Machining a large radius, on a large part, on a manual mill
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 22
  1. #1
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    4

    Default Machining a large radius, on a large part, on a manual mill

    We received an RFQ from a very steady customer to make a 'heavy duty' version of an assembly we have been making for them for many years. For the most part it the same thing we've always made, just bigger. But, there is one feature of one part that has me thinking twice about the approach.

    We need to machine a 2.25" radius 'half moon' into the side of a 1"x3" piece of CRS 1" deep into the flat side and all the way through the short side. On a 'standard duty' version of this part the feature is a .75" radius so we use a 1.5" diameter indexable mill and plunge mill to the required .375" depth - no problem. That same technique on this HD part would require a 4.5" mill. Again, no problem, except that our shop is 100% manual with R8 spindles. I'm concerned I'm going to beat our mill(s) to death trying to cut that feature plunging a 4.5" mill. A rotary table is out of the question because this part is 175" long. So far, it's just one part for one assembly, so maybe I can get away with it. However,in the event it shows up again I would like to have a reliable solution.

    I would love to hear some ideas if anyone has any. Of course it could be subbed out or I could rent some time on a buddy's CNC (6 hour round trip with a 14' long piece of steel) but I would like to avoid that if possible.


    hd-radius.jpg

  2. #2
    Join Date
    Oct 2009
    Location
    Olympia, Wa
    Posts
    628
    Post Thanks / Like
    Likes (Given)
    304
    Likes (Received)
    178

    Default

    I would use a boring head set to that radius and just step it over a little bit at a time. No it wouldn't be as quick as plunging with a large endmill, but you can get the job done.

  3. #3
    Join Date
    Jul 2004
    Location
    Houston, TX USA
    Posts
    30,027
    Post Thanks / Like

    Default

    Drill close little holes in an arc, bust out that chunk, then finish up with the boring head / flycutter or whatever

    Naturally it won't be as fast

    The point is is that it gets done with the least fooling around making chips on inadequate machinery at your disposal

    On Edit - a job made for the K&T 2D rotary head mill
    Last edited by johnoder; 01-15-2020 at 10:01 AM.

  4. Likes eKretz, Pathogen, Dumpster_diving liked this post
  5. #4
    Join Date
    Mar 2005
    Location
    Kansas
    Posts
    7,573
    Post Thanks / Like
    Likes (Given)
    438
    Likes (Received)
    3493

    Default

    I would scribe the radius and mill close to the line with a 3/4 rougher. I would then finish it with a boring head.

    If you are fabricators, I'd rough the radius in with OA torch (or plasma, if you have one that big). Knock the high spots off with a grinder. Then finish with a carbide tipped boring bar.

  6. Likes CalG, Erich liked this post
  7. #5
    Join Date
    Mar 2005
    Location
    Northwest Indiana
    Posts
    4,216
    Post Thanks / Like
    Likes (Given)
    845
    Likes (Received)
    846

    Default

    I wouldn't take a torch anywhere near that thing. The end of that bar would be bent to high heaven by the time you got that burned out. I'd run with the drill method that John mentioned. Quick and easy and done in one setup. It is also worth mentioning that if you take all that out of one side of a piece of cold-rolled you're going to end up with a bend anyway as the stress relieves itself when that much steel is removed from only one side.

  8. Likes eaglemike, Matt_Maguire, NC Rick liked this post
  9. #6
    Join Date
    Jul 2010
    Location
    corvallis,or
    Posts
    871
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    365

    Default

    Volstro rotary milling head

    Sent from my XT1710-02 using Tapatalk

  10. #7
    Join Date
    Sep 2005
    Location
    Dunstable, UK
    Posts
    31
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    18

    Default

    Quote Originally Posted by Blazemaster View Post
    I would use a boring head set to that radius and just step it over a little bit at a time. No it wouldn't be as quick as plunging with a large endmill, but you can get the job done.
    Definitely use a boring head, the stiffer the better .

    Tony

  11. #8
    Join Date
    Dec 2012
    Location
    Se Ma USA
    Posts
    1,532
    Post Thanks / Like
    Likes (Given)
    116
    Likes (Received)
    855

    Default

    Rough it out with an annular cutter. I'll bet that as its a partial circle you could rough it with a decent hole saw. Plenty of chip evacuation with the open side. Bend it back straight before finish pass.

  12. Likes JohnMartin liked this post
  13. #9
    Join Date
    Mar 2014
    Location
    Michigan
    Posts
    759
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    270

    Default

    Depending on how tight the tolerance is, I’d rough it on the shaper within .010”, mount the fat wheel on the surface grinder, dress the radius and finish to size. If they don’t want a sharp edge at the top, dress the entire form on the wheel and have at it. If you ever have to make another, you have a wheel ready to go.

