G71... Please help! What is wrong with this program? - Page 2
Close
Login to Your Account
Page 2 of 5 FirstFirst 1234 ... LastLast
Results 21 to 40 of 83
  1. #21
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,603
    Post Thanks / Like
    Likes (Given)
    254
    Likes (Received)
    1582

    Default

    Brent, this program just ran on the Oi-TC without any problems:

    %
    O0105 (YARD)
    G54
    G00 G53 X-5. Z-5.
    G50 S700
    G00 G99 G40 G54
    G00 G97 T202 S150 M03
    G00 X3.5 Z0.1
    G96 S450
    G71 U.05 R.025
    G71 P31 Q32 U0.03 W0.003 F0.012
    N31 G01 X1.4854 Z0.
    G03 X1.495 Z-0.0063 R0.005
    G01 X1.2726 Z-0.4213
    G02 X1. Z-1.4566 R4.
    G01 X1. Z-2.01
    G02 X1.76 Z-2.39 R0.38
    G01 X2.94 Z-2.39
    G01 X3. Z-2.42
    G01 X3. Z-3.316
    N32 G01 X3.5
    M09
    M05
    G00 G53 X-5. Z-5.
    M30
    %

    The final path was significantly different from the Haas path, but it has not in any way overcut the part.
    I ran with .05, .1, .15 and .02 DOC-s, and there were no unusual moves.

    The Haas always does a final "smoothing" pass on the profile between the P-Q blocks with a Type II cycle, while the Fanuc
    did it's thing on the unidirectional section once, and then again only on the tapered section ( That is why I like the single line G71 better )
    Nonetheless, it has not made any funky ( and yes, absolutely dangerous ) moves at all!

  2. #22
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    Re-post the program using I/K Circular Interpolation Format and test to see if you still have the issue.

    Regards,

    Bill
    Hi Bill,
    I'm not sure I know how? I've always used R format for ease of reading at the control, I haven't took the time to completely understand it. I really don't post anything, I draw it up in Autocad, set my UCS, then with the help of a handy lisp routine ad I pick the entries, the lisp routine sends the entries to a text file in G1XZ G2XZ or G3XZ I add the R's by hand I then copy the tool path and paste it in my program. I have a feeling reprogramming in I&K will fix it.

    What's your gut feeling on why this is happening? Best I can tell all the points figure out correctly. And why isn't SeymourDumore experiencing the same thing, seems like both controls would process the numbers the same.

    Both times I've had an issue like this it was around a larger radius. Strange!

    Brent

  3. #23
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by SeymourDumore View Post
    Brent, this program just ran on the Oi-TC without any problems:

    %
    O0105 (YARD)
    G54
    G00 G53 X-5. Z-5.
    G50 S700
    G00 G99 G40 G54
    G00 G97 T202 S150 M03
    G00 X3.5 Z0.1
    G96 S450
    G71 U.05 R.025
    G71 P31 Q32 U0.03 W0.003 F0.012
    N31 G01 X1.4854 Z0.
    G03 X1.495 Z-0.0063 R0.005
    G01 X1.2726 Z-0.4213
    G02 X1. Z-1.4566 R4.
    G01 X1. Z-2.01
    G02 X1.76 Z-2.39 R0.38
    G01 X2.94 Z-2.39
    G01 X3. Z-2.42
    G01 X3. Z-3.316
    N32 G01 X3.5
    M09
    M05
    G00 G53 X-5. Z-5.
    M30
    %

    The final path was significantly different from the Haas path, but it has not in any way overcut the part.
    I ran with .05, .1, .15 and .02 DOC-s, and there were no unusual moves.

    The Haas always does a final "smoothing" pass on the profile between the P-Q blocks with a Type II cycle, while the Fanuc
    did it's thing on the unidirectional section once, and then again only on the tapered section ( That is why I like the single line G71 better )
    Nonetheless, it has not made any funky ( and yes, absolutely dangerous ) moves at all!


    Well damn! This is just crazy. I appreciate your time. Thanks again...

