1018 steel face grooving tips and speeds etc
Close
Login to Your Account
Results 1 to 18 of 18
  1. #1
    Join Date
    Oct 2012
    Location
    los angeles
    Posts
    159
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default 1018 steel face grooving tips and speeds etc

    have to hog out steel with a face grooving tool capable of 1.2 inch depth .. The lathe is 25 hp and the groove is around 5 inch to 3 inch from center on a 6.5 inch part diameter..

    I do machine some stainless from time to time but have not done too much steel on this lathe and am looking for some tips on what folks do to for tool paths and feeds speeds as well as a good tool brand tips for this sort of thing.. Will have to make a bunch of these and have some money for tooling on this job..

    any recommends on this type of thing i would really appreciate..
    thank you

  2. #2
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    7,375
    Post Thanks / Like
    Likes (Given)
    674
    Likes (Received)
    3482

    Default

    Wouldn't it be quicker and cheaper to rough out the slugs on a mill?

  3. #3
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,583
    Post Thanks / Like
    Likes (Given)
    1207
    Likes (Received)
    2562

    Default

    This is Iscars HFHR/L I like the square shank, the double ended inserts, the positive screw down clamp, and the variety of insert grades and chipbreakers.

    heliface_medium-diameter1a_2a.jpg

  4. Likes Chip Burns liked this post
  5. #4
    Join Date
    Mar 2011
    Country
    SWITZERLAND
    Posts
    1,006
    Post Thanks / Like
    Likes (Given)
    122
    Likes (Received)
    413

    Default

    It would be nice to have a live tool on A or B axis. You could mill-turn the face groove, a matter of two minutes. Else buy a sturdy tool (holder), plunge in at about 100 m/min and gentle feed. You want steel to become warm enough to almost burn the chips in order to keep them breaking into small pieces. Nothing’s worse than strings in a face groove!

  6. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,685
    Post Thanks / Like
    Likes (Given)
    4297
    Likes (Received)
    2845

    Default

    Quote Originally Posted by Dualkit View Post
    Wouldn't it be quicker and cheaper to rough out the slugs on a mill?
    A lathe can usually do this in a fraction of the time a mill can. (if it has any type of profile other than just a square groove)

  7. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,685
    Post Thanks / Like
    Likes (Given)
    4297
    Likes (Received)
    2845

    Default

    I'm a Sandvik guy, but when it comes to grooving, it's hard to be better at it than Iscar.
    That being said, any top brand will have capable tooling.
    Ideally you'd be running approximately 800sfpm, .004ipr minimum depending on width of insert.
    Peck or not is your choice, but I would at least chip break the first cut on a groove that deep. Then you could treat it like a boring bar or a turning tool depending on if you start at the inner or outer portion of the groove.

    Some people like to take the first cut to depth, others like to take the whole groove profile to depth at the same time, meaning a depth cut of the entire groove profile until final depth is reached.

    If you have a good, stable setup and holders get a 5/16 wide insert or so.
    The wider the insert the quicker the job will go.

    1018 is gravy, especially compared to stainless. I've been cutting it for over 30 years.

  8. #7
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,218
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1014

    Default

    Quote Originally Posted by Mtndew View Post
    I'm a Sandvik guy, but when it comes to grooving, it's hard to be better at it than Iscar.
    Is Manchester gone now ?

  9. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,685
    Post Thanks / Like
    Likes (Given)
    4297
    Likes (Received)
    2845

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    Is Manchester gone now ?
    I've never used Manchester here in Michigan, and I doubt there is a rep even nearby.

  10. #9
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,583
    Post Thanks / Like
    Likes (Given)
    1207
    Likes (Received)
    2562

    Default

    For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

    R

  11. #10
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,218
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1014

    Default

    Quote Originally Posted by Mtndew View Post
    I've never used Manchester here in Michigan, and I doubt there is a rep even nearby.
    You made me go look

    Manchester cutoff tools - Where to get!!!

    Well, kinda poo but maybe not altogether. Iscar, pisscar, Manchester was THE best for cutoff and face grooving.

