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'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 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

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

Something is not right .

!600 RPM is certainly a bit too fast for a 6,5 mm cutter in EN3b but nevertheless in the presence of coolant cutter edges should have lasted long enough to make a few successful cuts .

EN3b in small section bright bar form is not something readily bought off the shelf and it is at least possible that you've got something else – quite likely gauge plate . Nothing wrong with gauge plate for making your components but much lower cutting speeds needed .

The other possibility is that slot drill is not a slot drill – what does it look like on cutting end ?

A common problem with cutting materials at two fast a speed is that the corners of the cutter get knocked off very early on – then all is lost .

MikeW

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

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