    Brent

  4. #24
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,112
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1216

    Default

    Quote Originally Posted by yardbird View Post
    Hi Bill,
    I'm not sure I know how? I've always used R format for ease of reading at the control, I haven't took the time to completely understand it. I really don't post anything, I draw it up in Autocad, set my UCS, then with the help of a handy lisp routine ad I pick the entries, the lisp routine sends the entries to a text file in G1XZ G2XZ or G3XZ I add the R's by hand I then copy the tool path and paste it in my program. I have a feeling reprogramming in I&K will fix it.

    What's your gut feeling on why this is happening? Best I can tell all the points figure out correctly. And why isn't SeymourDumore experiencing the same thing, seems like both controls would process the numbers the same.

    Both times I've had an issue like this it was around a larger radius. Strange!

    Brent
    Hello Brent,
    I can't read the dimensions of your drawing well enough,nor do I know the TNR you're using (although that could be determined if I could read the drawing dimensions to compare with your program code), otherwise I would have Posted a copy of your code in I/K Format.

    Without the benefit of being able to compare your code with the drawing dimensions, it would seem that your code is written to use TNR Comp at the Control, but there is no G42 specified anywhere. The "R" address of the G03 radius at the start of your profile should be the Radius of the TNR, plus the Radius of the feature if not using TNR Comp at the Control; hence my reason for thinking the profile is written for Comp at the Control.

    Not saying it is the cause of your issue, but the reason R Format sometimes give unpredictable results, is that the Control must ultimately calculates where the centre of the Circular Move is, whether by using I and K, or R Format.

    1. When using I and K Format, the resulting values for these addresses are calculated using accuracy far better than the Least Programmable Increment setting of the Control. Accordingly, the Centre of the Circular Move calculated by the Control is accurate.

    2. When using R Format, the numbers used by the control to calculate the Centre of the Circular Move have already been Rounded to the Least Programmable Increment of the Control. Accordingly, the resulting Centre may not be quite so accurate.

    I believe that if you were to run your current Code as a Finish Tool Path (No G71 Cycle), there will be no error such as you're experiencing. Coupled with the control calculating the Arc Centre using Rounded numbers, it is also calculating partial moves of the Profile Definition for the Roughing Moves. So my gut feeling is that the version of the control may have something to do with the fact that the Roughing Cycle fails with you (under particular conditions) and not with SeymourDumore.

    I've seen some peculiar behavior with similar controls. One was where a programmed Circular Move that started at any other point other than a quadrant boundary (3,6,9,12 o'clock) would raise an alarm. The arc move could finish anywhere; it just had to start on the quadrant. The problem was fixed with an upgrade of the software version of the control. I'm sure Kevin, aka Vancbiker, would concur with such possibilities.

    Post a sketch with bigger numbers, and specify the TNR being used.

    Regards,

    Bill

  5. Likes yardbird liked this post
  6. #25
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    I can't read the dimensions of your drawing well enough,nor do I know the TNR you're using (although that could be determined if I could read the drawing dimensions to compare with your program code), otherwise I would have Posted a copy of your code in I/K Format.

    Without the benefit of being able to compare your code with the drawing dimensions, it would seem that your code is written to use TNR Comp at the Control, but there is no G42 specified anywhere. The "R" address of the G03 radius at the start of your profile should be the Radius of the TNR, plus the Radius of the feature if not using TNR Comp at the Control; hence my reason for thinking the profile is written for Comp at the Control.

    Not saying it is the cause of your issue, but the reason R Format sometimes give unpredictable results, is that the Control must ultimately calculates where the centre of the Circular Move is, whether by using I and K, or R Format.

    1. When using I and K Format, the resulting values for these addresses are calculated using accuracy far better than the Least Programmable Increment setting of the Control. Accordingly, the Centre of the Circular Move calculated by the Control is accurate.

    2. When using R Format, the numbers used by the control to calculate the Centre of the Circular Move have already been Rounded to the Least Programmable Increment of the Control. Accordingly, the resulting Centre may not be quite so accurate.

