Problem with program or tool comp
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 42
  1. #1
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default Problem with program or tool comp

    I have been playing with this part, trying to get it make the part correctly. On the finish cut, it makes a little step right under chamfer. Also this last time i run it, it gave me an error and halted the finish right where the taper meets the next diam. This is just something i made up to learn on the machine so if its not perfect no big deal. Just wanted to get the machine half way figured out before i need to do a real job. The error was something about causing excesive under cut. This is on a fanuc oi control.
    Attached Thumbnails Attached Thumbnails 20200213_130241.jpg   20200212_233148.jpg  

  2. #2
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    Actually that other picture wasnt the program i ran when getting the error message. This is it.
    Attached Thumbnails Attached Thumbnails 20200213_160738.jpg   20200213_160730.jpg  

  3. #3
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    I figured out the reason for the error. The one inside radius is only .06 but tool is set up in the machine as .062. But why does it make the little cut right before the chamfer.

  4. #4
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    746
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    246

    Default

    Quote Originally Posted by cuttergrinder View Post
    I figured out the reason for the error. The one inside radius is only .06 but tool is set up in the machine as .062. But why does it make the little cut right before the chamfer.
    your start point or end point numbers are wrong.
    look at your rad on z axis and if its a .062 rad it should start .062 thousanths from your end point, on the x it should be .124 from your x start point.

    is this finger banged? or cad.
    also you have to put the rad of the tool in the offsets not the rad of the part you want.

  5. #5
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    This program was written with bobcad. I did put the radius of the tool in the offsets of the machine. This insert has a .062 radius.

  6. #6
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    The program was made with bobcad but i did type into the control so i could have made a typo.

  7. #7
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    746
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    246

    Default

    Sorry I didnt see you corrected the rads in your above post.
    thats a big tool rad. nothing wrong with it, I just assumed you used a .032r.
    as far as your tool comp I never use it on a lathe so I wouldn't be one to offer any help. undercuts are usually cause by having the wrong numbers as well as the face making a false cut is usually cause by not turning on the tool comp farther ahead and I believe you also have to have a false move bigger than the tool nose rad. .
    dont know about the newer machines but older ones always needed that.

  8. Likes Lastuneste liked this post
  9. #8
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    Thanks for the reply. I believe the error message was because my tool radius in the offset page of the lathe is listed as .062 and By mistake for the one radius in the program, I typed .06 instead of .062, so it is probably saying that my tool radius is too big. Yes now the problem I need to fix is that false cut on the face. Bobcad turns on the G42 comp as the picture shows. Is it ok to apply the comp before the 2 G71 lines?

  10. #9
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    746
    Post Thanks / Like
    Likes (Given)
    66
    Likes (Received)
    246

    Default

    Quote Originally Posted by cuttergrinder View Post
    Thanks for the reply. I believe the error message was because my tool radius in the offset page of the lathe is listed as .062 and By mistake for the one radius in the program, I typed .06 instead of .062, so it is probably saying that my tool radius is too big. Yes now the problem I need to fix is that false cut on the face. Bobcad turns on the G42 comp as the picture shows. Is it ok to apply the comp before the 2 G71 lines?
    Oh yeah your using g71 also, I couldn't answer that question at all. I am sure angle or some other guys would have a good answer for that.

  11. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,752
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1477

    Default

    Hello cuttergrinder,
    Post a picture of the Offset Page where you have the Tool Data registered. Also, Post a copy of your part drawing.

    Regard,

    Bill

  12. #11
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,659
    Post Thanks / Like
    Likes (Given)
    1261
    Likes (Received)
    1425

    Default

    Quote Originally Posted by cuttergrinder View Post
    The program was made with bobcad but i did type into the control so i could have made a typo.
    Typing cam generated programs into a control is tedious operation, fraught with error.

    You appear to have a card slot there to the left of the screen.

    Get yourself a CF card, a PCMCIA adapter for it, and a CF card reader for your pc. All cheaply available. Do your homework on here first to make sure you get a CF card that will work.

  13. #12
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    Quote Originally Posted by gregormarwick View Post
    Typing cam generated programs into a control is tedious operation, fraught with error.

    You appear to have a card slot there to the left of the screen.

    Get yourself a CF card, a PCMCIA adapter for it, and a CF card reader for your pc. All cheaply available. Do your homework on here first to make sure you get a CF card that will work.
    I have a card and reader ordered but at the time i didnt know i needed a pcmcia adapter. The caed is supposed to come today. This machine also has a rs 232 port but its in the back where you turn on the power. The cord is pretty long though.

