Need help with radius grooving.
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 49
  1. #1
    Join Date
    Nov 2017
    Country
    PORTUGAL
    Posts
    65
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    3

    Default Need help with radius grooving.

    Hello, Self learning cnc lathe and I need help/advice on which tool and cycle to use for "grooving" a Radius.
    Control Fanuc OiT
    Machine Kia SKT 200.
    Thanks in advance.
    Regardspolia.jpg

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,568
    Post Thanks / Like
    Likes (Given)
    1206
    Likes (Received)
    2547

    Default

    I would use a full radius grooving tool. Maybe 3mm wide. You can use G75 to Rough it out.

    R

  3. #3
    Join Date
    Nov 2017
    Country
    PORTUGAL
    Posts
    65
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    3

    Default

    Quote Originally Posted by litlerob1 View Post
    I would use a full radius grooving tool. Maybe 3mm wide. You can use G75 to Rough it out.

    R
    Humm... Thanks, I will look into it.

    While i am at it, Can you please confirm that, to setup that type of tool for cutter comp on fanuc control i must use position 8 and specified the radius of of 1.5 for in this example Ø3mm full radius tool?

  4. #4
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,568
    Post Thanks / Like
    Likes (Given)
    1206
    Likes (Received)
    2547

    Default

    Yes 8 (3 works too) and yes the Radius of 3mm is 1.5mm.

    R

  5. #5
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    85
    Post Thanks / Like
    Likes (Given)
    239
    Likes (Received)
    33

    Default

    I would use a neutral tool holder with a 35 degree insert for that.
    Attached Thumbnails Attached Thumbnails lathetool.jpg  

  6. #6
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    619
    Post Thanks / Like
    Likes (Given)
    49
    Likes (Received)
    210

    Default

    Quote Originally Posted by Fancuku View Post
    I would use a neutral tool holder with a 35 degree insert for that.
    There weak and they suck unless your finishing only.


    like bob said in his post or even a toplock full rad insert. plunge to rough then follow it with a finish pass.

  7. Likes litlerob1 liked this post
  8. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,687
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1449

    Default

    Quote Originally Posted by Fancuku View Post
    I would use a neutral tool holder with a 35 degree insert for that.
    Hello Fancuku,
    You won't be able to use that tool and insert, as it will interfere with the Start and End area of the radius.

    Regards,

    Bill

  9. #8
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,250
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    225

    Default

    Interference is not very obvious because the drawing is not to-scale. Actually, it is half circle! Only full-radius tools can be used.

  10. #9
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    85
    Post Thanks / Like
    Likes (Given)
    239
    Likes (Received)
    33

    Default

    Quote Originally Posted by angelw View Post
    Hello Fancuku,
    You won't be able to use that tool and insert, as it will interfere with the Start and End area of the radius.

    Regards,

    Bill
    You’re right. I just realized that it’s almost half circle. That tool doesn’t have the clearance to make that radius.

  11. #10
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,132
    Post Thanks / Like
    Likes (Given)
    228
    Likes (Received)
    2103

    Default

    Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

    Unfortunately I don't speak Fanuc

  12. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    619
    Post Thanks / Like
    Likes (Given)
    49
    Likes (Received)
    210

    Default

    Quote Originally Posted by gustafson View Post
    Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

    Unfortunately I don't speak Fanuc
    bobs 3mm was a full rad insert, I didnt mean a full rad insert the size of the part rad. ie a form tool.
    you can get all kinds of sizes of full rad inserts.

  13. #12
    Join Date
    Nov 2017
    Country
    PORTUGAL
    Posts
    65
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    3

    Default

    Quote Originally Posted by gustafson View Post
    Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

    Unfortunately I don't speak Fanuc
    Thanks Gustafson, can you explain wich tool. I am also under the impression that it (the half circle )may only be possible by using a round (full radius) tool.

    I have a Sandvik lf123h25-2525bm tool available with parting inserts, however the round inserts for it are to expensive for me to make it a try.
    Can anyone recommend a tool that takes cheapo round or other inserts? I was thinking about some MGEHL 2525.
    Regards

  14. #13
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,250
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    225

    Default

    Quote Originally Posted by gustafson View Post
    Using a full radius tool does not teach him what he wishes to know. Using a smaller radius tool enables him to create any radius groove [larger than the tool] that he wishes to.

