Could Smid Have Made a Mistake? (TNR/Facing Example)
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 29
  1. #1
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,073
    Post Thanks / Like
    Likes (Given)
    776
    Likes (Received)
    419

    Default Could Smid Have Made a Mistake? (TNR/Facing Example)

    Hi Everyone!

    I was always told to ignore TNR in lathes because it's stupid and causes more problems that it is worth, etc. Nevertheless I want to at least learn about it. Please see the attached picture. The very last sentence on the page he says, "If the above program is modified to the following version, the face will never be completed! Think about it!"

    Well I HAVE thought about it and cannot figure out why the face wouldn't be completed! It seems to me that N21-N24 which are identical) would both face the part to X-.07 the same. The chamfer even looks like it would end up being the same to me. The only difference I see is the path the tool would take to end up at X1.0 Z0.1

    Can anyone explain what I am missing on this??

    Thank you!

    img_39841.jpg

  2. #2
    Join Date
    Jan 2014
    Location
    ATL, GA, USA
    Posts
    588
    Post Thanks / Like
    Likes (Given)
    824
    Likes (Received)
    232

    Default

    Pretty sure l have that book. And it is chock FULL of typos and mistakes. Makes learning a pain in the ass. But, it's almost all there is on the subject.

    Here I think he means the tool will never reach the minimum X dimension commanded thus leaving a tit. I don't see where he has given you the TNR of the cutter being used. So I can't be certain.

    I have heard the same response from many on this forum. Once you see it done it is really easy for most turning jobs you will do and is a time saver. I have seen where guys have gone to great lengths building up spreadsheets just to work around using the built-in capabilities of TNR compensation.

    My main issue is being too lazy to record the TNR of the tools I used when I ran the program last.

  3. Likes Nerdlinger liked this post
  4. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    602
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    I believe the tool will gouge the face of the part as it immediately shifts from left comp to right comp in the line labeled "wrong." Part of that might be because of the inclusion of a Z axis component in the call. In the section before what's shown in your picture titled, Minimum Distance Required, a rule is written suggesting that comp should be added clear of the work by at least twice the tool nose radius offset. Sample one has that. Sample two does not. I don't know... break the rules... scrap the part.

    Also I believe there will be no tit as is suggested, as the machine has already completed the correct facing move by the time the errant call is made. That or as I said above, the tit will really be a divot.

    Dave

  5. Likes Nerdlinger liked this post
  6. #4
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,423
    Post Thanks / Like
    Likes (Given)
    15510
    Likes (Received)
    11366

    Default

    2nd example. Comp on, and you are not pulling out straight in Z, instead making
    an acute triangle.

    Easier to think about in a mill example. Full D/R comp on, coming into an acute
    triangle, the tool will never ever reach the point of the triangle. Even if its
    a right angle.

    Look at the incorrect approach box.

    Also bad mojo to randomly switch from left to right without clearing the part first.
    And I haven't hand coded a lathe in forever, can you even just switch sides without
    cancelling comp first?

  7. Likes Nerdlinger liked this post
  8. #5
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    602
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    Quote Originally Posted by WayneC369 View Post
    Here I think he means the tool will never reach the minimum X dimension commanded thus leaving a tit.
    Quote Originally Posted by Bobw View Post
    coming into an acute triangle, the tool will never ever reach the point of the triangle. Even if its a right angle.
    By golly I think they've both got it! Wish I'd thought of it. What can I say but... lathe noob.

  9. Likes Nerdlinger liked this post
  10. #6
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    163
    Post Thanks / Like
    Likes (Given)
    410
    Likes (Received)
    50

    Default

    Moral of the story is to not use tnr in facing. Only activate OD and ID profiles.

  11. Likes chet liked this post
  12. #7
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,073
    Post Thanks / Like
    Likes (Given)
    776
    Likes (Received)
    419

    Default

    Quote Originally Posted by Bobw View Post
    coming into an acute
    triangle, the tool will never ever reach the point of the triangle.
    Thanks, Bob! I think you're right - not only is it bad mojo, but the look ahead with cutter comp activated would cause it to cut that corner bad...meaning I do not think the tool would reach the target X-0.07 because of the tool path dictated in the following block! And the tit would get worse as the Z clearance in the following goes down.

    So:

    N24 G01 X-0.07 F0.007;
    N25 G00 G42 X1.0 Z0.1;

    would leave a smaller tit than:

    N24 G01 X-0.07 F0.007;
    N25 G00 G42 X1.0 Z0.05;

    hmmmm, I do also wonder if the G42 would gouge the part, as 13Engines suggested.

    Is it common to use cutter comp when facing? I suppose I would face the part at Z0.0 down to X-0.04 or whatever and then come out in Z and THEN activate cutter comp as I go into the profiling op.

    Thanks, again!

