Page 1 of 2 12 LastLast
Results 1 to 20 of 24
Like Tree1Likes

Thread: Programming with tool nose radius.

  1. #1
    MBG
    MBG is offline Hot Rolled
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    672

    Default Programming with tool nose radius.

    Who here programs with tool nose radius? If I program with tool nose radius, my program is created
    with all my depths and everything deeper by half the tool nose radius. If I choose to program this way, I have to
    tell the machine the tool nose in the machine?

    By choosing to NOT program with the tool nose radius, basically, a point to point program, will I have any problems?

  2. #2
    chainfeed is offline Cast Iron
    Join Date
    Aug 2008
    Location
    ma
    Posts
    387

    Default

    unless your parts have no chamfers/angles/radii/etc. you'll need to figure for the nose radius.

  3. #3
    MBG
    MBG is offline Hot Rolled
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    672

    Default

    Now if I program for tool nose radius, do I have to enter a raidus in the machine under the tool nose comp?

  4. #4
    autocad monkey is offline Plastic
    Join Date
    May 2013
    Location
    Spring texas, (north Houston)
    Posts
    33

    Default

    Depends, are you using a program to generate the code or manually coding it at the machine?

  5. #5
    MBG
    MBG is offline Hot Rolled
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    672

    Default

    Quote Originally Posted by autocad monkey View Post
    Depends, are you using a program to generate the code or manually coding it at the machine?
    Using a CAD system, it just doesn't make any sense because .180" depth bore the machine will program to .188". How and why would a depth change for tool nose if I touched off the tool with the tool setter with the same cutting nose??

  6. #6
    pcasanova is offline Aluminum
    Join Date
    Mar 2008
    Location
    vacaville ca
    Posts
    140

    Default

    if you can post the code to the contour. I've had similar happen when I used the the wrong cutter comp on the sub-spindle.
    But the cam systems I've seen you can have it do the tnr for you and the coded will be changed from the print.
    Personally I would never do it that way. I perfer to have all code to the print and use the control to comp and do the math.
    EnderDRM likes this.

  7. #7
    Hertz is offline Stainless
    Join Date
    Apr 2009
    Location
    Ontario, Canada
    Posts
    1,081

    Default

    I define my TNR in my cad. It compensates for the chain I select to cut, whether it be mill or lathe. I let Mastercam decide the code. Programming center of the cutter on a mill is old school compensation. Didn't even know people still did that, lol.

  8. #8
    litlerob's Avatar
    litlerob is offline Hot Rolled
    Join Date
    Jun 2009
    Location
    PDX, OR
    Posts
    547

    Default

    What line of code is the G40 on? I have had similar issues depending on what line the comp. cancel is on. work around was duplicating the move once off the part,
    G1 X 2.5
    G1 X 2.5 G40
    Also are you using a canned cycle or long hand?

  9. #9
    alphonso is offline Stainless
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    1,579

    Default

    My only experience, 23+ years, with CADCAM is Edgecam and its predecessor Pathtrace. It has a facility called "Pathcomp" in which all the TNR comp is handled to whatever TNR you tell it to use. On the first lathes I programmed, I set the R value to zero for all tools on the machine. Never had a problem with unexpected cuts or "no cuts".

    On the POS Anilam control I do not use "Pathcomp" with the canned cycles. It wants to do a TNR comp(of unpredictable amounts) even if the R value is set to zero in the table. Set the R value to what tool I'm going to use and most of the time the result is acceptable. If I'm not using a canned cycle, "Pathcomp" handles comp correctly because the machine isn't using a G41/G42.

    Fanuc controls I program without 'Pathcomp" because the control works okay.

    Fagor controls I mostly use the conversational stuff.

  10. #10
    NodecoMachine is offline Aluminum
    Join Date
    Sep 2011
    Location
    NJ, USA, Lebanon
    Posts
    85

    Default

    On the Anilam 4100T control I run its very important to have the proper "L-Code" set in the offsets/tnr/wear window. The L-Codes tell the control how the tool is positioned in relation to the workpiece (Boring bar has a L-Code separate from a turntool). The result if the L-Code was wrong would be the diameter of the part would end up 2X the tnr big or small depending on your compensation(g41/42).

  11. #11
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,108

    Default

    Quote Originally Posted by MBG View Post
    Now if I program for tool nose radius, do I have to enter a raidus in the machine under the tool nose comp?
    That depends on if you're using cutter comp. or not. I guess it depends upon what control you have also.

    Some of the answers you're getting here appear to be overcomplicating things.

  12. #12
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    385

    Default

    Are you programming to the tip of the radius or to the center of the radius?

  13. #13
    MBG
    MBG is offline Hot Rolled
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    672

    Default

    Here is my sample code that is confusing me.

