3 Flute High Helix Endmill Problem

[Joe_CNC]

I've been having a bit of a strange problem with 3 Flute High Helix Endmills designed for aluminum. They cut very nicely with less vibration than 2 or 4 flute endmills, but the bottom surface of the cut comes out rather rough compared to a 2 or 4 flute. The profiled walls of the cut are fine.

Specs:

Haas Super Mini Mill
0.5" HSS 3 flute high helix endmill for aluminum, Centercutting
4,000 rpm - 10,000 rpm (500 SFM - 1300 SFM)
15 - 75 ipm (.001 fpt - .005 fpt)
.075 - .15 Axial DOC

6061-T651 Aluminum

Has anyone else experienced this problem?

When I run at the same speeds/feeds with a standard helix 3 flute, the bottom surface is much better, but still not as good as a 2/4 flute.

Thanks,
Joe

[steele]

Maybe it has something to do with thrust forces. That high helix is trying to suck the spindle out of the head-there's no upward thrust on the spindle bearings (preload lost?). I think you'll have to take an extra pass on the bottom or change tools. You might try putting a major hone on the cutting corners. With a hand stone grind the corner back so you have .010-.020" netural (0 deg.) rake on the very bottom of the end mill. Same as you would do to a drill that grabs when you break through on a piece of brass or stainless.
Jim
www.picopascal.com

[HuFlungDung]

I would guess that there is something wrong with the end grind of the teeth.

If the teeth are gashed to center with a simple vertical face, they will not cut very freely, so if you cannot improve the angle by regrinding with more rake, then a slightly concave end relief seems to work better, IMO.

If you are using a knee mill, the vertical head could be slightly out of adjustment and causing end of the endmill to drag along, too. It is something to check.

[Joe_CNC]

Thanks for the suggestions -

The mill is a brand new Haas VMC CNC (4 months old) and it seems to be in perfect alignment with no spindle runout or axial play.

The poor surface finish seems to be independent of cut depth, even a 0.001 Axial DOC cleanup pass still comes out rough.

When I replace the 3 flute high helix with a cheap 2 flute endmill, the bottom of the cut comes out like a mirror, but the performance of the pocketing operation is not nearly as efficient as with the 3 flute.

I've tried pretty much every speed/feed/doc combination, but still experience the same problem.

[ESjaavik]

Check the bottom surface with a magnifier. The nature of the roughness may give you a clue to the reason. Chatter marks, marks from a dull bit or wrong ground bit, and other causes usually looks different.

[dcook]

3 flute high helix endmills are meant to be used in a climb cut. Conventional cutting with one will tend to force chips to the bottom of the tool where they get recut several times before being ejected. The end-grind of a center cutting 3 FL EM is very difficult since all 3 flutes have to be ground perfectly. I would suggest a high quality carbide endmill. Also if you run the endmill at 10K rpm your feed can be much higher, more like 125 to 150 IPM. Never had this problem with carbide tools, never tried high speed.

[Paul_S]

End Cutting will always have a worse finish then the side cutting at the same feed. If you are trying to get a good finish on an end cut you must go much slower than you would use for a side cut.

If you know the angle on the bottom of the end mill you can calculate for a approximate finish.

I assume a 1.5 deg angle.

And I calculate for a 125 finish to start, and see how it looks.

I make my feed calculation as if I only have one flute cutting. (With a good end grind with a 2 of 4 flute the feed can be increased by the number of flutes maybe.)

For a 125 finish I calculate 250E-6/tan 1.5 x RPM

250E-6/tan 1.5 will give you a feed of .0095 per revolution.

For a 63 finish I calculate 126E-6/tan 1.5

Which gives me .0048

Again this is per revolution. Not per flute.

So for a 125 finish .0095 IPR
For 63 finish .0048 IPR
For 32 finish .0024 IPR

Now if the cutter has a radius on it, you can go a little faster and get the same or better finish.

To calculate a finish with tool radius, the method is more accurate and predictable.

Using the following equation:

Were the finish is for example 32 becomes 32E-6 ( 32. x 10^-6)

4 x sqr(32E-6x(radius - 32E-6)) = IPR

If you want closer to a Ra or RMS finish the correction is:

sqr(183/125) x 4 x sqr(32E-6 x (radius - 32E-6)) = IPR for a RMS type finish.
sqr(183/111.52) x 4 x sqr(32E-6 x (radius - 32E-6)) = IPR for an Ra finish

63 would be 63E-6 in the equation, 125 would be 125E-6 in the equation.

If a finish is not as good as you think it should be or an inspector says it isn't as good. Make a IPR correction as follows.

old IPM (or IPR) x sqr(finish wanted/known finish) = corrected IPM (or IPR)

For sharp end cutting tools, end cutting, use a direct ratio.

old IPM (or IPR) x (finish wanted/known finish) = corrected IPM (or IPR)

Note, all finish feed rates should be calculated by IPR not IPT.

Only end cutting one might be able to increase the feed per tooth. Only with ground EM. Otherwise always IPR.

I hope this info will help.

One more thing, some materals may require as much as 20% decress in feed. Which can be calculated/corrected as noted above.

[machiner11]

1st off, I think you're at the high end of your SFM. 500SFM is pretty quick for a HSS end mill. Why not go carbide? Kodiak Cutting tools has zirconium coated, aluminum cutting geometry, end mills that work great!!

2nd, how are you holding the tool? Collet Chuck? Milling Chuck? or with a single setscrew in the side of the toolholder?(the worst possible way for good finish)

3rd, place an indicator down at the end of the cutter and indicate the runout of the .5 dia. Is it running out more than .001? That would cause a problem.

next, the bottom of all end mills are a concave in shape. As such, the way the three flutes come together in the very center does not matter, because as you cut across the face/bottom, only the outter tips of the cutter should be engaged.

Coolant....Sometimes coolant can make a huge difference. I was using a cutoff tool in a lathe and had terrible tool marks using "AstroCut". I switched to a Master Chemical product and the marks vanished.

The material....Sometimes aluminum sucks!! I forget which one but either 6061-t6 or 7075 have a quirky heat treat process done to them. Very difficult to drill and have a good finish. Maybe it's just the material?