# Aluminum Roughing End Mill: Recommendations?



## wildo (Apr 22, 2019)

I have a few ZrN coated, high helix (45*), 3 flute end mills that are exceptionally free cutting in aluminum. There is a clear difference between these and my ALTiN coated end mills. So I figured that the ZrN coating would be the way to go for aluminum/titanium roughing. I was searching around and found this guy which looks pretty nice:






						ZrN Coated 1/2 dia 3 Flute High Helix Carbide Rougher X 2.0 loc MariTool
					






					www.maritool.com
				




But then I started researching a bit more and discovered the TaC coating. These guys claim as much as 20 times tool life in 6061 with no aluminum build up on the tool. That's beyond interesting. I found this end mill which states that it's for HEM, so I'm not sure it's as useful in a manual Bridgeport type mill. But it does have an aggressive chip breaker and might work nice as a roughing end mill for aluminum:






						IMCO | Product Search
					






					www.imcousa.com
				





I did notice that Niagara Cutter only lists end mills coated with TiCN for aluminum work. It's interesting to me that I can't find any ZrN end mills from Niagara, but perhaps I'm reading too much into that?

Thoughts?


----------



## mikey (Apr 22, 2019)

Gotta' try one of those someday. 

Niagara has those wavy tooth cutters but not recommended for aluminum. Big bucks so I'll wait until I have the need.


----------



## wildo (Apr 22, 2019)

I also found this one via PM- it seems that Lakeshore Carbide is recommended over there when folks are asking about variable pitch aluminum specific end mill:









						rougher/finisher variable flute end mill for aluminum
					

thread mill,thread mills,radius tools,chamfer tools,rotary broach,hex broach,thread milling,carbide threadmill,endmill,end mill,carbide endmill,carbide end mill,high performance endmills,variable flute,drill mill,roughers,carbide roughing end mill,endmill,npt,nptf,spot drills,hex broaches,vari...



					www.lakeshorecarbide.com
				




Looking at the speeds & feeds chart for this end mill, they call for 200-2000 SFM, and .006 IPT. I put those values into a calculator and get these results:

200 SFM @ 1/2" Diameter = 1528 rpm
2000 SFM @ 1/2" Diameter = 15279 rpm

My max mill spindle speed: 2600 rpm, so:
Max SFM for my mill: 340 SFM

2600 rpm x .006 ipt x 3 teeth = 46.8 ipm, or .78 inches per second.

Basically- assuming 1D for profiling, and .5D for slotting- I can't push that rougher to failure. What a beast!! Seems like I found what I was looking for!


----------



## mikey (Apr 22, 2019)

Let us know how it works out, Willy. Now you just have to hope your mill is rigid enough to handle what you're going to throw at it!


----------



## wildo (Apr 22, 2019)

mikey said:


> Let us know how it works out, Willy. Now you just have to hope your mill is rigid enough to handle what you're going to throw at it!



Will do. I ordered both the Maritools corncob rougher and the Lakeshore Carbide rougher/finisher. (I have a lot of aluminum work coming up in future projects)


----------



## pstemari (Apr 23, 2019)

wildo said:


> ...
> I did notice that Niagara Cutter only lists end mills coated with TiCN for aluminum work. It's interesting to me that I can't find any ZrN end mills from Niagara, but perhaps I'm reading too much into that?



I've only seen ZrN available on carbide tools, although Niagara appears to be moving away from HSS. Niagara also cut back substantially on its coating options: as I recall they dropped TiN entirely and are recommending AlTiN for steel and TiCN for aluminum.

My understanding is that TiN, TiAlN, and AlTiN are not suitable for cutting aluminum, especially the TiAlN & AlTiN. The problem as I recall is that aluminum chips will happily weld themselves to all of those coatings even faster than they weld to bright uncoated endmills.


----------



## petertha (Apr 24, 2019)

I'm no expert & certainly not production oriented but I do favor uncoated for aluminum, particularly 6061 which is stickier over 2xxx and 7xxx.
Mine are different brand but this website is kind of a nice pick & choose categorization. The roughers are so much better for hogging material & they make nice almost granular chips. Just seems easier on everything, part stability & the mill itself. I really noticed this on my lighter RF-45 mill where you just dont have the same mass & power as a Bridgeport style. Finishing wise, these helix style do a nice job & just seem to cut effectively. They make a different chip than conventional EMs (and btw are the nastiest daggers to embed in your skin). Good luck!

https://www.the-carbide-end-mill-st...fine-pitch-for-aluminum-3-flute/uncoated.html


----------



## wildo (Apr 24, 2019)

It’s super interesting to me that a few of you recommend uncoated EMs. I’m a beginner and haven’t tried bright end mills and that’s mostly because everything I read about ZrN coating indicates it’s a better surface for aluminum. Do you guys disagree??


----------



## ddickey (Apr 24, 2019)

SPT Suncoast Precision Tools is running a sale on 3 flute cutters for aluminum.


