View Full Version : Dry Machining Aluminum With An Idexable Mill??

08-27-2006, 09:14 AM
Anybody dry machining 6061 aluminum with an indexable endmill?? If so, what tool are you using? Right now, I am running carbide with flood coolant and it is a mess to clean-up. I was wondering if a small air-nozzle to clear the chips and a good 2 flute helical indexable would do the trick? Any experience out there?

Forgot to mention that I am limited to a cutter size of 1/2" diameter for the parts I am running.


08-27-2006, 11:33 AM
try this set up http://toolsupply.com/2000/Web%20Library/Kool%20Mist/KMGPMistingSystem.html
if you try to cut dry the alum. will weld to tool

Tru Cut Machine
08-27-2006, 05:28 PM
I recommend Kool mist. In aluminum you must have something (even an occasional spray of wd-40) to prevent cutter load up. Cheers.


08-27-2006, 08:43 PM

I run Iscar Hellimills all the time dry in 6061-T6511..

But mine are all 3/4" and up..and I machine light and fast..typicly .075 to .100 depth of cut..with the APCR inserts..Grade IC28..these are the polished high rack AL inserts..cut like Dream..

I looked and Iscar makes a .500 holder..but it is only a 1 effective ..all mine, being bigger , are 3 or 4 effective...

I believe I've seen some smaller insert ones that have more inserts....I think Nano Turbo is the name..Seco I think...

08-27-2006, 09:16 PM
I have been the kool mist route in the past too. It created a "fog" in my garage; which I did not care too much for. Made it difficult to breathe. I guess if it was in a large open shop it might not be so bad. I have been running flood, and it does a great job, but it is a pain to clean-up at the end of the day.

I have looked at the Seco / Carboloy cutters a number of times; and have wondered if they were worth the investment. What type of speeds / feeds are you running your Iscar cutters? I have some outer profiling on my parts that I could use a larger diameter cutter on.

08-27-2006, 10:05 PM
I run the 1" 4 fl Helimill at 5200 to 5600 RPM and feed at 100ipm..with those depth of cuts..(.075 to .100). 90 percent engagment is about normal for me..

If you want a really good mister that doesn't fog your shop try a FOGBuster..plus you can use it for just air too..


Defiantly worth ever penny..

08-27-2006, 11:30 PM
I have been using my Lovejoy Face Mill....dry on Mic6....no problem at all....not sure if running dry will lessen the index insert life.....

08-28-2006, 01:10 AM
[QUOTE=snakebit95]I have been the kool mist route in the past too. It created a "fog" in my garage; which I did not care too much for. Made it difficult to breathe. I guess if it was in a large open shop it might not be so bad. QUOTE]

The nozzles on the spray misters are adjustable, if you tighten them you get a fine mist, if you loosen it, you get more fluid and less mist! I have mine set to a slow dribblel and it keeps the cutter very wet! I hate all that spray mist too, it sticks to my eyeglasses!

08-28-2006, 06:56 AM
Thanks guys!! I am still not sure what I am going to try. I may pick-up one of the smaller seco cutters when they are on sale, and run it dry to see what happens.

08-28-2006, 07:20 AM
we use high polished uncoated carbide and an oil mist However In my opinion nothing cuts aluminum like high speed steel

08-28-2006, 11:47 AM
I think you'll be disappointed with the performance of an indexable endmill in aluminum, unless you have a high speed machine and controller. (I'm not talking about face milling)

The real advantage of using insert tooling is being able to take advantage of the very high surface speeds. With large facemills, this is easy, but with small cutters (like 0.5") and aluminum, it is quite difficult to attain the proper surface speeds unless you have a very fast machine spindle and controller.

My spindle limit is only 7500 rpm, so I have been VERY dissapointed in my 3 flute 0.75" Seco Turbo in aluminum, because I can't spin it fast enough. However, it does a great job in steels (because it can go fast enough for steel). It can't clear the chips when used in aluminum unless I use a light cut, and the resulting material removal rate is inferior to 2 or 3 flute solid carbide tools.

