[cnczoner]

I'm going to order endmills for aluminum cutting and facing and looking for a good finish. So far with a used unknown HSS 2-flute bit I can get decent results in 6061-T6 (which will be the material I'd use). My mill is a CNC'd HF geared head benchtop mill (a bit bigger than an X3), 1500rpm max.

So far I've figured out, learned, deduced, and decided I need 2-flute, un-coated HSS, high-helix angle, centercutting. I'll probably get roughers and finishing endmills. But how do I know the difference between one manufacturer's endmills and the other? Is there any other spec I should be looking for, or enquiring about? In other words, should I get the on-sale ones at Enco or Discount Tools, or should I be looking at Seco, Kennametal, Dataflute etc? I know not to get the HF ones. And how would I know that they do what they say? I'm not a production shop, but will be doing my prototypes and one-offs for customers so it'll be very low volume, so not sure that the big names would even want to speak with me.

Finally, what sources are good for these endmills? I know of Enco, MSC, Discount Tools and American carbide, but haven't found some specific types yet (such as bevel-cutting bits).

Any info appreciated. Thanks,
-Neil.

[Shotout]

If you look on the MSC website under Single Endmills they have a sub section on Alum cutting, all the tools in it are rated by the manufacture for cutting alum. Use the drop down menus to select length and dia etc to narrow your selections and sort by price.

Beveled cuts, if you mean chamfers search drill mills. All sizes of 90deg (cuts 45deg chamf) cutters there. I use these a lot to chamfer holes just to clean the edges or before tapping to give a better tapped hole, chamfer to print spec as well as chamfers down of .005 along the contours of a part just to break edges for a better finished part. A search for chamfer will bring up chamfering tools of various degrees and dia as well. Every part we make (excluding countersinking screws) call for 45deg chamfers when one is called for so I prefer drill mills over regular chamfering tools and even use them as spotting drills sometimes to minimize the number of tools I have in a program.

Hope this helps
Scott

[Surfacefeet]

Check out this link for Minicut:http://www.minicut.com/index.html

[Swiss]

I've spoken to the technical help people at a milling bit company and asked them about milling aluminium. What they told me was that aluminium is quite a sticky metal, and tends to weld itself to the tool, creating a built-up edge. This effectively makes the tool behave as if it were blunt. Some tools are coated with TiAlN, which reduces the amount of welding which happens, and lets the tool last much longer than an uncoated one.

One of the tools we use for alu is a 4mm diametre, 4 flute, TiAlN coated, 45 degree rake angle. It cuts well at 5000prm and 0.006mm feed per tooth.

hugo

[SRT Mike]

We mill a decent amount of aluminum. I've found the really cheap endmills don't work so well (the Chinese import junk from Grizzly or Harbor Freight). They are sort of OK in a pinch, but they dont last long and I think the tool geometry isnt very accurately ground, because finish sucks.

Then you have the regular mills you get at MSC and McMaster. Thats what we use for 99% of our cutting. Solid carbide works better than HSS, and TiAlN (I believe it's that - the gold one) helps prevent gumming of the bit and chips welding to the end. You're limited on RPM's and feed with a smaller machine, but I can tell you we experienced a WORLD of difference between crappy mills and decent ones from MSC, both on a Grizzly mill-drill and a Leadwell V-40 40x20 VMC and a Leadwell MCV-0 mini-VMC.

You probably want to use a 2-flute for slotting and most pocketing, but for a really nice finish, we find a high-helix 4-flute (or even higher, maybe 6 flute) with as much RPM and a real light cut (maybe a few thou) produces very nice results. You can sort of see the toolmarks, but you can barely feel them, nice crisp corners with no burrs, etc.

The grade of Al matters too... if it's from a known supplier it should be fine, but I've sometimes found offcuts that werent marked that didnt machine very well. I suspect they were sold as 6061 but probably were another alloy.

[Geof]

.... I'll probably get roughers and finishing endmills.....-Neil.

Definitely get the roughers; I forget what they call them...gash toothed or something. When you are limited in speed and power they make the world of difference in removing metal quickly.

And regardless of your cutter type for a good surface finish some form of cutting fluid is essential. A readily available and cheap alternative to regular cutting fluids is ATF automatic transmission fluid. Paint it along the cut line or have a little sprayer can, you don't need much. Or you can go with regular cutting fluids and a mister system but that needs an air supply.

