the feed rate. If we assume a 2 flute cutter at 1600rpm a feedrate of 40mm/min gives a chip load of about half a thou per tooth. That's pretty small; it's inviting the cutter to rub rather than cut. I suspect that's why the cutters are being blunted.

Why not try a speed of 1000rpm and a feedrate of 80mm/min?

Regards,

Andrew

I find that the biggest problem is heat, slot drills do an awful lot of work and running them too fast can kill one pretty quickly.

The metal was sold as BMS EN3B. I had already milled some 1.6 mm slots for the cotter pins at top speed, about 2500. with no problem, albeit I took tiny cuts and advanced very slowly.

My mill is an Amadeal 25LV.

I cannot do anymore until I order some new mills but I will take the consensus advice and use a slower speed, 600 rpm. I also plan to remove most of the metal by chain drilling most of the slot.

Thanks for all the advice.

Peter

Mike

I bought the metal from Folkestone Engineering who stock a wide range of small BMS bar stock in EN3B.

All

I found a new 6mm slot drill in my drawer and decided to have another go having chain drilled most of the slot. This time I ran at 600rpm with between 0.5 and 1mm cuts. Now I could 'feel' the tool cutting the metal and whilst I had to wind harder there was little sign of heating. Having cut the central slot I then widened each side to the 6.8 mm target.

Job done!

Thanks again for all the help.

Peter

One other thing not mentioned so far is the effect of hand feeding. To be kind to small cutters, it is important that the feed depth per tooth is reasonably consistent; this is easy with power feed, next to impossible with hand feeding. When hand feeding you will get some revs when no, or almost no, metal is cut, and some where too much is cut. Too little means the tool edge will rub, and blunt, too much and it risks breaking, or again blunting. If you have to use hand feed, try to get it as constant as you can, and if you pause, back out and don't leave it rubbing (if you do that with stainless or titanium your tool will be blunt in an instant).

On the type of cutter, the 2-flute ones are definitely the type to use for cutting slots. Three flute cutters, though not as bad as 4-flute ones, will not cut neat slots, especially with hand feeding. Yes, you can always use an undersize cutter and then go back and widen the slot, but (a) that means far more work, (b) you risk making the slot oversize, and (c) you are using an even smaller (and weaker) cutter. I don't believe that a 3 flute cutter is stronger than a 2 flute cutter; in fact, given that it has 3 gaps in it instead of 2 it may even be weaker. I have recently cut several slots with 2-flute cutters, using a cutter sized for the slot, and they come out dead to size (pieces of brass of the same size are a firm push fit in the slot). Two flute cutters are not called slot drills for nothing!

David

All very valid points and well raised David

Well..... the FC 3 cutters are all 3 flute cutters and they are excellent for slots. Use them exclusively for all small sized slotting. Tend to give a better finish due to lower levels of vibration by reducing springback in the tool.

The trick is to have a rigid mill, and a decently held bit of work, and to cut at the correct speed AND toothload. A 1/4 " FC 3 (which is not far off a 6.5 mm cutter - .264) will cut very well at 2000 rpm though 1500 RPM is about 100fpm. Thats more or less what I cut at all the time, simply because its a recommendation for a general purpose steel, and it happens to be the H2 ratio on the mill.

If the stuff is EN3b, it is common or garden free cutting mild, with a direct equivalent of 070M20 in new money. Nothing special - just lovely soft stuff specifically for machining.

So Andrew has to be right - its either the feed rate, which shouldn't be more than a couple of thou per tooth per rev, or the cooling is up the duff. Might not be enough, or it could be neat that should be dilute so one is not getting the flow removing chips, or heat transfer out of the work. As Andrew suggested, 2k RPM might be trotting on a bit, but it is not outrageous - but the 600s as suggested are probably way too slow, because the likelihood is that one will have far too high a tooth load which leads to tool bending and breaking. Still, if one has a blunt cutter, the wise thing to do is to maintain revs, and increase tooth load slifghtly to prevent rubbing.

Edited By mgj on 22/02/2012 17:40:54

I also agree with Andrew. I've been doing alot of milling of BDMS, SS, and black mild steel of late. I'm using about 1200 rpm for 1/8" and 1/4" FC3 cutters and about 800rpm for 1/2" slot drill. I tend to be optimistic about depth of cut and blase about climb milling for smaller cuts.

Tubal Cain's milling catchphrase was 'keep up the feedrate' and a three-tooth cutter at 1600 rpm needs to move at 4.8" a minute to have a tooth load of 0.001" - that's winding the handle pretty m,uch flat out.

These things are all inter-related. I try to set the speed so the mill is happy when I wind the feed at a steady rate of about 40 rpm (about 2-2 1/2" per minute). With variable speed and the ability to wind slower or fsater its about feel and judging what is keeping the cutter happy - generation of decent swarf (type depending on the material) and lack of heavy vibration tells you when teh cutting is going well.

Neil