[touser]

Hello everyone, i am in the process of teaching myself how to use a cnc mill i purchased and am going insane with breaking end mills. I am trying to mill 6061 aluminum with 1/16" 1/8" and 1/4" end mills and i keep breaking the 1/8" and smaller end mills. Does anyone know the maximum safe feed rate/depth per cut running at 5600rpm with carbide end mills? Thank you all for the help in advance!

[Mcgyver]

a rule of thumb is depth should be less than 50% of the dia - for frail little cutter like 1/8 or 1/16 id go way less than 50%. you've got to state speed in terms surface speed of the periphery of the cutter - ie feet per minute. For carbide in AL 1000 fpm is probably ok. feed (inches per tooth) is .002 according to machinery's handbook (btw what are doing cutting metal with one? tsk tsk), but thats also a function of depth - total force on the cutter. I could be that backlash/climb milling is part of the problem

With HSS you can see the cutter deflect which is usually a good indication to slow down whereas carbide is just going to snap. Unless you have the rigidity to spin at 5400 rpm and advance at a good rate of feed, you are not getting an advantage out of those carbine cutters anyway. You might find hss at a slow speed would remove the same volume per minute without the breakage

[trubleshtr]

Not sure but, I don't think carbide and aluminum are a good mix. Carbides are usually used on hard,tough metals. Carbide itself is "brittle"(for lack of a better word) and shock loading or pulse loading it will surely snap it. Aluminum tends to "pick up" as it cuts and can bind and plug up an endmill if coolant is not used.
Stick to a Hss endmill, 2-flute if plunging, 4 if facing,ect. If you can aford em, I hear the spiral endmills are good. You won't necesarily need coolant, but at that rpm you should be able to 1/8 depth cuts at moderate feed rates....

Ops, appears I am too slow a typer

[touser]

Thank you both for the replies i appreciate it! I was unaware that carbide wasnt a good choice for aluminum, i figured the stronger the better but sense HSS will work thats great on the wallet! So assuming each cut is only a depth of 0.042" what would you say is the maximum safe feed without coolant at 5600rpm? Also about what would it be with coolant? If i can run without coolant i prefer it.

[Ken_Shea]

Touser,
Go here and get ME Consultant, you will find it invaluable, in milling, drilling, threading etc, if you can I would recommend the pro version for $50, however the freebie is a great start and you can upgrade anytime. I would be lost without it.

Funny how different things work for different people, I always use carbide on aluminum, I like 3 flute, 2 flute with no coolant to flush out the chips. You do need to watch carbide, it takes heat very well but you will likely trash them if you get them real hot and then suddenly cool them with coolant.

http://www.mrainey.freeservers.com/

Shows about 7 IPM with carbide 2 flute .042 DOC at 5600rpm

[HuFlungDung]

Recently, when I was composing a tool list, I researched a lot of tool catalogues, and came up with a simple rule to get started with any diameter endmill: .0001" per flute chipload for every 1/64 inch of cutter diameter, if the cutter is cutting at about 50% overlap (which would be good technique, to avoid plugging).

Eg.1: For a 1/64 two flute endmill .0002" per rev feedrate, so at 5600 rpm that = 1.12 inch/min.

Eg.2 For a 1/8" three flute endmill, that's eight sixty fourths, so .0008 * 3flutes * 5600 rpm = 13.4 ipm

For full width cuts, I'd cut these feeds in half, because plugging of the tool can become a problem in aluminum.

[little bubba]

HuFlungDung -- Thats seems like a pretty decent rule of thumb, I never really thought about it, but it seems to get you pretty close.

For the OP the quick formula, RPMs * feed per rev(which is chip load per tooth * # of teeth) = feed rate in ipm. Just in case.

Trublshtr, I'd have to disagree on carbide not being good for aluminum, I used to think that, why waste a high dollar tool to cut something that is just on the fun side of wood. Some cheap carbide endmills do appear to be brittle and blow up before your eyes, however for the small stuff, 1/8 and under I really like the extra rigidity of carbide, at that diameter, you can't usually take advantage of the additional surface footage, but you can keep a reasonable chip load whereas a HSS tends to deflect and bounce around leaving burrs and a crappy finish. I'd say give them a fair shot, once you go carbide, you'll never go back, well, I still like my cobalt roughers but thats another story.

[ghyman]

I know that cutting aluminum dry is the popular practice ("because we CAN!"), but I've found that for heavy loads / small tooling, carbide with a good coolant flood (or even an oil mist) keeps the tool from getting loaded up with chips... an endmill with a fairly sharp edge will last forever if you can keep it from getting gummed up with welded-on chips.
Cobalt and HSS tools are fine as well, but I like the carbide for it's rigidity on smaller tools.

