Best milling finish on 6061

[SRT Mike]

Can someone suggest feed/speed and type of cutter to get the best finish on 6061-AL?

We face the part (need a good finish on that operation). Right now we're using a 2 flute 3/4" endmill for that. The parts vary in size but mostly we're talking 3" x 4" 3/4" thick. We also run around the sides of the part to clean it up. Sometimes it looks excellent, sometimes there are little scallop marks in the finish. I guess those marks are some slivers of material being dragged through the cut or something?

McMaster sells what they call "finishing" end mills. Are they worth the price? Does the rigidity of solid carbide help with a finish cut in AL? Should I go with a 3 flute (or more) and just take a light skim coat? Does cutter diameter matter? Does TiN or other coatings help?

The parts go into a vibratory bowl to remove machining marks so the less time they stay in the bowl the better, and the better finish we can get going in, the crisper the lines stay after the bowl does it's job.

Thanks!

[cdlenterprises]

Dataflute AFI endmills. They tend to be a little pricey but they last forever and I have not found anything that cuts aluminum better....

[HuFlungDung]

High helix angle flutes and high shear angle facemills seem to work the best for me. I also use flood coolant, as it is important to keep the cutter cold, so that the tendency of chips to weld to the tool are lessened. I think this accounts for the scuffing of an otherwise nice surface. Also, the chips need to be removed immediately from the cutting zone, so either flood or air is required to do this.

I would face mill a large surface, rather than zipping around it with a small tool.

I've found that Iscar helimills will do a really excellent job for finishing the bottoms of pockets. You need the special polished insert for aluminum, though. But for side milling, a high helix multiflute on an endmill designed for aluminum is going to give best chance at best results.

[SRT Mike]

Originally Posted by cdlenterprises Dataflute AFI endmills. They tend to be a little pricey but they last forever and I have not found anything that cuts aluminum better....

Hmm never heard of 'em. Are they specifically used for finishing or rough cutting also?

Right now we just buy either coated HSS or solid carbide mills from McMaster. They seem to last "OK" in Aluminum (we don't cut a ton of it, up until now) but I'd love something that lasts a long time.

[SRT Mike]

Originally Posted by HuFlungDung High helix angle flutes and high shear angle facemills seem to work the best for me. I also use flood coolant, as it is important to keep the cutter cold, so that the tendency of chips to weld to the tool are lessened. I think this accounts for the scuffing of an otherwise nice surface. Also, the chips need to be removed immediately from the cutting zone, so either flood or air is required to do this. I would face mill a large surface, rather than zipping around it with a small tool. I've found that Iscar helimills will do a really excellent job for finishing the bottoms of pockets. You need the special polished insert for aluminum, though. But for side milling, a high helix multiflute on an endmill designed for aluminum is going to give best chance at best results.

Thanks Hu. We were thinking of getting one of those big honking Iscar insert-able face mills - ever use those? The machine has a 6krpm max spindle speed but it's fully enclosed and we run Blaser 2000 series flood coolant. The little gouge marks seem to happen when slotting mostly (and sometimes we did that trying to squeeze as many parts into a sheet as possible) but lately we've been trying to space them out slightly more and running a very light cut around the perimeter at the end to clean up. I'll maybe try a high-helix 6-flute or something and just take a light shaving off on the side-milling pass at the end. Maybe the helix angle was what the miills marked "aluminum finishing" were all about. The less I can pay to the chromer the better

[mc_n_g]

Multiple influences on finish!
6061 is just miserable! Try to use 7075 or 2024 if possible.
Face finishing or side finishing (two different things). Finishing mills are best for side cuts.
HSS or indexable endmill?? If HSS use fast helix with raduised corners (not 90 degree). You will get slight gouge marks with any vibration. Use coolant. If Indexable use a polished insert for aluminum with rounded corner. Rounded corners do not dig in as much and provide a better surface finish provided they are run right. If you use coated it will gall to the coating or smear aluminum as it tries to cut it. You need a razor sharp edge (ground/polished) as opposed to the regular pressed insert. Don't skimp! Cheapness comes back to bite you in the ass later. Use as large of a diameter of end mill as possible for facing.

Stability of mill and bed. Don't expect mirror finish from a mill with a lot of backlash. CNC is better than manual if possible (providing you can code it right!)

The Iscar indexable endmills are nice. Anything which uses the APKT10.. series insert is usable providing you get a good polished/ground insert. High rate of rpm and cutting speed for final cut if indexable.

Use as short of an endmill as possible to reduce deflection and vibration. Also do not allow the quill to extend too far, try to keep it closer the top to help with stability.

mc_n_g

[cdlenterprises]

Originally Posted by SRT Mike Hmm never heard of 'em. Are they specifically used for finishing or rough cutting also? Right now we just buy either coated HSS or solid carbide mills from McMaster. They seem to last "OK" in Aluminum (we don't cut a ton of it, up until now) but I'd love something that lasts a long time.

They make a rougher and a finisher. The AFI stands for "Aluminum Finisher" and is a 3 flute higher helix. The roughers are called ARF or "Aluminum Rougher/Finisher". These are two flutes.

Another type is an SGS Ski Carb. I've used both with excellent results but if I had my choice I'd go with the Dataflute.

[RICHARD ZASTROW]

Keep the cutting speed above the weld point. I believe your marks in the finish are most likely caused from recutting chips. Personally I'd use an air blast/stream along with micro-drop coolant to blow them clear and cool the tool. Works for me.

[dcrace]

I also agree...as of yet, the best endmills I have run for aluminum are Data Flute. We recently have been using the new AFDH 1/2'' 5 flute for finishing and the finish we are getting both for end and side milling is incredible! Mostly running 15000 RPM and about 250''/min.

[joecnc1234]

The ski carb is a great endmill. I don't know the length of cut you're talking about, but I suspect the marks on the side of the part are form chatter or vibration. Use a high helix carbide em 3flutes seem to offset vibration well, as for facing use a shell mill, I think it is a kennametal or iscar with side mount inserts and sharp tips on the inserts. awesome finish. radius endmills work great for facing but poor for side mill finishing the tip is taking all the pressure where you want the sides to have some pressure on them to reduce chatter.
We used to rub the flutes with a penny to take the sharp edge off on long endmills to add a little tool pressure and take some vibration away. I hope this helps

[SRT Mike]

Thanks for the info gentlemen.

To answer some questions, this is on a VMC so we are using flood coolant. Max RPM available is 6,000. The depth of cut for the side milling is around .25" on one part and around .75" on the other part. I'd like to be able to use either a 1/2" or 3/4" mill - 1/2" probably better so I can pack them in a bit better on the fixture with less space between.

I looked at Dataflute - the AFDH. Supposed to be very good for Al finishing. I think I'll give that mill a shot. Anyone have any comments on pricing compared to other mills? For example 1/2" EM, 1/2" shank, 1" DOC perhaps? I can call around and ask but if it's one of those $300+ endmills I already know it's not gonna happen But if it's close to a regular high-helix mill that's OK. I just hate calling the reps if I don't end up buying anything because they hound me and ask to stop by and try to sell us stuff, or they just stop by uninvited! heh.

On the face mill...I had looked at the Iscar ones as well as the Kennemetal and Ingersoll. There are so many different options for an indexable face mill, like the number of inserts, insert geometry and the cutting head geometry. Again, I'd rather not call up a rep and tell him I want pricing on 30 different parts, so anyone got any suggestions on where to start with a face mill? Something around a 4" size would probably be perfect.

[cdlenterprises]

The Dataflute's should run you around $50-$60 a piece for an uncoated. Not sure about a facemill but they usually go for less than $300. Look for a package deal with the inserts and cutter body...they are usually cheaper.