How to program both sides of a turn/groove tool OSP7000


Results 1 to 10 of 10

Thread: How to program both sides of a turn/groove tool OSP7000

  1. #1
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default How to program both sides of a turn/groove tool OSP7000

    Hi All.

    Can anyone help me with how to program using a turn/groove tool, a profile between 2 shoulders.

    Ive attached a sample profile.

    I have had partial success using a G85 LAP cycle and calling a different tool offset partway along the bottom of the groove. I,e, T030303 to T130313

    Using the attached sample profile, I started with a radial plunge at Z48 so I need the control to use what will be the trailing edge of the tool for its TNR comp as it works down the chamfer to the bottom of the groove. Will this be G41 or 42? Tool is working in -X and -Z direction

    After this it changes to T130313 halfway along the profile bottom, do I then change to G41/42 as the tool now will move in +X and - Z direction.


    For the TNR comp values: Tailstock side of tool: X0.4, Z-0.4 Chuck side of tool : X4, Z4


    This is doing my head in.

    If someone can help clarify this for me I would be so appreciative.

    A sample program based on the attached example drawing would be helpful too using a G85 Cycle


    Thanks to a great community

    Regards, Iain.

    Similar Threads:
    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-sample-turn-groove-bmp  


  2. #2
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Is this not something people do?

    Am I going about this all wrong.



  3. #3
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    hi gibsoni, let's consider a groove tool at post 01 that should deliver a part with length = 7.3

    drop the tool senzor and measure XZ inside main offset (= 01 ); here Z should be measured with the turret going towards the chuck

    now measure XZ inside another offset ( i recomand = 21 ); here Z should be measured with the turret going towards the tailstock

    if X_offset_01 <> X_offset_21, and you are not satisfied with this difference, simply input inside X_offset_21 the value from X_offset_01; on osp300 you may code this VTOFX [ 21 ] = VTOFX [ 01 ], or VTOFX [ VETLN + 20 ] = VTOFX [ VETLN ]; this 2nd code requires a T comand before; by coding it, you will avoid the need to manually update X_offset_21 each time X_offset_01 is changed; i can develop this even futher if you wish ups, i forgot you are on osp7000

    Z_offset_21 - Z_offset_01 = insert_width

    now let's write a program that will cut the face, and will cut the part off :
    Code:
        turret @ safe position
        G97 S1234 M42 M08
        T010101; more precise, since this code don't uses radius comp, T0101 ( or T101 or T+01*101 ) is more than enough
        G00 X=part_dia+5 Z0
        G01 X-2*radius F0.15 G95
        Z0.3
        G00  X=part_dia+5
        Z-7.3 T21
        G01 X-2*radius
        G00 X=part_dia+5
        stop the spindle, stop the coolant, turret @ safe position
    i hope that the code is easy to understand i don't use G85 ... kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  4. #4
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    if you wish for an G85 example, pls share an image + a code + how you wanna the cnc to behave; i will try to edit the code

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  5. #5
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Hi Team and Deadly Kitten, thanks for your help.

    Drawings attached showing the dimensioned part and also a schematic to describe tool. (refer to these when reading program and my comments)


    4MM Grooving/turning tool.

    T040404 set as standard RH tool offset (tool moving toward chuck)
    TNR X= 0.4 Z= 0.4

    T140414 set as standard LH tool offset (tool moving away from chuck)
    TNR X= 0.4 Z= -0.4

    (Not using tool P value. Choosing alternative method of indicating direction of radius centre from theoretical sharp tool point as per manual.)


    Program for tool path whether for use in G85 or just as a tool path.

    I don't know if this is correct in terms of G41/G42.

    G00 X400 Z200
    T140414 (call for +Z side of tool - traditional LH side) [edge b or e)
    G00 X22 Z23 G42 (rapid to clearance and call RH TNR comp?) [edge b or e)
    G01 X21 Z22.42 F1 (position to start) [edge b or e)
    G01 X16.32 F0.2 (feed x) [edge b or e)
    G02 X14.32 Z21.42 I0 K-1 (rad) [edge b or e)
    G01 X14.32 Z15 (position part way along flat to change to other side of tool) [edge b or e)
    G01 X14.32 Z5.81 T040404 G42 (feed to end with G42 using other side of tool - traditional RH side, -Z side to tool [edge a or d]
    G01 X20 Z2.83 (cut chamfer) [edge a or d]
    G00 X30 G40 (clearance plane) [edge a or d]


    From the attachment:

    At the start the tool is moving -X and -Z. The tool will ultimately be doing most of the cutting with the ‘a’ corner as this is the leading edge once it starts the turning along the Z axis. However I want to program using the b corner as this is the edge cutting the radius etc at this side of the groove. Does this matter? Do I call this G42 from the pre-positioning of the tool before ‘a-b’? Will the control be ok using TNR comp on the ‘b’ corner moving backwards? i.e. the theoretical sharp point is now behind the TNR centre, not infront of it.