  14. #13
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    I fixed the one incorrect radius in the program and i also put my g42 before the G71 cycle. It finishes the whole part now but still puts the little step in the face. It also doesnt seem like it picked up the comp. The outside radii that are supposed to be .062 are sharp.
    Attached Thumbnails Attached Thumbnails 20200214_124525.jpg   20200214_124422.jpg   20200214_130819.jpg  

  15. #14
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    Here is the rest of the program
    Attached Thumbnails Attached Thumbnails 20200214_124356.jpg  

  16. #15
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,752
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1477

    Default

    Quote Originally Posted by cuttergrinder View Post
    But why does it make the little cut right before the chamfer.
    Hello cuttergrinder,
    The issue with the Step at the front end of the parts has Zero to do with TNR Compensation. I suspect that its caused by:
    1. The Z Workshift is incorrectly set for the Workpiece
    or
    2. The Geometry, or Wear Offset for the tool being used is incorrect.

    In the following picture, I believe that the features that are indicated with Coordinates will correspond to your actual Workpiece.

    tnr-comp1.jpg

    You can Check this out via MDI by calling the Tool with its Offset and move the tool by Hand-wheel to touch the end of the Workpiece; observing the Absolute Z coordinate display will tell you where the end of the Workpiece is. Further, if you touch the Tool on the Z surface that is cut, the Absolute Z display should show a value equal to the Z Finish Allowance set in the 2nd G71 Block.

    When using a Tool Set as a Type 3 Tool (providing it actually is a Type 3 Tool), then the True Tool location when cutting surfaces that are parallel to the respective X or Z axis, is the same whether TNR Comp is used or not. Accordingly, check the Offset setting for the Tool involved, and the Workshift Offset.

    Many Fanuc Control Models ignore TNR Comp completely in G71. If TNR Comp is used in the G71 profile definition it will be correctly executed when the G70 cycle is run. The only Fanuc models that it could be consistently said that TNR Comp in G71 was a feature are FS10, 11 and 12 controls and was well documented in the Fanuc Manual.

    Regards,

    Bill

  17. #16
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    You may be right about the offset not being set correctly. I only have one tool in the machine and it is not set by the tool setter because I cant get it to work either. It gives me an alarm message every time I try to press the button to bring it down. Whats weird is it makes the chuck come on when you press the tool setter button. Seems like it is orienting the spindle. Our Mazak never does this. The tool wear offsets are set to zero for this tool.

    I used this tool to face the part by hand and then pressed the offset button, then work offset soft key, then scroll down to G54 until the "Z" is high lighted of the G54 and then pressed Z 0 and pressed the measure soft key and the display changes to z zero. Then I run the program. It never cuts this step into the part while roughing. It does it all on the finish pass while using the G70.

  18. #17
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    I think I figured this out(hopefully). When I set my 54, I didn't have the tool offset active and that tool has a -.0329 offset. I guess what I need to do is use mdi to call up the tool offset before I set the g54. On a Mazak you don't have to do this. On a Mazak, if the tool is in position to cut, the tool offset is always active. Even when you just start up the machine(after homing). On this fanuc, if I never turned off the tool offset, why doesn't it stay active. It seems to loose the tool offset as soon as the program ends. The machine keeps the G54 active.

  19. #18
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,752
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1477

    Default

    Quote Originally Posted by cuttergrinder View Post
    I think I figured this out(hopefully). When I set my 54, I didn't have the tool offset active and that tool has a -.0329 offset. I guess what I need to do is use mdi to call up the tool offset before I set the g54. On a Mazak you don't have to do this. On a Mazak, if the tool is in position to cut, the tool offset is always active. Even when you just start up the machine(after homing). On this fanuc, if I never turned off the tool offset, why doesn't it stay active. It seems to loose the tool offset as soon as the program ends. The machine keeps the G54 active.
    Hello cuttergrinder,
    What you're saying is the reason for the step doesn't make sense. The G70 Cycle is executed using the same Tool as used in the Roughing (G71) Cycle, without any interruption between the G71 and G70 Cycle. You're saying that the Step occurs when the G70 Cycle is run and not the G71 Cycle. Accordingly, if you had an issue with the G54 Workshift Offset, it would be observed in both the G71 and G70 Cycle. The Finish Allowance specified in Z is only 0.005"; the Step appears to be far greater than that.

    After you have run the G70 Cycle, and with the Step present the face at the start, is the measured dimension shown with the question mark in the following picture, 1.25"

    tnr-comp1.jpg

    Also, you have specified TNR Comp Start before the G71 Cycle and before the P specified Block N100 and the TNR Comp Cancel before the call of G70. Therefore, when the G70 Cycle executes the Part Profile, commencing at N100, it will do so with TNR Comp Turned Off.

    Regards,

    Bill

  20. #19
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    I have run the program multiple times with the G42 in different locations and the result is always the same. Im going to go to the shop and play with this and try to figure this out. During work hours, I have so many other things going on, I just don't have to play with it. I have 5 huge 34" dia. bronze bushings I am working on the 50" manual Lathe.

    Should the machine keep the tool offset active as long as I don't cancel it(even when powering the machine down). It does keep the G54 active even after powering it down.

  21. #20
    Join Date
    Mar 2007
    Location
    Salem,Ohio
    Posts
    623
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    313

    Default

    I will check the dimension when i get to the shop. Here is a picture of whats keeing me busy.
    Attached Thumbnails Attached Thumbnails 20190917_084418.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
  •