Mazak QTN100-2 Tool Nose Radius Compensation Question
Close
Login to Your Account
Results 1 to 13 of 13
  1. #1
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    842
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    370

    Default Mazak QTN100-2 Tool Nose Radius Compensation Question

    Fusion Matrix control

    Ever since I got my lathe I struggle making correct radii on smaller features (i.e. .015R on a .250 Dia).

    Well I'm trying to turn a 4° taper to 0,0 and I'm getting an approx .020" Diameter tit at the center. I would like to minimize this.

    So I checked my turret for alignment by running my tool to zero machining a piece of stock and I get the tit. If I run it passed zero the tit is minimized to next to nothing and would be satisfied with results.

    I've also swept a drill holder and turret is aligned there.

    I checked to confirm my TNR in my tool setting was correct and it is.

    I made a .010 Diameter offset in X to see if it would disappear. I.e. my 1.125 OD now measures 1.115, but the tit is the same size diameter.

    IS there some sort of tool nose compensation setting I can check to see if proper parameters are set?

    Any other ideas?

    As always - Thanks for the assistance!

  2. #2
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    133
    Post Thanks / Like
    Likes (Given)
    110
    Likes (Received)
    17

    Default

    Sounds like the turret is out on it or the tool/insert is not the correct height. Every one I have been on compensates for the tool radius and actually goes past center when doing a facing unit. I would take the tool out and setup a indicator on the flat and translate X to see if its the turret out.

  3. #3
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,236
    Post Thanks / Like
    Likes (Given)
    4745
    Likes (Received)
    1631

    Default

    Quote Originally Posted by countryboy1966 View Post
    so I checked my turret for alignment by running my tool to zero machining a piece of stock and I get the tit. If I run it passed zero the tit is minimized to next to nothing and would be satisfied with results.
    You have to feed passed zero the radius of the tool to get the titty to be gone. I was using a 3/16 round tool feeding to X-.094 to get the titty flat.

    Since you can face it flat then my guess is that it's not a tit but rather the small of the part is rolling over the tip of the tool due to how flimsy/small it is.

    Brent

  4. #4
    Join Date
    Apr 2006
    Location
    Illinois
    Posts
    205
    Post Thanks / Like
    Likes (Given)
    277
    Likes (Received)
    155

    Default

    Quote Originally Posted by countryboy1966 View Post
    Fusion Matrix control

    Ever since I got my lathe I struggle making correct radii on smaller features (i.e. .015R on a .250 Dia).

    Well I'm trying to turn a 4° taper to 0,0 and I'm getting an approx .020" Diameter tit at the center. I would like to minimize this.

    So I checked my turret for alignment by running my tool to zero machining a piece of stock and I get the tit. If I run it passed zero the tit is minimized to next to nothing and would be satisfied with results.

    I've also swept a drill holder and turret is aligned there.

    I checked to confirm my TNR in my tool setting was correct and it is.

    I made a .010 Diameter offset in X to see if it would disappear. I.e. my 1.125 OD now measures 1.115, but the tit is the same size diameter.

    IS there some sort of tool nose compensation setting I can check to see if proper parameters are set?

    Any other ideas?

    As always - Thanks for the assistance!
    Witch process are you using.

    Facing

    Or

    Bar face

  5. Likes Red James liked this post
  6. #5
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    842
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    370

    Default

    Quote Originally Posted by INTEGREX GEEK View Post
    Witch process are you using.

    Facing

    Or

    Bar face
    Using Bar Out. I think this is part of the problem because while my roughing pass feeds from larger to smaller diameter, the finish pass is finishing from small diameter to larger diameter. Was hoping I could cheat it seeing that my finish pass was only .003".

  7. #6
    Join Date
    Apr 2006
    Location
    Illinois
    Posts
    205
    Post Thanks / Like
    Likes (Given)
    277
    Likes (Received)
    155

    Default

    Quote Originally Posted by countryboy1966 View Post
    Using Bar Out. I think this is part of the problem because while my roughing pass feeds from larger to smaller diameter, the finish pass is finishing from small diameter to larger diameter. Was hoping I could cheat it seeing that my finish pass was only .003".
    Facing goes past center Bar out doesn't.




    Offset your X minus 2 x tool Rad
    Add 2 x tool rad to diameter if needed.

  8. #7
    Join Date
    Jan 2013
    Location
    Plainfield, Indiana, USA
    Posts
    1,747
    Post Thanks / Like
    Likes (Given)
    1329
    Likes (Received)
    928

    Default

    Integrex Geek is spot on with the cause; I suggest you learn how 'Bar Face' works . . . once you learn it you will find it very useful.

  9. #8
    Join Date
    Apr 2006
    Location
    Illinois
    Posts
    205
    Post Thanks / Like
    Likes (Given)
    277
    Likes (Received)
    155

    Default

    Example

  10. #9
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,236
    Post Thanks / Like
    Likes (Given)
    4745
    Likes (Received)
    1631

    Default

    I didn't realize this was on the Mazak board when I posted even though it's clearly in the title.

    Brent

  11. #10
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    842
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    370

    Default

    Quote Originally Posted by INTEGREX GEEK View Post
    Facing goes past center Bar out doesn't.




    Offset your X minus 2 x tool Rad
    Add 2 x tool rad to diameter if needed.
    Thanks. I found benefit with those offsets.

    Is there anyway to taper with the face command?

  12. #11
    Join Date
    Apr 2006
    Location
    Illinois
    Posts
    205
    Post Thanks / Like
    Likes (Given)
    277
    Likes (Received)
    155

    Default

    Quote Originally Posted by countryboy1966 View Post
    Thanks. I found benefit with those offsets.

    Is there anyway to taper with the face command?
    Nope

    Only BAR FACE

    Sq 1 facing
    Sq2 bar face

  13. #12
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    842
    Post Thanks / Like
    Likes (Given)
    191
    Likes (Received)
    370

    Default

    Quote Originally Posted by INTEGREX GEEK View Post
    Facing goes past center Bar out doesn't.




    Offset your X minus 2 x tool Rad
    Add 2 x tool rad to diameter if needed.
    Thanks. I found benefit with those offsets.

    Is there anyway to taper with the face command?

  14. #13
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,554
    Post Thanks / Like
    Likes (Given)
    551
    Likes (Received)
    930

    Default

    On my T-2 when turning a taper starting at X0, the finish pass begins at X-0.0262 (with a .032 nose radius) using a Bar out. There may be a parameter setting for that on a Matrix. I am surprised anybody would have it set up like that.


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
  •