Endmill flutes concentric with the shank

Hi all,

We currently have an aluminum job where we have to buy an endmill with a long length of cut. The finished part is 4 inches thick so we were going to buy a 4 inch loc endmill (I'm pretty sure you can go .030" past 4 inch depth with 4" loc endmill and be okay). I think we are going to go with a 1" diameter endmill to provide more rigidity at that long length.
We aren't looking for bottom of the barrel but we also aren't looking for the most expensive either.

I think we are going to buy a garr endmill. It was recommended to us by another very knowledgeable machinist who said that the flutes on a garr have minimum runout in relation to the shank and that the flutes of a garr have a very close concentricity tolerance with the shank. He said he bought cheaper brand endmills where this was not so. He said the flutes on some cheaper brands were not nearly as concentric with the shank and the flutes had a bit of runout (assuming your holder is running out <.0001 in the spindle).

My question is have any of you guys bought long endmills, or any endmill, that had runout or concentricity problems?

Thanks,

Chris

Personally I've never seen an endmill with eccentric flutes, but I never buy the cheapest stuff. Any reputable brand should have runout closer than you can reasonably measure. Make sure to put it in a quality holder, preferably shrink fit. You can use a torch if you don't have an induction machine.

I think runout in the tool is a negligible concern. Much more your toolholder is the concern. I have not had endmill concentricity problems... I mainly buy Morse.
Will you be side cutting with all 4” of flute length?

You said part as in 1 off. I'd go 4 or 6fl bright HSS either 1 or 1 1/4". Either should work just fine. I say that knowing very few details of the actual part. Like others have said, likely the holder will have the most effect on runout.

Yes we will be side cutting with all 4 inches of flute length. I was going to buy carbide since it is so much stiffer than hss (less chatter problems with carbide) but hss would probably work okay. I would imagine you would want the most flutes possible to make the endmill more stout. What feeds and speeds and radial step over for carbide? CAM calculated it to be 1000 ft/min, 125 in/min feed, .011 feed per tooth. Maybe a bit fast for an endmill this length? Don't want to produce any chatter or harmonics

cgrim3 said:

What feeds and speeds and radial step over for carbide? Fusion 360 calculated it to be 1000 ft/min, 125 in/min feed, .011 feed per tooth.

Click to expand...

That’s what I was going to ask you If you find a recipe that gives you 4” engagement with a 1” EM without chatter please let me know. I think those numbers are going to squeal like the dickens, but I am a wuss when it comes to pushing tooling hard.

13engines said:

You said part as in 1 off. I'd go 4 or 6fl bright HSS either 1 or 1 1/4". Either should work just fine. I say that knowing very few details of the actual part. Like others have said, likely the holder will have the most effect on runout.

Click to expand...

Nah, get a decent carbide and use it for the next 500 jobs that need it too.

cgrim3 said:

Yes we will be side cutting with all 4 inches of flute length. I was going to buy carbide since it is so much stiffer than hss (less chatter problems with carbide) but hss would probably work okay. I would imagine you would want the most flutes possible to make the endmill more stout. What feeds and speeds and radial step over for carbide? CAM calculated it to be 1000 ft/min, 125 in/min feed, .011 feed per tooth. Maybe a bit fast for an endmill this length? Don't want to produce any chatter or harmonics

Click to expand...

Run it that fast and endmill concentricity would be the least of you problems.

I think your 'very knowledgeable machinist' has led you down the garden path, causing confusion where in reality it's likely a non-issue.

If you think it's an issue take new endmills you have on hand and check them for concentricity.

If it was me I'd use 3 flute YG-1 Alu-Powers and not loose any sleep over percieved issues.

Destiny Tool - Destiny Tool

Call these folks, priced right and the feeds and speeds they give you will work.

I see now that the OP, and a fellow Minnesotan have no qualms about spending what, 6-7-$800.00 + on an end mill? I'm sure I would too if I was making a lot more then one of something out of Aluminum, but to me it doesn't make sense. Why?

1) Cost compared to measures that could likely get the job done. (HSS in this case)

2) That costs effect on job profitability and even winning the quote to begin with.

3) You're buying a tool with little use elsewhere unless these types of parts, whatever they are, are somewhat the norm in your shop.

4) This tool will be material specific to a high degree because you won't get a coating, if one is added at all, that will work on materials other then aluminum. Helix angle and grind type might also play in to this.

5) Real important... can your machine(s) even run a 1" carbide end mill with 4" of engagement? It'd better be big, stiff and heavy. Case in point - I have two 40 taper CNC machines. I can run 3/4" carbide in Aluminum effectively in both, (though never tried 4" DOC) but on one machine it has to be dialed in or it'll squeal, piss and moan. (It's even a way machine.) On the other machine it would be more of a stand off as to which would complain first, the tool or the machine. Little dialing necessary, other then of course you try to run a tool to its best ability. If the OP's shop has experience running 1" carbide effectively, then why not? That is if it still makes sense after points 1-4 above are considered.

6) So you buy your expensive end mill and then find you cant make it work. Drats you say! Still the bright side is, at least you've now got a cool tool you can pass around the shop exclaiming to one another.... "isn't it cool how heavy this thing is?" Almost as good as making a profit. :-)

Another option, relieve the flutes on a 3/4" an inch behind the tip and finish the profile 3/4" at a time.

I've seen parts 3"+ done this way on a Fadal and there's no noticeable step between passes.

In that case just use a relieved/necked endmill. There's at least one company that mentions they radius the transition of upper flute edge to lessen the ridge that's left with each pass.

But if the machine and toolholder is up for it, why not use an expensive endmill if it fits the process and cost scheme? I've done it where needed. 1" isn't cheap, but it's not insane...

13engines said:

I see now that the OP, and a fellow Minnesotan have no qualms about spending what, 6-7-$800.00 + on an end mill? I'm sure I would too if I was making a lot more then one of something out of Aluminum, but to me it doesn't make sense. Why?

Click to expand...

Because in the long run you're better off investing in quality tooling. If OP is making one of these now, chances are over the next few years they'll make several more parts somewhat like it. A quality carbide aluminum specific endmill can last months in production if run right. When doing prototypes and one offs it'll last until you crash it. I've got a 5/8" Helical bull for aluminum that's been in the holder for three years.

You can't just figure the price of the tool; you have to include the labor and downtime for figuring out the old one is worn out, ordering a new one, maybe waiting for it to arrive if you didn't order it early or get extras the first time, etc. That can add up to a fair amount of opportunity cost.

Plus, the carbide is simply the better tool for the job. It will be significantly more rigid.

I've worked in shops that always choose the cheapest tool for the job, and I can tell you their overall efficiency sucks. Things are always wearing out, not working right, and a huge amount of time is spent fighting with the lesser tooling or waiting for replacements.

End mills run very good TIR shank to flutes. Sticking out 4" plus and your spindle bore error will be magnified.

You might chuck up a 1" x 6" straight round bar and check your run-out to see if that method (end mill) will work to your needs before spending 4 to 600 bucks for a one-time use cutter(end mill).

If your EM has .002 run out/wobble the part may be .004 out of square one side to the other or to the end, plus what you get from fixturing.

You can likely trepan the job with existing tooling and have squareness as good as your tram.

A variable pitch end mill will help reduce chatter.

As others have pointed out, if you don't actually need to do the whole depth at once, relieved shank endmills are good. If you can use a 1.5" diameter instead of 1", I've had very good luck with the Korloy Pro-x mill. I have a few different lengths of shell mill holders.

cgrim3 said:

Yes we will be side cutting with all 4 inches of flute length. I was going to buy carbide since it is so much stiffer than hss (less chatter problems with carbide) but hss would probably work okay. I would imagine you would want the most flutes possible to make the endmill more stout. What feeds and speeds and radial step over for carbide? CAM calculated it to be 1000 ft/min, 125 in/min feed, .011 feed per tooth. Maybe a bit fast for an endmill this length? Don't want to produce any chatter or harmonics

Click to expand...

I'll be able to hear that thing chatter from here! Get a reduced shank 3/4" length of cut 1" diameter. Reduce the shank so it does not drag on the wall. If Garr does not have it they will make it for you in a few days. Keep your corner radius small as you can get chatter from there as well. Do your pocket or whatever in steps, 1/4 or 3/8 or so. Make sure your corner radius is bigger than 1/2" or it will talk to you in every corner and leave a crap finish. I routinely mill 4" deep pockets in 7075T6 with a 6" long reduced shank 3/4 LOC 1/2" Garr end mill with minimal chatter issues and get a very good finish as well. Another strategy I have used Is to drill out as much material as possible before milling. This helps as I am using a V2XT Bridgeport, one of the most flexible CNCs ever made.

Our machine is a box way daewoo 3016 dmv 3 axis mill, 8000rpm spindle. The machine is mostly used for stainless and titanium. Its a pretty rigid machine and the pioneer tool holders we have runout less than a tenth. We were already awarded the job...we included 400 dollars in the quote for pricing on the endmill. I found garr has a 1" diameter variable helix 4 inch loc for about 340 dollars give or take, uncoated or 20 dollars more for ticn coating. The hardest part will be dialing in the speeds and feeds and radial doc so it doesn't chatter.

Garr part numbers for the endmill we are looking at is 42360 & 42364

We are not used to running aluminum. 95 percent of our work is 316 stainless and titanium

Also, we are not machining any pockets. It's just side milling with the cutter on the outside of the part.


We looked into endmills with a reduced shank but decided to go with a 4" loc endmill. We will revisit the reduced shank endmills and see what we can come up with

cgrim3 said:

Our machine is a box way daewoo 3016 dmv 3 axis mill, 8000rpm spindle. The machine is mostly used for stainless and titanium. Its a pretty rigid machine and the pioneer tool holders we have runout less than a tenth. We were already awarded the job...we included 400 dollars in the quote for pricing on the endmill. I found garr has a 1" diameter 4 inch loc for about 340 dollars, uncoated or 20 dollars more for ticn coating. The hardest part will be dialing in the speeds and feeds and radial doc so it doesn't chatter.

We are not used to running aluminum. 95 percent of our work is 316 stainless and titanium

Click to expand...

I buy up high dollar tooling I don't need when I see a good deal just for situations like that.

Anyway, I don't do much aluminum either and if I was in your position and didn't already have the tool I would buy something for cutting SS and use it to run the aluminum. Then when you are done you have a high dollar tool that you will likely use.

Despite what they say I have ran TiAlN coatings cutting aluminum at reduced speed with coolant successfully. Maybe look for a SS tool that is TiCrN coated.

The rigidity of the machine is the last place chatter will manifest itself. So daewoo or fadal, the machine (unless it’s a Bridgeport) is the strongest link.
In my experience, in order of weakest link to strongest its; workholding (stiff worholding is often too time consuming for a one-off), part geometry, tool length/diam/material, toolholder length/type, machine.
I used to say to myself “they wouldn’t sell a tool that couldn’t actually use all the flute length”. But they do.
Point is, I think you are either spec’ing the wrong tool for the strategy or the wrong strategy for the tool. But I’m happy to be proved wrong, just pass on your S/F so I can use them too