545,767 active members*
1,802 visitors online*
Register for free
Login
Page 1 of 3 123
Results 1 to 20 of 43
  1. #1
    Registered
    Join Date
    Oct 2004
    Posts
    198

    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.
    Attached Thumbnails Attached Thumbnails Chamfer Example.jpg  

  2. #2
    Moderator HuFlungDung's Avatar
    Join Date
    Mar 2003
    Posts
    4826
    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
    Gold Member
    Join Date
    Jul 2005
    Posts
    12177
    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
    Posts
    4826
    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
    Member
    Join Date
    Jul 2003
    Posts
    1220
    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
    Posts
    524
    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
    Gold Member
    Join Date
    Jul 2005
    Posts
    12177
    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
    Member
    Join Date
    Jul 2003
    Posts
    1220
    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
    Member
    Join Date
    Jul 2003
    Posts
    1220
    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
    Posts
    1498
    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
    Posts
    1498
    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
    Gold Member
    Join Date
    Jul 2005
    Posts
    12177
    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.

  13. #13
    when a drawing shows a 45 deg chmf it is in relation to the view rather than the surface of the material unless otherwise specified ,at which it should be interpolated or contoured along the corner to get an even chamfer all the way around
    to use a 4th axis or any other means to accomplish a 45 to all surfaces will have an end result of a multituted of different angles ,if it s for simple corner break it may be acceptable ,if it is meant to seat a mating part or screw , the seating will be improper

  14. #14
    Registered
    Join Date
    Mar 2005
    Posts
    1498
    070401-1202 EST USA

    Geof :

    Was your MACRO based on equations like the above? If so how slow was the machine? My guess is that doing it in HAAS is pretty bad vs generating the code externally.

    It is not clear yet what the purpose of this chamfer is.

    .

  15. #15
    Gold Member
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by gar View Post
    070401-1202 EST USA

    Geof :

    Was your MACRO based on equations like the above? If so how slow was the machine? My guess is that doing it in HAAS is pretty bad vs generating the code externally.

    It is not clear yet what the purpose of this chamfer is.

    .

    I can't tell you but I presume so. I simply told my guy to figure out a general macro for this type of chamfer. I wanted it general because our holes intersect the cylinder both on center and off center by different amounts.
    He did also do it via CAM but that resulted in an enormously long section of program which of course was not general. In both cases the time factor made it not worthwhile; it is more efficient to do hand deburring while the machine is running on the next batch of parts.

    In our case the purpose of the chamfer is to remove sharp edges. As dertsap points out if the purpose of the chamfer is for a screw head or something then it has to be concentric with the hole and the fact that the intersection width varies is irrelevant.

  16. #16
    Registered
    Join Date
    Oct 2004
    Posts
    198
    Thanks for the input guys, thanks Kiwi, I'll give it a try when I get a chance.
    Holy hell, it's a bit more complicated than I first thought, the chamfer isn't to suit mating parts, it's only for a better looking part.

  17. #17
    Registered
    Join Date
    Aug 2007
    Posts
    7
    umm just keep you're way lube full...

  18. #18
    Moderator tobyaxis's Avatar
    Join Date
    Jan 2006
    Posts
    4396
    Quote Originally Posted by Darc View Post
    Thanks for the input guys, thanks Kiwi, I'll give it a try when I get a chance.
    Holy hell, it's a bit more complicated than I first thought, the chamfer isn't to suit mating parts, it's only for a better looking part.
    Then it would be easier to use a 90 Degree Mill Drill, LOL. You could CCW Interpolate that too.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

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

    www.refractotech.com

  19. #19
    Registered
    Join Date
    Apr 2006
    Posts
    133
    KIWI
    I just ran a 4 inch dia. hole on a 44 inch dia. part as a test of the time to machine the chamfer. I ran the program using 360 points and it took 1 min and 6 secs at 12.566 ipm feed rate on our Haas simulator. Figuring some lost time for aproach and retract it doesn't seem to loose any time processing the code as it machines the circle.
    Here is a devil's advocate question. Can you write a routine that will repace the X axis move with a A axis move , the Y axis moves would be the same and leave Z axis at the original start point? This would be the same as the cylinder mapping that Haas uses.
    Thanks for the 2nd routine, I think I will be able to use it in the future.

  20. #20
    Member
    Join Date
    Jul 2003
    Posts
    1220
    JWK42
    There shouldn't be any lose of calculating time during machining as this has been done by your PC.

    Should be able to alter as required.
    I guess the numbers are the same, just the letters altered.
    What order should the axis letters be?
    Please post a couple of modified lines of code as you want them.

Page 1 of 3 123

Similar Threads

  1. Chamfer hole located on an angled
    By colby2000 in forum CNC Swiss Screw Machines
    Replies: 1
    Last Post: 04-17-2014, 08:34 PM
  2. Cross Hole Chamfer (G16? G12.1?)
    By Ovrclck350 in forum CNC Swiss Screw Machines
    Replies: 4
    Last Post: 02-14-2014, 04:32 PM
  3. tapped hole chamfer with iscar chamfer tools
    By dcutler35 in forum Mastercam
    Replies: 7
    Last Post: 12-07-2012, 02:30 PM
  4. CHAMFER FOR TAPPED HOLE
    By dcutler35 in forum Mastercam
    Replies: 11
    Last Post: 07-03-2012, 09:11 PM
  5. Depth Calculator - Chamfer a hole
    By jcnewbie in forum Mastercam
    Replies: 3
    Last Post: 10-23-2009, 11:55 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •