Simplest question ever. How to mill a notch, 1/4 x 1/4 x 3/4?
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    473
    Post Thanks / Like
    Likes (Given)
    235
    Likes (Received)
    395

    Default Simplest question ever. How to mill a notch, 1/4 x 1/4 x 3/4?

    This is the simplest question, and yet I live a sheltered life, maybe I can learn something.

    I have a part, made from cold drawn 1018 3/8 x 3/4 and saw cut to 1-1/2" long.

    In the first opp, I need to mill the saw edge square and then come back and mill off a 1/4 x 1/4 notch off the end. That will leave me 1/8" sticking out 1/4. This is a part in a fixture that get's hot swapped.

    Currently it is running in a Fadal and I'm just using an Ingersol 1-1/4"dia 3 Flute APKT160408 insert and it works fine.

    Since it works fine, lets F it up. I mean polish it a bit. I would love to move this off the fadal and onto the brother. The parts are fixtured 3/4" apart.

    Ultimate question then, in a Brother Speedio, what would be quickest way to mill off that end notch?

  2. #2
    Join Date
    Feb 2005
    Location
    Akron, OH
    Posts
    1,996
    Post Thanks / Like
    Likes (Given)
    331
    Likes (Received)
    1523

    Default

    3/8" 4 flute AlTiN endmill, trochoidal path, .08" per pass, .01 cleanup pass sides and bottom, 150IPM, 9000 rpm. So that's 5 passes of 1/2" length or so at 150 ipm. So 1.2 second in the cut, another second doing the return passes, and then a Speedio doesn't corner that hard on tight radiuses, so another second for the reversals.

    Four second per feature, give or take?

  3. Likes Homebrewblob, Strostkovy liked this post
  4. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    613
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    300

    Default

    Use a short loc 1/2” 4 flute end mill around 4500 rpm and 75 ipm and hit it in one pass. Just make sure you have a good hold on those little things.

  5. #4
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    290
    Likes (Received)
    634

    Default

    Quote Originally Posted by Spruewell View Post
    Use a short loc 1/2” 4 flute end mill around 4500 rpm and 75 ipm and hit it in one pass. Just make sure you have a good hold on those little things.
    I agree with this. With a cut this shallow in Z, hard to beat just taking it in one shot, less air cutting. Short length of cut 1/2", 4 or 5 flute, short side lock holder and hold those parts! Total cycle time to machine ends and step, 10 to 15 seconds I estimate.

  6. #5
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    473
    Post Thanks / Like
    Likes (Given)
    235
    Likes (Received)
    395

    Default

    Good lord, been making this part for years and I screwed up at the start.

    The cut is a roughing cut only, 1/4 deep axially, and 1/2" radially and 3/4" long. So a 1/4 deep X 1/2 notch.

    In a speedio.800-fixture.jpg
    The red cuts are what I am trying to do and want to avoid using a large insert cutter.

  7. #6
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    290
    Likes (Received)
    634

    Default

    I thought it was a .25" x .25" step. If it needs to be 1/2" radially, I would probably do that in two passes. One pass is probably doable with a 5/8 cutter but two quicker passes with smaller tool may work out about the same...

  8. #7
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    919
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    528

    Default

    From the looks of the picture I think you spend more time taking the parts in and out of the fixture than machining it.

  9. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,898
    Post Thanks / Like
    Likes (Given)
    5568
    Likes (Received)
    3759

    Default

    5/8" or 3/4" endmill single pass, either solid carbide or in the style of the Sandvik R390.

  10. #9
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    850
    Post Thanks / Like
    Likes (Given)
    192
    Likes (Received)
    972

    Default

    Have you considered running it in an older, slow (cheap) machine like a Fadal? Maybe with a large inserted cutter?

    I’m just kidding, I can read

    Still what I would do... a shallow depth of cut 1018 part. Perfect job to abuse an old machine (and make your least favorite employee run it... noisy, dirty and smelly... the job, not the employee).


    Sent from my iPhone using Tapatalk

  11. #10
    Join Date
    Apr 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,020
    Post Thanks / Like
    Likes (Given)
    1272
    Likes (Received)
    679

    Default

    Best, but most expensive - get one of those cutters bodies built onto a 30 taper, 3/4" to 1" diameter.
    2nd best, get the screw on type, holder from Mari, and cutter body from whoever using your bestest favorite insert.
    3rd best, likely cheapest, get a cutter with 3/4" shank (or 1" and turn it down?). IIRC I found a 1" cutter with 3/4" shank, and shortened the shank, milled a flat, and use it in the shortest Mari holder. You can likely find one that uses that same inserts you have now.

  12. #11
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    473
    Post Thanks / Like
    Likes (Given)
    235
    Likes (Received)
    395

    Default

    There are two fixture plates. The parts are all held in place with 1/2" blunt edge pitbulls. Two pitbulls on the LH side and only 1 on the right hand side with the lighter cuts.
    While one is running, it takes about 5 minutes to use an electric torque driver to bust those loose, blow it off and reload.
    The cycle is about 12 minutes I think.

    I do have a couple of those screw top endmills on the BT30 shank that take my common inserts, I just wasn't sure how much a 16K speedio would like pushing a 25MM 2 flute APKT1604 thru that cut.

    I reckon its time for some tests again.

    Not really an option on dumping it on an employee. For now it is just me and my son and with luck I'm retiring in another 5 years. SO I want the long term job nicely running for thousands of parts into the future on ANY machine.


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
  •