584,800 active members*
4,822 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 39
  1. #1
    Join Date
    Jan 2008
    Posts
    25

    Type II G71 Stock Removal on Fanuc 0i-TB

    I am trying to turn 270 degrees of a sphere on the end of 1.125" bar stock using Type II G71 and it isn't working. I'm getting an overcutting alarm 41 for the tool nose radius compensation. Here is the program below. Any help is greatly appreciated!!! (Tool nose is .0312 with imaginary tool nose 3)

    G0T0404(TURNING TOOL)
    G96S650M03
    G0X1.145Z0.
    G1X-0.05F.004M08
    G0X1.125 Z0.05
    G71U.06R.02
    G71P101Q201U.01W0F.006
    N101G0G42X0.Z.05
    G1Z0.F.003
    G03 X0.7071 Z-0.8536 R0.5
    G01 X1.125
    N201G0G40Z0.05
    G70P101Q201
    G80M09

  2. #2
    Join Date
    Mar 2003
    Posts
    2932
    I would try something like this:

    G0 T0404(TURNING TOOL)
    G96 S650 M03
    G0 X1.145 Z0.
    G1X-0.05 F.004 M08
    G0 X1.125 Z0.05
    G71 U.06 R.02
    G71 P101 Q201 U.01 W0F.006
    N101 G0 G42 X0. Z.05
    G1 Z0. F.003
    G03 X0.8012 Z-0.7992 R0.5
    G02 X0.4279 Z-0.8536 R0.034
    N201 G01 X1.125
    G70P101Q201
    G0 G40 X6.0 Z6.0
    G80M09

  3. #3
    Join Date
    Jan 2008
    Posts
    25
    thanks a bunch dcoupar, but do you mean to have the G02 line read this?:

    G02 X0.8558 Z-0.8536 R0.034

  4. #4
    Join Date
    Mar 2003
    Posts
    2932
    Yes. That is to keep the TNR from causing interference in the corner.

  5. #5
    Join Date
    Jan 2008
    Posts
    25

    Attn: Dcoupar

    The only way I could get it to work was by having the N201 line have G40 in it like I originally had. Why would the canned cycle not work without the line there?

    I had to N201G0G40 back to the start point. I noticed you didn't return the tool back to the start point in your canned cycle yet the Fanuc book tells you to do this.

    Thanks a lot!

  6. #6
    Join Date
    Jan 2008
    Posts
    25
    Are there parameter settings to adjust with this case?

  7. #7
    Join Date
    Mar 2003
    Posts
    2932
    lowehardware,

    None of my Fanuc manuals say to return the tool to the start point. What manual are you looking at? Also, please post the program that you finally got to work.

  8. #8
    Join Date
    Sep 2007
    Posts
    116
    Well, since this thread was started twice, I'll copy my response from the other one.

    Without going deeper into the code and geometric accuracy, I think your Q block is incorrectly placed.

    G00 T404 (TURNING TOOL)
    G96 S650 M03
    G00 X1.145Z0.
    G01 X-0.05 F.004 M08
    G00 X1.125 Z0.05
    G71 U.06 R.02
    G71 P101 Q201 U.01 W0 F.006
    N101 G00 G42 X0. Z.05
    G01 Z0. F.003
    G03 X0.7071 Z-0.8536 R0.5
    N201 G01 G40 X1.125 <---- N201 moved to here.
    G00 Z0.05
    G70 P101 Q201
    G80 M09

    Actually sort of surprized that you're not getting a "Non Monotonous" error.
    In TypeII roughing your X may vary in the + or - direction, but your Z must still be monotonous either + or - direction. That N201 sent it back to Z.05 withing the cycle.
    Now, depending on the control itself, you may still get an overcut at the back. Note that your G03 ends at Z-.8536, and then you move only up in X.
    The way I've changed your code would probably overcut on the Haas, because in this block:
    G01 G40 X1.125 would move the tool in the Z direction by +.0312 as well.
    I'm pretty sure Fanuc does the same thing, or perhaps worse by moving by 2X tool R in the +Z direction.
    So, the way I'd do this cycle is to make a clearance move at the back of the radius, perhaps a little more than your tool R.

