G71... Please help! What is wrong with this program? - Page 3
Close
Login to Your Account
Page 3 of 5 FirstFirst 12345 LastLast
Results 41 to 60 of 83
  1. #41
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    OK I've PM'd PM member Paul Anderson aka "LockNut" an applications engineer at Doosan to see if he will have a look at this thread and possibly comment on the matter. Hopefully he will?

    Brent

  2. #42
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    Quote Originally Posted by angelw View Post
    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.
    I'm
    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
    Hi Bill,

    Is this the original posting of this post? Or has it been edited? I don't recall seeing this post with this exact text. Regardless if it was or it wasn't I used the numbers without comp figured in. Witch then I have no fuckin clue about the step on the face? I ended up using the original finish pass in the OP witch looked fantastic .005rad on the front corner and everything. It's been a long day, I've had some beers, I'm outta here for now. Lol....

    Thanks folks!

    Brent

  3. #43
    Join Date
    Mar 2017
    Country
    CHINA
    Posts
    1,979
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    909

    Default

    Quote Originally Posted by yardbird View Post
    Why does this happen at just one specific DOC?
    My wild-ass guess would be tolerance stackup. Plus you know that computers can't actually do correct decimal math ? They run base 2, the rest of the world is base ten, it doesn't always come out the same. Add in the different ways different people use different data types (truncate the number, round up, round down, etc etc) add in your tool nose radius comp and whatever your calculator does and you have a recipe for the occasional screwup.

    At least with i and k the control will usually get as close as possible with the radius interpolation then do a little jerk to get to the correct end point. It's not lovely but that's better than my girlfriend and her damned gps driving around in circles forever Computers are stewpid.

    Keep at this long enough and you'll ditch the damned macros and tool nose offset, start using APT and programming to cutter centerline. Then the machine will go where you tell it

  4. #44
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,486
    Post Thanks / Like
    Likes (Given)
    236
    Likes (Received)
    1507

    Default

    While you're waiting for an answer, a small tangent ....

    Quote Originally Posted by yardbird View Post
    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.


    Brent
    Wow Brent!

    That is pretty much EXACTLY what I do, except instead of a LISP routine ( which I did write one of some 18+ years ago doing the very same text file ), I went
    with Bobcad V17 and later V21-Express.

    I draw my toopaths ( individually for rough, finish, ID rough, ID finish, groove rough, groove finish etc. ), mark X and Z0 with a circle in ACAD, then export
    all of the selected as one single DXF, then into BobCAD and all I have to do is move the UCS to the center of each circle and then do a cut-chain.
    There is no "post" to speak of so Bob does not output anything but the appropriate G codes and the X/Z ( of X/Y coordinates for milling ).
    I don't have to mess with anything but fill in the rest.

    (on edit)
    Just to continue, that part you're making would take me 3 minutes to draw the rough, finish toolpaths for ( using the CAD file in ACAD) AND save it as a DXF, and then literally
    in 3 more minutes I have a finished program.
    Problem: BobCAD CAD/CAM Company no longer supports ANY of my rightfully purchased and owned licenses!
    IOW, if I was to reload my PC with the very same stuff I have on it now ( or just simply replace my hard drive and mirror my last week's backup ), I would be shit-out-of luck!
    Why?
    Because they will not re-license my software!

    Anyhow, did not mean to rant but I do find it interesting that you're doing the very same thing as I, but a bit of a longer and more troublesome way.

  5. #45
    Join Date
    Mar 2017
    Country
    CHINA
    Posts
    1,979
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    909

    Default

    Quote Originally Posted by SeymourDumore View Post
    While you're waiting for an answer, a small tangent ....

    Wow Brent!

    That is pretty much EXACTLY what I do, except instead of a LISP routine ( which I did write one of some 18+ years ago doing the very same text file ), I went with Bobcad V17 and later V21-Express.
    You guys, ouch

    I have an old copy of Personal APT I can send you.

  6. #46
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Post

    Quote Originally Posted by SeymourDumore View Post
    While you're waiting for an answer, a small tangent ....



    Wow Brent!

    That is pretty much EXACTLY what I do, except instead of a LISP routine ( which I did write one of some 18+ years ago doing the very same text file ), I went
    with Bobcad V17 and later V21-Express.

