Speed Feed Question With Volumill or Adaptive Clearing Toolpaths
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Jan 2011
    Location
    Kansas
    Posts
    696
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    53

    Default Speed Feed Question With Volumill or Adaptive Clearing Toolpaths

    What's a good rule of thumb for speed and feed increase when you are using volumill or adaptive clearing toolpaths? For example, if I am milling in 304 at 200 SFM and 10 IPM with a 1/2 inch carbide endmill, what should I be at with a adaptive clearing toolpath?

  2. #2
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,913
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2579

    Default

    Quote Originally Posted by munruh View Post
    What's a good rule of thumb for speed and feed increase when you are using volumill or adaptive clearing toolpaths? For example, if I am milling in 304 at 200 SFM and 10 IPM with a 1/2 inch carbide endmill, what should I be at with a adaptive clearing toolpath?
    .
    many end mill makes give a chart of sfpm and ipt when slotting, heavy peripheral and light peripheral milling.
    .
    usually tool length sticking out, tool holder length, machine rigidity and hp and part and fixture rigidity become a factor.
    .
    crude but many operators keep trying higher rpm and feed and see what the sudden tool failure rate and tool life rate becomes. that is if you go 150% rpm and 200% feed and you get a 1% sudden tool failure rate. does the sudden tool failure rate become enough of a problem its better to back off for higher reliability. that is if tool suddenly breaks causing many hours of rework and that extra cost calculates as not a time and money saving it becomes more a math and statistic thing spread out over the whole year. that number crunching often determines feeds and speeds

  3. #3
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    20

    Default

    Quote Originally Posted by munruh View Post
    What's a good rule of thumb for speed and feed increase when you are using volumill or adaptive clearing toolpaths? For example, if I am milling in 304 at 200 SFM and 10 IPM with a 1/2 inch carbide endmill, what should I be at with a adaptive clearing toolpath?
    Look into Radial chip thinning factor. It's the math that determines the thickness of a chip at a specific stepover. There are calculators online. I know it doesn't help you, but mastercam has a little button called "RCTF" that does the math for you. That's not to say I use it all the time, most of what I program is based off trial and error. I can tell you ide be at about 585sfpm with a chip load of about .006 per tooth, maybe a little more, depending on the end mill.

  4. Likes Mtndew liked this post
  5. #4
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,411
    Post Thanks / Like
    Likes (Given)
    3990
    Likes (Received)
    2612

    Default

    Quote Originally Posted by munruh View Post
    What's a good rule of thumb for speed and feed increase when you are using volumill or adaptive clearing toolpaths? For example, if I am milling in 304 at 200 SFM and 10 IPM with a 1/2 inch carbide endmill, what should I be at with a adaptive clearing toolpath?
    Have a look at HSM Advisor, it's very handy for these types of toolpaths.

    With a 1/2" 4 flute and a 1" l.o.c. and using a 10% stepover you should be around 400sfpm and .005 per tooth feedrate.
    3185rpm and 65ipm

  6. Likes mhajicek, gkoenig, eaglemike liked this post
  7. #5
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    20

    Default

    ...At 12 percent. I forgot the important part.

  8. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,411
    Post Thanks / Like
    Likes (Given)
    3990
    Likes (Received)
    2612

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    many end mill makes give a chart of sfpm and ipt when slotting, heavy peripheral and light peripheral milling.
    .
    usually tool length sticking out, tool holder length, machine rigidity and hp and part and fixture rigidity become a factor.
    .
    crude but many operators keep trying higher rpm and feed and see what the sudden tool failure rate and tool life rate becomes. that is if you go 150% rpm and 200% feed and you get a 1% sudden tool failure rate. does the sudden tool failure rate become enough of a problem its better to back off for higher reliability. that is if tool suddenly breaks causing many hours of rework and that extra cost calculates as not a time and money saving it becomes more a math and statistic thing spread out over the whole year. that number crunching often determines feeds and speeds
    Why do you even bother responding, you never directly answer anyone's questions.

  9. #7
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    727
    Post Thanks / Like
    Likes (Given)
    641
    Likes (Received)
    413

    Default

    I use HSM Advisor and the Helical Machining Advisor Pro. There are many factors that go into choosing the optimal cutting parameters, and they both take them into account.

  10. Likes Mtndew, 5 axis Fidia guy liked this post
  11. #8
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,077
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    1427

    Default

    Quote Originally Posted by BRIAN.T View Post
    Look into Radial chip thinning factor.
    Yes, this. Depending on your CAM, you might have an option to apply RCTF right in the CAM project. This is Mastercam, with a 1/2" 6-flute endmill @ 6% stepover:

    rctf.jpg

    Note that the non-RCTF feed rate would be 96 IPM, so RCTF makes a big difference.

    Regards.

    Mike
    Last edited by Finegrain; 04-12-2019 at 01:46 PM. Reason: Why do pics

  12. Likes Mtndew liked this post
  13. #9
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,242
    Post Thanks / Like
    Likes (Given)
    352
    Likes (Received)
    575

    Default

    If you're running Gibbs Helical Advisor is built in to it in version 12 or later, it gives me very similar numbers to my seat of g-wizard.

  14. Likes Mtndew liked this post
  15. #10
    Join Date
    Apr 2015
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    89
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    14

    Default

    I've found the Iscar chip thinning calculator to be quite useful. ITA Calculators

  16. #11
    Join Date
    Jan 2011
    Location
    Kansas
    Posts
    696
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    53

    Default

    thank you. appreciate the responses


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
  •