So, for my machine, I am better off using solid carbide tools and deeper cuts. For example, with a 0.5" 2 flute solid carbide endmill, I routinely remove 19.2 cubic inches per minute dry cutting. (40% engagement, 0.8 DOC, 120 IPM @ 5000 rpm) Why not go 7500 rpm and 180 ipm? Because I don't need to go any faster, and I don't want to listen to my cogged spindle belt at that speed.

To be realistic, I'm not really crazy about running this dry for long operations because it builds up a lot of heat in the toolholder. The surface speed still isn't really fast enough to pull the heat away in the chip.

Also, with 6061, you will still [probably] need some sort of mist coolant if you want to dry or MQL machine your parts.

08-28-2006, 12:07 PM
THANK YOU VERY MUCH!! Very informative feedback based on real-world experience. Exactly what I was looking for!! My spindle is limited to 5K, so it does not sound as if the indexable mills will perform very well on my machine / application. I have been running carbide successfully, but was just looking for alternatives that would allow me to eliminate the messy coolant.

Would you mind sharing what carbide endmills have been working well for you when machining aluminum? I have had very good luck with the Hanita 3-flute high-helix endmills; and was also relatively happy with the Travers Superceed 3-flute high-helix cutters. I have been hestitant about trying either of them dry due to clogging. Perhaps the 2-flute high-helix would be better suited to dry machining?

08-28-2006, 02:08 PM
SGS Ski-carbs.

Accupro ZrN 2 flute endmills (fairly cheap, it is a usual msc monthly special). The 3 flute version cannot be fed as fast as the two flute, but leaves a better finish.

I recently bought some SGS S-carb endmills for an upcoming production run. I tried the 3/16" size...and BAD chatter under very conservative cutting conditions, but I'm blaming the very long flute length. I'll try the 0.5" and 0.75" in the next week or two.

After re-reading my initial post, I may have been unclear about what I meant about a high speed spindle "and controller." With elevated feed rates, the machine controller needs to be able to keep up with the high feedrates that will be possible with the high spindle speeds. Having said that, if I were able to "slap" a 20,000 rpm, 30 hp spindle on my machine, my machine's controller will be worthless at 300+ ipm. (sure, it can "do" it, but not with any sort of accuracy...it tries to lead turn corners, and then overshoots)

08-28-2006, 04:52 PM
I have never tried the Ski-carbs. Their advertisement makes me feel like it is almost a gimmik - LOL. I do not believe much of cutter company's advertisement, since I have been disappointed in the past with cutting expectations. I try to rely on real-world feedback before I spend the money on these high-dollar cutters. We use a lot of Hanita stuff at my regular job, and that is how I started using them on my home machine. Thanks again for your wealth of cutting information!!

08-28-2006, 05:23 PM
Yeah, I hear you on the advertising. I'm very skeptical also until I see things for myself. Just because of the price, I wouldn't touch a Ski-carb until a friend recommended it. They are my favorite, but most of the time the job cannot justify the price.

IMO, the biggest advantage of the Ski-carb is the consistently good finish. From a material removal standpoint, the 2 flute ZrN Accupro does just as well. However, a 3 flute Accupro with a reduced feed rate will usually leave the same finish as a Ski-carb, but sometimes you get one from Accupro that will leave a "stripe" on a profiled wall.

I'm being really critical on the finish quality...and I'm not sure if it matter that much in the first place because the part is likely to get a noticeable scratch against the nice finish the first time it is handled.

I've had people mistake the profile finish from a "good" Accupro 3 flute ZrN endmill for being a ground finish (same with Ski-carb). But I'm also using a hydraulic toolholder, which helps a little.


08-28-2006, 07:08 PM
I have good success with Hantita's 2 flute. I use flood coolant though. I have run dry just not very long. I would be worried about at least some build up on the tool edge. If you had to run dry though I would use a 2 flute.

08-29-2006, 04:24 PM
Yes, I was thinking 2-flute too. There does not seem to be enough clearance on the 3-flutes to run them dry, and probably would not eject the chips as well either. I have not tried the 2-flute Hanita's yet. I noticed they offer quite a few styles. Which one are you running?

08-29-2006, 06:36 PM
I will have to check it out when I get to work tomorrow. I will post it then. For the life of me I can't remember. Man I'm not even 30 and forgeting details. Is it all downhill from here?