    I draw my toopaths ( individually for rough, finish, ID rough, ID finish, groove rough, groove finish etc. ), mark X and Z0 with a circle in ACAD, then export
    all of the selected as one single DXF, then into BobCAD and all I have to do is move the UCS to the center of each circle and then do a cut-chain.
    There is no "post" to speak of so Bob does not output anything but the appropriate G codes and the X/Z ( of X/Y coordinates for milling ).
    I don't have to mess with anything but fill in the rest.
    Hey Bub,

    If your interested I'd be willing to send you my lisp routines to have a loook? Actually I'd be interested if you know all the (I'm running Autocad 2011) stuff that need to be saved so you can export all settings from one box to another box and have your complete Autoocad environment from one PC box to another? I guess a complete backup, because on any given day with no particular reason I will go home to return to a different box and would love to be able to import settings an be done instead of jack around with the same shit I always do.

    Later.....

    Brent
    Last edited by yardbird; 11-30-2017 at 10:08 AM. Reason: got rid of red face guy icon...

  7. #47
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,027
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1192

    Default

    Quote Originally Posted by yardbird View Post
    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

    Attachment 214132
    Hello Brent,
    I only needed your TNR because your early Post seemed not to use TNR Comp at the control, but the numbers in the code suggested that Zero was being used as the TNR when creating the program.

    The Profile Code from the following, used as a finish path, would require TNR Comp at the Control.

    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

    With regards to your issue, as I've suggested in earlier Posts, I believe your original "R" Format Code will run OK as a Finish Tool Path and I believe that the the I/K Format Code using ALL your numbers, will run successfully in the G71 Cycle.

    I think that the issue is a combination of the R Format and the Control calculating the intersection points for the DOC and the Part Profile and then the partial movement on any element of the profile that is encountered; a software issue. I agree with Kevin, report the matter to Fanuc, via the MTB agent.

    There should be no step in the face as long as the face is being machined to Z Zero. The Code clearly shows that the tool is driven to Z Zero before swinging the 0.005 Radius. You would have to Post your Code for the Finish Pass showing how G42 was implemented.

    In your earlier Posted Code, G42 is being applied traveling from Smaller to Larger Diameter; accordingly, Right Trending Offset G42 is correct.

    G0X1.1Z.2
    G0G42X1.35Z.1
    G1Z.0

    When using the following Code for the Finish Pass:

    N31 G00 X1.4854 Z0.1
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050

    I would Start the Tool at X1.4228, or less and apply the G42 on the Z0.0000 move as follows:

    G00 X1.4228 Z0.1
    G42 G01 Z0.0000
    G01 X1.4854
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050

    X1.4228 would work for 0.03125 and smaller TNR inserts.

    Regards,

    Bill
    Last edited by angelw; 11-30-2017 at 07:48 AM.

  8. #48
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    Quote Originally Posted by angelw View Post
    Hello Brent,
    I only needed your TNR because your early Post seemed not to use TNR Comp at the control, but the numbers in the code suggested that Zero was being used as the TNR when creating the program.

    The Profile Code from the following, used as a finish path, would require TNR Comp at the Control.

    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

    With regards to your issue, as I've suggested in earlier Posts, I believe your original "R" Format Code will run OK as a Finish Tool Path and I believe that the the I/K Format Code using ALL your numbers, will run successfully in the G71 Cycle.

    I think that the issue is a combination of the R Format and the Control calculating the intersection points for the DOC and the Part Profile and then the partial movement on any element of the profile that is encountered; a software issue. I agree with Kevin, report the matter to Fanuc, via the MTB agent.

    There should be no step in the face as long as the face is being machined to Z Zero. The Code clearly shows that the tool is driven to Z Zero before swinging the 0.005 Radius. You would have to Post your Code for the Finish Pass showing how G42 was implemented.

    In your earlier Posted Code, G42 is being applied traveling from Smaller to Larger Diameter; accordingly, Right Trending Offset G42 is correct.

    G0X1.1Z.2
    G0G42X1.35Z.1
    G1Z.0

    When using the following Code for the Finish Pass:

    N31 G00 X1.4854 Z0.1
    G01 Z0.0000
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050

    I would Start the Tool at X1.4228, or less and apply the G42 on the Z0.0000 move as follows:

    G00 X1.4228 Z0.1
    G42 G01 Z0.0000
    G01 X1.4854
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050

    X1.4228 would work for 0.03125 and smaller TNR inserts.

    Regards,

    Bill
    Hi Bill,

    Given the fact that the G71 cycle ignores TNRC the only time I turn it on before roughing is if I'm calling a G70 afterwards.

    I have always tried to turn on comp with a X&Z move a little more than twice the radius of the tool. Possibly turning it on with the G42 G1 Z.0 move at a smaller X would be the fix IDK?

    I run the finish tool numbers exactly as listed above in post 31 and to be honest I haven't a clue as to why the step is in the face?

    As a fix I ended up running the exact finish pass as listed in the OP and it looked as its supposed to so I'm not getting why the start numbers and turning on comp would work for one tool path and not the other. Its just odd to me? I've done this shit hundreds of time this way and never any issues. Well ok 1 other issue.

    Actually lately I've been a bit gun shy after the episode with the canned cycle and the unexplained step on the fave. I haven't had a wreck in a awfully long time and I'm having a hard time trusting the sumbitch.

    Hopefully LockNut will show up and weighs in on the matter. I have his work email if he doesn't show up here after bit I'll send him a email and see if he'll have a look?

    Thanks Bill

    Brent

  9. #49
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    600

    Default

    It looked to me from the graphic that the G71 was bombing on the final smoothing pass. Would be interesting to compare param 5105.2 on Yardbird's lathe and Seymore's. It sounded like Seymore's lathe was not making a full smoothing pass. Type 2 G71 follows the contour, so the smoothing pass may be kind of redundant, and turning it off might change the way the machine calculates the cycle.

    My lathe doesn't do Type 2, so I can't test.

    The book seems to say TNRC is cancelled and restarted on each pass of the G71 cycle.
    When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel command (G40) outside the blocks (from the block specified with P to the block specified with Q) specifying a target finishing figure.

    If a tool nose radius compensation command (G40, G41, or G42) is specified in the G70, G71, G72, or G73 command, alarm PS0325 is issued.

    When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled again at the return to the cycle start point after term ination of cycle operation. Start-up is performed again according to the next move command.
    The digging in on the finish tool appears to be a function of where the G42 was specified in the program. (why I don't use TNRC on the lathe).

  10. #50
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    Quote Originally Posted by jancollc View Post
    My lathe doesn't do Type 2, so I can't test
    No kidding? What do you have an old 6T?

    What is parameter 5105.2?

    My R format finish path and then when I took Bills I&K numbers pasted them in the very same program both had the exact same approach. So I'm I to understand that the approach, when and where TNRC is activated has to be different when using R format than when using I&K format?

    Brent

  11. #51
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    600

    Default

    Quote Originally Posted by yardbird View Post
    No kidding? What do you have an old 6T?
    No, it's an Oi-TB. They didn't add type 2 till Oi-TC. It might have been an option on the TB, but there's nothing in the books about Type 2.

    Quote Originally Posted by yardbird View Post
    What is parameter 5105.2?
    That turns the smoothing pass on or off. Setting to 0 runs the smoothing pass, setting to 1 does not run the smoothing pass.

    Quote Originally Posted by yardbird View Post
    My R format finish path and then when I took Bills I&K numbers pasted them in the very same program both had the exact same approach. So I'm I to understand that the approach, when and where TNRC is activated has to be different when using R format than when using I&K format?

    Brent
    That's not how I read it. TNRC shouldn't care whether you use R or I & K. Where did you call up the G42 in your finish path? On the G1 Z0 line? That would undercut if it's putting the X tangent point of the TNR at Z0.

    Your initial numbers fed from the cycle start position to the start of profile (the P block). I think if you put the G42 in that line, it would not undercut the end.

    I think if you did nothing else but take out the R and replace with I,K on that 4" rad it would have run fine. That looked to me like the problem block.

    Like I said, I don't run Type 2, so I follow the rules for Type 1 which is no Z position in the P block. For me, that is always a rapid move in X axis to the first tangent point, followed by the G1 Z0 line to the start of the profile.

    Type 2 needs the Z or W in that block, so your initial numbers were legal in the sense that you were starting the profile in a G1 move. You had a .100 feed move in Z, which is plenty enough movement to pick up the TNRC.

