584,860 active members*
5,037 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 27
  1. #1
    Join Date
    Oct 2006
    Posts
    8

    Tooltip radius compensation help!

    I need to program a cutting path from no. 1 to no.3 as shown in the jpeg attachment, and i understand that G42 should be used to compensate the tool nose radius, but which tool tip number should i use? how should i program it so that i will get an accurate finished product?
    Attached Thumbnails Attached Thumbnails Tooltip.jpg  

  2. #2
    Join Date
    Jul 2003
    Posts
    1220
    Normally your cam program would calculate this for you. Just enter the diameter of your cutter and the type. eg Ball nose.
    Do you need many of these points or just the four illustrated.
    If you require just the four points you could draw the profile with circles tangent to the profile lines. Then calculate the tool path as per the attached drawing.
    Attached Thumbnails Attached Thumbnails Tool Path1.jpg  

  3. #3
    Join Date
    Jul 2005
    Posts
    12177
    Do the pictures help? I captured them out of a manual.

    I think for your application 8 will be the correct tip number to use.
    Attached Thumbnails Attached Thumbnails ToolNose1.jpg   ToolNose2.jpg  
    An open mind is a virtue...so long as all the common sense has not leaked out.

  4. #4
    Join Date
    Oct 2006
    Posts
    8
    Thanks for the prompt reply, well there shouldnt be any problems if the codes were generated using cam, however, is there any way to hand-code it correctly?

    Geof, the pictures u attached does help, however, the cutting path involves 3 different tool tips and if i am not wrong, G42 only allows using compensation for one tool tip for one cutting cycle..

  5. #5
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by Predator View Post
    ....Geof, the pictures u attached does help, however, the cutting path involves 3 different tool tips and if i am not wrong, G42 only allows using compensation for one tool tip for one cutting cycle..
    How do you get 3 different tool tips? You are not going far enough around the nose radius for the side of the tool to be cutting. You are using the same tool for the entire path in your picture and the toolpath is symmetric, tip 8 works for a symmetric path.

    If your angle was steeper you would need to do it with two tools: The front and OD would be done with a tool like that shown for tip 9 and would use tip 9 and the back angle would be done with a tool like tip 4 and use tip 4.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  6. #6
    Join Date
    Oct 2006
    Posts
    8
    i am actually using a tool holder similar to the tool tip number 3.. not the one in the pic i attached earlier on... the angle of the holder is steeper than the slope i need to cut...

    However, my main concern is the tool tip will be cutting the material using one end of the insert on the first slope, however when it reaches the 2nd slope, it will use the other end of the insert to cut the material right?

    Pls correct me if my theory is wrong...
    was wondering if the 2nd slope will be affected as the cutter is using different sides to cut the material as it moves from the 1st slope to the 2nd..

    hope u understand what i mean...
    Attached Thumbnails Attached Thumbnails ToolPath.jpg  

  7. #7
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by Predator View Post
    ....However, my main concern is the tool tip will be cutting the material using one end of the insert on the first slope, however when it reaches the 2nd slope, it will use the other end of the insert to cut the material right?....
    My understanding of the tip 8 tool compensation operation is that the controller corrects for the nose radius on both slopes. It takes the tool past the programmed path by the amount necessary to compensate on the back slope.

    If you have a machine that has a good graphics display you can write a little program which follows the tool path first without compensation and then repeats with compensation and you can see from the trace what the compensation is doing.

    However, if your tool is actually a different shape you will have to select the tip number for that shape and the path that it follows.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  8. #8
    Join Date
    Jul 2003
    Posts
    1220
    Predator:
    My pictures are for a milling path.
    On further examination I see you need this for a Lathe.
    Sorry to put you wrong.

  9. #9
    Join Date
    Oct 2006
    Posts
    8
    kiwi, its ok, i wasnt clear in the first post, anyway i will try and figure that using a simulator...

  10. #10
    Join Date
    Nov 2004
    Posts
    110
    Use two tools.

    use on like the #3.

    and then use one like the #4.


    Your TRC values would be 3 and 4

  11. #11
    Join Date
    Oct 2006
    Posts
    8
    using 2 tools will have no problem with the compensation, however is it possible to use one tool all the way? the tolerance for the workpiece is only 20 microns and it will be much more difficult to control if i were to use 2 tools for finishing...

  12. #12
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by Predator View Post
    using 2 tools will have no problem with the compensation, however is it possible to use one tool all the way?...
    You can use one tool with a profile the same as you had in your first sketch provided the tip angle on the tool is small enough that the sides of the tool do not touch the angle on either side of the part. This way the tool is only working on the nose radius.