08-29-2006, 09:56 PM
Don't feel bad.......it has taken me 34 years to learn not to buy China-made machine tools - LOL. I think it is probably better to be forgetful, than hard-headed!!

08-30-2006, 09:04 AM
I use the Javelin Series 2, but like I said I don't run it for long periods of time dry so I can't guarantee how well it holds up before some build up occurs.

08-30-2006, 12:52 PM
I have been using the Javelin 3-flutes, and they have worked really well under flood coolant; especially with ejecting the chips (and coolant). Next time I order, I will get a couple 2-fluters to try dry and see what happens. Worse case is I snap them off or stir-weld some parts. Anybody need any aluminum parts stir-welded?? LOL.

09-03-2006, 10:16 PM
If you do not have the RPMs (1500 sfm would require 12000) you will be disappointed. I would suggest three flute carbide and small DOC and very high chip load. The trick is to prevent the heat from cutting moving ahead of the cut. Climb cutting is mandatory because the heat tends to remain with the chip and not in the work piece. If you see the finish changing, up the feed to help. Very few machines have enough RPM to over speed a .5 tool in 6061. Guestimate for profiling would be something like... All the RPM machine will give, .05 radial DOC and .005 chip load. Yes this is not aggressive but you are trying to go dry. A tight spiral on tool will help. I would not attempt to cut pockets without something to flush chips even on horizontal.

09-04-2006, 07:41 AM
Thanks for the feedback ctate2000. With everybody running such light cuts and high feeds, I may be forced to hang with coolant on my old slow machine. I am still planning to try some of the 2-flute endmills (recommended above) dry, just to see what happens. It will not be the first time I ruined a brand new tool.

09-04-2006, 11:54 PM

You could try OSG Blizzard series, or Garr 242 series. They are both really goo and relativly cost effective, compared to Hanita. Atleast in my area. If you are looking for the bottom of pockets to have a good finish go with Garr, the OSG's Relief angles on the bottom of the cutter are pretty aggressive(Good for ramping and helical interpolation but sacrifice bottom finishes).

I hope this helps yah out Snake.

09-18-2006, 10:48 PM
I use an Accupro S/C ZRN ALUM EM 01150648. S4000 F32.0 z-0.25. When running dry the goal is to remove as much of the heat as possable in the chip load. (Research Stainless) as far as the misters go, you could make one that fills your needs with parts from the hardware store. It's all about your needs.

09-18-2006, 11:16 PM
I use that exact endmill quite a bit. For your listed rpm, you can double your feedrate in a slotting cut, and triple it in on a 40% profile cut. (seriously)

BTW, at IMTS, I talked to an applications guy in the Sandvik booth about dry cutting aluminum with insert tooling. He said that you need at least some sort of oil mist to keep the surface from galling, even with aluminum specific inserts. He specifically said that dry just doesn't work, and aluminum needs some sort of lubricity to maintain a good finish.

Also, one of my friends set up a machine demo for IMTS. He tried to do a 6061-T6511 aluminum dry cutting demo (42,000 rpm spindle), and they were snapping endmills left and right until they eventually had to use an oil mist. The tool company kept telling him that it should work dry.

Speaking of that, I didn't see anybody cutting aluminum dry at IMTS. (most used flood or through spindle coolant)


09-23-2006, 02:03 AM
Matsuura definately wasn't cutting that engine Block Dry!!!!!!!!!!

I did see Hyundai, finishing that Bust dry on the horizontal though!

09-26-2006, 07:19 PM
I run production so dry or slow is not the way I like to move, and it just does not sound manly. Still the gumming effect that alluminium(Did I spell that right?) or any other soft metal happens with or without coolant. It's about balance, If your tool is clogging up at the bottom of the flutes speed up the spindle, if your work piece has metal rolling back or oozing out of it then increase your feed rate.(Slowing down is for welders) The problem then becomes tool quality. I start off by seeing what it takes to break it. First thing in the morning I will be destroying a perfictly good 86593TF F5SRW-3204 1/2 x 1/2 5FL REG SE H-45 FUTURA CARBIDE. It will be fun.