    The only real problem was the R4 on the smoothing pass- the control is not executing that correctly with the small DOC. Getting rid of the smoothing pass by setting 5105.2 to 1 might get rid of that issue, I don't know. Seymore didn't have the problem on his Oi-TC, which is why I was wondering about the parameter settings on his and your lathes.

  12. #52
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    Quote Originally Posted by jancollc View Post
    No, it's an Oi-TB. They didn't add type 2 till Oi-TC. It might have been an option on the TB, but there's nothing in the books about Type 2.
    I thought type 2 was pretty much a standard option on all i controls? We have an old Fanuc 0-T that does type 2 roughing.

    That turns the smoothing pass on or off. Setting to 0 runs the smoothing pass, setting to 1 does not run the smoothing pass.
    I had no idea this was even available? Interesting!

    That's not how I read it. TNRC shouldn't care whether you use R or I & K. Where did you call up the G42 in your finish path? On the G1 Z0 line? That would undercut if it's putting the X tangent point of the TNR at Z0.

    Your initial numbers fed from the cycle start position to the start of profile (the P block). I think if you put the G42 in that line, it would not undercut the end.

    I think if you did nothing else but take out the R and replace with I,K on that 4" rad it would have run fine. That looked to me like the problem block.

    Like I said, I don't run Type 2, so I follow the rules for Type 1 which is no Z position in the P block. For me, that is always a rapid move in X axis to the first tangent point, followed by the G1 Z0 line to the start of the profile.

    Type 2 needs the Z or W in that block, so your initial numbers were legal in the sense that you were starting the profile in a G1 move. You had a .100 feed move in Z, which is plenty enough movement to pick up the TNRC.

    The only real problem was the R4 on the smoothing pass- the control is not executing that correctly with the small DOC. Getting rid of the smoothing pass by setting 5105.2 to 1 might get rid of that issue, I don't know. Seymore didn't have the problem on his Oi-TC, which is why I was wondering about the parameter settings on his and your lathes.
    99.99 percent of the time my programs run exactly as posted in post 25. I've had 2 issues ever, and both with this control.

    Brent

  13. #53
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    600

    Default

    Quote Originally Posted by yardbird View Post
    I thought type 2 was pretty much a standard option on all i controls? We have an old Fanuc 0-T that does type 2 roughing.

    Brent
    Actually mine's an Oi Mate-TB, which is kind of a stripped-down version. The machine is a 2005- not all that old, but old enough I guess.

    I don't care about the Type 2, but I wish it would rigid tap...

  14. #54
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,027
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1192

    Default

    Quote Originally Posted by yardbird View Post
    Hi Bill,

    Given the fact that the G71 cycle ignores TNRC the only time I turn it on before roughing is if I'm calling a G70 afterwards.

    I have always tried to turn on comp with a X&Z move a little more than twice the radius of the tool. Possibly turning it on with the G42 G1 Z.0 move at a smaller X would be the fix IDK?

    I run the finish tool numbers exactly as listed above in post 31 and to be honest I haven't a clue as to why the step is in the face?


    Brent
    Hello Brent,
    As I said, it depends on how/when you applied the G42. If you ran the program starting as shown below, where the tool was in X prior to the N31 Block would be the cause of the step in the face. Programming your part with the TNR compensated for in the Code, you need to start the tool with the centre of the TNR in X inline with the X centre line of the 0.005 corner radius. That X coordinate would be 1.4854 - TRN x 2. Starting at X1.4854 is at a larger diameter than where the tool needs to be to swing the radius. The control will do that for you when TNR Comp is turned on, but if the tool was at X1.4854 prior to TNR Comp being turned on, the control will take the tool to X1.4854 - TNR x 2 from the larger diameter of X1.4854. G42 turned on would cause the tool to move Right of the tool path and therefore, into the face of the work.

    N31 G00 X1.4854 Z0.1
    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
    etc

    Starting as follows will work fine.

    G00 X1.4228 Z0.1
    G42 G01 Z0.0000
    G01 X1.4854
    G03 X1.4950 Z-0.0063 I0.0000 K-0.0050
    etc
    Quote Originally Posted by yardbird View Post
    So I'm I to understand that the approach, when and where TNRC is activated has to be different when using R format than when using I&K format?
    Nothing to do with it whatsoever. I/K, or R Circular Interpolation Format is simply the method used to convey information to the control so it can calculate the centre of the arc move.

