3dprintforums logo

CNCzone Network:  RFQwork :: 3Dprintforums :: Welderzone :: Google+ :: Our Facebook :: Twitter :: SiteMap



Page 1 of 4 1234 LastLast
Results 1 to 12 of 41

Thread: How to correctly chamfer a hole?

  1. #1
    Registered
    Join Date
    Sep 2004
    Location
    Australia
    Posts
    196
    Downloads
    0
    Uploads
    0
    Rep Power
    10

    Talking How to correctly chamfer a hole?

    I'm attempting to chamfer a hole in a cylindrical shaft, obviously very easy to do, that only reason I'm having a problem is that I'm trying to chamfer the correct distance all the way around the hole, rather than using a 90 tool and plunging straight down.
    You can see from the pic what I mean, the smaller hole is what you normally achieve (the chamfer changes size on the way around the hole) but I'm trying to achieve much the same as the larger hole.

    I'm trying to achieve this without cad/cam, is there a way to calculate this using a spreadsheet?
    Thanks.

    Similar Threads:
    Attached Thumbnails Attached Thumbnails -chamfer-example-jpg  


  2. #2
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0
    Rep Power
    16
    Why not make a real challenge out of it, and forbid using a calculator?

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Registered
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12115
    Downloads
    0
    Uploads
    0
    Rep Power
    21
    I suppose it is cheating Hu's limitation because you are using the machine as the calculator but you can write a macro. Which basically is not too much different to using CAM because you are approximating a compound curve with zillions of straight moves.

    We make thousands of parts a year that need chamfers at each end on holes intersecting cylinders both on and off center so I did get one of my guys to write a macro. It worked but the problem was it took as long or longer to generate the chamfer than it did to bore a 7/8" hole through 2-1/4" stock in the first place.

    So we stayed with the old fashioned way, a handheld deburring tool.



  4. #4
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0
    Rep Power
    16
    I was just kind of kidding around, hoping maybe somebody like Geof would come in and give a pat solution

    The more I think seriously about such a problem, the less chance I see of a simple formula working. The curve around the edge of the hole is a spline. And, unless the diameter of the through hole is always exactly the same ratio to the cylinder's diameter, each spline is going to be unique in shape, and not simply a scaled up version of one spline.

    Also, given that the programmer may have differing requirements from time to time, on how many pieces the spline is interpolated into, this would also cause a major perturbation of the spreadsheet layout.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  5. #5
    Registered
    Join Date
    Jul 2003
    Location
    New Zealand
    Posts
    1151
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    Here is a simple program that will produce the GCode for the edge profile of a hole in a curved face.
    Using G41, not sure how even the chamfer width will be.

    Attached Files Attached Files


  6. #6
    Gold Member
    Join Date
    Dec 2004
    Location
    Newtown, CT, USA
    Age
    70
    Posts
    522
    Downloads
    0
    Uploads
    0
    Rep Power
    10
    The problem is not clearly stated. Unless you have a 4th axis, the angle of the chamfer with respect to the surface will change. That is probably not what you want.

    Ken

    Kenneth Lerman
    55 Main Street
    Newtown, CT 06470


  7. #7
    Registered
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12115
    Downloads
    0
    Uploads
    0
    Rep Power
    21
    Quote Originally Posted by lerman View Post
    The problem is not clearly stated. Unless you have a 4th axis, the angle of the chamfer with respect to the surface will change. That is probably not what you want.

    Ken
    This is why our macro did it so slowly. We had it set up to chamfer across the intersecting surfaces on a plane bisecting the intersection angle. This seemed the only way to get a worthwhile chamfer which was as non-sharp as possible.



  8. #8
    Registered
    Join Date
    Jul 2003
    Location
    New Zealand
    Posts
    1151
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    This is not as simple as it first appears.
    Would using a ball nose cutter along the hole profile with no compensation give a satisfactory chamfer?



  9. #9
    Registered
    Join Date
    Jul 2003
    Location
    New Zealand
    Posts
    1151
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    Modified the Hole Chamfer program.
    This now cuts the chamfer with a constant face width using a pointed cutter.
    The angle of the cut is half the cutter angle from the axis of the hole.
    Hope this is of some use.

    Attached Files Attached Files


  10. #10
    Registered
    Join Date
    Mar 2005
    Location
    USA
    Posts
    1498
    Downloads
    0
    Uploads
    0
    Rep Power
    11
    070401-1001 EST USA

    Kiwi:

    I do not open .exe files and therefore I have no idea what you proposed.


    Darc:

    You need a 4 axis machine or use surfacing to obtain a uniformly wide chamfer as has been mentioned above.

    If the constant width and angle to the cylinderical surface is not required, then the following equations will define the locus of the intersection of two cylinderical surfaces where their axises are intersecting and perpendicular.

    The CNC machine x-axis is coincident with the axis of the cylinder in which the hole is bored. The CNC y-axis is perpendicular to the axis of the bored hole. The CNC z-axis is coincident with the bored hole axis.

    "a" is the variable angle from the x-axis and I am making "a" the independent variable as I would assume you would probably program for small incremental changes in "a".

    "R1" is the radius of the tube or rod coincident with the x-axis. Certain choices of R1 and R2 can produce a non-continuous physical edge. Obviously a hole larger than the rod.

    "R2" is the radius of the hole.

    x = R1 * cos a
    y = R1 * sin a

    y squared + z squared = R2 squared
    z = sq-root ( R2 squared - ( R1 * sin a ) squared )

    If processed as a MACRO this may slow the machine.

    .



  11. #11
    Registered
    Join Date
    Mar 2005
    Location
    USA
    Posts
    1498
    Downloads
    0
    Uploads
    0
    Rep Power
    11
    070401-1035 EST USA

    Note: if the hole is in a tube you may want to use the ID radius for "R2" to provide uniform mating of another tube into the hole.

    I did not previously indicate but I would assume use of cutter comp.

    .



  12. #12
    Registered
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12115
    Downloads
    0
    Uploads
    0
    Rep Power
    21
    Quote Originally Posted by gar View Post
    x = R1 * cos a
    y = R1 * sin a

    y squared + z squared = R2 squared
    z = sq-root ( R2 squared - ( R1 * sin a ) squared )

    If processed as a MACRO this may slow the machine.

    .
    No kidding see Post #3.



Page 1 of 4 1234 LastLast

Tags for this Thread

Posting Permissions



About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed