OSP7000- Cant get program to chamfer a corner


Results 1 to 9 of 9

Thread: OSP7000- Cant get program to chamfer a corner

  1. #1
    Registered
    Join Date
    May 2009
    Location
    Australia
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default OSP7000- Cant get program to chamfer a corner

    Hi Guys,

    Im pretty new to CNC but am having some success. Learnt a HEAP from you guys thankyou!

    Ive attached a drawing of a part. I cannot get it to break the edge with a slight chamfer at Z50. I don't know if it program related or TNR comp or what.


    Basic program layout is face, groove in the middle as clearance to start in heading to chuck (z-) and then pick out the rest towards Z50 with a left hand tool.


    I program in a longer tool path for the 'chamfer' so that it clears the part and any 'non concentric surface of the 2" bar. Code line in RED

    P value for tools:
    T1 = P2
    T2= P2
    T3= P2
    T4=P1
    T5=P1

    Program below.

    Thanks for your assistance guys. Im lost.

    Iain.



    (Drive Block 2" VNMG picking)
    (proven and backsaved )
    (Material 4140 2" Bright)
    (Bar 80mm out from jaws)
    (Z0 15mm from jaw face)
    (JAW PRESSURE 150)
    G50 S2000
    G90
    G95
    G40
    M42
    VZSHZ=15
    DEF WORK
    PS LC,[0,0],[99,51],4
    END
    DRAW
    NSTAR
    G00 X400 Z200
    T010101 M08

    (ROUGH FACE CYC)
    N0102 G00 X51 Z64 G96 S100 M03
    N0103 G85 NAT01 D1 F0.25 U0.5 W0.3

    (FINISH FACE CYC)
    N0201 G00 X400 Z200
    T020202
    N0202 G96 S100 M03
    G00 X51 Z64
    N0203 G87 NAT01

    (FACE CONTOUR)
    NAT01 G82 G42
    N0001 G00 X50.8 Z56.8 F0.1
    N0002 G01 X50.22 Z58.07
    N0003 G01 X25 Z62.7
    N0004 G01 X-1
    G40
    G80

    (GROOVE 4mm TOOL 'Z+ programmed')
    G00 X400 Z200
    T140414
    G00 X53 Z45
    M03 G96 S100
    G01 X46 F0.1 M08
    G00 X53
    G00 Z0
    G01 X43 F0.1
    G00 X55 M09
    G00 X400 Z200

    (LEFT HAND OD 'RH VNMG' )
    G00 X400 Z200
    T030303
    G00 X51 Z41 M08
    N0203 G96 S100 M03
    N0204 G85 NAT02 D2 F0.18 M08

    (EXT CONTOUR)
    NAT02 G81 G42
    N0000 G00 X45.3 Z41
    N0001 G01 X45.3 Z6
    N0002 G01 X47.3 Z5
    N0003 G01 X47.3 Z-1
    G40
    G80
    M09

    (RIGHT HAND OD 'LH VNMG')
    G00 X400 Z200
    T050505
    G00 X52 Z38
    N0303 G96 S100 M03
    N0304 G85 NAT03 D2 F0.18 M08 U.8 W.2
    (RH OD FIMNISH)
    G87 NAT03 D1 M08

    (EXT CONTOUR)
    NAT03 G81 G41
    N0000 G00 X45.3 Z40 F0.1
    N0001 G01 X45.3 Z45
    N0002 G01 X47.3 Z46
    N0003 G01 X47.3 Z50
    N0004 G01 X50.4 Z50
    N0005 G01 X51.22 Z50.41
    G40
    G80
    M09
    N5555

    (CHAMFER VNMG RH)
    G00 X400 Z200
    T030303
    G00 X52 Z4 M08
    G00 X48 Z3
    G96 M03 S100
    N0401 G85 NAT04 D1 F0.1

    (CHAMFER CONTOUR)
    NAT04 G81 G42
    G00 X47.3 Z2
    G01 X43.3 Z0
    G01 Z-2
    G40
    G80
    G00 X400 Z200 M09

    (PARTING)
    T121212
    G96 M03 S100
    G00 X53 Z0 M08
    G01 X5 Z0 F0.1
    G01 X-1.0 F0.03 M03 G97 S1000 F.03
    M05 M09

    (BAR RESET)
    G00 X400 Z200 M09
    N9999
    G00 X400 Z200
    T101010
    G00 X-10 Z65
    M00 (PULL BAR)
    G00 X400 Z200
    GOTO NSTAR
    M02

    Similar Threads:
    Attached Files Attached Files


  2. #2
    Registered OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1049
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    T5 is using P1 as if it were a boring bar. Should be P4 with proper radius.