    G97 S1000
    G1 Z-2.6472 F.015
    G0 X3.648 Z-2.6382
    Z.06

    I am wanting to turn the diameter in Z to 2.6"... I don't see what the tool nose radius has to do with making the machine cut deeper. PLEASE EXPLAIN!!

    I understand why the tool has to go further in X to face the part but further in Z? I touch off on the lead edge as shown in the pictures.



    Image - TinyPic - Free Image Hosting, Photo Sharing & Video Hosting

  14. #14
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,108

    Default

    If you're touching off the leading edge of the tool, and you want the leading edge of the tool to be 2.6 deep, then you program it to Z-2.6.

    How did you end up with the Z-2.6472?

  15. #15
    MBG
    MBG is offline Hot Rolled
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    672

    Default

    Quote Originally Posted by Dave K View Post
    If you're touching off the leading edge of the tool, and you want the leading edge of the tool to be 2.6 deep, then you program it to Z-2.6.

    How did you end up with the Z-2.6472?

    Not having Cutter Compenstion Turned on. It programs to Z-2.6..

  16. #16
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,108

    Default

    Quote Originally Posted by MBG View Post
    Not having Cutter Compenstion Turned on. It programs to Z-2.6..
    When you don't have cutter compensation turned on, that's when it programs to Z-2.6? What exactly is programming it? Are you using cad/cam?

  17. #17
    angelw is offline Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,612

    Default

    Quote Originally Posted by MBG View Post
    Here is my sample code that is confusing me.

    G97 S1000
    G1 Z-2.6472 F.015
    G0 X3.648 Z-2.6382
    Z.06

    I am wanting to turn the diameter in Z to 2.6"... I don't see what the tool nose radius has to do with making the machine cut deeper. PLEASE EXPLAIN!!

    I understand why the tool has to go further in X to face the part but further in Z?
    If the above code is as output by the Post Processor of your CAM package, then its an issue with either the Post, the configuration of the tool being called from a tool library, the description of the tool if being specified manually, or the geometry that you've created. The program specifies Z-2.6472, so that's where the tool will go under control; its not going to end up at Z-2.6000. Post more of the code that precedes the G97 S1000 block.


    Regards,

    Bill

  18. #18
    Dave K is offline Diamond
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    6,108

    Default

    Lets say you're programming a 1" diameter turn, that goes 1.5" back, then goes to 2" diameter with a .015 radius on the corner. Tool in the machine has a .032 radius tip on it.

    Without cutter comp. the program should look like this:
    G00 X1.00 Z.1
    G01 Z-1.5
    G01 X1.916
    G03 X2. Z-1.542 R.042
    G1 blah blah blah

    Now with cutter comp:
    G00 X1.0 Z.1
    G1 G42 Z0
    G1 Z-1.5
    G1 X1.99
    G03 X2. Z-1.51 R.01
    G1 blah blah blah

    The only thing cutter comp. really effects is how you program your radius or chamfers on shoulders or corners. The O.D. and I.D. diameters and depths are programmed the same either way.
    Now, if you're programming on cad/cam, and you're getting numbers that are compensating for the radius of the tool you're using on your depths and diameters, that sounds like a setting that needs to be changed in how the cad/cam uses cutter comp. Perhaps you might be better off asking your question in the cad forum? I'm not real fluent on those systems, or maybe you have an odd control at the machine?

  19. #19
    Philabuster's Avatar
    Philabuster is offline Titanium
    Join Date
    Jul 2006
    Location
    Tempe, AZ
    Posts
    2,728

    Default

    Quote Originally Posted by MBG View Post
    I am wanting to turn the diameter in Z to 2.6"... I don't see what the tool nose radius has to do with making the machine cut deeper. PLEASE EXPLAIN!!
    Looks like Tool Nose Radius is described incorrectly in the tool file. You have a +.0472 when you should have a -.0472 number for example in Z value. The .047" value is the distance from the edge of the tool to the center of the radius for a #3 radius insert. You do not state what radius you are using, so this is just an assumption.

  20. #20
    tq4517 is offline Plastic
    Join Date
    Jun 2013
    Location
    California,USA
    Posts
    14

    Default

    I would be very interested in knowing what machine your programing, control and with what software. I either wright the program by hand exactly like Dave K said using the G42 and put the tool nose radius and tool type in the offset page. Or when I use Virtual Gibbs I tell Gibbs that information and get something like the following. I have had machines that if I put it in would automatically comp for the Rad if put in the offset page so since I have already compensated with the software and no need for it I don't put that information in the offset page the software has already done the compensation.
    G0X.2078
    G1X.1875F.004
    G2X.1835Z.117I-.002K-.0035
    G1X.1575
    Z.2118

Page 1 of 2 12 LastLast

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
  •