tiny endmills, big problems

[Mike_ICE_Pro]

im cutting some fairly soft steel with a 3/32 enmill at .03 depth. the tool will get through about 5 min. before breaking. it is only hss and i have already ordered some cobalt and carbide bits. does anyone have any sugesstions? thanks in advance

[JazzBass]

Mike,

 

What kind of steel?

[robk]

What are your speeds & feeds?. It's been a while since I even saw HSS. Take a shallower cut, but increase your spindle speed and feed.

[robk]

BTW, welcome to the forum

 

quote:

---

What kind of steel?

---

+1

[Threept82]

For something like 1040 crs

IF POSS. RPM 6200 @ F2.4 at .030 deep.

3 flt, best

4 flt, ok

2 flt, hope not

flood coolant

[Eeyore-nonhuman forum member]

I would go :metric for end-mill 2.5 mm end mill with coating Ic900 (iscar classification ) or X-power Y-|G grade on mold steels :

depth of cut 0.25 mm slotting

s11000 f900

Cooling air 4 fleets extra-short (rigid)

Good balancing of toolholder is the must

of for spindels like mine with 8000 rpm

S7850 f750

tool life hours !

HTH

[Kevangel]

If you can tip the milling head a few degrees this can help you cut.... if you can and you have enough parts to justify this...carbide,carbide,carbide.there are some low cost carbide sources out there.

[The Iron Chef]

Runout is a problem with small cutters. Check it with an indicator. you will have problems with anything more than .0005. tir

 

HTH

-Keith from home

[ChuckM]

Use a coated carbide... TiN at a minimum and TiCN or TiAlN depending on the type of cut. You'll likely want as much rpm as you can get. At something like 10000 rpm, you're 3/32 end mill is only achieving ~245 sfm. If you can achieve 300+ sfm for carbide, that will help boost your productivity.

 

+1 to the 3-flute recommendation and using a short LOC. Robbjack makes a very economical 3-flute "Tuffy" end mill and other companies offer something similar. I would run a chip load somewhere around .0004-.0005 per tooth, 20-30% of diameter in axial depth of cut. Use your best tool holders (least TIR) and high pressure coolant or cold air.

 

Good luck.

 

-Chuck

[TKDBB]

.03 WAY to deep for a .093 cutter. Try .008-.01 per pass

[Threept82]

RPM 6200 @ F2.4 at .030 deep.

3 flt, best

[Paul McGarr]

quote:

---

If you can tip the milling head a few degrees this can help you cut

---

Ok, I have to ask. What would tiping the head do?

 

Paul

[Threept82]

quote:

---

Ok, I have to ask. What would tipping the head do?

---

Me to. Tilting the head would result in a

radial slot.(Much less pressure on end mill)

He would then have to square head to finish slot. (If that’s what you mean.)

 

That being the case, ruff with ball mill, finish with square end mill.

[Paul McGarr]

[robk]

quote:

---

RPM 6200 @ F2.4 at .030 deep.

3 flt, best

---

Man, if those are the speeds and feeds for HSS I would fall asleep for most of the day

I agree on the 3 flute part, but spend the $20.00 or so on coated carbide and get the job done in a timely manner. JMO

[Threept82]

I agree.

But Mike Egbers said he was using H.S.S.

[Charlie Pierson]

I would bet the problem is runout.

On one job we have (using 3/32 xtra length carbide .05 depth / pass in alumium ) we used to go through 3 endmills a day. Changed holder to Nikken Mini-Mini chuck and now we use 1 endmill per month (job runs 24/5).

[Kevangel]

"Tilting head", oops.. thought he was using ball end mill. I am in too big of a hurry. If, its a ball cutter ,by tilting head you can cut more on the side(down near the bottom of the ball the surface speed is real low) An old toolmaker showed me this trick years ago, it works!

[Eeyore-nonhuman forum member]

Not to brag ,I do not regard this mill as tiny ,

I work on mold steels and hardened all the time and have only 8000 rpm on my main mill, anyway I mill on copper and steel with mills 0.5,0.3 mm and with good tool life .

.

A key to success- good tooling ,perfect collets ,extra-clean ,good mills ,Good coating if possible ,reasonable depth of cut and feed fast enough .

I mean I prefer to reduce depth of cut and to enlarge feed .

My credo :

The tool must cut ,otherwise it will not stand long enough .

IOW,better greater feed than slower feed .

And good technology ,the way you cut is always important .

I prefer as much teeth aas possible ,for tools 1.5 -2 mm diameter 4 teeth is OK ,they are strong enough ,and with reasonable (not too big ) depth of cut you will get greater feed .

HTH

[ChuckM]

Ahh, "small" and "large" are all a matter of perspective. The company I use to work for machined features as small as .015 wide on a regular basis. Now everything I work with is 3/8" and up. Doesn't really matter one way or the other... other than issues with TIR and getting enough sfm to be productive. Charlie Pierson makes a real good point about his findings with TIR. If you do a lot of small tool milling, might be worth looking into a toolholder like Lyndex's "Bullseye" etc and nip that stuff in the bud.

 

I am of the school of machining which would suggest the largest depth of cut possible in this case. Don't think horsepower will be an issue.

If you run .010 doc, you're gonna need to go 36 ipm to equal the metal removal rate you could get at .030 doc and 12 IPM. So it's always important to look at MMR when estimating the productivity of an operation. I do this a lot when looking at different milling operations.... quite revealing.

 

If you can get away with 1xD in doc like Degmc has had success with... do it! I would take a serious look at the reduction in cycle time versus the cost of replacing the tool. It may very well save you money to change the tool after every part. Never know til you crunch the numbers.

 

Good luck.

-Chuck

 

[ 12-29-2004, 08:03 PM: Message edited by: ChuckM ]

[Mike_ICE_Pro]

thanks to everyone, yall have been very helpful for a green machinist. could work hardening be an issue?

[Threept82]

Depends on material type but with soft steel it should'nt be a problem.

[MCam Newbie]

Quote:"Ok, I have to ask. What would tipping the head do?"

 

If you could do it, tipping the head would avoid the "Zero S.F.M." at centerline of cutter, thereby reducing radial pressure on the cutter. This assuming the tilt shifts the cutter center out of cut, or to the trailing edge of the cut.

 

M-Cam Newbie

[Threept82]

But...

It also puts move side pressure on the end mill

so depending on l.o.c or how far out of the holder

the end mill is, it could create move headaches then he already has.

[mrainey]

Would you still get a flat bottom if you were slotting with the head tipped?