    G00 T404 (TURNING TOOL)
    G96 S650 M03
    G00 X1.145Z0.
    G01 X-0.05 F.004 M08
    G00 G42 X1.125 Z0.05 <--- Note the comp-on BEFORE the cycle
    G71 U.06 R.02
    G71 P101 Q201 U.01 W0 F.006
    N101 G00 X0. Z.05
    G01 Z0. F.003
    G03 X0.7071 Z-0.8536 R0.5
    G01 Z-.8856
    N201 G01 X1.125
    G70 P101 Q201
    G00 G40 X1.125 Z.05 <--- Ramp-off move here.
    G80 M09

    Please note that the code may not be all kosher. I never use G70 due to all the minor radiuses and edgebreaks during the finish pass, but with G71 or G72 I always comp-on prior to, and comp-off after the cycle. Better control over exact tool position at each step.

    And to re-iterate, sending the tool back to the start point is not only not needed, but should not even be possible due to the non monotonous Z motion.

  9. #9
    Join Date
    Jan 2008
    Posts
    25
    Dcoupar, you're right. My manual doesn't tell me to return to the start point. I'm going to modify things a bit and see where I go from here. I can post a similar program I used to make a part which isn't as simple as the example I used for this thread.

    I always end up shifting arcs around so I don't overcut. Then I don't use a G70 but run a new toolpath for the finish cut.

    Thanks also to SeymourDunmore. When I need to make the part again I'll mess around with your method.

  10. #10
    Join Date
    Jan 2005
    Posts
    304
    Your code was not too bad to start with but you are turning on comp with a move in the wrong direction. Try this.


    G0T0404(TURNING TOOL)
    G96S650M03
    G0X1.145Z0.
    G1X-0.05F.004M08
    G0X1.125 Z0.1 (*********)
    G71U.06R.02
    G71P101Q201U.01W0F.006
    N101G0X0 (*********)
    Z.05 (*******)
    G01G42Z0F.003 (********)
    G03 X0.7071 Z-0.8536 R0.5
    G01 X1.125
    N201G0G40Z0.05
    G70P101Q201
    G80M09

  11. #11
    Join Date
    Jan 2008
    Posts
    25
    is that even Type II? in the N101 line you have to specify Z0.1 (where the tool starts) Correct?

  12. #12
    Join Date
    Sep 2007
    Posts
    116
    Actually it doesn't matter where you turn on that comp. IN fact I'd suppose that cogsman's method won't even work in this instance, as the toolR is .0312 and the move from Z.05 to Z0 is less than the .062 required, and would likely cause overcut on Fanuc OR "Tool too big" error on Haas.

    lowehardware
    The next time you get this or similar part where you're forming a sphere, see if you can re-define your tool to be Dir8 rather than Dir3.
    The really cool thing about it is that it truly uses the tool as it was a ball forming a ball, and you can dial in OD and sphericity variations easily.
    Also, your comp-on and off moves become easier to manage, as you can plunge-in and retract in a straight move in front and back of the ball.
    You can use the same tool as right now, all you have to do is add -.0312 to your Z offset and change the tool definition to 8.
    I do turn a decent amount of balls, and this method gives me straight plunges for roughing and finishing, AND I can dial in the part to be spherical within .0002.

  13. #13
    Join Date
    Jan 2005
    Posts
    304

    Will work on BOTH types

    I have used this format on both types and it works perfectly. You do NOT have to start twice the radius away that is a very old myth. The moves I have from the rapid (Z.1) before the N101 followed by the (Z.05) after entering the cann cycle will allow the machine to see which direction you are coming from and will work. I used to cut ball valves +/-.0003 and learned this method works no matter what machine(Lathe) I was using. Mori, Mazak, Nakamura, Tsugami, Citizen, Hitachi, and more. Some of these use different codes for their rough cycles but once in the cycle, this format is flawless. Some don't need the extra moves but all accept it.

  14. #14
    Join Date
    Sep 2007
    Posts
    116
    Agreed on the comp-on move.
    For some reason I was stuck on that you've ramped in the N101 block at Z.05 as Lowe's original code. That would in fact would have put the tool to Z-.012 after the N101 block.

    Quote from original post:
    """
    G0 X1.125 Z0.05
    G71 U.06 R.02
    G71 P101 Q201 U.01 W0F.006
    N101 G0 G42 X0. Z.05
    """

    Nonetheless, you've still got a return move inthe N102 block, which is not allowed even in Type II roughing. Your Z has changed fromZ-.8536 to Z.05, thereby changing direction from negative to positive.
    Not happening on Fanuc Oi-Tc or on Haas.

  15. #15
    Join Date
    Jan 2005
    Posts
    304

    check all programs

    I spent some time checking as many of my proven programs as I could for the different machines. The only difference I found was on a couple I had to cancel comp BEFORE the N102 ending line, but everyone always ends with the retract to the starting point off the face. I remember having an issue if I tried to retract to a position that was NOT the exact same as the starting position. This would be the position BEFORE the "G71" line.