    I believe that if you were to run your current Code as a Finish Tool Path (No G71 Cycle), there will be no error such as you're experiencing. Coupled with the control calculating the Arc Centre using Rounded numbers, it is also calculating partial moves of the Profile Definition for the Roughing Moves. So my gut feeling is that the version of the control may have something to do with the fact that the Roughing Cycle fails with you (under particular conditions) and not with SeymourDumore.

    I've seen some peculiar behavior with similar controls. One was where a programmed Circular Move that started at any other point other than a quadrant boundary (3,6,9,12 o'clock) would raise an alarm. The arc move could finish anywhere; it just had to start on the quadrant. The problem was fixed with an upgrade of the software version of the control. I'm sure Kevin, aka Vancbiker, would concur with such possibilities.

    Post a sketch with bigger numbers, and specify the TNR being used.

    Regards,

    Bill
    Hi Bill,

    Thanks for you help! tool is .0313 radius. The entire original program is at the bottom. No comp in the rougher finishing with separate tool separate tool path. I will try to get bigger pictures of the drawing later when i get in.

    Brent

    %
    :1050(80-506 1050 1ST OP)
    (80-506 1050 REV 2 11/20/17)
    (STANDOFF 2)
    (3 1/2"ROUND x 13"LONG)
    (JAWS IN .266)
    (PH4140)

    (G54 SET Z 5.7)

    N10(FRONT STOP)
    M5
    G0G99G40G54X14.Z10.T0
    T0404
    G0X.5Z.05
    M0
    (MOVE MATERIAL TO STOP )

    G0W.5
    G0G40X14.Z10.T0
    M1

    N20(ROUGH FACE)
    G0G99G40G54X14.Z10.T0
    T0101
    M41
    G97S200M4
    G0X3.8Z.15M8
    G50S700
    G96S350
    G72W.15R.05
    G72P21Q22U0W.01F.01
    N21G0Z0
    G1X-.035
    N22G0Z.15
    M9
    G0G99G40G54X14.Z10.T0
    M1

    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31G1X1.4854Z.0000
    G3X1.4950Z-.0063R.005
    G1X1.2726Z-.4213
    G2X1.0000Z-1.4566R4.
    G1X1.0000Z-2.0100
    G2X1.7600Z-2.3900R.38
    G1X2.9400Z-2.3900
    G1X3.0000Z-2.4200
    G1X3.0000Z-3.3160
    N32G1X3.5
    M9
    G0G99G40G54X14.Z10.T0
    M1

    N40(FINISH FACE OD)
    M24
    G0G99G40G54X14.Z10.T0
    T0505
    M41
    G97S150M4
    G0X3.2Z.2M8
    G50S700
    G96S450
    G0Z-2.3885
    G1X1.76F.012
    G0Z.0
    G1X-.04
    G0X1.1Z.2
    G0G42X1.35Z.1
    G1Z.0
    G1X1.4854
    G3X1.4950Z-.0063R.005
    G1X1.2726Z-.4213
    G2X1.0000Z-1.4566R4.
    G1X1.0000Z-2.0100
    G2X1.7600Z-2.3900R.38
    G1X2.9400Z-2.3900F.016
    G1X3.0000Z-2.4200F.012
    G1X3.0000Z-3.1160
    G1X3.2
    G0G40Z.5
    M9
    G0G99G40G54X14.Z10.T0
    M25
    M1

    N50( CENTER DRILL)
    G0G99G40G54X14.Z10.T0
    T1212
    M41
    G97S350M3
    G0X0Z.1M8
    G1Z-.350F.0035
    G0Z.5M9
    G0X8.
    G0G99G40G54X14.Z10.T0
    M1

    N60(MSG, 5/16" .3125 DRILL)
    G0G99G40G54X14.Z10.T0
    T1010

    #1=.02 (FEED SHORT OF)
    #2=.1 (PECK EVERY)
    #3=.0 (START DRILLING AND LOCAL VARIABLE)
    #4=1.25 (STOP DRILLING)
    #5=.1 (RAPID BACK SHORT OF)
    #6=.005 (FEED RATE)