    I would then move to ‘c’ and call T040404 which uses ‘d’ corner. I presume this continues along as G42 along the bottom of the contour, up the chamfer and out.

    Is this the correct way to do this?

    What P value would I assign to a grooving tool like this in the tool setup page if I was to use it? Happy not to use P as I think I have a handle on assigning the positive or negative TNR offsets if that’s just as good for this.

    Most of all I cant get my head around whether the control can comprehend that I am wanting it to compensate for the TNR at edge ‘b’ even though it is moving in the other direction. I.e. ‘b’ is really the trailing edge of the tool.


    Thanks very much!
    Iain.

    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-tool1-jpg   How to program both sides of a turn/groove tool OSP7000-dimensioned-groove-profile-jpg  
    Last edited by gibsoni; 06-02-2018 at 10:15 PM.


  6. #6
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    hi this is how i would program that finish cut :

    check image 01 : i draw the part, i draw the toolpath with some clearance, i convert toolpath to G-code
    Code:
          ( X23.800 Z22.420 )
        G01 X16.320 Z22.420
        G02 X14.320 Z21.420 I0 K-1
        G01 X14.320 Z05.810
        G01 X23.800 Z00.836
    putting a cut tool w4r0.4 at post 1 :
    ... i measure towards X- and Z+ at offset 01
    ... i measure towards Z- at offset 21 and i input in X_offset_21 the value from X_offset_01
    ... i input X&Z radius = 0.4 at both offsets
    ... i input P4 at offset 01 and P3 at 21
    ... it takes me much longer to write this post for you, than actually creating the code

    Code:
        G00 safe position
        rpm coolant, etc
        T010101
        G00 X23.8   Z22.42 G42 F G95
          ( X23.800 Z22.420 )
        G01 X16.320 Z22.420
        G02 X14.320 Z21.420 I0 K-1
        G01 X14.320 Z05.810 T21
        G01 X23.800 Z00.836
                           G40
        safe position, spindle stop, etc

    Not using tool P value : my dear Gibsoni, about the P quadrants, pls, learn them .... i can show you how to avoid them, i can give you a code that does not require P, but i recomand strongly to understand them; after that, you can mess with them

    Will the control be ok using TNR comp on the ‘b’ corner moving backwards ? : actually, the control does not care ... look, in comp mode, you may describe a circle with the tool, thus the ' contact point ' will go 360*

    Happy not to use P as I think I have a handle on assigning the positive or negative TNR offsets if that’s just as good for this : yup, the P again; pls be aware that you may not use negative radius comp on a lathe; if this program works, pls try to change all radius from 0.4 to -0.4 and check what happens; go slow, be safe, and you may end up with an identical part; i can show you how to use negative comp, but this is too much for now

    Most of all I cant get my head around whether ... even though it is moving in the other direction : pls remember that you may describe a full circle; i hope i will find an easy way to explain this to you, but now i can't make it easier ...

    pls check that image : you don't need the dimensions marked with yellow
    and pls consider to keep Z0 in front of the part, not towards the chuck : in this way, a negative Z is always in front of the part





    ok, now let's put that code for an osp300; i know you don't have osp300, but i shared this because i like it

    Code:
    OS01
    
    
        NGHOST G305
        IF [ VRSTT NE 0 ] NEND
    
    
        NOEX V1 = 1234   ( rpm  )
        NOEX V2 = 0.15   ( feed )
        NOEX V3 = 0.4    ( nose radius )
    
    
      ( * )
    
    
        NOEX VNSRX [ LINK      ] = V3
        NOEX VNSRZ [ LINK      ] = V3
        NOEX VNSRX [ LINK + 20 ] = V3
        NOEX VNSRX [ LINK + 20 ] = V3
        NOEX VTOFX [ LINK + 20 ] = VTOFX [ LINK ]
      ( CALL OCHK* ) ( verify offsets )
        G304
    
