Is it possible to make this feature on a Haas Y-axis lathe? - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 35 of 35
  1. #21
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    2,779
    Post Thanks / Like
    Likes (Given)
    991
    Likes (Received)
    936

    Default

    Quote Originally Posted by implmex View Post
    tiny nibbly cutters.
    There's no need to use tiny cutters though. There are no internal angles less than 90 degrees, so no reason you can't do a single 4 axis toolpath around the base of the stem using simple corner rad endmill, and use the corner of the same endmill to surface the remaining material.

  2. Likes Bobw liked this post
  3. #22
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,123
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1404

    Default

    So short of EDM cutting this, I cannot see a way to get the geometry; sinkering it is easy because the electrode is easy to make; it's just half a hole with an octagon cross hole and it's just dropped over the rough post and burned until it touches the cylinder.
    However it's slow and it's expensive, and as was pointed out previously by The Sidetalker, how close is "close"??

    So yeah, I was talking out my ass a bit when I said "YOU CAN'T" and with enough time money and toys you can get pretty damn good.
    I'll betcha on a 5 axis machine with a cone shaped cutter and Hypermill you can get it to look pretty nice; maybe as nice as you could get it on the sinker but it'll be one gold plated post!!.

    Cheers

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

  4. #23
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,178
    Post Thanks / Like
    Likes (Given)
    11019
    Likes (Received)
    9065

    Default

    How big is the boss, and how big is the feature..
    If I missed that info, I'm sorry..

    I'd be inclined to go with what I think Tony said, way up at the
    top of this tread.. F'it and file those corners out.. Probably
    wouldn't take but a minute or 2 per part.. Especially if you
    don't have a million of them to do, and if you did, Investment Casting.

    Probably going to have to come into that little corner area with some
    type of abrasive wheel or brush to make it look not like shit anyways.

  5. #24
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,123
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1404

    Default

    Hi Gregor:
    Yes, you're right if you can accept a radius at the junction of the stem and cylinder, but with a simple 4 axis toolpath using the cutter oriented parallel to the axis of the post it'll be washed out in the corners on the 45 degree faces, so you'd have to come in eitheron the orientation I show in JPG #9 where my cutter is perpendicular to the 45 degree face to nibble out those corners or stay normal to the cylinder face unless you can get tiny cutters in there to minimize the washout.
    If you roll the job to try to pick out the corners you have to position the cutter so it stays centered over the axis of the cylinder as it traverses the junction of the boss and cylinder and that position changes as you go from a 90 degree face to a 45 degree face in order to keep the cutter engagement tangent to the corner. and the end face of the cutter oriented correctly relative to either the cylindrical surface or the angled boss face
    So yeah, you can get in there because as you point out there are no features where the included angle of two adjacent faces is less than 90 degrees, but not without a fancy toy to get into the corners, and it ultimately is still a fake because you have to surface at least one face instead of simply contouring it.

    Cheers

    Marcus

  6. #25
    Join Date
    Apr 2012
    Location
    AR, USA
    Posts
    763
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    124

    Default

    The boss is about 1.25" and the peg is 3/16" square. The lathe has C axis control which is the main lathe spindle, but no A or B rotational axes.

  7. #26
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,854
    Post Thanks / Like
    Likes (Given)
    3231
    Likes (Received)
    6251

    Default

    "C" is "A" in this case.


    ----------------------

    Think Snow Eh!
    Ox

  8. Likes Bobw, kevin66 liked this post
  9. #27
    Join Date
    Apr 2012
    Location
    AR, USA
    Posts
    763
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    124

    Default

    Thanks for everyone's input, especially implmex. I see that is not possible on this machine (well I guess it may be possible with a .020" ball nose, but I'm not interested in trying that...). I'll tell them we can't do it.

  10. #28
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    2,779
    Post Thanks / Like
    Likes (Given)
    991
    Likes (Received)
    936

    Default

    Hi Marcus, I think we are more or less on the same page! Hard to put these things into words though.

    A very rough example I knocked out. Pale blue is a 3 axis swarf path, followed by yellow which is a 4 axis swarf path. The remaining material that needs to be removed by surfacing is clear(ish) to see. The intersection between shaft and stem is fully cut although simulation artifacts make it a little difficult to see. This is simulated with a sharp corner endmill.