[tauntdesigns]

2 -flutes works for just about everything alum.. climb cut the finish passes.

toothed roughers work well but I always liked the 3-flute, and crest cut cutters for roughing (hogging) ops.

[John3]

We cut tons of 5052 alum sheet which tends to be gummier than 6061. We have had great luck with single flute aluminum cutting carbide router bits from Onsrud. The single flute has plenty of chip clearance. We run them fast. 3/16 at 12,000 to 15,000 rpm, 3/8" at 5,000 to 6,000 rpm. We run these on our router, in our VMC and on CNC-Knee mills.

Boelube is a great coolant lubricant for this work if you are spray misting. Brush-on we've had good success with kerosene and Tap-Majic for Aluminum.

For more conventional work we find that two flute HSS aluminum grind endmills work good. On the east coast US, Travers Tool Company is usually more competitive price wise than MSC for what we buy and they have next day delivery too.

John

[cnczoner]

Wow, someone woke up this thread
Timely-ish though, as I finally got around to ordering the end-mills on Monday (I had some setbacks with re-building my CNC controller) and they'll be here by Friday. I got some high-helix HSS 2-flute cutters, some ball end mills, some drill-mills, and a rougher. For now, I went with some enco parts, but did n't see anything I thought would be great for for finishing from them. I'll probably be trying out a Hanita 2-flute 1/2" bright HSS end mill from MSC, or perhaps some other cutter from a different source. I do order regularly from McMaster (other things), but have never checked out their end-mill selection.

In my discussions with tool companies (manufacturers and outlets who know end-mills, rather than just Enco etc who seem to be catalog houses), research, and some experimentation, I found out some interesting things...
- Coatings extend tool life, rather than create a better finish. Apparently a coating results in some rounding at the cutting edge rather than uncoated which can be sharpened to a very sharp edge. This is the first I've heard about that TiAlN though.
- Coolant/lube is a must with aluminum. I'm currently using WD-40 (and plently of it), which most say is decent, but I'll find something more optimal (such as a misting or drip system) later.
- Aluminum grade is critical. See my other post here. I picked up some 2024 and 7075, but have not yet tried those.
- High spindle speeds is a must. Since my mill will only do 1500rpm, the recommendation was to cut very slowly. I got better results with a light finishing pass at 2ipm rather than at 10ipm (spindle at 1500 rpm in both cases). I am working on adding a VFD/motor change in the future.
- A larger diameter cutting bit will increase surface speed of the cutting bit.
- I got better results cutting a "light" finishing pass (maybe 10-20 thou) than I did cutting a "super-light" cutting pass (such as a few thou). Don't know if the latter is small enough that the backlash/flex causes the mill to "go around" the material that cut through it. That's the theory running thru my newbie head right now. Note that my mill is sturdier than the X2, X3 etc.
- Backlash will cause finish issues. I'm working on doing a ballscrew conversion in the near future.
- Many suggested that 3-flute high-helix will work just as well as 2-flute, but everyone felt that 4-flute would be worse.
- Best bang for the buck with my existing setup will be to use a rougher first, at a higher cut speed (say 20-30ipm), then finish at a few ipm. My thought is to remove as little material as possible for roughing so I'm going to try a 1/4" or 3/16" rougher. Then for finishing I'll use a 1/2" or larger 2-flute HSS high-helix.

I'll post results when I get some.

Cheers,
-Neil.

[SRT Mike]

- Coatings extend tool life, rather than create a better finish. Apparently a coating results in some rounding at the cutting edge rather than uncoated which can be sharpened to a very sharp edge. This is the first I've heard about that TiAlN though.

Yep we get a lot more time out of TiAlN before we toss 'em than with uncoated mills.

- Coolant/lube is a must with aluminum. I'm currently using WD-40 (and plently of it), which most say is decent, but I'll find something more optimal (such as a misting or drip system) later.

Look into an air blast. I dunno if the lube is as important as just keeping it cool. We use flood coolant - before that we got gummy torn edges, now they are razor sharp.

- Aluminum grade is critical. See my other post here. I picked up some 2024 and 7075, but have not yet tried those.

7075 machines beautifully. Its harder than 6061 so it solves the gummy issue and it tends to cut rather then be pushed by the cutter. I love 7075, except you cant anodize it, its heavy, and its expensive

- High spindle speeds is a must. Since my mill will only do 1500rpm, the recommendation was to cut very slowly. I got better results with a light finishing pass at 2ipm rather than at 10ipm (spindle at 1500 rpm in both cases). I am working on adding a VFD/motor change in the future.

