[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]

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.

[Triv]

Item #1:
indicate? :bat:

Item #2:
Indicate.

Item #3:
INDICATE! :idea:
Something that small must be running true.

Item #4:
Double-check the slop or play in the spindle.
It is normal to have some indicator deflection
when you press against the spindle...
But does it return exactly to the same point?
Try pressing from different directions...
(hint: Any rotating spindle will have some deflection.
To limit the deflection, you would have to weld the spindle ---
Then the spindle would not rotate.)

Item #5:
Feedrates can vary from .00002 to .00007 per tooth.
If you are using Robb-Jack's endmills,
then call them for the for their advice on your situation.




What SCADVICE said is also true. If the stock is not perfectly flat and perpendicular to your tool, start your cuts from the highest point, not the lowest. A few thousandths extra material will kill the tool.

Good luck!

(PS: air-tool spindles may help, but they must be precision-built, not from a $20.00 die-grinder)

[David Bord]

Guys, if you dont mind, would you be willing to give me some feedback on the specific questions listed above? Specifically, if you are limited to 4500 rpm, do you prefer HSS or Carbide and 2 or 3 flt? Ive read that HSS is generally sharper and some on this thead say sharper is better on these small EMs. Again this is for Alum pocketing.

If possible, I would prefer using an average cost tool due to risk of breakage and the limited use I have for them, unless a medium cost tool just doesnt make sense. I should note Im just a hobbiest.

Any safe feeds you would recommend in 6061 with a 1/32 em either HSS or Carbide? (waiting for advice before I purchase) This is for a .01 deep pocketing opp, somewhat like engraving. Ive already noted the 20-30% DOC.

Any sound advice would be greatly appreciated!

David

[scadvice]

... Also, get "stubbies". Just be aware, that they will wear faster... as much as 10 xfaster. So...depending on the number of parts, a carbide might be a better buy, because of downtime to replace the cutter, touch off risk, and time lost. Your call...
I almost never use HHS anymore, Carbide endmills are so good now that even the cheap ones in the major catalogs will be far longer lasting than the HHS. 3 or 4 bucks difference is cheaper than your down time to change the tool.
Steve

P.S. The finger nail burr scratch still applies to wear testing the cutter.

[David Bord]

thanks! for my application 2 or 3 flt carbide? any starter feeds to experiment with in 6061 alum at 4500rpm with .03125" em with a 25% percent DOC?

[scadvice]

thanks! for my application 2 or 3 flt carbide? any starter feeds to experiment with in 6061 alum at 4500rpm with .03125" em with a 25% percent DOC?

if you can get stubbies, I would cut the whole .01" depth at a feed of .0002 per tooth for a 2 flt. (1.8 in feed per minute) and .00017 per tooth for a 3 flt.
(about 2.3 in per min.)

[David Bord]

Thank you very much!

[mc-motorsports]

HSS 2 flute stubby as possible every day of the week... No carbide or 3 flute EM's for that job, not if I was running it.

And yes, HSS is always sharper, carbide takes much more pressure to cut, but the simple fact that it can take much more heat makes it an excellent cutting tool for high speed machining of aluminum, steel, steel alloys and even the nickle alloys. HSS is better suited to your application.

[AM_MCM]

Hello all,

I noticed this topic and could use some advice on it. Here's the information I can provide:

1) Roku-Roku HC-548EX - Up to 32,000 RPM
2) Cylindrical die block 5" dia x 2" - 56-60 Rc, S7 Tool Steel
3) Finished part ranges from 0.25"-4"+ diameter
4) Depth of cuts ranges from 0.1"-0.7"
5) Currently using air, oil mister on the way
6) Using OSG Exocarb-WXS cutters - Ball nose, Stub length, 2 flute. Tools sizes:

DIAMETERS LOC
3.5mm (.1378") - 2.8mm (.1102")
1.6mm (.0630") - 1.3mm (.0512")
1.0mm (.0394") - .80mm (.0315")
0.8mm (.0315") - .60mm (.0236")
0.5mm (.0197") - .40mm (.0157")
0.4mm (.0157") - .30mm (.0118")
0.3mm (.0118") - .24mm (.0094")
0.2mm (.0079") - .16mm (.0063")
0.1mm (.0049") - .08mm (.0031")

I know that's a lot of info, but just wanted to get all the questions from the first reply answered. We are having success with the 3.5mm-0.3mm, but would like to optimise the feeds & speeds. However, the 0.2mm-0.1mm are the two trouble makers. We've been trying different F&S for these, but getting limited success. If anyone has any recommendations, please let me know!

One more thing, our tools are set by a blum laser (0.00001" tolerance).