    Unfortunately I don't speak Fanuc
    As suggested earlier, make a rough shape by calling G75 multiple times, shifted sideways suitably and modifying X value every time. This to be followed by a finish cut with radius compensation. Actually, a tedious method, but can make the part.

  15. Likes litlerob1 liked this post
  16. #14
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,568
    Post Thanks / Like
    Likes (Given)
    1206
    Likes (Received)
    2547

    Default

    Quote Originally Posted by sinha View Post
    As suggested earlier, make a rough shape by calling G75 multiple times, shifted sideways suitably and modifying X value every time. This to be followed by a finish cut with radius compensation. Actually, a tedious method, but can make the part.
    It is tedious. Were it me, I would just long hand 3 or 5 Rough passes from the OD, then a Finish pass. I wouldn't use G75 for such a small Groove.

    R

  17. #15
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,783
    Post Thanks / Like
    Likes (Given)
    390
    Likes (Received)
    6477

    Default

    With a cnc one just goes in and profiles it.
    A 1/8, 3/16, or 1/4 inch full nose tool works.
    You do not show the rad inside dia. but it looks awful close to what a "V" insert can cut in a flat axial rake.
    Anyways you want to have a vee bottom or other groover in your collection of toolholders.
    If making 5,000 or more I'd just buy a custom tool to plunge and done. None of that cnc dancing around lost time.

  18. #16
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,687
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1449

    Default

    Quote Originally Posted by CarbideBob View Post
    If making 5,000 or more I'd just buy a custom tool to plunge and done. None of that cnc dancing around lost time.
    Hello Bob,
    That's a frag over 6mm deep with a 14.16 diameter tool, equating to a bit more than 20mm contact between insert and workpiece. Good luck with that.

    Regards,

    Bill

  19. #17
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    7,783
    Post Thanks / Like
    Likes (Given)
    390
    Likes (Received)
    6477

    Default

    Lol;, that's not even a inch wide plunge cut.
    Bob

  20. #18
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,687
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1449

    Default

    Quote Originally Posted by CarbideBob View Post
    Lol;, that's not even a inch wide plunge cut.
    Bob
    Hands up all those that have taken an inch wide plunge cut in other than plastic, on your typical sized Turning Centre found in most machine shops, not built like a Brick Shit House (typical of a Kia SKT 200), and could still hear the radio over the chatter.

  21. Likes tay2daizzo8, ApexMachining liked this post
  22. #19
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,250
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    225

    Default

    I have no experience of machining with round inserts. Therefore, i have a question. Can it be used for usual turning operation with, say, 0.5 mm DOC and 0.2 mm/rev feedrate?
    If yes, at least for large diameter jobs which can withstand the associated radial thrust, then G71 type 2 or G73 can also be used for making the groove.

  23. #20
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,687
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1449

    Default

    Quote Originally Posted by sinha View Post
    I have no experience of machining with round inserts. Therefore, i have a question. Can it be used for usual turning operation with, say, 0.5 mm DOC and 0.2 mm/rev feedrate?
    If yes, at least for large diameter jobs which can withstand the associated radial thrust, then G71 type 2 or G73 can also be used for making the groove.
    Hello Sinha,
    Absolutely, but with a whole lot more Feed/Rev. 0.2mm/rev is conservative roughing feed rate with a 0.8 TNR and a much greater DOC.

    I took over 30 minutes out of a client's 60 min. cycle time on a large, deep face groove using a 12 diameter button tool, using 0.5 DOC and 3.0mm feed/rev to bi-directional face. Basically, its the same principle as HSM common to Machining Centres, implemented on a Turning Centre. I've also used the same technique in OD turning operations.

    The slow feed rate you suggested would result in bird nest swarf.

    It would be difficult to use with a Multi-repetitive cycle, as the indeed for the DOC can't be anything near like the feed/rev used in a Turning, or Facing operation (only one Feed Rate can be specified in these Roughing Cycles)

    Regards,

    Bill


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
  •