[DareBee]

I agree with Bubba, the main reason for using the carbide cutters is deflection (or lack thereof).
As Ghyman says I feel coolant as extremely important for lubrication and chip evacuation.
If coolant is inconvenient for you get a microdrop mister.

[ynneb]

What I cant understand is if you are cutting with lots of passes and small step downs, then you are wearing out the bottom of your tool and leaving the rest of your tool untouched. It is hard to sharpen the tool so that it is the same diameter along its length. It hurts me to disguard a tool that is only worn at the end. Whats the solution?

[Ken_Shea]

Benny, you don't throw those away just use them for profiling and not center cutting.

[Mcgyver]

Here are some ideas on your choices, and a related digression into lowering the cost of material removal. Firstly get the most mileage that you can when its sharp – stuff like use coolant, right speed & feed etc. The wear is NOT linear, if you are cutting at a theoretical maximum, a little slower can really increase tool life.

When it is dull, obviously it’s trash or it needs to be sharpened. Various set ups let you grind off the bottom but that wastes a lot tool life. The ultimately solution is a tool and cutter grinder. Then you are sharpening the periphery – and will get many, many sharpenings.

Of course most home shops don’t have a T&C grinder. When you consider the cost of cutters and that tool life is usually a matter of hours before sharpening is required, maybe more should consider this. I finally did, and man does it improve your workmanship. This is mainly for HSS; with carbide the dust is unhealthy (and requires different wheels).

I also think many are running their gear to fast and prematurely using up cutters. Why? Every machine, as a function of its HP and rigidity is only capable of doing so much work, or removing so many cubic inches of material per minute. A .500 carbide cutter can be spun at 8k in AL, however, whether you do this at 8k @.0001 per tooth or 800k @ .001 per tooth will not change the amount of work you are doing. It will have an impact on tool life.

The pro’s are more concerned with time but for us home shop types the goal is maximizing the material removal/$. The ideas are… HSS, sharpening capability, slow things down, coolant and the right feeds. This assumes you’re are not running a 25000 lb behemoth at home or using carbine for its other properties like rigidity or hardness.

[HuFlungDung]

I have tool and cutter grinders, etc, and most of our work is low volume production. However, I really cannot be bothered with regrinding the flutes anymore. I prefer to shorten the endmill to remove the worn flute area, which would typically be a length reduction equivalent to the radius of the cutter, each time it is done.

If only the corners of the flutes are chipped, grind chamfers (with proper clearance) and use the tool as a rougher. This can be done offhand. It really does not matter if all the chamfers are the same: if they differ, then you just acquired yourself one of those expensive "stepped endmills"

My reason is that the factory outside grind and flute geometry is worth preserving, instead of botching it up on the tool and cutter grinder.

Time is a factor, too. I can shorten an endmill by grinding the end off and regrinding the clearance in 5 minutes, just offhand on the grinder. The most important thing is to have CBN wheels for high speed steel, and natural diamond for carbide. With the proper wheels, the tools grind easily. Using aluminum oxide or silicon carbide wheels is far too much work attempting to maintain the wheels in a true form which you can depend on. That is just my opinion, I'm not belittling Mr Macgyver's opinion

[Mcgyver]

HuFlung, everything you said rings true, any difference is i think home vs businesses...you're fighting against $100/hour in overhead and I'm trying to lower tool consumption costs from $5/hour to $3 . When overhead is considered, working 1/2 hour to sharpen the periphery of a $15 cutter makes no sense, but I can make a decent job of it and hobby economics are different.

are you using ventilation for with the carbide or is it s wet system? I've always shyed away from it becuase of the health hazard.

I am messin with balancing and truing aluminum oxide wheels, you a right, its a pain.

[DareBee]

I am surprised neither of you mentioned the preservation of the coating.
My carbides either get pitched or ground like Hu mentioned. Simple fact of the matter is (actually 2 points) programming is easier with nominal sized cutters (for those of us that leave the ATC full and program with a tool library) and the fact that we pay large premiums to have fancy coatings on our cutters (such as Tialn) and you don't want to grind that off.

[Mcgyver]

in the sense that its better to grind off from the bottom than periphery the coating is preserved? good point, but to me, more applicable for you pros - I don't have very much coated tooling and have bins of un coated old end mills to sharpen and use up. better to buy uncoated and sharpen 10 times. the potential flaw in this logic, is of course how many cutters could I have bought for the price of the T&C grinder . Well, I'm still convinced that frugality demanded the purchase and it will have at most have a couple of year payback