11-28-2006, 11:50 AM
Hey Guys I posted this as a solo but got nothing so I thought I'd tag along on this thread hoping for some answers...
Need some quick advise.

Background: I run a small machine shop and I am just getting familar with the new machine. I really have only used cheap mcmaster and enco mills on our manual bridgeport and need to improve on quality on our CNC. I would like to make a good investment in some quality tools and money shouldn't be much of a problem so I need your help to stock up.

I work manly with 6061Al.

I need some roughing tools, facing tools and some kick-butt mills. I have a air cool sprayer and we squirt tap master to lube up. I have never used inserts and very curious how and when to use them.

Please recommend me on type, coated/uncoated, brand, # flutes or inserts.

I took notes from this thread and have been thinking about contacting vendors and have them compete for my business. Any tips on how to make this a success send them my way!

much appreciated and open for your questions,


11-28-2006, 05:03 PM
For facing in aluminum we use Sandvik R245 Cutters with their H10 grade I believe. They are uncoated and the periphery is ground. Surface finish should turn out resembling a mirror pretty much.

For endmills Most of my experience is with Garr. For 6061 stick with the 242M series. They work quite well, or else try OSG Blizzards Both of these are not really expensive, but performance is more than adequate.

What speeds will you be running?

11-28-2006, 05:05 PM
Sorry on really delicate parts we used Robb Jack roughing endmills running essentially as fast as the machine would turn(15K) and light depths of cut(0.04") and feeding fast as the machine would permit(up to 400ipm).

I will warn u that this was with full flood coolant, or thru the tool coolant.

12-01-2006, 04:57 PM
Our top speed is 3300 or 4500 in the red.

Here is my list thus far to seek competetors:
Robb Jack

What i've been hearing is that cutters with inserts are economical way to go once you buy the tooling and go with someone who's been around so you can find inserts latter on down the road and at multiple places.

But I question...insertable cutters, are they more practical for faster machines? Should I stick to a stardard end mills? I get teh hunch I should go with 2 flutes. Carbide or HSS or a coated.


12-01-2006, 07:26 PM
wut Ø cutters will u b using?

12-04-2006, 11:17 AM
I need to probably start off with a range or set for any job...so probably 1/8 - 4"

12-11-2006, 07:57 PM
That is a big list. As far as I am concerned there are only 3 brands of end mill, everything else will get thrown in a drawer and get ignored after putting these to the test.

Aluminum - Accupro Gold 2fl Carbide TiN - now there is a trick to running dry in alum. First is the limit of 3300rpm This should allow you to run around 20ipm with 0.500 - to control heat, the spindle must be spinning fast enough to throw the chips (and Heat) from work piece. Do not worry about heat when it comes to carbide. (YOU ARE NOT SUPPOSED TO GET CARBIDE WET) Carbide end mill break because people use coolant, the rapid expansion and contraction causes fractures in the mill. Caution tool will be extremely hot(That's the way it is the strongest.)
Second, you can not baby carbide. It is designed to cut not skim. if you do not run fast enough to take the bite to match rpm you will sheer off the end mill.
Third, alum gums up when it gets hot, this also lets you know your feeds and speeds are off. (HSS requires coolant because you cant be mean enough to stop the gumming) using the above mention end mill you will be able to throw the chips and help stop the gumming. Sometimes you have a problem with material sticking to the end mill, especially when using cheaper material like 2024 and such. To stop this you will need a cocktale made of 1 part cutting fluid and 1 part mineral spirits. (I prefer Varsal) Just throw across work piece and mill will take what it needs. *(this also helps with engraving in Alum)

Steal - YG 5 fl Carbide no coating all above rules apply I run 0.500 60 ipm @ 7500 rpm dry in tool steal. The first drop of coolant causes them to shatter.
they are rated @ some were around 112 ipm @ 11500 rpm (That is not a typo, I checked, twice)

Insert mills - Seco, nough said!

P.S. If you took all the other catalogs in the world and added them to gether you might get the diversity of one Seco catalog, Maybe. You might have to throw in some car parts catalogs or something.

OH, and I know about the end mills listed above from trial and error, and a lot of dead soldures.

