Roughing stock left for finish
Close
Login to Your Account
Results 1 to 9 of 9
  1. #1
    Join Date
    Oct 2015
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    372
    Post Thanks / Like
    Likes (Given)
    212
    Likes (Received)
    317

    Default Roughing stock left for finish

    I'm curious since I have a lot of time in this profession, but not a lot of variety.

    If you are roughing, then finish milling after. How much stock do you leave to clean up on both radial and floor?

    For Aluminum?
    Radial = A
    Floor = B

    For carbon Steel
    Radial = C
    Floor = D

    And why that amount?

    My answers for carbide end mills are

    A= .02
    B= .01

    C= .01
    D= .03

    I like a little more floor on the steel so that it hopefully gets a little more heat in the cut and doesn't tear the floor.

  2. #2
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,704
    Post Thanks / Like
    Likes (Given)
    3197
    Likes (Received)
    2141

    Default

    A .003/.005
    B .003
    C .003/.005
    D .003

    Because of habit.

  3. Likes dstryr liked this post
  4. #3
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    2,507
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    968

    Default

    Maybe I should have a number, as I can't tell you the number of parts I've wrecked by not leaving quite enough to clean up. That also includes "saving" money by sawing raw stock a bit too close.

  5. Likes Bobw, Davis In SC liked this post
  6. #4
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    171
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    108

    Default

    A .005/.01
    B .005
    C .01/.02
    D .005/.01

    If I use the same finishing tool for roughing and finishing for aluminum I sometimes leave 0 but apply a spring pass. Some other factors are the total depth of cut apply which may end up with multiple spring passes.

  7. #5
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    8,536
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2275

    Default

    Quote Originally Posted by Houndogforever View Post
    I'm curious since I have a lot of time in this profession, but not a lot of variety.

    If you are roughing, then finish milling after. How much stock do you leave to clean up on both radial and floor?

    For Aluminum?
    Radial = A
    Floor = B

    For carbon Steel
    Radial = C
    Floor = D

    And why that amount?

    My answers for carbide end mills are

    A= .02
    B= .01

    C= .01
    D= .03

    I like a little more floor on the steel so that it hopefully gets a little more heat in the cut and doesn't tear the floor.
    .
    .
    depends on of course
    .
    1) cutter deflection
    2) part deflection
    3) machine tracking tool path accurately
    4) accuracy of setting tool dia and length comp
    .
    i have seen plenty of deflection over the years from long tools and raw horsepower. i have seen old cnc with wear and backlash problems at higher feed rates over .010" error following tool path is common. many many times i have seen roughing marks not clean up cause not enough stock left.
    .
    a source of common tool error is carbide insert mills where inserts on end the pockets are damaged and inserts rotated a bit. i have often seen inserts on end at .005 or smaller diameter than next set of inserts down. so a combination factors can easily combine and cause problems. carbide end mills i have seen many long length end mills bend quite a bit from cutting forces. depends if you are pushing the limits under a cloud of coolant smoke
    Attached Thumbnails Attached Thumbnails steam.jpg   longmill.jpg   toolrack.jpg  

  8. #6
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    34
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    8

    Default

    For me depends on the rough tool.
    But typ. Is .01 wall .005 floor but
    I run the wall first then floor with
    The spring pass of wall.

    A: .01
    B: .005

  9. #7
    Join Date
    May 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    135
    Post Thanks / Like
    Likes (Given)
    56
    Likes (Received)
    61

    Default

    I will usually leave .005 on the floor, .010 on walls for just about anything. If need be, I'll do a semi-finish pass on the wall, leaving .005 for a finish pass, if it's a deep wall (3x D or more).

  10. #8
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    715
    Post Thanks / Like
    Likes (Given)
    249
    Likes (Received)
    332

    Default

    Usually .01" and .01". Small tools I will go down to .005 and .005. I will do the floor first staying off the .005 or .01 and come back and finish the walls. If I'm surfacing something I'll typically leave .020 on the surface.

  11. #9
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    8,536
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2275

    Default

    obviously depends on length to diameter ratio of tools and what cutting forces or horsepower is involved.
    .
    2 hp or 20 hp, obviously can push part with tons of force. obviously 2" diameter end mill sticking out a foot not going to run same as 2" dia shell mill only 2" long
    .
    i have seen many parts vibrate easily over .010", raw horsepower can make parts weighing tons vibrate severely quite easily and sound can easily be heard 100 feet away
    .
    obviously a 6" dia facemill taking 5.5" width passes at 0.2" depth at 50" per minute can vibrate a part very severely. facemill can easily handle 60" per minute as long as part not vibrating. i have often seen chatter marks not clean even taking .015" for finish pass. aluminum parts same facemill at over 100 ipm many a part vibrating too much and have to reduce cutting rate. part cannot take 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
  •