    Andy

  14. #10
    Join Date
    Oct 2010
    Location
    Dewees Texas
    Posts
    2,395
    Post Thanks / Like
    Likes (Given)
    27
    Likes (Received)
    654

    Default

    So many ways to skin this cat, all of them pretty good. Choose the one that fits your personality and tools on hand best. Guy Lautard published a little hand book telling how to generate arcs and radii on manual machines. With a 1/2 or 3/4 end mill one could do that and have a bunch of cusps approximating the desired radius. Finish with a boring head or flycutter and you are there. A person could fake it by just scribing a line with a compass and milling up close to that line in .1 inch steps then finishing with the boring head/flycutter.

  15. #11
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,128
    Post Thanks / Like
    Likes (Given)
    1839
    Likes (Received)
    2455

    Default

    Quote Originally Posted by Hobby Shop View Post
    Depending on how tight the tolerance is, I’d rough it on the shaper within .010”, mount the fat wheel on the surface grinder, dress the radius and finish to size. If they don’t want a sharp edge at the top, dress the entire form on the wheel and have at it. If you ever have to make another, you have a wheel ready to go.

    Andy
    Must have missed the part about the material being 175" long? Radius dressed wheel then you are running the stock across the chuck? Must be a pretty big grinder.
    Fly cutter or boring head....One machine ,one setup.
    Cheers Ross

  16. Likes eKretz liked this post
  17. #12
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    768
    Likes (Received)
    1845

    Default

    Scribe the line with the boring head, plunge cut the bulk of the material with an endmill, then fnish with the boring head. Using the bolt circle function of your DRO (or some math) should lead you to a very predictable load on the finishing tool.

    If you think this will be a repeat, it may behoove you to build an adjustable flycutter to perform the finish cut.

  18. #13
    Join Date
    Jul 2006
    Location
    rochester, ny
    Posts
    1,927
    Post Thanks / Like
    Likes (Given)
    390
    Likes (Received)
    539

    Default

    Dimensions on the drawing are only to 2 places, hundreths of an inch. Seems a hole saw could hit that tolerance

  19. #14
    Join Date
    Oct 2005
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    15,542
    Post Thanks / Like

    Default

    ...and when this job is completed, start looking for a manual/cnc mill.
    One of those "easy to learn" bedmill type with no toolchanger.

  20. Likes AlfaGTA, Hbjj liked this post
  21. #15
    Join Date
    Mar 2014
    Location
    Michigan
    Posts
    759
    Post Thanks / Like
    Likes (Given)
    124
    Likes (Received)
    270

    Default

    Quote Originally Posted by AlfaGTA View Post
    Must have missed the part about the material being 175" long? Radius dressed wheel then you are running the stock across the chuck? Must be a pretty big grinder.
    Fly cutter or boring head....One machine ,one setup.
    Cheers Ross
    Yep, Totally missed the 175” part.

  22. #16
    Join Date
    Aug 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    1,423
    Post Thanks / Like
    Likes (Given)
    1014
    Likes (Received)
    618

    Default

    Do you have a DRO with a bolt circle function? Use it to plunge many times around the arc. Spacing of the plunges will depend on the diameter of your tool and the allowable scallop.

  23. #17
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    4

    Default

    So many good ideas, thank you all. The boring head seems so obvious now I'm almost embarrassed I hadn't thought of it myself.
    I'll likely rough it out by plunge milling with a smaller endmill to a scribe line and finish with the boring head (basically exactly what Cole suggested). I won't have to buy any additional tooling this way.
    As far as DRO goes... none of that here either (I know, I know, I've got quotes on new machines with 'all' the bells and whistles). Richard pointed out the loose tolerances, these features are +-.030 which is wide open - absolutely no problem to hit with any of the above mentioned techniques on my archaic machines.
    I've never heard of Volstro head until now, what a neat piece of equipment. This is a nearly perfect application for it.
    Again, thank you all. I'll be sure to let you know how it goes (assuming we get the job).

  24. #18
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,335
    Post Thanks / Like
    Likes (Given)
    275
    Likes (Received)
    2187

    Default

    Lemmee get this straight, 3 inch deep, 2.25 radius

    R8 spindle

    Punch a clearance hole in a piece of aluminum to act as a spacer[or make a soft jaw]

    Do the math for a half dozen spots on the radius, .02 under, with a 3/4 end mill, plunge

    finish with a boring head

    [edit] as you decided, no DRO sucks

    dammit man, get into the 1980's!

  25. #19
    Join Date
    Jun 2007
    Location
    Vancouver Island, B.C. Canada
    Posts
    1,796
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    203

    Default

    With such tolerances if you happen to have a 2.25" annular cutter then just clamp a scrap piece of 1x3 to the edge and drill through on the correct centre point. Very fast and easy.


    (Gustafson it is just a 1" deep bore)

  26. #20
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    441
    Post Thanks / Like
    Likes (Given)
    22
    Likes (Received)
    186

    Default

    I agree with the hole saw technique. It’s fast and super cheap. You can easily follow it with a boring head or a fly cutter to clean up the finish if necessary.


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
  •