Micro End Mill Speeds and Feeds

[Crashmaster]

Does anybody know of a resource for find speeds and feeds for micro end mills. Specifically from the .02-.08 range. Thanks!

[scadvice]

Maybe I can help. Tell me a few things:
1) machine type and spindle speeds possible?
2) stock material and size? Aluminum, stainless, cold roll steel, tool steel, ect.
3) size of finshed parts?
4) total depth of cuts?
5) is there coolant, air, or air mist available?
6) tell what type of cutter you plan on using if any? ie Carbide, HHS, number of flutes, coatings, LOC on the endmill?

I've cut most materials and with endmills from .006 diam. and up. 1/32 wide slots in p20 1/2 inch deep. You can cut almost any materials with the right cutters, machine, feeds and spindle speeds.

General rules are:
Ridgidly held stock.
Stiff machine (yes this is very important with small tools)
very good control of feeds and speeds

chip load and DOC... example .020 carbide talin coated 3 flt. 10% to 30% depth of cut, chip load about .0002 to .0003 per tooth in 303 ss or mild steel. Thats 5.6 in/min at 7500rpm and a depth of cut of around .006 to .007. Rate your cutter wear by the burr, if you can scrape it off with your finger nail it is still sharp. if not... it's about to break.

Robb Jack cutting tools had a good chart in their catalog, maybe you can find that info on the web.

I'll give some starting info...just answer my questions.

[Triv]

Most of the larger tool manufacturers post recommended speeds / feeds / depth of cut.
If you bought their product, you also bought their service and support... Call them and ask away.

You will probably need a speeder head to get optimum surface footage.

Good Luck!

Triv

[mc-motorsports]

Originally Posted by scadvice Maybe I can help. Tell me a few things: 1) machine type and spindle speeds possible? 2) stock material and size? Aluminum, stainless, cold roll steel, tool steel, ect. 3) size of finshed parts? 4) total depth of cuts? 5) is there coolant, air, or air mist available? 6) tell what type of cutter you plan on using if any? ie Carbide, HHS, number of flutes, coatings, LOC on the endmill?

WHOA!!! Somebody know's what they are doing! Dude, your supposed to just google it and post up some BS numbers that mean nothing and specifically came from nowhere and when you break tools, just slow it down... j/k!

Just glad to see someone get's it. Your the first person to ask what machine tool and spindle

[Crashmaster]

Well, that's one of the problems I know I am going to have, specifically with RPM's needed. I will be running this tool on an old Wasino lathe as a live tool. I beleive my live tooling max's out at 3500 rpm. Stock will be aluminum bar stock. The cut is actually on the face of the part. The total depth of cut will be around .1. Coolant will be available to use. I will be using a center cutting solid carbide .025 end mill.

[Triv]

.025" diameter tool?
3500 RPM?
Expect to do 20-30% depth of cut per pass.

Aluminum can be forgiving enough, but you are underspeed. If you cannot get a shear, it is like chiseling it with a rusty nail.
Optimum, HSS is around 350 sf, or 53,480 rpm

Uncoated carbide is about 3 times as fast.

[Crashmaster]

OK, so is this even going to be possible at the slow of an rpm? What kind of feed am I looking at?

[scadvice]

...you use a sharp tool, carbide is fine if you use uncoated two or three flute and a good brand. Stub endmills are better if your depth of cut allows it.
Just keep you chip load to RPM correct, as I said in the past post. Oh, and coolant. Its just going to take a little more time.
Steve

[David Bord]

Perfect timing, I was just looking for similiar advice.

Im looking at pocketing/engraving a logo on 6061 alum with an .03125" end mill to a .01 depth. The total size of work piece is about 2.3 inches. Held in a Kurt vise with soft jaws. My spindle speed is limited to 4500 (tormach mill).

Would you recommend HSS or Carbide in this case? How many flutes? Any reasonably priced brands? I dont plan on doing a great deal of work at this size.

What feeds and speeds and depths would you recommend to start at for the the above project? Lots of coolant available.... Machine and workholding should be rigid enough.

[Crashmaster]

Thanks Steve, We are looking to run these parts late this week or early next week. I will let you know how it turns out.
Joe

[rcpilot82]

kinda off topic but where are you purchasing your endmills this small from??

[scadvice]

...can be found in the MSC Industrial Supply Catalog and on their web site, pages 525 -529. Robb Jack's are the best but the most costly. I've used the others listed and they seem ok. I always look at all of them under a microscope and send any back that are poorly cut. I have not had to send any back for a long time. I use two and three flutes mostly but will use a coated 4 flute in ferrous material if the DOC is only 10 or 15% of diameter.
Again, use the shortest LOC you can. Also, hold it in the collet as far up into it as you can before it tapers down from the 1/8 " body size to cutting size. They will last as much as ten times longer that way.
the flatness of the cutting surface is very important with mini's if you think about it. Any doubts or cannot control that... start the first cut some of the expected deviation from flat.
Steve
Joe... I would like to hear how it works out for you.