What's new
What's new
By:
Advanced search…

What's the secret to stop chatter on a long 1" dia HSS end mill

M

Mr.Chipeater

Aluminum
Joined
Apr 20, 2021
Hey everyone,

I've got a 1" dia x 6" length 4 flute HSS end mill that I am using to finish a 2" long bore that is 5" deep in an aluminum part and I cannot for the life of me get it to stop producing a rifle barrel finish from all the chatter.

I've tried every combination from 130-315 sfm, 0.002-0.005 ipt, and 0.005-0.030 step over.

The "best" results which are still completely unacceptable seem to be with high sfm, low chip load, and light step over which seems to go against the general consensus of wanting to load up the cutter.


Any thoughts on other cutting conditions to try running?
 
Anything over 4xD stickout can be chattery even in carbide.

HSS has about 1/3 the rigidity of carbide, so even worse.

Long flute lengths further reduce rigidity, partially because you're missing material and partially because all that axial contact adds to the tool pressure. Ideally you'd have a relieved (necked) solid carbide shank with less than an inch of flute length on the tip.

If this is a one-off job and you have no other use for that HSS cutter, I'd grind away the flutes (maybe 0.010" off the radius) so that you're only left with about 1/2" of flute on the tip. Then finish the bore by helixing down at about 0.100" per rev.
 
Machine? Taper?

And how you holding it.. The tool and the part..

I agree with Orange Vise about grinding her back to limit your
contact. But I'd take it a step further.

You need to break up the harmonics. Like those fancy variable
flute and helix endmills do. I'd start by grinding a big chamfer
on one flute only.

And I'll tell you a quick story of why I would do that. Years ago
I had a series 10 Acroloc. And I was doing (trying to do) things
with that machine it wasn't intended to do. Even with a variable
flute/helix endmill, it would still scream at me, and then break
off one corner.. Sometimes that one corner would break off and
it would quiet down and cut good, other times, the broken corner
would destroy the endmill.

So, trying to get a leg up on the machine breaking the corners off
my endmills, I would take the endmill out of the tube, (brand new 1/2"
Imco, or HTC) and grind a 60 to 80 thou chamfer on one flute.. Worked
a treat, and I've used that trick on other machines in tricky situations,
and it works.. Not always, but its worked enough for me that I keep it
in my bag of tricks.

Also, if your machine isn't the most rigid thing going, ramping will add
pressure straight upwards, through the spindle and make your machine think
its more rigid than it is. If its going to move anyways, might as well
control the direction of movement and use it to your advantage,
big corner rads and chamfers can also help with that,
sort of simulating a high feed mill.
 
Bobw said:
Machine? Taper?

And how you holding it.. The tool and the part..

I agree with Orange Vise about grinding her back to limit your
contact. But I'd take it a step further.

You need to break up the harmonics. Like those fancy variable
flute and helix endmills do. I'd start by grinding a big chamfer
on one flute only.
Click to expand...

Machining it on a 40 tapper HAAS UMC750 so not the most rigid but seems to be adequate for aluminum jobs. Part is held nicely in 5th axis vise so I doubt that is contributing much.

I'd love for a nice variable helix carbide tool but as Orange Vise pointed out, I'd still have to get such a large diameter tool it would be cost prohibitive.

The chamfer idea is a neat trick I'll have to try sometime. The bore I'm machining is open on the other end so I'm machining as high up on the tool as I can so without the tip touching, I'm not sure chamfering the end will change anything. I suppose I could grind a spot in the middle of one flute as a way to break up some harmonics.

A boring head would also be great.... if I had one the right size.
 
130 SFM isn't all that slow, for HSS. I'd just keep going slower. It'll eventually shut up.

You could also try grinding down an entire flute or two. Make it a ghetto variable helix. Anything to break up the harmonics.
 
You’re talking about the bottom surface, not the cylindrical one, are you? The question arises with me, what a mad design or function can it be that demands such. If you need a very good bottom quality and can go a little deeper, push a neat disc in there.
 
OP mentions a "rifle barrel" finish, making it pretty clear it's the bore he cares about. And I agree with those that say boring head, if he's got any BH at hand he could kludge a cutter that (flimsy as it may be) would still be superior to a HSS EM.
 
Once again
Long HSS-Co mills for steel finishing

I had same problem and reducing speed and feed eliminated chatter, results were good

But this was for outside wall. If you got 1" in 2" hole, then the engagement angle is big. And against all logic, I think smaller diameter mill may work better.

Keep load and rpm minimal and it may work.
 
I (in theory) disagree about slowing it down. Normally* with chatter you either want to decrease sfm OR increase chip load.

*4" LOC may be the problem in itself however.
 
