What's new
What's new

Fillets v Chamfers on CNCd Parts

PM2.5

Plastic
Joined
Oct 17, 2017
Just looking to find out if it is easier to machine fillets or easier to machine chamfers on parts like aluminium (6061) and stainless steel (304, 316). I do Design Failure Modes Effects Analysis in a machine building company and am constantly coming acorss a mix and match of both. I'm thinking chamfers are the easier of the 2 to machine?
 
I assume you're talking about outside edges, then yes chamfers are typically the easier of the two because cutting fillets on outside edges requires a corner rounding form tool or a 3D toolpath.
Although the corner rounding form tool cuts a fillet just as fast as a chamfer tool cuts a chamfer, you have to be a lot more critical when setting the tool and programming it or else the tool could gouge easily.

tl;dr chamfer is more foolproof than a fillet for outside edges.
 
Not really any difference in CNC machining. Fillets create less stress points. We add fillets to nearly all the shafts and rollers on conveyors in food making machines that we work on.
 
I've attached images of a part where I thought fillets were diefinitely not required on outside edges. I thought chamfers would be fine.
The fillets on the inside would need to be hand filed I believe.

Fillets v chamfers 1.jpgFillets v chamfers 2.jpg
 
Fillets on turned parts, chamfers on milled parts. On your images, fillets could all be milled, but chamfers would be my preference. Milling fillets you have to have lots of different size corner rounding end mills. Chamfers , you only need a few. Tuned parts , you are programming the radius anyway , so size doesn't really matter. Any yes, inside radius on a turned part is stronger and eliminates a stress riser. My 2 cents.
 
Just remember, when designing a part, the prettier it looks the more it's gonna cost.
Put a small edge break where needed to get rid of sharp edges, and a larger chamfer where needed for interference relief.
Fillets on outside edges (of a milled part) look great on paper, but a chamfer will cost you less money to have it done.

Edit: as per above, if it's a lathe part fillets are zero issue and make the part look REALLY nice.
 
Hi PM2.5:
Those fillets will increase the cost of making the parts substantially, especially if you need them to be good looking or accurate.
The fillets on the outsides of the block will require two setups to complete the part, and to make them accurately will require that the second setup be accurate with respect to the location and orientation of the part.
By "accurate" I mean better than 0.0005" for the second side setup or else that underside fillet will look like a pig's breakfast, whether you surface mill it with a ball cutter or use a corner rounding cutter.
A chamfer there is much more forgiving, so an ordinary vise with a stop will be more than adequate.

On the cavity side, there are fillets you cannot mill as modeled, so if you NEED it to be exactly as modeled you have to sinker EDM it, and if you need it to be pretty good you can surface mill it with a tiny ball cutter and then pick out the corners with a file under the scope.
That makes it a five hundred dollar part instead of a twenty dollar part.

If you really don't give a damn, and all you need is for no one to cut up their hands when they handle it, you can just throw it in the tumbler or edge break it with a file.
Now it's a twenty dollar part again.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Cheapest way is to leave the model sharp and put a note on the print: "Break all sharp edges."

Second best is to model chamfers on external corners and fillets on internal corners. Allow enough tolerance on the fillets so they can use the corner radius cutters they already have, rather than having to order special ones just for you. And, this is a big one, corners in the X/Y plane need to be big enough to cut with a rotating cutter that has a reasonable length to diameter ratio; no .010" fillets 3/4" tall.
 
Hi PM2.5:
Those fillets will increase the cost of making the parts substantially, especially if you need them to be good looking or accurate.
The fillets on the outsides of the block will require two setups to complete the part, and to make them accurately will require that the second setup be accurate with respect to the location and orientation of the part.
By "accurate" I mean better than 0.0005" for the second side setup or else that underside fillet will look like a pig's breakfast, whether you surface mill it with a ball cutter or use a corner rounding cutter.
A chamfer there is much more forgiving, so an ordinary vise with a stop will be more than adequate.

On the cavity side, there are fillets you cannot mill as modeled, so if you NEED it to be exactly as modeled you have to sinker EDM it, and if you need it to be pretty good you can surface mill it with a tiny ball cutter and then pick out the corners with a file under the scope.
That makes it a five hundred dollar part instead of a twenty dollar part.

