APT High speed, high hardness end mills - anyone used them?

I have a little emergency project on the go - re-creating the locking wheel nut key I unknowingly lost a few weeks back and now need!. I've sorted out the design OK, but the only suitable material I have knocking around is some 25mm 304 stainless round bar, which is likely 50HRC absolute tops, probably less as I cut a billet off the rod with a hand hacksaw no probs. Now I have a couple of the above mentioned cutters which might do the job, but has anyone ever tried them on stainless, and if so what sort of DOC and feed worked best please?

Quote:

---

Originally Posted by Voicecoil

Now I have a couple of the above mentioned cutters which might do the job, but has anyone ever tried them on stainless, and if so what sort of DOC and feed worked best please?

---

Nobody can answer that,.! You haven't said the tool size for starters and APT makes lots of different cutters in various grades of materials and with different coatings.
However, even if you had given that information every machine is different and they don't know anything about your machine so at best it could only be a ball-park figure. Stainless can be bare to cut at best of times so trying to advise someone without any of this info is impossible.!

Have you tried taking the locknuts off with a gator grip? Attachment 27801

What style of locking wheel nut?

The biggest issue with stainless, is you need to be continually cutting. The moment your cutter rubs, it'll work harden, and then you need a lot more power and DOC to get through the hardened bit.
You can machine 304 with HSS, it's just carbide and coatings last longer.

Quote:

---

Originally Posted by JAZZCNC

Nobody can answer that,.! You haven't said the tool size for starters and APT makes lots of different cutters in various grades of materials and with different coatings.
However, even if you had given that information every machine is different and they don't know anything about your machine so at best it could only be a ball-park figure. Stainless can be bare to cut at best of times so trying to advise someone without any of this info is impossible.!

---

I have 6mm and 4mm High Speed, High Hardness cutters (as per the thread title) which APT recommend 16K and 20K RPM for which should work OK with my spindle which gives constant power between 12K and 24K.

They're the 4 pin style, like the cursed Peugot things, with a centre boss that's designed to shear off if you try welding anything onto it :thumbdown: Thanks for reminding me about the quirk of stainless, I learned that a few years ago when making an underwater camera mount for one of the Springwatch guys: yeah once you start you just have to keep going 'til you're through, no job for the fainthearted ... which was one reason I want to get a decent strategy planned before I press CYCLE START.

Quote:

---

Originally Posted by cropwell

Have you tried taking the locknuts off with a gator grip? Attachment 27801

---

No, I'm not sure how well they'd work on this type - it will depend on the size and spacing of the pins: there's basically 4 off 4.4mm holes on a 60 degree, 90 degree and 75 degree interval on 19.0 diameter, and a centre locating boss: but thanks for the suggestion anyway, if I can find one locally I might give it a try.
Attachment 27805
If you could get 3 or 4 pins in each I guess it would likely work, if it's just 1 or 2, I suspect not, the local garage have done them up well tight.

Quote:

---

Originally Posted by Voicecoil

I have 6mm and 4mm High Speed, High Hardness cutters (as per the thread title) which APT recommend 16K and 20K RPM for which should work OK with my spindle which gives constant power between 12K and 24K.

---

Not being funny here but you can't ask questions about feeds n speeds and expect any sensible reply if you don't give all the details. You say 4 and 6mm but no mention of # flutes. Then you still have the machine to factor into the mix.? Is this a router with 2.2Kw spindle.? or is it a mill.? These make a big difference to how you would tackle this job and esp this material.! . . For instance, I wouldn't even attempt to try to cut Stainless with a router unless it was built like a brick shit house.!

Perhaps I'm missing something but it looks to me more like a job for the lathe (to make the fundamentally cylindrical body), followed by the mill (to position and drill 4 holes), then bang some pins in the holes. How were you planning to use the end mills?

304 isn't actually very hard (typically HRB 70 ie it doesn't even make the bottom of the HRC scale) - and being stainless you can't through harden it either. Machineability is different to hardness. Some form of carbon steel would be a better, allowing you to machine it easily and then harden it with a torch and a bucket of water. Then you'll get something nearer HRC60.

If it's an emergency and you are short of carbon steel, how about using an old cold chisel, crowbar etc as a donor. Cut a bit off with an angle grinder, heat it up to a cherry red and let it cool. Then you should find it easy to machine. It's easy enough to harden up again using the bucket of water etc. You can get tools like this at Aldi etc for peanuts if you don't have any.

While you are figuring this out, you could be letting some penetrating oil slowly do its business....

+1 regarding Muzzer solution/ turning first op (don't machine the counterbore yet)then setup for dividing and drilling the four holes (drill right through so you can fuse the ends of the pins to the body) return to lathe and do the counterbore, make and fit pins.