  13. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,370
    Post Thanks / Like
    Likes (Given)
    5012
    Likes (Received)
    3335

    Default

    Quote Originally Posted by Nerdlinger View Post
    Is it common to use cutter comp when facing?
    You only need it when you're doing a contour.
    If programming by hand, it's not necessary. If programming at the control it will most likely spit out all moves with cutter comp.
    I started programming cnc lathes back in 1989, used cutter comp in just about every situation.
    There are exceptions of course. But more often than not the people who say to not use it either don't understand it or don't want to take the time to explain it.

  14. Likes Nerdlinger, SeymourDumore liked this post
  15. #9
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,334
    Post Thanks / Like
    Likes (Given)
    964
    Likes (Received)
    2953

    Default

    Quote Originally Posted by Bobw View Post
    .......can you even just switch sides without cancelling comp first?
    Yes you can. The operator manuals have a page or two of pictures showing what the resulting toolpath will be. Applies to mills too.

  16. Likes Bobw, Nerdlinger liked this post
  17. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,947
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1618

    Default

    Quote Originally Posted by Nerdlinger View Post

    hmmmm, I do also wonder if the G42 would gouge the part, as 13Engines suggested.

    Is it common to use cutter comp when facing? I suppose I would face the part at Z0.0 down to X-0.04 or whatever and then come out in Z and THEN activate cutter comp as I go into the profiling op.

    Thanks, again!
    Hello Nerdlinger,
    The assumption would be that the TNR is 1/32", based on the X-0.070 coordinate in the facing OP (the centre line of the TNR would be just past the Workpiece Centre Line). Accordingly, a move command of G00 G42 X1.0 Z0.1 wouldn't result in interference with the face. Even if G41 hadn't been replaced with G42, the tool would be on the Left Side of Z0.1 and clear of the the face at Z Zero by 0.035". Because, G42 has been executed, the TNR would be on the Right Hand Side of the Z0.1 coordinate and because of the Look Ahead to the next move, it would finish at Z0.1025.

    What you have suggested in your last paragraph is the common practice, but if you want to face right to centre line, then you have to program the tool to go to an X coordinate, twice the TNR on the negative side of centre line. Accordingly, if the TNR is 1/32", then the X coordinate would be X-0.0625. Its common to round that value to something like X0.07; particularly when using Finger CAM.


    Regards,

    Bill

  18. Likes Nerdlinger liked this post
  19. #11
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    602
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    One thing I've been wondering about through this whole post is when the control sees the acute angle as shown in Smids' incorrect scenario, wouldn't you simply get a Comp Error from the control, in a sense making the leave-a-tit or gouge-the-face and face-will-never-be-completed arguments mute points? I'm pretty sure that on a mill if it saw that angle while proceeding in G41 comp mode it would alarm out, or does the immediate G42 transition somehow negate what the control would otherwise see as an error? Be it lathe or mill.

    Curiosity is all...

    Dave

  20. Likes Nerdlinger liked this post
  21. #12
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,073
    Post Thanks / Like
    Likes (Given)
    776
    Likes (Received)
    419

    Default

    Quote Originally Posted by 13engines View Post
    One thing I've been wondering about through this whole post is when the control sees the acute angle as shown in Smids' incorrect scenario, wouldn't you simply get a Comp Error from the control, in a sense making the leave-a-tit or gouge-the-face and face-will-never-be-completed arguments mute points? I'm pretty sure that on a mill if it saw that angle while proceeding in G41 comp mode it would alarm out, or does the immediate G42 transition somehow negate what the control would otherwise see as an error? Be it lathe or mill.

    Curiosity is all...

    Dave
    Well I sure as hell don't know but that is bugging me, too. I hope someone answers that. Maybe I'll try it for myself when I have time. Full rapids and feeds, of course.

  22. #13
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,334
    Post Thanks / Like
    Likes (Given)
    964
    Likes (Received)
    2953

    Default

    I don't see that type move causing an alarm. The only wild card in there is switching G41 to G42. I've not tried that on lathe or mill. It can be done according to the book and I think I know what the resulting move would be.

    On an acute angle the tool will move until the tool radius is tangent to both the current line and the next line. That will be the end point of the current move with no alarm generated.

  23. Likes Nerdlinger liked this post
  24. #14
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,423
    Post Thanks / Like
    Likes (Given)
    15510
    Likes (Received)
    11366

    Default

    I just tried it on a fadal, which is really fast and loose with
    the cutter comp. You can even turn comp on on an arc.

    Error: Attempt to change sides without calling G40.

    I tried running it on a scrap of 2x4. Ended up coming up
    with a nice visual of why comp in that situation is going
    to leave a giant tit. I drilled the programmed points so
    I could see where they were, and then wanted to see what
    path the endmill would take... It didn't take a path.
    Then I ran it just straight up without switching sides.


  25. Likes Nerdlinger liked this post
  26. #15
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,073
    Post Thanks / Like
    Likes (Given)
    776
    Likes (Received)
    419

    Default

    Quote Originally Posted by Bobw View Post
    I just tried it on a fadal, which is really fast and loose with
    the cutter comp. You can even turn comp on on an arc.

    Error: Attempt to change sides without calling G40.

    I tried running it on a scrap of 2x4. Ended up coming up
    with a nice visual of why comp in that situation is going
    to leave a giant tit. I drilled the programmed points so
    I could see where they were, and then wanted to see what
    path the endmill would take... It didn't take a path.
    Then I ran it just straight up without switching sides.

    Brilliant! Thanks, Bob! I did not appreciate the look ahead involved with cutter comp on until now!

    Thank you, again, everyone!

  27. Likes Bobw liked this post
  28. #16
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,073
    Post Thanks / Like
    Likes (Given)
    776
    Likes (Received)
    419

    Default

    Quote Originally Posted by Vancbiker View Post
    On an acute angle the tool will move until the tool radius is tangent to both the current line and the next line. That will be the end point of the current move with no alarm generated.
    Excellent! Understood. Thank you, Vancbiker!

  29. #17
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    9,311
    Post Thanks / Like
    Likes (Given)
    507
    Likes (Received)
    7736

    Default

    The example seems correct to me.
    As Bobw says think of the same thing in a milling control.
    It just stops short to stay inside the triangle.
    On my controls no error code would be thrown. It just looks at the next line and says "I can not fit, stop short as needed for the next move."
    This would be only single block look-ahead which we are way past now.
    Older NC tape would make a mess of things but those controls are few and far between.
    Mill a triangle pocket with comp on, you never get to the corner coordinates as that would be a disaster. The look-ahead says no, not going there.
    Think a small whole bunch of small features down in that corner, maybe cut number ten after this plunge gets wiped out so the control does the "not going in that space" due to looking down the line.

    As I type Bobw produces the most excellent example.... I'll just go sit in the corner as a useless .

    A side comp swap on the out move or next line?
    When that comp is changed what happens to the move?
    On a lathe as here out in space so never seen, on a mill in a 2x4?
    The line becomes a leadout and leadin all on one line
    Bob

  30. Likes Nerdlinger liked this post
  31. #18
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,947
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1618

    Default

    Quote Originally Posted by Bobw View Post
    I just tried it on a fadal, which is really fast and loose with
    the cutter comp. You can even turn comp on on an arc.

    Error: Attempt to change sides without calling G40.
    Hello Bob,
    A Fanuc Control permits swapping CR Comp Side Direction without having to first cancel CRC with G40. It is generally swapped through the Offset Cancel Mode (G40), but can be switched without the Cancel Mode with the resulting tool path as shown in the following picture. This picture is a Copy and Paste directly from a Fanuc manual.

    cutter-comp-direction-switch1.jpg

    I also ran an approximate facsimile program to your example, but in fresh air and the move from G41 to G42 occurred without alarm on a FS18i control.

    Regards,

    Bill

  32. Likes Bobw liked this post
  33. #19
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,334
    Post Thanks / Like
    Likes (Given)
    964
    Likes (Received)
    2953

    Default

    Quote Originally Posted by angelw View Post
    Hello Bob,
    A Fanuc Control permits swapping CR Comp Side Direction without having to first cancel CRC with G40. ......
    The same is true for Mitsubishi controls. Additionally a new D value can be called while still in G41 or G42

  34. #20
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    602
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    211

    Default

    Quote Originally Posted by Vancbiker View Post
    Additionally a new D value can be called while still in G41 or G42
    A person can use that ability to correct errors in size or form of part features. As a simple milling scenario - say your part is for whatever reason coming out longer then you want but the width is fine. Swap in a new D offset number at say a transitioning corner chamfer or radius making the tool cut one offset in parts of the tool path and another during the rest. It can even be used to correct errors in angles, because the control will start transitioning to the newly called offset at the start of what would be a linear move, and not complete the full offset adjustment until it reaches the end of the same linear move. On the fly angle error correction if you will.

    An aside - D comp offsets are modal. Even though G40 and G41 are appearing all over the place in a tools' run, (same tool creating multiple discreet part features) you only have to call the offset once. That makes for slightly less finger punching, but I always tend to recall the D offset every time G41 comes around. Reason being is, if you call G41 without a D value, the control will use the last used value (As long as one has been set since Control On or Reset (depending on parameter setting?)) even if you've since changed it from what it is currently been using. Meaning G41 alone does not read Tool Offset Register D again but continues to use only what it already knows from the last time a D call came around.

    I tend to run multiple parts at a time, and may run a station or two, turn off the coolant and ramp down the spindle and make a measurement while the machine is still idling. (Some may not be allowed this luxury.) If after measuring I want to make a slight offset change, I can do that before hitting the green button and know that it will read the new value on the very next G41/D call and therefore give me the new desired size. This saves me the hassle of having to restart the tool from the beginning just to acquire a new comp.

    Just stuff. Hope it's without errors and can help someone. (Fanuc Based)

    Dave
    Last edited by 13engines; 04-30-2020 at 10:43 PM. Reason: Insanity :-)


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
  •