    G97S200M3
    G0Z.5
    G0X0M8
    G0Z-[#3]
    #3=[#3+#2]
    N200
    G1Z-[#3]F[#6]
    G0Z.1
    G0Z-[#3-#5]
    G1Z-[#3-#1]F.2
    #3=[#3+#2]
    IF[#3LT#4]GOTO200
    G1Z-[#4]F[#6]
    G0Z.5
    M9
    G0X10.
    G0G40X14.Z10.T0
    M0

    N70( 3/8"-16 TAP)
    G0G99G40G54X14.Z10.T0
    T0808
    M41
    G97S125M3
    G0X0Z.5M8
    G1Z-1.F.0625
    G1Z.5M4
    M9
    G0G40X14.Z10.T0
    M0

    N80(CUT OFF +.03)
    (TOOL TOUCHED OFF TIP 4)
    G0G99G40G54X14.Z10.T0
    T1111
    M41
    G97S150M4
    G0X3.3Z.5
    G50S600
    G96S250
    G0Z-2.916M8
    G1X.1F.004
    G0X8.M9
    G0Z.5
    G0G99G40G54X14.Z10.T0
    M30
    %

  7. #26
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,112
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1216

    Default

    Quote Originally Posted by yardbird View Post
    Hi Bill,

    Thanks for you help! tool is .0313 radius. The entire original program is at the bottom. No comp in the rougher finishing with separate tool separate tool path. I will try to get bigger pictures of the drawing later when i get in.

    Brent
    Hello Brent,
    Following are two Code Examples using I/K Circular Interpolation Format, one using Zero TNR for TNR Comp at the Control, the other with the TNR incorporated in the Code. Try these to see if the error still persists.

    Regards,

    Bill

    Without TNR Comp Included
    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31 G00 X1.4854 W0.0
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050
    G01 X1.2726 Z-0.4213
    G02 X1.0000 Z-1.4566 I3.8637 K-1.0353
    G01 Z-2.0100
    G02 X1.7600 Z-2.3900 I0.3800 K0.0000
    G01 X2.9400
    G01 X3.0000 Z-2.4200
    G01 Z-3.3160
    N32 G01 X3.5000
    M9
    G0G99G40G54X14.Z10.T0
    M1

    With TNR Comp Included
    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31 G00 X1.4229 W0.0
    G01 X1.4228 Z0.0000
    G03 X1.4929 Z-0.0456 I0.0000 K-0.0362
    G01 X1.2705 Z-0.4606
    G02 X1.0000 Z-1.4878 I3.8335 K-1.0272
    G01 Z-2.0413
    G02 X1.6975 Z-2.3900 I0.3488 K0.0000
    G01 X2.9034
    G01 X3.0000 Z-2.4383
    G01 Z-3.3160
    N32 G01 X3.5000
    M9
    G0G99G40G54X14.Z10.T0
    M1

  8. #27
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,041
    Post Thanks / Like
    Likes (Given)
    581
    Likes (Received)
    1533

    Default

    Quote Originally Posted by angelw View Post
    .....The problem was fixed with an upgrade of the software version of the control. I'm sure Kevin, aka Vancbiker, would concur with such possibilities.
    Software bugs from Fanuc are rare but I have seen a couple.

  9. #28
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    I hope these are visible the only thing I ccould think of to do was take a picture of the screen.


    Brent

    20171129_155137.jpg

    20171129_154201.jpg

  10. #29
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by Vancbiker View Post
    Software bugs from Fanuc are rare but I have seen a couple.
    You have a opinion on what is going on here? I don't understand why the DOC is what triggers the last move? If something in the numbers of the tool path was jacked up I'd think it would do it at whatever DOC.

    Brent

  11. #30
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,112
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1216

    Default

    Quote Originally Posted by yardbird View Post
    I hope these are visible the only thing I ccould think of to do was take a picture of the screen.


    Brent

    20171129_155137.jpg

    20171129_154201.jpg
    Hello Brent,
    Following is the Code based on your drawing dimensions. The only difference I get, compared to your original Code, is shown in Red.

    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31 G00 X1.4854 W0.0
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050
    G01 X1.2726 Z-0.4213 (X1.2726 Z-0.4214)
    G02 X1.0000 Z-1.4566 I3.8637 K-1.0353
    G01 Z-2.0100
    G02 X1.7600 Z-2.3900 I0.3800 K0.0000
    G01 X2.9400
    G01 X3.0000 Z-2.4200
    G01 Z-3.3160
    N32 G01 X3.5000
    M9
    G0G99G40G54X14.Z10.T0
    M1

    Regards,

    Bill

  12. Likes yardbird liked this post
  13. #31
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    Following is the Code based on your drawing dimensions. The only difference I get, compared to your original Code, is shown in Red.

    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31 G00 X1.4854 W0.0
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050
    G01 X1.2726 Z-0.4213 (X1.2726 Z-0.4214)
    G02 X1.0000 Z-1.4566 I3.8637 K-1.0353
    G01 Z-2.0100
    G02 X1.7600 Z-2.3900 I0.3800 K0.0000
    G01 X2.9400
    G01 X3.0000 Z-2.4200
    G01 Z-3.3160
    N32 G01 X3.5000
    M9
    G0G99G40G54X14.Z10.T0
    M1

    Regards,

    Bill
    Hi Bill,

    Well I typed your numbers in and it run without a hitch. I don't know what to think? Morale of the story run it through the graph first to see if any stupid shit is going to happen before you leter rip. Picture at the bottom is what happens when the jacked up program is run complete. Can't believe .0001 on one number and I&K makes that much of difference.

    This has only ever happened to me twice in my whole career and come to think of it both times on this Fanuc 0i-TD control.

    Thanks I appreciate your help everyone!

    20171129_170243.jpg

    20171129_170657.jpg

    Brent

    20171129_164627.jpg
    Last edited by yardbird; 11-29-2017 at 05:35 PM. Reason: edited post..

  14. #32
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    618
    Post Thanks / Like
    Likes (Given)
    421
    Likes (Received)
    239

    Default

    Quote Originally Posted by yardbird View Post
    Hi Bill,

    Well I typed your numbers in and it run without a hitch. I don't know what to think? Morale of the story run it through the graph first to see if any stupid shit is going to happen before you leter rip. Picture at the is what happens when the jacked up program is run ccomplete.

    Thanks I appreciate your help everyone!

    20171129_170243.jpg

    20171129_170657.jpg

    Brent

    20171129_164627.jpg
    Does it continue to simulate properly even if you change the DOC???

  15. #33
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by Nerdlinger View Post
    Does it continue to simulate properly even if you change the DOC???
    I haven't tried? I'll see here after bit. The program in the OP and in post 8 both run fine at .1 and .15 but both were jacked up at .05 DOC. Bills run fine at where the others didn't. I could see if I had the start and end points all fucked up and the control got lost trying to sweep a particular size radius and ended up with what you see. But before there is going to be a major malfunction it ought to puke an alarm first.

    Brent

  16. #34
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by Nerdlinger View Post
    Does it continue to simulate properly even if you change the DOC???
    Yes it does. Tried .075 .1 .15 and .2 and they all worked as it should. Maybe this is not considered a "bug" in the control by Fanuc but I can't see how it isn't?

    Brent

  17. #35
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,041
    Post Thanks / Like
    Likes (Given)
    581
    Likes (Received)
    1533

    Default

    Quote Originally Posted by yardbird View Post
    You have a opinion on what is going on here? I don't understand why the DOC is what triggers the last move? If something in the numbers of the tool path was jacked up I'd think it would do it at whatever DOC.

    Brent
    Hi Brent,

    I don't have anything better than Bill's assessment. I've never used R designation in turning as the era I did a bit of lathe programming in was before R became available.

    When I was doing field service, I saw many weird movement results when the toolpath numbers were not right and R was used. If the toolpath numbers are off and I and K are used the control will alarm if the error exceeds a small parameter set value. Showing the customer their math error and correcting it always fixed the problem. I looked at your original code and it looked good for using R.

    Is this on a newish control? If it is, I'd contact Fanuc about it. It may take a bit of pushing on your end to get some attention, but if you want to continue using R designation it would be worth trying to get a fix.

  18. Likes B-Mathews liked this post
  19. #36
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by Vancbiker View Post
    Hi Brent,

    I don't have anything better than Bill's assessment. I've never used R designation in turning as the era I did a bit of lathe programming in was before R became available.

    When I was doing field service, I saw many weird movement results when the toolpath numbers were not right and R was used. If the toolpath numbers are off and I and K are used the control will alarm if the error exceeds a small parameter set value. Showing the customer their math error and correcting it always fixed the problem. I looked at your original code and it looked good for using R.

    Is this on a newish control? If it is, I'd contact Fanuc about it. It may take a bit of pushing on your end to get some attention, but if you want to continue using R designation it would be worth trying to get a fix.
    Hello Kevin,

    Thanks! Actually yes it is relatively (3yrs ?) new machine the control is a Fanuc 0i-TD I don't know how new that is? The Sharpe mills we bought about a year ago came in with Fanuc 0i-MF so the D model I suspect have been around a good while?

    I ought to email one of the application engineers at Doosan and sick him on it. They are pretty good about stuff like that.

    Brent

  20. #37
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,041
    Post Thanks / Like
    Likes (Given)
    581
    Likes (Received)
    1533

    Default

    Quote Originally Posted by yardbird View Post
    .....I ought to email one of the application engineers at Doosan and sick him on it. They are pretty good about stuff like that.

    Brent
    That's better than my idea. They will have more leverage and better contacts than an end user.

  21. Likes yardbird liked this post
  22. #38
    Join Date
    Mar 2017
    Country
    CHINA
    Posts
    1,813
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1127

    Default

    Quote Originally Posted by yardbird View Post
    Can't believe .0001 on one number and I&K makes that much of difference.

    This has only ever happened to me twice in my whole career and come to think of it both times on this Fanuc 0i-TD control.
    Had a Westinghouse that would drive around in circles trying to find the endpoint with R if the math wasn't perfect. Once or twice I just watched it to see where it would end up. It would eventually overtravel and e-stop if you let it go long enough

    Or crash the chuck, which would be less humorous

    There's actually a reason I am old-fashioned and hate all this 'hep-you' stuff. It fucks up more than just writing the toolpath correctly in the first place.

  23. #39
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by SeaMoss View Post
    Had a Westinghouse that would drive around in circles trying to find the endpoint with R if the math wasn't perfect.
    That's the thing that gets me. My numbers were damned near perfect. I had one Z number that was .0001 different than what Bill posted. The canned cycle would only screw up if I used a DOC of .05". When I changed the the DOC to .1 .15 .2 that same canned cycle ran with those exact numbers. If the numbers were wrong, then in my mind they'd be wrong regardless of DOC? Yes?

    Why does this happen at just one specific DOC?

    Brent

  24. #40
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,896
    Post Thanks / Like
    Likes (Given)
    4253
    Likes (Received)
    1452

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    Following is the Code based on your drawing dimensions. The only difference I get, compared to your original Code, is shown in Red.

    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31 G00 X1.4854 W0.0
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050
    G01 X1.2726 Z-0.4213 (X1.2726 Z-0.4214)
    G02 X1.0000 Z-1.4566 I3.8637 K-1.0353
    G01 Z-2.0100
    G02 X1.7600 Z-2.3900 I0.3800 K0.0000
    G01 X2.9400
    G01 X3.0000 Z-2.4200
    G01 Z-3.3160
    N32 G01 X3.5000
    M9
    G0G99G40G54X14.Z10.T0
    M1

    Regards,

    Bill
    Hi Bill,

    I'm assuming after the fact but since you need to know the TNR that these numbers have comp figured into the tool path. I used those numbers in my finish tool pass with G42 and a R.0313 T3 registered in the geometry offset and when it was finished there was a .015" step on the face. Is that correct?

    I will say that the rougher is leaving a more uniform clean up pass than I'm typically used to.

    Brent

    20171129_191030.jpg


Tags for this Thread

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
  •