Quote:

---

Originally Posted by Muzzer

Perhaps I'm missing something but it looks to me more like a job for the lathe (to make the fundamentally cylindrical body), followed by the mill (to position and drill 4 holes), then bang some pins in the holes. How were you planning to use the end mills?

304 isn't actually very hard (typically HRB 70 ie it doesn't even make the bottom of the HRC scale) - and being stainless you can't through harden it either. Machineability is different to hardness. Some form of carbon steel would be a better, allowing you to machine it easily and then harden it with a torch and a bucket of water. Then you'll get something nearer HRC60.

If it's an emergency and you are short of carbon steel, how about using an old cold chisel, crowbar etc as a donor. Cut a bit off with an angle grinder, heat it up to a cherry red and let it cool. Then you should find it easy to machine. It's easy enough to harden up again using the bucket of water etc. You can get tools like this at Aldi etc for peanuts if you don't have any.

While you are figuring this out, you could be letting some penetrating oil slowly do its business....

---

Thanks for the input guys. Yes, I was looking to do the counterboring on the lathe, then start the 4 pin holes on the CNC, followed by drilling to full depth (cobalt drill, thankfully I have some from the previous project). The other task for the CNC is to cut a hex on the other end of the tool to put a spanner on. Sadly I don't have anything carbon steel of suitable diameter that could be sacrificed, about 18mm seems the biggest and it's far from straight. Normally it wouldn't be a problem, I'd go round to the local agri engineer and scrounge a bit - but of course things are not at all normal at the mo, and the nearest town is a bit away - not that I'd want to go there anyway. I do see one or two eBay metal traders still functioning though so if I can get by for a few more days of topping up the offending tyre that might be the way to go.

It would be interesting to know if anyone has experience of using these cutters anyway (they're 4 flute on a 1.8KW spindle Jazz
), they seem a bit of an oddity, but could be useful for other stuff as well. The high RPM is a bit unusual, and I know I'm going to have to keep on feeding steadily as discussed before; I might just do a test cut with a 0.5mm DOC (enough to undercut the hardened zone) and see how it goes.

don't think the body needs to be anything exotic, Mild steel would do and you could case harden the hex, make your pins out of silversteel then harden and temper. what diameter/length stock are you looking for ?

It would need to be 25mm/1" diameter to give enough meat around the pins and maybe 28....30mm long?

You have a PM
Mike

So I thought I'd do a test cut on an odd bit of steel to get a feel for what these cutters can do. The 6mm seems happy at 10mm/sec and 0.5mm DOC and gives a decent finish:
Attachment 27819
This means it'll take a few of minutes to cut the hex on the end of the piece, as I've only one cutter I might drop the feed back a bit - what's an extra minute on a one off job? It's not fast in the grand scheme of things, but it's interesting to know the machine will cut harder stuff, even if slowly.

Do you want it tonight ?

After a couple of delays due to other stuff I finally had the opportunity to have a go at it today, and I have to say I'm impressed with the APT cutters. Sequence of machining was:

1) Turn down outer of bar to size ont' lathe, spot drill either end for centering.
2) Peck drill pilot holes for the 4 pin holes on the CNC, 4mm cutter.
3) Transfer to drill press and drill pin holes to full depth.
4) Drill a 10mm centre hole for the recess (lathe) - this made the subsequent milling much less arduous.
5) Enlarge centre hole & machine counterbore on the CNC - I didn't do this with lathe as my boring tool was a bit shagged.
6) Flip it over and machine the hex at other end.

I had to quickly turn a couple of pointy things that fitted into the collets to achieve the centering, but they'll be useful in the future no doubt. Seems to have turned out OK, accuracy is fine (apart from a small centering error on the centre hole) and the finish is pretty good -not that it matters really, it's only a tool - but nice to know for future work.
Attachment 27866
Attachment 27867
Things that I've learned about the cutters are:

1) You need a good lot of coolant when using them on steel!!!. Thankfully the pump on my mister has quite a range and fairly gobs it out when you turn it up - just need to sort out some sort of drain/recirculation to avoid puddles on the floor now :whistle:
2) The stated RPMs on the APT site are OK for edging/shallow surfacing, but for anything deep & confined you need to take them down a fair bit: I ended up with 14K on the 4mm when drilling and it sounded fairly happy.
3) Although it seems to be possible to press on with a reasonable feed rate in X and Y, the Z plunge rate has to be far less.

But all in all these cutters are a useful thing - although you might have to take things gently, being able to machine steel on a DIY machine (made of aluminium!) is obviously useful. I'll get a few more next time I'm ordering from APT and maybe do some tests to see how hard they can be pushed.
PS thanks to Mike (Mekanik) for the bit of steel :-) )