Machining Hex to specific size
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default Machining Hex to specific size

    Apparently as somebody that rides the mazatrol short bus i have a couple more questions. I am playing around with trying to program a hex. I get the shape to come out correctly but i haven't been able to get it to dimension correctly. Can somebody shed some light on the correct procedure to accomplish this? Lets say i need the wrench flats to measure 1.5" using 5/8" end mill. How do i calculate what the control needs in the FPT-R/x Column?

    20191105_115745.jpg

  2. #2
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,532
    Post Thanks / Like
    Likes (Given)
    537
    Likes (Received)
    925

    Default

    Multiply 1.5 by 1.154. That will give you your FPT.

  3. Likes Philabuster liked this post
  4. #3
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    That seams easy enough. I figured i was missing something? 1.154 is used for all sizes?

  5. #4
    Join Date
    Jul 2009
    Location
    NW Illlinois USA
    Posts
    426
    Post Thanks / Like
    Likes (Given)
    101
    Likes (Received)
    134

    Default

    Your sketch shows an octagon...

  6. Likes Bobw liked this post
  7. #5
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Artist i am not! Nor a machinist the way it looks. Try this one!

    20191105_124221.jpg

  8. Likes Bobw liked this post
  9. #6
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    4,585
    Post Thanks / Like
    Likes (Given)
    18388
    Likes (Received)
    4303

    Default

    Quote Originally Posted by Blackhawkxp View Post
    Lest say i need the wrench flats to measure 1.5" using 5/8" end bill. How do i calculate what the control needs in the FPT-R/x Column?
    When using polar coordinates (green numbers), program to the corners of the hex. Take the radius value of your flat (1.5" / 2 = .75") and multiply it by 1.154 = .8655" to get the dimension from the center of the part to the corner of the flat.

    Then on your program you want to do a LEFT FACE, .625 width. The machine will compensate for the endmill diameter if your tool data page is correct.

    X .8655, Ang 0
    X .8655, Ang -60
    X .8655, Ang -120
    X.8655, Ang -180
    X.8655, Ang -240
    X.8655, Ang -300
    X.8655, Ang -360

  10. #7
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Just to verify the setting of the tool data the center of the end mill in a straight live tool holder has to be on the center line of the main spindle. This is how i have it setup and it worked perfect for milling the .5" flat on my last project. Since then i have been wondering since it is a lathe should the top edge of the end mill be at zero? I'm trying to take baby steps and i keep falling down the stairs.

    20191105_131701.jpg

  11. #8
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    4,585
    Post Thanks / Like
    Likes (Given)
    18388
    Likes (Received)
    4303

    Default

    Center of the endmill needs to be X zero. Same as you would set a drill bit.

    Here's my cheat sheet for milling a hex on the Mazak.
    Attached Thumbnails Attached Thumbnails 20191105_121732_resized.jpg  

  12. #9
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Using the formula it seems to cut mostly right. It seems to be small by .020" on all sizes that i tried. Then all of a sudden i think the control didn't apply cutter comp and it started cutting way small. It just happened out of the blue. Not sure if there is a way to toggle it on or off? There might be something going on with the machine? What is the best way to adjust for size?

  13. #10
    Join Date
    Jul 2006
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    4,585
    Post Thanks / Like
    Likes (Given)
    18388
    Likes (Received)
    4303

    Default

    Quote Originally Posted by Blackhawkxp View Post
    Using the formula it seems to cut mostly right. It seems to be small by .020" on all sizes that i tried. Then all of a sudden i think the control didn't apply cutter comp and it started cutting way small. It just happened out of the blue. Not sure if there is a way to toggle it on or off? There might be something going on with the machine? What is the best way to adjust for size?
    The only way to toggle off the cutter comp is to completely clear out the cutter diameter from the tool data page or you accidentally edited the program to be Line Center instead of Line Left. Editing the program accidentally is easy to do. If that's not the case, then I don't have a clue what is going on.

    If you have the correct endmill diameter registered in the tool data page, adjust the X axis offset +.020 as it sounds like your tool is off a bit.

  14. #11
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,532
    Post Thanks / Like
    Likes (Given)
    537
    Likes (Received)
    925

    Default

    Quote Originally Posted by Blackhawkxp View Post
    That seams easy enough. I figured i was missing something? 1.154 is used for all sizes?
    Yes.It does.

  15. #12
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    22
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    I think i figured out what my issues were. I didn't put the (-) sign in the degree column so cutter comp was offsetting to the inside of the tool path instead of the outside. I am slowly figuring out how the machine works. Thanks for all of your help. Its the simple stuff that seems to get me. Hopefully others will learn from this in the future and save them from the humility of having to ask for help! I'm sure i will be back with more questions.

  16. #13
    Join Date
    Dec 2008
    Location
    Bethlehem Pa USA
    Posts
    74
    Post Thanks / Like
    Likes (Given)
    27
    Likes (Received)
    17

    Default

    img_4858.jpg

    here is my cheat sheet I have printed out next to my lathe for when i do hex. I also just keep a program in machine and labeled it hex. Then I go into file explorer, and right click the program and make it read only. This way nobody can change or delete it. Just copy it.


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
  •