Fillets v Chamfers on CNCd Parts
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Oct 2017
    Country
    IRELAND
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    0

    Default Fillets v Chamfers on CNCd Parts

    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?

  2. #2
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,445
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    3417

    Default

    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.

  3. Likes Booze Daily, PM2.5, mhajicek, PegroProX440 liked this post
  4. #3
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,718
    Post Thanks / Like

    Default

    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.

  5. Likes PM2.5 liked this post
  6. #4
    Join Date
    Oct 2017
    Country
    IRELAND
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    0

    Default

    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

  7. #5
    Join Date
    Aug 2006
    Location
    greensboro,northcarolina
    Posts
    2,557
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    676

    Default

    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.

  8. Likes Mtndew, PM2.5, SeymourDumore liked this post
  9. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,445
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    3417

    Default

    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.

  10. Likes PM2.5, Bobw liked this post
  11. #7
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,882
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2557

    Default

    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

  12. #8
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,429
    Post Thanks / Like
    Likes (Given)
    1841
    Likes (Received)
    949

    Default

    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.

  13. Likes Camputer, ARB liked this post
  14. #9
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,676
    Post Thanks / Like
    Likes (Given)
    2251
    Likes (Received)
    2827

    Default

    Quote Originally Posted by implmex View Post
    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.

  15. #10
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,865
    Post Thanks / Like
    Likes (Given)
    591
    Likes (Received)
    326

    Default

    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.

  16. Likes Bobw liked this post
  17. #11
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    155
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    144

    Default

    Quote Originally Posted by mhajicek View Post
    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.

  18. Likes mhajicek liked this post
  19. #12
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,227
    Post Thanks / Like
    Likes (Given)
    2633
    Likes (Received)
    3955

    Default

    Quote Originally Posted by 706jim View Post
    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

  20. Likes 706jim, mountie liked this post
  21. #13
    Join Date
    Aug 2006
    Location
    greensboro,northcarolina
    Posts
    2,557
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    676

  22. Likes mhajicek, Mud, EnderDRM, mountie liked this post
  23. #14
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,429
    Post Thanks / Like
    Likes (Given)
    1841
    Likes (Received)
    949

    Default

    Quote Originally Posted by 706jim View Post
    And any corner rounding cutter I've seen was HSS
    I was going to mention Harvey, RJT beat me to it.

    Quote Originally Posted by Camputer View Post
    This. And if you really want to do us a favor, don't use fractional sizes, go up a little.
    I often use metric cutters for inch features, and vice versa. A 3mm (.118") endmill will cut a .125" radius fairly well.

  24. #15
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    14,227
    Post Thanks / Like
    Likes (Given)
    2633
    Likes (Received)
    3955

    Default

    Quote Originally Posted by RJT View Post

    Perfect.
    ..

  25. #16
    Join Date
    Feb 2020
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    155
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    144

    Default

    Quote Originally Posted by mhajicek View Post
    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.

  26. Likes mhajicek liked this post
  27. #17
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,256
    Post Thanks / Like
    Likes (Given)
    735
    Likes (Received)
    504

    Default

    Quote Originally Posted by PM2.5 View Post
    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.

  28. #18
    Join Date
    Aug 2014
    Location
    Noble, OK
    Posts
    866
    Post Thanks / Like
    Likes (Given)
    67
    Likes (Received)
    175

    Default

    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.

  29. #19
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    5,078
    Post Thanks / Like
    Likes (Given)
    1329
    Likes (Received)
    2873

    Default

    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

  30. Likes ChipSplitter, Bobw, TeachMePlease liked this post
  31. #20
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    2,412
    Post Thanks / Like
    Likes (Given)
    1250
    Likes (Received)
    1770

    Default

    Quote Originally Posted by litlerob1 View Post
    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.

    That's even worser in my book!

  32. Likes litlerob1 liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •