Help with programming and machining this part
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Dec 2017
    Country
    SOUTH AFRICA
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Help with programming and machining this part

    4.0mm-x-30-hole-die.jpg
    I need help programming the angled face end of this part.

    Any advice appreciated.
    Attached Files Attached Files

  2. #2
    Join Date
    Apr 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    814
    Post Thanks / Like
    Likes (Given)
    696
    Likes (Received)
    648

    Default

    Mill? Lathe? What have you tried so far? What do you need help with specifically?

    Way, way too open ended for anyone to be able to help you.

  3. #3
    tommy d Guest

    Default

    Quote Originally Posted by Johnny SolidWorks View Post
    Mill? Lathe? What have you tried so far? What do you need help with specifically?

    Way, way too open ended for anyone to be able to help you.
    exactly what i was thinking! if it is on a lathe i would use a LH dnmg set up for facing but there are a lot of options on how to do it, flip a boring bar over, trepans, etc.

  4. #4
    Join Date
    Dec 2017
    Country
    SOUTH AFRICA
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I need to make 20 all slightly different.
    I thought turning would be quicker but I don't know what tooling to use.
    The part is 316 stainless steel.
    I have tried in HSM works but again it will not accept a boring bar.

  5. #5
    tommy d Guest

    Default

    Quote Originally Posted by tline View Post
    I need to make 20 all slightly different.
    I thought turning would be quicker but I don't know what tooling to use.
    The part is 316 stainless steel.
    I have tried in HSM works but again it will not accept a boring bar.
    i had never heard of hsm works until today but i looked it up and it looks like the program is calling it a 55 deg diamond which i have a bad habit of calling a dnmg since that is pretty much all i use.

  6. #6
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,115
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1216

    Default

    Quote Originally Posted by tline View Post
    I need to make 20 all slightly different.
    I thought turning would be quicker but I don't know what tooling to use.
    The part is 316 stainless steel.
    I have tried in HSM works but again it will not accept a boring bar.
    Hello tline,
    I would use a Boring Bar similar to that shown in the attached picture; all you need is an approach angle that will give clearance on the angled face. No need to flip it, just set it as a conventional B/Bar.

    boring-bar1.jpg

    The example code is for a 0.8 TNR. DOC is conservative, as this insert shape and approach angle doesn't give a great cutting action with a DOC much over the TNR size when face cutting from small to large Dia.

    Regards,

    Bill

    Code:
    (55DEG. DIAMOND 0.8 TNR BORING BAR 100DEG APPROACH ANGLE)
    N1 G00 X-0.400 Z3.000
    G01 Z1.000 F1.00
    G01 Z0.260 F0.20
    G01 X30.246 Z-1.350 F0.25
    G01 X139.700
    G01 Z-1.050
    G03 X142.100 Z0.150 I1.200 K0.000
    G00 Z2.200
    G00 X30.147
    G01 Z-1.345
    G01 X58.793 Z-2.850
    G01 X139.700
    G01 Z-1.350
    G00 X58.693
    G01 Z-2.845
    G01 X87.340 Z-4.350
    G01 X137.373
    G01 X139.700 Z-3.186
    G01 Z-2.850
    G00 X87.240
    G01 Z-4.345
    G01 X111.700 Z-5.630
    G01 X134.813
    G01 X137.373 Z-4.350
    G00 X137.373 Z2.200
    (FINISH PASS STARTS HERE)
    G00 X142.100 Z2.200
    G01 Z0.000 F0.20
    G02 X140.000 Z-1.050 I0.000 K-1.050
    G01 Z-3.249
    G01 X134.937 Z-5.780
    G01 X111.684
    G01 X-0.400 Z0.109
    G00 Z2.200

  7. #7
    Join Date
    Dec 2017
    Country
    SOUTH AFRICA
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thank you Bill.
    Much appreciated.
    Mike

  8. #8
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,115
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1216

    Default

    Quote Originally Posted by tline View Post
    Thank you Bill.
    Much appreciated.
    Mike
    Hello Mike,
    If you were to use a Face Roughing cycle, such as a G72 cycle for a Fanuc Control, you only need to program the profile path and you can then play around with the DOC using the parameters of the cycle without having to re-post process the program.

    Regards,

    Bill
    Last edited by angelw; 12-28-2017 at 12:23 AM.

  9. #9
    Join Date
    Dec 2017
    Country
    SOUTH AFRICA
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Being really new to turning and an old fart to boot.
    What is DOC and TNR?

  10. #10
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    5,819
    Post Thanks / Like
    Likes (Given)
    219
    Likes (Received)
    2366

    Default

    Quote Originally Posted by tline View Post
    Being really new to turning and an old fart to boot.
    What is DOC and TNR?
    I would guess depth of cut and tool nose radius.

  11. #11
    Join Date
    Dec 2017
    Country
    SOUTH AFRICA
    Posts
    5
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    logical once one knows.
    Thank you again.


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
  •