    
        CALL ODYNX LPOS = 23.8 LCTR = 1 ( dynamic indexing )
        T+LINK*10101 M66 G97 S+V1 M03 M08 M42 G00 X23.8 Z22.42 G42 M63 F+V2 G95 K±1 ( so to keep the clearance, regardless of radius value )
          ( X23.800 Z22.420 )
        G01 X16.320
        G02 X14.320 Z21.420 I0 K-1
        G01         Z05.810 T21
             X23.800 Z00.836
        G40
    
        NEND NOEX
    
    
    RTS


    i would call the operation like this NN01 CALL OS01 ( w4 - P4P3 ) LINK = 01; also there is no need to declare the radius inside the comp table, and there is no need to update manually the X_offset_21 if X_offset_01 is changed; the code handles that; as a result there are 5 less input fields to be edited, thus at least 25 less keystrokes


    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  7. #7
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Thanks for your response.


    A quick comment and I will come back with more later.

    But, my control happily accepts -ve TNR values and according to the attached page, simply indicates on the machine coordinates where the TNR centre lies relative to the imaginary sharp corner.

    Is this not the same as P value? Im happy to use P values if I can get it right. However this page seems to say that they are the same, at least for P: 1,2,3,4

    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-tnr-jpg  


  8. #8
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Hi,

    I just had a play on the machine using what I've learnt here and it seems to be doing what I want it to...

    EXCEPT..

    When I call the tool offset change (other side of groove/turn tool) part way along the bottom flat of the groove, the tool physically shifts backwards (opposite direction to feed) to put the other edge in the place where the first edge was. This will mark the part and cause a spring cut as well.

    How can I stop the tool from moving when I call the other side so it continues on smoothly?

    Regards, Iain.



  9. #9
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    this is it : there are 2 comp codes, one for each T, linked toghether tangentially, without unnecesary movements ( that may lead to marks on the part and others things )

    using 2 T codes inside a single comp code is not possible on your toolpath, because there is the G02, arround which is not possible to change the T or to cancel the comp

    Code:
    
        G50 S1234
    
    
        G00 X400 Z50
        G97 S500 M03 M42 ( M08 )
        T030303
        G00 X23.8   Z22.42  G42 K+1 F0.75 G95 (*1a)
          ( X23.800 Z22.420 )
        G01 X16.320 Z22.420
        G02 X14.320 Z21.420  I0 K-1
        G01 X14.320 Z21.420                   (*2)
                            G40 K-1           (*2)
        G01 X14.320 Z05.810 G42 K+1 T230323   (*3)
        G01 X23.800 Z00.836 
                            G40 K-1           (*1b)
        G00 X400 Z50 M05 ( M09 )
    M02
    
    
    (*1a : K+1 so to always begin at X23.8, regardless of radius value )
    (*1b : K-1 so to always  end  at X23.8, regardless of radius value )
    (*2  : G01 at circle end point + imaginari vector, so to minimize and )
    (control the comp-lead-out movement )
    (*3  : new comp movement for the new T, with imaginary vector, so to )
    (control the comp-lead-in movement )
    
    M02


    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  10. #10
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Thanks for you helpful response and explaining your code.

    So, are you saying that I cannot change tool offsets without cancelling G42/G41? Cancel the TNR comp and call the new offset and re-call the G42... Is that correct?


    My control (osp7000) happily changed the tool offset on the run, but it did result in the Z shift of presumably the tool width, which is not good.

    Why are some of your coordinate numbers different? Ive attached the drawing of the tool path I was trying to follow.


    I have much to learn about the use of I and K values in this way.

    This is what I used:

    G00 X400 Z200
    T140414
    G00 X22 Z22.42 G42
    G01 X16.2 Z22.42 F0.2
    G02 X4.2 Z16.42 I0 K-6
    G01 X4.2 Z12
    G01 X4.2 Z11 T040404 G42 (resulted in tool moving backwards)
    G02 X20 Z2.83 I7 K0
    G00 X30
    G00 X400 Z200 G40
    M02

    Thanks so very much.