    Found this, too

    Manchester

    Not sure what it means tho ...

  12. Likes Mtndew liked this post
  13. #11
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,850
    Post Thanks / Like
    Likes (Given)
    10623
    Likes (Received)
    3243

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    You made me go look

    Manchester cutoff tools - Where to get!!!

    Well, kinda poo but maybe not altogether. Iscar, pisscar, Manchester was THE best for cutoff and face grooving.

    Found this, too

    Manchester

    Not sure what it means tho ...


    Looks like Widia bought Manchester?

    (Link is to a PDF catalog showing Widia-Manchester grooving tools)

    https://www.widia.com/content/dam/ke...-C_English.pdf

  14. #12
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,806
    Post Thanks / Like
    Likes (Given)
    392
    Likes (Received)
    6489

    Default

    And who now owns Widia which was part of Krupp and one of the first carbide suppliers?
    AFAIK Manchester did the first inverted vee which was big in stability over the other options.
    Iscar would grow exponentially playing on this concept.

    History or other is of no matter. What runs best today as I need to peel of steel is the only concern.
    Bob

  15. #13
    Join Date
    Aug 2012
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    86
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    28

    Default

    Quote Originally Posted by litlerob1 View Post
    For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

    R
    I agree with the round insert. If you have Mastercam, you can use the Dynamic Grooving toolpath which is supposed to keep the cutting load constant throughout the path. It generates a lot of lines of code, but it lets you feed the hell out of it to try to break chips. I think they have a video of it on their website.

    -Gene

  16. Likes Mtndew liked this post
  17. #14
    Join Date
    Oct 2012
    Location
    los angeles
    Posts
    159
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Litlerob1 suggested the HFHL holder which is what my ISCAR rep is saying on this.. Iscar is calling for a ic808 grade.. I would like to do this on the lathe if poss, not have to transfer to the mill to hog out first.. I will look at the tool paths that BOBCAD Has, i am running their software with this lathe, and i will try to run a 5/16 width or better insert as some one said above.. so off to speed and feed for this and whether to dive to the bottom or take it in passes, and whether to go across or straight down into part..
    any other feeds input or tooling methods you guys have i would appreciate hearing about.. Have a feeling there will be some trial and error here..

    thank you Zach

  18. #15
    Join Date
    Oct 2012
    Location
    los angeles
    Posts
    159
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    6

    Default

    Quote Originally Posted by litlerob1 View Post
    For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

    R
    so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..

  19. #16
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,685
    Post Thanks / Like
    Likes (Given)
    4297
    Likes (Received)
    2845

    Default

    Quote Originally Posted by zschary View Post
    so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..
    So your groove is a basic [ shape?
    What littlerob1 is suggesting and what I've done also is to basically groove it in the style of a facing toolpath.
    G01 Z-.05
    X down to your diameter
    Z.1
    Repeat.
    With a round style insert you can feed it pretty good. It's also less risky of busting tools by not having to take the tool to depth on the first pass.

    Another thing we do on large grooves is to use the groover to remove some stock, then swap to a boring bar and bore it out.
    Or use a reverse DNMG,VNMG tool to turn/face it out.

  20. #17
    Join Date
    Mar 2014
    Location
    Nebraska
    Posts
    364
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    228

    Default

    I agree with the HFHR recommendation from Iscar. If there is something else that even comes close I would be interested in hearing it but it sure isn't Manchester. That being said I have had to use Manchester on a few jobs where Iscar didn't have the right blade depth/diameter/width combination and Manchester did. There is no comparison.

  21. #18
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,583
    Post Thanks / Like
    Likes (Given)
    1207
    Likes (Received)
    2562

    Default

    Quote Originally Posted by zschary View Post
    so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..
    Correct. And you don't need software to generate the code, it's very basic. The benefit of the holder that I posted up there, is that itll take lots of different insert styles and shapes, including Round. With a Square cutting edge you'll need to slow down the feed, but with Round .025" per rev is not too much.

    R


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
  •