Angled hole to a flat surface
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Feb 2014
    Location
    Sonoma County, USA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    14

    Default Angled hole to a flat surface

    Good Morning,

    Looking for some tips on the correct way to machine the 2.125" holes into this plate. It's 5.5" diameter plate with a 2.25" x 4.437" rectangle boss centered on the back side. I know I'll have to use a sine plate in our CNC mill or keep it simple and grab the square boss in a vice and tilt the head on the manual mill Would a tooling ball be the correct way to locate the center of the hole?

    Thanks in advancecnc-help.jpg

  2. #2
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,579
    Post Thanks / Like
    Likes (Given)
    1062
    Likes (Received)
    1601

    Default

    In a word. Yes.

    Although with bores that size you could just set the plate at the angle you want, guestimate as close to location as you can, bore a smaller hole thru, check location, adjust and machine to size.

  3. Likes rokstarr999 liked this post
  4. #3
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,541
    Post Thanks / Like
    Likes (Given)
    15978
    Likes (Received)
    11570

    Default

    How should you do it? Its probably going to suck.

    If I had to do it where you are at now, my first thought is to
    use the rectangle to hold it, and ignore the round thing.
    Of course the round thing has to be down, which complicates things.

    2 soft jaws that are long enough to span 2 vises. One machined.
    One plain. Lay the jaw down, put in a pocket at the appropriate
    angle to hold the rectangle. Add a locating feature (this is where
    CAD comes in handy. Bolt jaws between 2 vises and bring the part
    up from underneath, squeeze and machine, maybe use a screwjack underneath.

    I probably would have preferred to start off with the bottom plate being
    square, and then machining it round last, after all the holes are in.
    Then you could have just grabbed it in some angled soft jaws.

  5. Likes rokstarr999 liked this post
  6. #4
    Join Date
    Feb 2014
    Location
    Sonoma County, USA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    14

    Default

    Quote Originally Posted by Bobw View Post
    How should you do it? Its probably going to suck.

    If I had to do it where you are at now, my first thought is to
    use the rectangle to hold it, and ignore the round thing.
    Of course the round thing has to be down, which complicates things.

    2 soft jaws that are long enough to span 2 vises. One machined.
    One plain. Lay the jaw down, put in a pocket at the appropriate
    angle to hold the rectangle. Add a locating feature (this is where
    CAD comes in handy. Bolt jaws between 2 vises and bring the part
    up from underneath, squeeze and machine, maybe use a screwjack underneath.

    I probably would have preferred to start off with the bottom plate being
    square, and then machining it round last, after all the holes are in.
    Then you could have just grabbed it in some angled soft jaws.
    I didn't think about laying a soft jaw down and machining the angle in it. Much easier than fixturing to a sine plate. And the 5.5" diameter is at that top of the hole so grabbing the boss will work great.

  7. #5
    Join Date
    Feb 2014
    Location
    Sonoma County, USA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    14

    Default

    Quote Originally Posted by Booze Daily View Post
    In a word. Yes.

    Although with bores that size you could just set the plate at the angle you want, guestimate as close to location as you can, bore a smaller hole thru, check location, adjust and machine to size.
    This would work. The shift after sweeping the tooling ball at that angle is only .008" Took me a while to draw this up in cad. Fusion isn't very cooperative...or I just don't know how to use it very well...lolcapture.jpg

  8. #6
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    5,774
    Post Thanks / Like
    Likes (Given)
    204
    Likes (Received)
    1975

    Default

    The only tolerance I see on the drawing is a +0.003/-0" on the diameter of one of the holes. Is there a note on the drawing about the others? That would influence how this is approached.

    Rokstar999 talks about the first problem I see here and that is just where do you need to line up to locate the angled bore. Just putting the tooling ball in a center hole on the original surface of that side does not place the center of that tooling ball on the axis of the needed hole. There will be some offset and he claims he has calculated it at 0.008". That sounds high to me, but he did not say what size tooling ball he was assuming and the offset will change with that size. (The 0.008" offset with an angle of 1.5 degrees seems to imply a tooling ball who's center is about 0.305" above it's base. Perhaps not as high as I first thought.)

    As to how it is held, again that depends on those stupid little things called tolerances. If the angle needs to be held down to arc seconds, that is one thing, but +/- 1/2 degree is another.

    My approach would definitely depend on the needed tolerances.

    Another fuzzy thing on the drawing is the location of the point where the axis of the two holes meet (square one and angled one). It appears to be at the right side of the overall plate, but that is not really clear. This is an important point when calculating the offset from the center of the tooling ball.