12-11-2006, 11:09 PM
Just tried this endmill 3 flute solid carbide 10000rpm and 100ipm 1/2" Dia 1/2" depth of cut, and no problems. What mega dude says about running carbide dry, does not apply to all grades of carbide. I challenge him to cut 316 stainless dry for any length of time without lighting up the cutter. I'm sure it can be done, but try to do it productively.

THis gorilla this was my first attempt at using variable flute and pitch geometry, and I'm now a believer in this technology.

Here is my best advice. Whatever tools you decide to go with, must be readily available in your area. It's no good to have a $100K machine waiting for a $50 tool. do the math, it doesn't make sense. You also have to look at the machines that will be running the job. there is no point running tools with 3k minimum rpm on a 2k machine. Get a local rep in with some stuff to try. Make sure you get a few reps in. Once the guys on the floor trust what they are using, they should start pushing the limit. IF they don't start pushing maybe they aren't the right guys to have in the shop.

01-03-2007, 08:50 PM
6061 you lucky dog!, when i get alum its alumold or comparable, i tell my co-worker to run it wet but he dosent and he gets build up, so in conclusion, i reccomend full flood coolant for any and all alum. or at least mist.

once had a carbide tipped cold saw, had to run with mist or buildup would make bad parts. (cutting extrusions)

saco,iskar both good.

01-03-2007, 08:51 PM
whatever happened to ski-cut lol

01-04-2007, 01:57 AM
Just a few misc. thoughts on the previous posts.

Indexables vs solid endmills: Under 3/4 inch endmills are cheaper to run especially if you pull them before destruction and have them reshaped, Above 1 inch dia. indexables are cheaper. Either way you need tools designed specificity for aluminum. Aluminum needs higher rakes and more heel clearance than steel.

Your not supposed to get carbide wet: Well yes and no. The problem here is thermal shock. When milling the tool heats up while in the cut then comes out and gets hit with the cold coolant. This starts small microcracks perpendicular to cutting edge which then grow until the tool breaks. C-5 and C-6 carbides have added tantalum carbide which helps stop this and it all depends on hot hot the tool gets. Lower engagments (width of cut) reduce how hot the tool gets. Higher feedrates put more of the heat into the chip and the tool runs cooler. I've seen huge increases in life turning the coolant off in steel but aluminum seems to always like coolant or oil of some kind. I've never seen thermal cracking while cutting aluminum although maybe this would be a problem in some of the more exotic alloys. C-3 carbides are designed just for aluminum (a fine grain size, and a little less cobalt in the mixture, usually with just a touch of tantalum). Carbide does not get stronger when its hot. Its a sintered powered metal and can't be heat treated. It simply retains it's original hardness and strength at higher temperatures.

Coatings: Aluminum cutting tools have to be up sharp and have a polished top face. This means PVD coatings only and a thin TiN coating is probably best although I don't really see much life improvement here. My primary coating source (Ti-Coat in Utica,MI) has a new coating just for aluminum (TiB2) which they claim can extend tool life 5 times. I haven't been able to try it though as all my customers have gone to PCD tips for machining aluminum and I long ago learned that a lot of coating claims are hogwash.

It's interesting to see the preferences of one source or another as best in the indexable market. All of the big guys (Kennametal, Seco, Iscar, etc. ) make top notch products and offer a range of geometries and grades to cut just about anything. People move around between these companies all the time and the guy or gal designing your cutter at Seco today probably worked for Sanvick or Kennametal in the past. There are no secret formulas in the carbide business. The trick is to find a knowledgeable sales person who can recommend the right tools for your application and of course a reliable distributor who can deliver when you need them.

Oscar F1
03-18-2007, 04:28 AM
I am wondering if it is possible to cool with air?

A small airstream directed to the bit.

03-18-2007, 01:21 PM

If you can't use coolant, then air will help get chips out of the way. Recutting chips, is harsh on cutters, regardless of type, coating, or material.

If you want to use it for cooling, the a blast not a small stream would be more beneficial.

Oscar F1
03-18-2007, 04:29 PM
the a blast not a small stream would be more beneficial.

"A blast " ?

You mean a big stream ?

03-18-2007, 05:24 PM
I mean as much air as you can possibly get to the tool tip with out deforming the workpiece.:cheers: