Do I need tool with 0 nose radius to do that?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 22
  1. #1
    Join Date
    Apr 2021
    Country
    SWEDEN
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    1

    Default Do I need tool with 0 nose radius to do that?

    Hi

    I have a job the required doing an OD groove, the above two edges of the groove require to have R0.005 on both edges as attached. Do I need a 0 nose radius insert to do that?


    323323232.png

  2. #2
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,492
    Post Thanks / Like
    Likes (Given)
    13835
    Likes (Received)
    5469

    Default

    An OD groove can be programmed with any nose radius tool that will fit into your groove...

  3. #3
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    8

    Default

    I would cut groove first before finish pass on OD then on finish pass create geometry to have the rads included on od pass. Still learning lathe programming but that would be how I would approach it.

  4. Likes Bobw liked this post
  5. #4
    Join Date
    Apr 2021
    Country
    SWEDEN
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    1

    Default

    Quote Originally Posted by TeachMePlease View Post
    An OD groove can be programmed with any nose radius tool that will fit into your groove...
    Thank your for your reply

    In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?

  6. #5
    Join Date
    Aug 2008
    Location
    Paso Robles, CA
    Posts
    189
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    35

    Default

    By programming a toolpath that takes into account the nose radius of your tool. You might even be able to do it with your grooving tool.

  7. #6
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    6,337
    Post Thanks / Like
    Likes (Given)
    2525
    Likes (Received)
    3137

    Default

    In cam, no. Free hand i don't know

  8. #7
    Join Date
    Apr 2021
    Country
    SWEDEN
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    14
    Likes (Received)
    1

    Default

    Quote Originally Posted by David Ferguson View Post
    By programming a toolpath that takes into account the nose radius of your tool. You might even be able to do it with your grooving tool.
    OK using Cam software. For example I will use 0.03 nose radius.. Can that do the 0.005R?

  9. #8
    Join Date
    Aug 2008
    Location
    Paso Robles, CA
    Posts
    189
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    35

    Default

    sure, you draw your profile with the 0.005 R included, and tell it to take a finish pass with a tool defined to have a 0.03 nose radius. Now the tool needs to fit in the slot (which was why I suggested using the grooving tool if it can cut on the sides), Otherwise you might need to use both left and right hand tools for the appropriate corner.

  10. #9
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,492
    Post Thanks / Like
    Likes (Given)
    13835
    Likes (Received)
    5469

    Default

    Quote Originally Posted by M Code View Post
    Thank your for your reply

    In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?
    Trust me, I'm not the one who didn't understand the question.


    Edit: That was rude.

    Any OD radius can be created by any OD radius tool by programming a radius that incorporates the radius of your turning tool as well as the radius you wish to create on the part.

  11. Likes wheelieking71, AARONT, Winterfalke liked this post
  12. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by M Code View Post
    Thank your for your reply

    In fact I am not talking about the R value inside the groove I am referring to the above two edges of the groove need to be 0.005R just to break the sharp edges. How that can be done?
    Hello M Code,
    They are external radii, therefore, as TeachMe suggests, they can be cut with a any tool nose radius of a tool that will fit inside the groove. It's very common to rough the groove and then finish the profile of the groove, including external corner radii with each side of the grooving tool, taking into account the corner radius of the grooving insert.

    When actually executing the finish pass you have to be mindful of the feed rate being used in the area of the corner radii. It needs to be less than the corner radius, otherwise it could be missed in one revolution of the part. The feed rate has to be substantially less than the radius feature being cut so as to cut that feature accurately.

    Following is example code to cut a 0.25" wide by 0.25" deep groove 1.0" from the end of a 2.0" diameter shaft, using a grooving tool with 0.03" corner radii. The groove has 0.005 external corner radii.

    When using each side of a grooving tool to finish a groove and particularly if the sides of the groove have tolerances, its good practice to use a tool offset for each side of the insert. Doing so allows for the position of each side of the groove to be controlled.


    G00 X2.0400 Z0.5000 T0101 (TOOL OFFSET FOR FRONT SIDE OF INSERT - TOOL STYLE 3)
    G01 X2.0400 Z-1.2300 F0.50
    G01 X1.5100 F0.005
    G04 X0.25 (DWELL 1/4 SEC)
    G00 X2.0400
    G00 Z-1.2850
    G01 X2.0000
    G02 X1.9300 Z-1.2500 I-0.0350 K0.0000 F0.002
    G01 X1.5000 F0.005
    G01 Z-1.2400
    G00 X2.0400
    G00 Z-0.9650 T0121 (TOOL OFFSET FOR BACK SIDE OF INSERT - TOOL STYLE 4)
    G01 X2.0000 F0.010
    G03 X1.9300 Z-1.0000 I-0.0350 K0.0000 F0.002
    G01 X1.5000 F0.005
    G01 Z-1.0100
    G00 X2.0400


    Regards,

    Bill

  13. #11
    Join Date
    Aug 2005
    Location
    CT
    Posts
    8,445
    Post Thanks / Like
    Likes (Given)
    464
    Likes (Received)
    2266

    Default

    OK, so my way of doing this ( multiple times a day even ) is to pick up your grooving tool with 2 separate offsets.
    Offset #1 is Direction 3, which will be doing the back side of the groove.
    Offset #2 is Direction 4, and will be working on the front wall of the groove.

    As far as the Radius of the grooving tool, any size R will do the external radius on the edge of the groove, but in order to program it accurately and without overcut
    your limiting factor here is the inside radii of the groove for the tool Rad.

  14. #12
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,284
    Post Thanks / Like
    Likes (Given)
    917
    Likes (Received)
    515

    Default

    You would only need a small radius corner tool (.005” or smaller) if that .005” dimension was an INTERNAL corner. Since it is an EXTERNAL corner you can do it with any radius tool….think about facing and chamfering/radiusing the front of a part with a turning tool….any nose radius can produce any chamfer/radius on the front edge of the part. Your CAM software really should allow you to enter in the corner rad of your grooving tool as well as apply the .005” edge break with no problem. Good luck!

  15. #13
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,335
    Post Thanks / Like
    Likes (Given)
    9824
    Likes (Received)
    9384

    Default

    The controlling factor here is how the code is generated.
    Are you programming with CAM software? Or are you manually writing code?

  16. #14
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1777

    Default

    Quote Originally Posted by wheelieking71 View Post
    The controlling factor here is how the code is generated.
    Are you programming with CAM software? Or are you manually writing code?
    Why so? An external corner radius is an external corner radius and a tool nose radius is a tool nose radius, with neither of them changing irrespective of the method used to create the program.
    Last edited by angelw; 08-04-2021 at 06:15 AM.

  17. #15
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,949
    Post Thanks / Like

    Default

    My Cam program puts out tool path like this. Red dot is the reference point of tool.

    groove-toolpath.jpg

  18. #16
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,762
    Post Thanks / Like
    Likes (Given)
    631
    Likes (Received)
    8670

    Default

    On caveat when programing this small of an entrance rad.
    If the OD was not cut by the same tool and that OD is say .002 oversize or undersized you end with rather poopy blend be it a notch in the OD lots or rad missing.
    A workaround is to only program 80 to 87 degrees of rad swing,
    A form tool made to cut this as a second op will have at least 2 and as much as 8 degrees outwards on this rad for this reason dependent on expected OD tolerance.
    Life is so much easier if the same tool did the OD work.

    Other as Bill has said is feedrate. You have to go way slow around this corner or it will not be there. This is not a machine response thing but a sort of threading action of the cutting tool.
    If feeding .004 per rev using a 0 rad tool... that .005 rad is not there. Or is sort of there. Rotate the part, check it again and many confusing things.

    These small rads are a pain. Note also that this the remove burr idea so programming in the plunge cut may not do what is asked for.
    This dance best done after the groove to size.

    There is no zero rad cutting tool once it sees a cut.
    Bob

  19. #17
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    7,335
    Post Thanks / Like
    Likes (Given)
    9824
    Likes (Received)
    9384

    Default

    Quote Originally Posted by angelw View Post
    Why so? An external corner radius is an external corner radius and a tool nose radius is a tool nose radius, with neither of them changing irrespective of the method used to create the program.
    I guess my wording could have been better.
    Maybe I should have said: "the controlling factor of the answer to your question" treating the question more of a how-to, than a yes/no.
    My bad for being vague (very, LOL).
    The simple answer to his question we all know is "NO".

  20. #18
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    237
    Post Thanks / Like
    Likes (Given)
    593
    Likes (Received)
    68

    Default

    There is no tool with zero nose radius.
    When you program the finish move you need to add the .005 radius value plus the radius of the groove tool. Lets say the tool has a .007 nose radius so your R value will be R0.012.

  21. #19
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,762
    Post Thanks / Like
    Likes (Given)
    631
    Likes (Received)
    8670

    Default

    Quote Originally Posted by Fancuku View Post
    There is no tool with zero nose radius.
    When you program the finish move you need to add the .005 radius value plus the radius of the groove tool. Lets say the tool has a .007 nose radius so your R value will be R0.012.

    One may need to tweak be it called out .007 or .03125 rad on the cutting tool when making a .005 resultant.
    I make cutting tools and insets. Lots of true to form and location things happening here.
    It works in the CAD and on paper. Not so much real world let alone checking that .005 rad and lead/end smear or tangent.
    I know it is corner break but if needed to hold or will be checked........
    Option two is a tool ground to do it in a single plunge and no fancy G-code. In/out done. But at .005 corner I would not quote this.
    .006 sort of the bottom in carbide and it will wear to a .007. In PCD one can go smaller.
    Bob

  22. #20
    Join Date
    Jun 2021
    Country
    ROMANIA
    Posts
    13
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    0

    Default

    Can you really measure that 0.005 after you machine it? Probably someone is making fun of you.


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
  •