Couple thoughts....obviously i dont know the part or what you have available to use. Since it is a bore....I agree with the boring head idea. Or can you grab or fixture it in a lathe? Can you ry to "helix bore " it. I have had success helix boring with an endmill to reduce chatter. It gets some of the pressure pushing axially and can help....obviously it is slower than a regular old G2 or G3
 
Mr.Chipeater said:
Machining it on a 40 tapper HAAS UMC750 so not the most rigid but seems to be adequate for aluminum jobs. Part is held nicely in 5th axis vise so I doubt that is contributing much.

I'd love for a nice variable helix carbide tool but as Orange Vise pointed out, I'd still have to get such a large diameter tool it would be cost prohibitive.

The chamfer idea is a neat trick I'll have to try sometime. The bore I'm machining is open on the other end so I'm machining as high up on the tool as I can so without the tip touching, I'm not sure chamfering the end will change anything. I suppose I could grind a spot in the middle of one flute as a way to break up some harmonics.

A boring head would also be great.... if I had one the right size.
Click to expand...

But you can still "bore" it with long endmill. Go to pedestal grinder and grind away about 0.2-0.5 mm of the mill edge, except the last 5mm (or even less) at the end. Now it has much smaller load and you can go helix. Almost like boring head.
 
I'm in the relieve the flutes and helical interpolate it crowd. If you can't, I second trying conventional. You could also try running it slow. Like 50SFM and .0015IPT.
 
When I bought my first Bridgeport at 15 years old the very first tool I bought was an Enco boring head that would do your 2" bore down in the part no problem.

You have a Haas machine that is one of their fancier turds and you don't have a boring head for a 2" bore?

I was kinda in your shoes once with a tall outside profile that chattered. I was at Western Tool discussing my problem and they pulled out a big box of custom ground carbide tools that were wrong or returned for some reason. I found a 6" long 3/4" 2 flute carbide endmill in there that was relieved for all but the final 1/2" of flutes.

I bought that endmill for $15 and it ran production for about 10 years in one of my VMC's. At one point, the toolchanger dropped that tool and broke one of the flutes off. It still ran forever that way with no change.
 
Mr.Chipeater said:
Hey everyone,

I've got a 1" dia x 6" length 4 flute HSS end mill that I am using to finish a 2" long bore that is 5" deep in an aluminum part and I cannot for the life of me get it to stop producing a rifle barrel finish from all the chatter.

I've tried every combination from 130-315 sfm, 0.002-0.005 ipt, and 0.005-0.030 step over.

The "best" results which are still completely unacceptable seem to be with high sfm, low chip load, and light step over which seems to go against the general consensus of wanting to load up the cutter.


Any thoughts on other cutting conditions to try running?
Click to expand...

Radial chip thinning at .005 radial and .005 feed puts your actual chip thickness at .0007. that's VERY small. Kick your feed up significantly. .015 per tooth minimum at .005-.010 stock.
 
Milland said:
OP mentions a "rifle barrel" finish, making it pretty clear it's the bore he cares about. And I agree with those that say boring head
Click to expand...

Then a no-brainer, boring head, or if you can clamp work on lathe, turning. Ecocut is also nice, made by Ceratizit. Plunge and turn/bore with one tool
 
An end mill is sharp on the od so any little run out will make the hole a tiny bit oversized and leave a spiral going in. The best fix is to finish the hole with a reamer. A reamer has an OD circle-land that holds the tool center and cutting on the end only.

Carbide end mill most likely to do the very same thing.

Yes, to ream finish the hole the original bore would be a 1/64th or so smaller than the reamer.

Oh, do assure that the end has an end cutting grind..that is one having a flute going to center with enough end gullet (space) so the chips can flow without bunching up. Still, the end mill likely will leave a rifle barrel finish

and end cutting tools/cutters need more end clearance 10 to 14* is good.
 
Since you are using a haas have you tried using a G13 pocket milling cycle? In aluminum I have good luck using these pocket milling cycle.
 
Try doing multiple passes in 1" stepdowns or helix down in 1" increments. If your taking the 5" length in one pass your 5x diameter on depth. In my experience anything after 2x diameter deep is just asking for it to sing you a song. Use the shortest reach tool holder you have and preferably use a collet chuck and choke the end mill up as short as you can in the holder. I'm with the others on the boring head route though.

Sent from my moto g power using Tapatalk
 
You must log in or register to reply here.

Similar threads

J
Need advice on milling a 1-1/4" wide x 8" long slot into 1/2" mild steel plate.
2 3 4
Replies
76
Views
5K
surplusjohn
S
D
Turning long tapers (42-47")
2
Replies
25
Views
2K
Whetstone
W
dandrummerman21
Time to make a bunch of mill soft jaws; What features do the rest of you add to them?
Replies
10
Views
1K
mhajicek
mhajicek
C
Chipped corner on 2 flute end mill. Any fixes?
2
Replies
33
Views
4K
implmex
I
wheelieking71
Struggling with chatter on semi-tall profile finish pass, help!
2 3
Replies
52
Views
7K
Noah Katz
N








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top