    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-radius-groove-jpg  


  11. #11
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Why are some of your coordinate numbers different? : pls be specific image from post 10 is not the same as the one from post 5


    So, are you saying that I cannot change tool offsets without cancelling G42/G41? : no, i said that is not possible for your particular toolpath, because of the G02; however, i have succeded by breaking the long line into segments, but this causes interruptions; i did not shared that code, because, even if it works, it has auxiliary movements so, if the toolpath permits, you can change the offset without canceling the comp ( part from post 5 does not permit it )

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  12. #12
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Sorry, I didn't realise I hadn't posted that other groove.

    I am struggling to get a part to come out the right length I presume owing to TNR comp.

    Its a fairly long program.

    If you are able to look at it for me, should I post it here or PM you with it?

    Many thanks for all your help.

    Something that would be helpful on here - how to use I and K values with TNR comp cancel and what they do etc?

    Regards, Iain.



  13. #13
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Something that would be helpful on here - how to use I and K values with TNR comp cancel and what they do etc?
    pls check post13 in here : https://www.cnczone.com/forums/okuma...extra-0-a.html

    I am struggling to get a part to come out the right length ...
    i don't have time to test such programs; is faster for me to write it from zero; so, pls share an image or describe accurately :
    ... tool geometry
    ... part dimensions before and after the operation that needs improvement
    * describe a bit what bothers you that's all ...


    is better for you to receive a code that works, than for me to debug a random code that does not work yup, something like that ...



    about inputting tool data from the panel, or from code, pls check attached image; i can't believe that there is no system variable for the P quadrant

    kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  14. #14
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Thank you again for your help and offer to look at my part problem.

    I have attached drawing.

    As you can see this is a thin wall part and I finish the inside first.

    All machined with TNR comp.

    I then rough out the green section then the purple section with TN tool using G85 and then finish them both together with a finishing cut.

    I then move onto the brown segment with VN tool running again in G85 with very shall DOC.

    I run all my tool paths to 4mm past the end of the part as a clearance to part off with 3mm parting blade.

    When I go to part off I am left with about 0.5mm flat section after the point part. i.e. the part is too short and it seems as though its owing to wrong geometry in the brown section.(maybe its theoretically 0.4mm short (TNR)).


    Thanks for any ideas.


    (Sorry, I learnt to program with Z-zero at the chuck side of the part. Im stuck with it :-)



    Thanks.

    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-profile-jpg  
    Last edited by gibsoni; 06-06-2018 at 07:09 PM.


  15. #15
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Geometry of actual part in green,

    Planned geometry in yellow.

    Attached Thumbnails Attached Thumbnails How to program both sides of a turn/groove tool OSP7000-tip-geometry-jpg  


  16. #16
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    hi, in attached image :
    ... left : part dimensions and toolpath ( yellow ) with clearance dimensions
    ... right : toolpath dimensions ( or coordinates, etc )

    Code:
        with    vectors :
    
        G00 X60       Z+04.290
            X2*25.240 Z+04.290 G42 K±1 (*1)
        G01 X2*23.745          F G95
            X2*20.435 Z-01.290
                               G40 I+1 (*2)
        G00 X60
    
    (*1) ( use K+1 or K-1, so X_cnc to be equal with program value )
    (*2) ( use I+1 or I-1, so Z_cnc to be equal with program value )
    
     
       without vectors :
    
        G00 X60       Z+04.290
            X2*25.240 Z+04.290 G42
        G01 X2*23.745          F G95
            X2*20.435 Z-01.290
                               G40
        G00 X60
    
        for both samples, pls use P4
    pls, if possible, make your images easier to read kindly !

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  17. #17
    Member
    Join Date
    May 2009
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    Thanks Deadly Kitten,

    Can you please explain why I must program 1.5mm either side of the geometry I want?

    The 1.5mm in the Z- DIRECTION will be a problem as there is no material left.

    Thanks for your help.

    Regards, Iain.



  18. #18
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: How to program both sides of a turn/groove tool OSP7000

    those are clearance movements ( in & out ) : tool positioning above the part + cutting the taper + getting out of the part

    exit movement is tangential to the part geometry, so to avoid marks on the part, and reduce servo demands

    this is pretty simple; however, i don't know your setup, this is how i imagine it ...


    and why there is no material left ? isn't it the material bar ? or you are clamping the parts one by one ? but in each case, a bit of clearance, is needed

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

How to program both sides of a turn/groove tool OSP7000

How to program both sides of a turn/groove tool OSP7000