If you really don't give a damn, and all you need is for no one to cut up their hands when they handle it, you can just throw it in the tumbler or edge break it with a file.
Now it's a twenty dollar part again.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

As Marcus said, in your left view of part, top face, the sharp intersections would need edm, or a quick hack if acceptable, mini files to sharpen the radii that will be left between fillets into a *sharp* corner... Or just model the same fillet rad inbetween and then it's all 3d milled.
 
I've done both corner rounded fillets and chamfers. The corner rounding cutters work well but only if the surface is absolutely FLAT.The smallest variation in planar flatness (maybe you moved the part to a different vise)will cause a visible line from the edge of the cutter. This is not a problem with a chamfer. And any corner rounding cutter I've seen was HSS, not an insert cutter like most chamfer tools. (I'm guessing that solid carbide corner rounding mills are made somewhere but I've never used them.)

So if you have any say in the design of the part I'd go with chamfers instead of rounds.
 
And, this is a big one, corners in the X/Y plane need to be big enough to cut with a rotating cutter that has a reasonable length to diameter ratio; no .010" fillets 3/4" tall.

This. And if you really want to do us a favor, don't use fractional sizes, go up a little.

ie. instead of .125 rads +/-.005, do .140 or .300 instead of .250. Our tools come in fractional sizes, so give them a little room to work.

Again, this only applies to rads between walls, and not fillet rads on the bottom of a pocket. For those do the opposite.
 
I've done both corner rounded fillets and chamfers. The corner rounding cutters work well but only if the surface is absolutely FLAT.The smallest variation in planar flatness (maybe you moved the part to a different vise)will cause a visible line from the edge of the cutter. This is not a problem with a chamfer. And any corner rounding cutter I've seen was HSS, not an insert cutter like most chamfer tools. (I'm guessing that solid carbide corner rounding mills are made somewhere but I've never used them.)

So if you have any say in the design of the part I'd go with chamfers instead of rounds.

Swiftcarb/Superbee makes carbide insert corner rounders.
I wish someone made corner rounders that had a slight leadin instead of full 90° radius, would make applying radii much easier when it's just for appearance
 
I often use metric cutters for inch features, and vice versa. A 3mm (.118") endmill will cut a .125" radius fairly well.

We do as well here, but I've worked in shops with much less of a tooling budget and it was always a PITA. Opening up those interior rads is such an easy way to increase the machinability of your parts, but most engineers seem to like the hard numbers. I always try to design my tooling to be as friendly as possible.
 
Just looking to find out if it is easier to machine fillets or easier to machine chamfers on parts like aluminium (6061) and stainless steel (304, 316). I do Design Failure Modes Effects Analysis in a machine building company and am constantly coming acorss a mix and match of both. I'm thinking chamfers are the easier of the 2 to machine?

On a lathe, you can do either rather easily. For Okuma it's G76 or G75 plus the "L" chamfer/radius amount. On Fanuc/Mits it's usually an "R" or a "C".

On mill, a bit more, as you'll need either a corner rounder or a chamfer mill. The corner rounder needs a "little" but of care when programming/setting up.

Generally I like to give radii on turned/milled parts whenever possible as it feels nicer in the hand. But, if a print says "chamfer" then chamfer it is.
 
Chamfers are easier to get a consistent surface finish from top to bottom. Corner radius cutters have a wide swath of SFMs from the bottom to the top of the radius. For example, we'll use a Harvey carbide 5/8" diameter 1/4" radius corner rounding EM with a .120" (or whatever the exact size is) nose. Using the major diameter of the tool, 5/8", for the SFM calculation at say 1000 SFM, you'll end up with only 200 SFM at the bottom of the radius. This can cause faceting if you're not running really low IPM. Using a large diameter nose and small corner radius helps, but then these are really only available in HSS.
 
What does CNC'd mean? I can Turn a part, I can Burn a part, I can Mill a part, hell, I can even deburr a part. Deep thought--can I CNC a part? Computer Numeric Control is a description not a fucking verb.

R
 
What does CNC'd mean? I can Turn a part, I can Burn a part, I can Mill a part, hell, I can even deburr a part. Deep thought--can I CNC a part? Computer Numeric Control is a description not a fucking verb.

R

Prolly about the same as "lathing" a part from aircraft-grade bill-utt on a See and See machiner. :toetap:

That's even worser in my book! :angry:
 








 
Back
Top