Dunno about that... we were able to get great results on an old Bridgeport CNC conversion with a 3k rpm spindle. RPMs are great for high speed machining, but you can cut AL just as well with 2000rpm (or 1500rpm). You gotta keep it cool though or any RPM will end up bad

- I got better results cutting a "light" finishing pass (maybe 10-20 thou) than I did cutting a "super-light" cutting pass (such as a few thou). Don't know if the latter is small enough that the backlash/flex causes the mill to "go around" the material that cut through it. That's the theory running thru my newbie head right now. Note that my mill is sturdier than the X2, X3 etc.

If your toolmarks from the roughing are bigger than 5 thou, then a 5 thou finish pass won't take them all off - that could have been the issue too.

- Backlash will cause finish issues. I'm working on doing a ballscrew conversion in the near future.

Probably more of an issue on direction changes, I'd think. Once the nut is loaded it should be able to provide a pretty consistent finish. On direction changes, the time it takes to take up the backlack causes a 'dwell' which changs your feedrate and can affect finish (and allow heat to build up and gum up the cutter, in extreme cases).

- Many suggested that 3-flute high-helix will work just as well as 2-flute, but everyone felt that 4-flute would be worse.

For light finishing passes? really? Wow I am surprised they said that. Hasnt been my experience. You get those little "scallops" when you look at the side of a milled part. With a 4 flute (at the same RPM), the scallops are more numerous and each one is less deep. High helix makes the little scallops less tall. A larger diameter cutter has less deflection and gives a nice finish. A 4 flute 1" end mill taking a .010 finish cut down the side of a piece of 6061 with flood coolant provides a very nice finish, provided the RPM's are high enough and the fixture is solid. I'd think a 4-flute would somewhat make up for your lack of RPM's. I'd try it, for sure, you may be surprised how well a 4 (or 6) flute works on a side milling finish pass!

- Best bang for the buck with my existing setup will be to use a rougher first, at a higher cut speed (say 20-30ipm), then finish at a few ipm. My thought is to remove as little material as possible for roughing so I'm going to try a 1/4" or 3/16" rougher. Then for finishing I'll use a 1/2" or larger 2-flute HSS high-helix.

Dont you want to remove as much as you can during roughing? Roughing is where you don't care about finish so much. Are you profiling? If you're not, I'd go with the biggest end mill that your machine can reasonably turn that will fit in the spaces of the part. A 1/4" rougher is going to have a fair amount of deflection compared to a 1/2" or 3/4".

Good luck! Keep us posted.

I'll post results when I get some.

Cheers,
-Neil.[/QUOTE]

[JROM]

First you can anodize 7075 you just have to tell them the alloy.
next forget HSS, carbide is the way to go. It is more money up front but your finished parts will be much better with carbide. Try to find a Garr dealer in your area. These are very high quality cutters with good prices. I cut alot of 6061t6 and I use three flute 50 deg. helix carbide endmills uncoated. If you can run at about 7,000 rpms 100 IPM with a 3/8 or 1/2 dia cutter. Also use cutting fluid, alight cutting oil will work fine I've used kerosene (Colman fuel)
or any good water based coolent. These cutters work like the desplays you see at the trade shows. Give it a try

[big_mak]

You can try the Garr VHX roughers. They don't mention using them in ally, But I'm running them @ 10,000 RPM and 200+ inches a minute @ roughly .25" deep. Garr 242M seris is the 2-flute version for aluminum. Works like a hot damn. OSG makes some nice aluminum mills too.

[big_mak]

SRT,

Spindle speed is pretty crucial if you are intent on spending the money on Solid carbide. Your not going to see any of the performance benefits that will justify the cost. 1" HSS and 1" Carbide endmill are no where close in cost. with a 1500RPM machine, I wouldn't bother with Carbide. Lube is gonna be critical, otherwise what's to stop the material from sticking to the cutter.

[big_mak]

For aluminum as well, if you need a cheap alternative for form tools, you can use carbide router bits.

[cnczoner]

Look into an air blast. ...

Oops, I forgot that. I am using air blasts from a small compressor/tank/nozzle and manually blowing out chips. I need to regulate the pressure down a bit as it's blowing chips quite far and I'm guessing it's blowing the WD-40 away as well.

7075 machines beautifully. ... its expensive

Hence my intent to use 6061-T6.