    And the toolpaths (red is the 3 axis path, blue is the 4 axis path):


  11. #29
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,047
    Post Thanks / Like
    Likes (Given)
    573
    Likes (Received)
    1064

    Default

    So the C will position, but not feed right? Okay got it.

    I think this thread is dead, but to the geometry....

    I have been thinking about this. We had a similar feature (was a Triangle shape, but a Boss on a Cylinder) we used a Surface Finish Flowline Toolpath to get it done, the blend into the Cylinder looked crappy, but we got it done.

    Using Gregors image as an example, the facing angle being the one to work on.
    In my minds eye, assuming you were using a Truly flat Endmill parallel to the walls of the Boss. Start point would be X=OD of the Cylinder, Y=zero. Feed the C clockwise and feed Z minus and Y positive past the breakout of the angle and radius of the cutter, while maintaining the X position on the OD. It seems would be correct. I can't get the right Toolpath in Mastersuk to do it, it keeps showing me Gouges like a MFer. Large diameter cutter.

    What my point is, is the the rotation of C is not going to cause a Gouge in the Cylinder, and while rotating you can feed the cutter wherever you want in YZ, still not causing a Gouge on the Cylinder, and if the cutter starts and stops before and after the Tangencies there shouldn't be a Gouge anywhere, but my software is showing Gouging, or just not running it. Not that I praise Mastercam ever, but it seems that it should be possible.

  12. Likes gregormarwick liked this post
  13. #30
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    6,173
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    4996

    Default

    Even if undercut.
    How does one get the nice turned dia. in the area of the pin to match the rest of the shank?
    Boatloads of rotational milling?
    I'm missing something...
    Bob

  14. #31
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    2,779
    Post Thanks / Like
    Likes (Given)
    991
    Likes (Received)
    936

    Default

    Quote Originally Posted by CarbideBob View Post
    Even if undercut.
    How does one get the nice turned dia. in the area of the pin to match the rest of the shank?
    Boatloads of rotational milling?
    I'm missing something...
    Bob
    You're not missing anything. The cylindrical section will indeed have to be cut using either polar on the end or rotary with a radial live tool.

    I'm not advocating this as the best method, simply that its possible.

  15. Likes litlerob1 liked this post
  16. #32
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,854
    Post Thanks / Like
    Likes (Given)
    3231
    Likes (Received)
    6251

    Default

    The C axis is feedable on any Y axis machine, and most any live tooled machine built since 2000. You hafta be back in the 90's to find an "indexing" C axis. (likely referred to as a "B" at that time)


    Bob - that was the part in my earlier post about getting a flat bottomed mill @ Y0 and feeding in C. To clean up the rest of the "340*" (or whatever it would be).


    -----------------------

    Think Snow Eh!
    Ox

  17. Likes litlerob1 liked this post
  18. #33
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    2,001
    Post Thanks / Like
    Likes (Given)
    557
    Likes (Received)
    944

    Default

    Quote Originally Posted by CarbideBob View Post
    Even if undercut.
    How does one get the nice turned dia. in the area of the pin to match the rest of the shank?
    Boatloads of rotational milling?
    I'm missing something...
    Bob
    CNC Machining Mori Seiki Lathe - YouTube

  19. #34
    Join Date
    Apr 2007
    Location
    Pillager, MN
    Posts
    5,251
    Post Thanks / Like
    Likes (Given)
    1664
    Likes (Received)
    4471

    Default

    Quote Originally Posted by Bobw View Post
    This is one of those parts that makes me think that engineers shouldn't be driving the train, they should be thrown under it.
    ^^^^this...............................

  20. #35
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    22,854
    Post Thanks / Like
    Likes (Given)
    3231
    Likes (Received)
    6251

    Default

    Quote Originally Posted by david n View Post
    ^^^^this...............................
    They should just hafta werk the floor for some time to understand the MFG side of "parts" is all. The CAD jockey doesn't know w/o asking.

    This is really the result of skewling someone to doo what should be learned from the ground up, with a few classes thrown in here and there, instead of trying to blanket it all - and then from a textbook.

    I think that the Krauts doo it the other way. ???


    --------------------

    Think Snow Eh!
    Ox

  21. Likes Kaszub 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
  •