  9. Likes rokstarr999 liked this post
  10. #7
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    572
    Post Thanks / Like
    Likes (Given)
    198
    Likes (Received)
    360

    Default

    If the angle is relatively shallow I would clamp a square sided vise, like a Kurt 3600, at the correct angle in another vise. It is a really convenient way to hold parts at a shallow angle. Just hide the vise handle for the lower vise, it makes you feel real dumb if you loosen it by force of habit.

  11. Likes rokstarr999 liked this post
  12. #8
    Join Date
    Feb 2014
    Location
    Sonoma County, USA
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    14

    Default

    Quote Originally Posted by EPAIII View Post
    The only tolerance I see on the drawing is a +0.003/-0" on the diameter of one of the holes. Is there a note on the drawing about the others? That would influence how this is approached.

    Rokstar999 talks about the first problem I see here and that is just where do you need to line up to locate the angled bore. Just putting the tooling ball in a center hole on the original surface of that side does not place the center of that tooling ball on the axis of the needed hole. There will be some offset and he claims he has calculated it at 0.008". That sounds high to me, but he did not say what size tooling ball he was assuming and the offset will change with that size. (The 0.008" offset with an angle of 1.5 degrees seems to imply a tooling ball who's center is about 0.305" above it's base. Perhaps not as high as I first thought.)

    As to how it is held, again that depends on those stupid little things called tolerances. If the angle needs to be held down to arc seconds, that is one thing, but +/- 1/2 degree is another.

    My approach would definitely depend on the needed tolerances.

    Another fuzzy thing on the drawing is the location of the point where the axis of the two holes meet (square one and angled one). It appears to be at the right side of the overall plate, but that is not really clear. This is an important point when calculating the offset from the center of the tooling ball.
    According to the drawing I have +/- 1 degree on all angles which makes zero sense. Everything else is +/- .005 for .xxx This drawing is dated 8/12/70. And your correct about the tooling ball height being .312" from center to shoulder. I think my plan for the angled features is to machine a soft jaw at the correct angle, sweep the ball, run one pocket and then spin the part around and run the other pocket. I'll ream .250" holes for the tooling ball when I cut the rectangle boss.

  13. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,541
    Post Thanks / Like
    Likes (Given)
    15978
    Likes (Received)
    11570

    Default

    Quote Originally Posted by kenton View Post
    Just hide the vise handle for the lower vise, it makes you feel real dumb if you loosen it by force of habit.
    Been there and done that countless times, so I made a bunch of these.
    Vise Stops.


  14. #10
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,579
    Post Thanks / Like
    Likes (Given)
    1062
    Likes (Received)
    1601

    Default

    Quote Originally Posted by kenton View Post
    Just hide the vise handle for the lower vise, it makes you feel real dumb if you loosen it by force of habit.
    Kinda like when you're running a fixture in the CNC lathe and forget to put a block of wood under the unchuck pedal?

  15. Likes Bobw liked this post
  16. #11
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,541
    Post Thanks / Like
    Likes (Given)
    15978
    Likes (Received)
    11570

    Default

    Quote Originally Posted by Booze Daily View Post
    Kinda like when you're running a fixture in the CNC lathe and forget to put a block of wood under the unchuck pedal?
    I move it as far away as I can, and put a box over it.

  17. #12
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,579
    Post Thanks / Like
    Likes (Given)
    1062
    Likes (Received)
    1601

    Default

    The lathe I run now has a barloader. I just put it in barloader mode and the pedal doesn't work.

    Wasn't always that way.

  18. Likes Bobw liked this post
  19. #13
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    313
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    93

    Default

    It’s such a shallow angle. Me, in my ignorance, would attempt to do them flat in the vise and interpolate it with a boring type spiral toolpath. It’s slightly undercut on one side, so a tool like a dovetail cutter (flat bottom, multiflute, single point contact) with a .02 radius, and use .005-.01 step downs. Too bad it has that step where the angled bore meets the straight, but a smaller diameter cutter(1/2” or smaller) would leave an acceptable crisp step for the tolerances, I would expect.

    No fancy setup, just cnc. The cycle would take way longer, but reliable and takes the human error aspect out which is usually where my setups fail. If just a few I’d trade reliability for speed any day.


    Or you can clamp it to a tilting/rotary table.
    Last edited by vmipacman; 01-24-2021 at 08:56 AM.


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
  •