----------



## ChrisAttebery (Apr 24, 2019)

Is this for a manual 2-3hp milling machine? If so, I think you'd be better off spending $17 on a good HSS end mill such as this one:

http://www.yg1usa.com/feature/item_...d=1&sub_sub_id=37&pre=STANDARD&pre2=&name=HSS 

I'd start it at 2600 rpm, 1" DOC, .25" WOC, 16" IPM (.003" IPT). 

Here's a $37 cobalt 3 flute rougher that would also be a good match for your machine:
http://www.yg1usa.com/feature/item_...&sub_sub_id=88&pre=STANDARD&pre2=&name=COBALT 

I'd start this one at 2600 rpm, 1" DOC, .25" WOC, 21" IPM (.0027" IPT).

With either end mill above, increase the feed up in steps up to .006" IPT. I'd bet that you'll find the machine's limits before you find the end mill's limits. 

Carbide and the fancy coatings are for the guys with high hp high rpm CNC machines. If you're running into chips sticking to the end mills I'd recommend building or buying a mist type coolant system. 

For reference, I have a G0704 that's converted to CNC. 1100W motor, 6750 rpm belt drive. I use the 3/8" version of the 2 flute above. 6000rpm, 60 IPM, .5" DOC, .04" WOC. I can run it harder, but this setup will run reliably for hours.


----------



## wildo (Apr 24, 2019)

Chris- that all seems like good information, but can you qualify the statement below with any documentation?

"Is this for a manual 2-3hp milling machine? If so, I think you'd be better off spending $17 on a good HSS end mill"

Why is that a true statement? From my (admittedly limited) experience, as well as what I read when looking into coatings, the fact is that ZrN coating adds lubricity that bright finish end mills simply don't have. On top of that, the coating increases tool life due to the increased hardness as well as temp resistance. I can't find the lubricity rating for bright finish micrograin carbide tooling, but I did find it for the ZrN coating (at 0.5). I think it's easy to make the case that high speed machining DOES require much faster and more efficient chip evacuation than slower spindle speeds, but I don't see why that eliminates specialty coatings from being effective for manual machines. With the increase in temp resistance and hardness, it seems like a big win to me. Am I missing something obvious?


----------



## ChrisAttebery (Apr 24, 2019)

First off: This is all based on cutting aluminum. If you're cutting steel that's a different conversation.

When I first got into CNC I was buying 3/8" 2F carbide end mills for aluminum. Someone on CNC Zone talked me into trying a "good" HSS end mill. He was using them on a larger machine than mine. I gave them an honest try and I've been using them ever since. There are a few arguments for them on a HP limited machine:

1. HSS is cheaper than carbide. In my case $12 vs. $20 for my most common end mill (1.6X). In your case it's $17 vs. $55 (3.2X). 
2. Carbide is brittle and chips easier than HSS. Chip one corner on that $55 end mill and it's scrap.
3. Since you're running a manual machine you're more likely to stall or crash the machine. The HSS is more likely to survive.
4. Carbide is brittle and can't hold as sharp of an edge as HSS so it takes more HP to remove the same amount of metal. Your machine is HP limited so using HSS will allow you to sustain a higher MRR than carbide. The HSS end mill isn't the limiting factor on your machine, it's the low spindle speed and limited feed rates that the average human can produce.  

Like I said, if you're trying to cool and lubricate the end mill you're better off setting up a mist/fogless coolant system.

BTW: I do use carbide end mills under 1/4" as they can handle a higher MRR in carbide than HSS.


----------



## pontiac428 (Apr 24, 2019)

I agree completely with Chris.  Coated tools are like inserts in that they are efficiency enhancers for maximum production.  Even when I did work in a production shop, we did all of our aluminum work in the mill department with HSS and steel with cobalt, nothing more.  Tapping titanium is one place where ZrN would be used, but never on Al.  Coatings have come a long way, but for those of us turning handwheels, there isn't any justification for the added cost.  Tool life and finish quality has more inputs than coating, inputs that can be eliminated with better bearings in the quill, good tool holders, correctly adjusted gibs, proper cuts, and mist coolant.  I'd rather buy HSS and spend the money saved on improving my setup.  In a rigid machine, an HSS end mill can run 24/7 for weeks in aluminum before sharpening or replacement.


----------



## mksj (Apr 24, 2019)

ZrN or any coating isn't going to do you any good if you do not have a system to get rid of the chips. On aluminum I have tried both uncoated polished and ZRN coated, to be honest I will do something stupid that will break a tip on a carbide end mill before it wears out from use. I have been using Hanita carbide 3Fl high helix and Niagara HSCO TiCN coated, and they both last a year or more with 1/2" end mills in aluminum. I also pick them up on eBay, the last batch of 1/2" carbides were $25 a piece. The major downside of carbide is that they are very brittle, bounce a tip or tap anything and you will break a tip. I still continue to use them for roughing out material, the carbide is razor sharp. At $25 a pop they are not worth resharpening, and the price difference vs. HSCO is minimal vs. longevity. CNC is a different situation, were I typically see 2Fl 1/4 or 3/8" end mills used, and more continuous run with dedicated high flow coolant systems.

My experience is similar petertha. I like to use cobalt end mills and also the powdered metal cobalt ones by Minicut, the 3Fl wave type (930PM) does very well in aluminum for manual milling with fast metal removal. I do not do CNC, but for manual I prefer the 3Fl.  If you want to remove a lot of aluminum quickly, i would recommend a 4 or 5Fl 3/4-7/8" rougher. They will shower you with a pile of chips very quickly, much faster than a 2 or 3 Fl end mill in my experience. You will need a more rigid mill with 2-3 Hp to use the larger rougher.

Milling 2500 RPM  0.20 x 0.60 DOC 10 IPM passes using a 7/8" HSCO TiCN 5 flute fine rougher



I haven't found that the coatings make much of a difference at my level of milling in aluminum. If using carbide, you also will have better luck with a small corner radius on the flutes. I have worn out HSS end mills, but not my carbide ones in aluminum (I have only used HSCO and carbide). The biggest factor with milling aluminum (at my level) is chip evacuation, climb cutting and cutter profile in my experience. See attached article which discusses factors to get an optimal surface finish in aluminum.


----------



## wildo (Apr 24, 2019)

Well I'm hesitant to post this since I really don't know what I'm doing- so I made the video unlisted. But I did say I would so... enjoy? ha.

This is the Maritool 1/2" roughing end mill I linked to in the OP.
For profiling it is running at 327 SFM, 1.0" ADOC, 0.110" RDOC, and 4 IPM.
For slotting it is running at 327 SFM, 0.5" ADOC, and 2.4 IPM
1HP machine.

The Lakeshore Carbide rougher arrives tomorrow.


----------



## ChrisAttebery (Apr 24, 2019)

At those feed rates the tool is just rubbing the material away. You need to increase your feed by 8-10x. Try taking a .25” deep x .125” wide cut and get used to how fast you can push the end mill. Then start increasing the DOC.


----------



## wildo (Apr 24, 2019)

ChrisAttebery said:


> At those feed rates the tool is just rubbing the material away. You need to increase your feed by 8-10x. Try taking a .25” deep x .125” wide cut and get used to how fast you can push the end mill. Then start increasing the DOC.



 I don't know man. Either I'm not being clear in my point, or you're not reading it. The feeds & speeds I used are literally direct from the manufacturer. The question isn't if it can be optimized more- of course it can. Even the manufacturer states as much. The question is if your uncoated end mill can keep up. Now I've proved that the coated end mill can handle a pretty fast feed given a very slow speed. The end mill handled a full feed of 4 IPM at 2D ADOC and .25D RDOC at only 40% of the recommended SFM without any chip welding or other issue. Can the bright end mill hang? That is the question.


----------



## ChrisAttebery (Apr 25, 2019)

3 flutes, 2500 rpm, 4 IPM is only .00055 IPT. Are you sure it isn’t 40 IPM?


Sent from my iPhone using Tapatalk


----------



## wildo (Apr 25, 2019)

Wow! The Lakeshore Carbide one is night and day better. Insanely smooth performance and begs for more. I found a winner!


----------



## ddickey (Apr 25, 2019)

It's an inch shorter. Could be why you're seeing better performance.


----------



## wildo (Apr 25, 2019)

ddickey said:


> It's an inch shorter. Could be why you're seeing better performance.



Good point; I didn't consider that. It also creates way different chips, leaves a near mirror finish, and doesn't "scream" like the corncob one from MariTool.


----------



## ChrisAttebery (Apr 25, 2019)

I noticed that the Mari end mill was howling in the video too.


----------



## ddickey (Apr 25, 2019)

It's howling because of the length/lever action on the spindle.
Mine does the same with an end mill holder. Creates a long lever. Some sort of resonance.


----------



## wildo (Apr 25, 2019)




----------



## ddickey (Apr 25, 2019)

Whining End Mill
					

I have this new 1" Niagara rougher end mill I acquired. Of course I had to get an end mill holder for it.  Mistake as it is unusable even at the lightest cut. Made a short vid on a piece of scrap.




					www.hobby-machinist.com


----------



## mikey (Apr 25, 2019)

Looks good, Willy. I've been meaning to try that variable helix thing for some time now. Still not sure how much difference the coating makes. My uncoated cobalt roughers seem to last forever and do not gall in aluminum so ...

I agree with the length or stickout thing. I'm sure the other guys have a better way to do it but I try to order end mills with a flute length about double the diameter or less. For a 3/8" end mill, I want 3/4" flute length. This lets me maximize my ADOC and RDOC while minimizing deflection. Getting the end of the flutes up close to the collet and using an ER collet also reduces deflection and vibration, which is what is causing that howling you guys are talking about.

Roughers are awesome but remember to size them so you have about 0.010" left to finish. As nice as the finish is with that new rougher, it will still leave marks that will need cleaning up on a presentation face.


----------



## ChrisAttebery (Apr 26, 2019)

That looks good. Now start feeding it as hard as your motor and mill can handle. That end mill can handle .01" IPT.


----------



## darkzero (Apr 26, 2019)

So.... how do my roughing chips look like that I made yesterday? Don't ask me all the numbers cause I dunno really. Feel, sight, & what my mill yells at me is what I go by these days most of of the time.


----------