    This program does part of a sphere using Tip 8 and a tool like your sketch. It does not go far enough down the sphere for the sides of the tool to touch.


    %
    N1000 T101
    N1001 G00 X1.5 Z1.
    N1002 M03 S1800
    N1003 X0.6 Z0.15 M08
    N1003 G42 G01 X0.3693 Z0.1 F0.01
    N1005 G03 R0.5 X0.5057 Z-0.8009
    N1006 G40 G00 X1.15
    N1007 Z0.18
    N1003 G42 G00 X0.3593 Z0.1
    N1005 G03 R0.5 X0.4957 Z-0.8009 F0.005
    N1006 G40 G00 X1.15
    N1023 G00 X2. Z5.
    N1024 M99
    N1025 (----)
    %
    An open mind is a virtue...so long as all the common sense has not leaked out.

  13. #13
    Join Date
    Jun 2007
    Posts
    87
    if you're having a hard time with toolnose radius compensation (G41/G42) then just compensate the tnr in your program, you don't have to use the g41/g42 code.

  14. #14
    Join Date
    Oct 2006
    Posts
    8
    if i am not wrong the slopes will not come out correctly if i were to compensate the tnr in my program right? anybody knows?

  15. #15
    Join Date
    Jun 2007
    Posts
    87
    Quote Originally Posted by Predator View Post
    if i am not wrong the slopes will not come out correctly if i were to compensate the tnr in my program right? anybody knows?
    sure it will, it the same thing the machine is doing when you use g41/g42, the only thing is you computed and compensated it to the program yourself. actually rarely use g41/g42 in my programs as its really bit of a problem when turning features which uses both sides of the tip.

  16. #16
    Join Date
    Mar 2003
    Posts
    2932
    Predator,

    Assuming you're using a Fanuc or Haas or similar, the Tip # simply tells the control where you've set the tool (virtual tip). For an OD tool, use #3. It will compensate for the radius correctly as long as you keep the tool to the right side (with G42). It doesn't, however, look at the trailing edge of the insert, so you need to be sure that the insert you're using clears the backside.

    Dave

  17. #17
    Join Date
    Feb 2006
    Posts
    1792
    You cannot use two different tools because there will always be a sharp line where the two toolpaths meet. So, if the side of a neutral tool is found to interfare with the defined profile, use a tool with a round insert. And do not worry about which side of the nose cuts the material. The control automatically makes this adjustment. But the tool tip number has to be correct, which is 8 for the orientation in the first sketch.

  18. #18
    Join Date
    Mar 2003
    Posts
    2932
    The "tip type" simply tells the control where you set the "virtual tip" when you touch off your tool.

    If your tool holder is similar to #3 in Geof's jpg, then you probably set the tool on the face of the part and the OD. This establishes a tip type #3. That's what you should use in the offset table T register.

    If you were using a 1" tool holder that looked like #8, then you might touch the face of the HOLDER off the face of the part and adjust the Z offset -0.500. Then you would use T #8.

    In either case you only need 1 offset to cut your profile with G42.

  19. #19
    Join Date
    Jan 2005
    Posts
    304
    Tip #8 is what you need for comp. To do it yourself longhand you need to comp at each corner. The amount you comp depends on your radius and the angle you are going too. See the attachment for examples of how to use those values.
    Attached Thumbnails Attached Thumbnails Radius-Comp.jpg  

  20. #20
    Join Date
    Feb 2006
    Posts
    1792
    Quote Originally Posted by cogsman1 View Post
    Tip #8 is what you need for comp. To do it yourself longhand you need to comp at each corner. The amount you comp depends on your radius and the angle you are going too. See the attachment for examples of how to use those values.
    The figure does not appear to be correct. The start/end X/Z will also depend on the inclination of the taper.

Page 1 of 2 12

Similar Threads

  1. Tool Radius Compensation
    By davidmb in forum Uncategorised CAM Discussion
    Replies: 6
    Last Post: 10-03-2012, 10:31 AM
  2. Fanuc 5 axis radius compensation
    By d.a.v.e in forum Fanuc
    Replies: 1
    Last Post: 10-06-2008, 08:52 AM
  3. Help needed DynaPath 20 Tool-radius-compensation
    By dogstar in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 0
    Last Post: 02-14-2007, 01:42 AM
  4. Radius compensation in Mach3
    By kayakman in forum Mach Mill
    Replies: 20
    Last Post: 12-06-2006, 05:43 PM
  5. Radius compensation in Mach2?
    By MrBean in forum Uncategorised CAM Discussion
    Replies: 3
    Last Post: 03-19-2005, 02:49 PM

Posting Permissions

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