    If you Post a copy of the program that caused the step, the confusion can be explained away.


    Regards,

    Bill

  15. #55
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,486
    Post Thanks / Like
    Likes (Given)
    236
    Likes (Received)
    1507

    Default

    Quote Originally Posted by jancollc View Post
    Would be interesting to compare param 5105.2 on Yardbird's lathe and Seymore's. It sounded like Seymore's lathe was not making a full smoothing pass. Type 2 G71 follows the contour, so the smoothing pass may be kind of redundant, and turning it off might change the way the machine calculates the cycle.

    Hmmm .... I ain't got Par 5105 on mine!

  16. #56
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,027
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1192

    Default

    Quote Originally Posted by jancollc View Post
    Actually mine's an Oi Mate-TB, which is kind of a stripped-down version. The machine is a 2005- not all that old, but old enough I guess.

    I don't care about the Type 2, but I wish it would rigid tap...
    Hello jancollc,
    Type II Multi-repetitive cycles are options as are Multi-repetitive cycles themselves, but are included by most MTB to the extent that most assume that they are standard features of the control. Type II for G71/G72 was introduced with the Fanuc 6T Model B control, circa 1980.

    Regards,

    Bill

  17. #57
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    600

    Default

    Quote Originally Posted by SeymourDumore View Post
    Hmmm .... I ain't got Par 5105 on mine!
    Well whadya know! I looked at an Oi-TC manual, and they make no mention of Par 5105. The Oi-TD manual has it. My Oi-TB makes no mention of it either.

    According to the book, the final G71 pass on your lathe is not a continuous path- it does the "monotonous" part of the profile first, and then comes back and does the concaves.

    The Oi-TD manual shows a continuous smoothing pass as the final pass, and has the option to use it or not via. par 5105. They also appear to have reversed the order that pockets are finished- your's starts with the pocket closest to the chuck, and the Oi-TD starts with the pocket furthest from the chuck. (I could be misinterpreting that- those diagrams are hard for me to follow)

    Here's the manual I have been looking at for the Oi-TD:

    http://www.sharp-industries.com/site...S%20MANUAL.pdf

    After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool
    temporarily returns to the cycle start point. At this time, when there is a position whose height equals to that at the start point, the tool passes through the point in the position obtained by adding depth of cut Δd to the position of the figure and returns to the start point. Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes through the point in the obtained position (to which depth of cut Δd is added) when returning to the start point.

    Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

  18. #58
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,452
    Post Thanks / Like
    Likes (Given)
    697
    Likes (Received)
    1806

    Default

    Is it possible that the older control of the O.P. needs to use "I" and "J", instead of "R" for those radii? I know it can use R on a straight forward 90 degree angled radius, but maybe it needs the center of the radius to be defined on those radii that are not a complete quadrant?

  19. #59
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    157
    Likes (Received)
    600

    Default

    Quote Originally Posted by angelw View Post
    Hello jancollc,
    Type II Multi-repetitive cycles are options as are Multi-repetitive cycles themselves, but are included by most MTB to the extent that most assume that they are standard features of the control. Type II for G71/G72 was introduced with the Fanuc 6T Model B control, circa 1980.

    Regards,

    Bill
    Yeah, I understood it to be an option.

    Can I add rigid tapping to my Oi Mate-TB?

  20. #60
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,863
    Post Thanks / Like
    Likes (Given)
    4144
    Likes (Received)
    1422

    Default

    Quote Originally Posted by angelw View Post
    If you Post a copy of the program that caused the step, the confusion can be explained away.

    Regards,

    Bill
    Hi Bill,

    I believe this is the exact finish pass that left the step. Basically all I did was copy and paste your I&K numbers in what I already had. Same with the canned cycle, it ran without issue. I think I'm now seeing that after the G1 Z.0 I need a G1 X1.485 to position the tool to make next G3 move. It's hard for to read the I&K numbers and apply it to what the tool is going to do. I guess that is why I'm hung up on the R format.

    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
    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
    G1X3.2
    G0G40Z.5
    M9
    G0G99G40G54X14.Z10.T0
    M25
    M1


    Brent
    Last edited by yardbird; 11-30-2017 at 06:36 PM. Reason: fixed stuff...


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
  •