Dont you want to remove as much as you can during roughing? Roughing is where you don't care about finish so much. Are you profiling? If you're not, I'd go with the biggest end mill that your machine can reasonably turn that will fit in the spaces of the part. A 1/4" rougher is going to have a fair amount of deflection compared to a 1/2" or 3/4".

Actually not, as my parts will mostly be made from 3/8" or 1/2" alum plate, and most features will get cut through, so a thin rougher should eat through each circle quicker. Here is an example of a small version, but others will be maybe up to 16" x 8" with more holes and some may even look like picture frames with only about 1/2" edge left...


FWIW, I'm not sure I would get a great finish on the top surface, so I'm thinking I'd lightly hand-sand and polish or brush with a wire wheel.

BTW, these are plates to hold automotive gauges.

Cheers,
-Neil.

[cnczoner]

... But I'm running them @ 10,000 RPM and 200+ inches a minute @ roughly .25" deep. ...

... If you can run at about 7,000 rpms 100 IPM with a 3/8 or 1/2 dia cutter. ...

You folks are running bigger/faster/more powerful machines that I am. My max spindle speed is 1500rpm right now, with a 1.5hp motor. Whereas machining speed is not a big deal to me (my products will be very low-volume), I'm sure that the cutter selection will be much different for my setup.

Cheers,
-Neil.

[SRT Mike]

Actually not, as my parts will mostly be made from 3/8" or 1/2" alum plate, and most features will get cut through, so a thin rougher should eat through each circle quicker. Here is an example of a small version, but others will be maybe up to 16" x 8" with more holes and some may even look like picture frames with only about 1/2" edge left...


FWIW, I'm not sure I would get a great finish on the top surface, so I'm thinking I'd lightly hand-sand and polish or brush with a wire wheel.

BTW, these are plates to hold automotive gauges.

Cheers,
-Neil.

Cool parts. Bear in mind you won't want to go more than about 1/2 the bit diamater for depth of cut. So with a 1/4" bit, you would be about 1/8" DOC. If you are making that out of 1/2" that would be 4 passes. If you moved up to 1/2" bit you could do it in two. Also, the 1/2" will be a lot more rigid, but it depends on whether you have the power to take the cut (but I bet you can easily take 1/4" DOC w/0.5" mill).

One other thing to keep in mind if this isn't a part you've cut before, is what happens to the slug when it's cut. Sometimes it helps to leave tabs that you can cut out later because sometimes when those slugs of metal you're cutting start to come loose, they shake all around and gouge up the part, or get smacked into the part when they finally come loose and the cutting fires them across the machine

[Geof]

....One other thing to keep in mind if this isn't a part you've cut before, is what happens to the slug when it's cut. Sometimes it helps to leave tabs that you can cut out later because sometimes when those slugs of metal you're cutting start to come loose, they shake all around and gouge up the part, or get smacked into the part when they finally come loose and the cutting fires them across the machine

My experience is that they nearly always break the cutter.

An alternative to the tab idea is drill holes at the center of each slug and bolt the stock through these holes as well as clamping the edges. Then the slugs stay in place.

It is a play off between spending the time drilling the holes and bolting or leaving the tabs and then spending the time cleaning up the lump that is left after breaking them. Using bolts means the circles are fully finished on the machine and have an even finish all round; it is very difficult to blend in the tab removal nicely.

[SRT Mike]

My experience is that they nearly always break the cutter.

An alternative to the tab idea is drill holes at the center of each slug and bolt the stock through these holes as well as clamping the edges. Then the slugs stay in place.

It is a play off between spending the time drilling the holes and bolting or leaving the tabs and then spending the time cleaning up the lump that is left after breaking them. Using bolts means the circles are fully finished on the machine and have an even finish all round; it is very difficult to blend in the tab removal nicely.

Good advice. What we did with the tabs was leave them during roughing and then use a dremel to cut the tabs and remove the slug, before the finishing operation - then use the finishing to clean up the leftover material from the tab. The only reason we did this was so we didn't have to make a fixture for bolt holes.

Bolting the slugs down (or securing them somehow) is *definitely* the way to go if you're making multiples of the same part, and tabs can be helpful too for one-offs.

[Geof]

... The only reason we did this was so we didn't have to make a fixture for bolt holes. ...

These days my company makes multiples but back in the days when I was doing one-offs for people I had a variety of plates with holes tapped on 1/2" or 1" centers. Nearly always when I needed to bolt something down I could drill it to use these pre-existing fixture plates. They also came in handy for holding parts down with perimeter clamps and because there were numerous holes it was a snap to move the clamps to finish a complete perimeter.