  16. #16
    Join Date
    Sep 2007
    Posts
    116
    Interesting.
    Unfortunately I cannot copy/paste from teh Fanuc Oi-TC manual, so I'll just quote a segment from Page 145, which describes TypeII roughing:

    """
    Note that, however, the profile must have monotone decrease or increase along the Z axis.
    """

    This is word for word.

    I know for a fact that the Haas would complain and not run with the return, but I'll check it out on the Mori sometime this weekend.
    I do know that I never did send the tool back, as the cycle itself does that automatically in every case. In fact I don't even program a clearance move after the cycle and before a toolchange, knowing that the tool will be in the clear no matter what.

  17. #17
    Join Date
    Sep 2007
    Posts
    116
    Ok, with great dismay I must stand corrected!!!
    The Fanuc - despite the manual's statement - accepts the code with the return in the Q-block. It will do goofy things, but does accept them.
    I have modified an otherwise functional code by adding a return to the start point.

    %
    O0104
    G54
    / G28 U0 W0
    G50 S1400
    G00 G53 X-8. Z-7.
    G00 G97 T101 S600 M03
    G00 X5. Z.33
    G96 S550 M08
    G72 U.05 R.025
    G72 P10 Q50 U.015 W.005 F.01
    N10 G00 Z0
    G01 X2.3
    N50 G00 X5.
    G00 X5. Z0.05
    G71 U.1 R.025
    G71 P100 Q150 U.01 W.005 F.012
    N100 G00 X2.8995
    G01 X2.8995 Z0.
    G01 X2.9995 Z-0.05
    G01 X2.9995 Z-0.23
    G01 X5. Z-0.23
    N150 G00 Z.05
    M09
    G97 S400 M1003
    G00 G53 X-8. Z-7.
    M30
    %

    Here is the thing.
    The G72 block will become useless, as there are no other motions between the P and Q block other than the retract of .025 3 times. That's it.
    The G71 however will function just as it does with the proper, no-return code.

    Same code on Haas - correctly I might add - result in a "Non Monotonous" error.

    So anyway, that's all for the tangent discussion.

  18. #18
    Join Date
    Feb 2006
    Posts
    1792
    Quote Originally Posted by SeymourDumore View Post
    G00 T404 (TURNING TOOL)
    G96 S650 M03
    G00 X1.145Z0.
    G01 X-0.05 F.004 M08
    G00 G42 X1.125 Z0.05 <--- Note the comp-on BEFORE the cycle
    G71 U.06 R.02
    G71 P101 Q201 U.01 W0 F.006
    N101 G00 X0. Z.05
    G01 Z0. F.003
    G03 X0.7071 Z-0.8536 R0.5
    G01 Z-.8856
    N201 G01 X1.125
    G70 P101 Q201
    G00 G40 X1.125 Z.05 <--- Ramp-off move here.
    G80 M09
    The tool is actually at X1.125 Z0.05 before this command. So, should we not use a different X/Z value in the Ramp-off move? Even if the same values are permitted, the tool will move towards the job, with an inadvertent overcutting.

  19. #19
    Join Date
    Sep 2007
    Posts
    116
    While it might move towards the part, it would not cause overcutting as this point is in fact exactly the same point from where the cycle started from, therefore there cannot possibly be any material left to overcut.

  20. #20
    Join Date
    Feb 2006
    Posts
    1792
    Still I feel that it is a good practice to move the tool away from the job during the ramp-off move. Maybe we should use X1.2 (say) instead of X1.125 in the ramp-off move, even though it is not required in this case.

Page 1 of 2 12

Similar Threads

  1. Type II G71 Stock Removal on Fanuc 0i-TB
    By lowehardware in forum G-Code Programing
    Replies: 1
    Last Post: 01-09-2008, 12:55 AM
  2. Fanuc 0i-MC and ARM type toolchanger
    By ddanutz in forum Fanuc
    Replies: 4
    Last Post: 08-27-2007, 10:57 PM
  3. fast stock removal on steel
    By dynamotive in forum MetalWork Discussion
    Replies: 11
    Last Post: 02-02-2007, 04:02 AM
  4. gettys fanuc type 10 motor
    By najnielkp in forum Fanuc
    Replies: 1
    Last Post: 05-07-2006, 02:47 PM
  5. Fanuc 0T Stock Removal Cycles
    By M@T in forum Uncategorised CAM Discussion
    Replies: 4
    Last Post: 11-02-2003, 01:43 AM

Posting Permissions

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