  3. #3
    Registered
    Join Date
    May 2009
    Location
    Australia
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    Thanks so much for taking the time to look at this Okumawiz,, I really appreciate it.


    I did think the P value was wrong so went and checked a drawing I have - attached. (p value.png)


    I understood that although the turret is on the back side of the spindle (as the user looks at it) and the tooling is upside down, that nothing has changed as the tool is theoretically just rotated about the spindle axis 180 degrees and the X+ and Z+ direction haven't changed.


    I must be wrong in thinking this way.


    I have just looked up another document I have - P value Okuma (attached)


    This seems to be correct.


    So it does matter which side of spindle you are on?



    Once again, I am very thankful for you taking the time to help me.


    Regards, Iain.

    Attached Thumbnails Attached Thumbnails OSP7000- Cant get program to chamfer a corner-p-value-okuma-jpg   OSP7000- Cant get program to chamfer a corner-p-value-png  


  4. #4
    Registered
    Join Date
    May 2009
    Location
    Australia
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    Okumawiz,

    Jumped on the machine this morning, changed the P value to the correct one and re-ran the program.

    The X-Z positions seem correct as I watch them. The tool moved in a 45 degree motion, its just completely clears the corner and so doesn't cut.

    As I watched the X-Z positions I noticed they were correct per the programmed contour in the lap cycle. I do not usually see this on a chamfer or radius with TNR comp active. I presume I usually see the actual tool position having compensated for the TNR.

    So- I wonder if then TNR comp is not actually turning on. This would make sense as far as it missing the part - it is using the imaginary sharp corner.


    Is there something in the program that is not allowing it to turn on?


    Thanks for your help. Iain.



  5. #5
    Registered
    Join Date
    May 2009
    Location
    Australia
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    Ok....

    Someone told me that the control wont recognise the G41,G42 etc when on the G81/82 line.

    I moved the G41 down to the first line of the contour where it rapids to the start of the actual contour/profile and it worked like a charm.

    Is this the accepted protocol?

    Thanks again for your help okumawiz!

    (EXT CONTOUR)
    NAT03 G81
    N0000 G00 X45.3 Z40 F0.1 G41
    N0001 G01 X45.3 Z45
    N0002 G01 X47.3 Z46
    N0003 G01 X47.3 Z50
    N0004 G01 X50.4 Z50
    N0005 G01 X51.22 Z50.41
    G40
    G80
    M09
    N5555



  6. #6
    Registered OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1049
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    The G41 should not be on the G81 line. Move it down to the G00 line that is most likely the issue. Spindle rotation direction doesn't matter P4 is correct. Values will not be exact program values if comp is on unless comp value is zero. What TNR value are you using? it will not cut the corner if the actual tool is .03" but comp is .015" for example.

    Experience is what you get just after you needed it.


  7. #7
    Registered OkumaWiz's Avatar
    Join Date
    Apr 2009
    Location
    United States
    Posts
    1049
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    What the...

    we replied at the same time?!

    :-)

    Experience is what you get just after you needed it.


  8. #8
    Registered
    Join Date
    May 2009
    Location
    Australia
    Posts
    32
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    Thanks Okumawiz!

    Your help is truly appreciated and your contribution to this forum is second to none - thanks mate.



  9. #9
    Registered deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2462
    Downloads
    0
    Uploads
    0

    Default Re: OSP7000- Cant get program to chamfer a corner

    I have just looked up another document I have - P value Okuma (attached)
    hy gibsoni, in image 1, X+ is towards up, and the tool that has to cut your part is in P4, just like mr Wizard noticed

    in image 2, X+ is towards down, thus you have 2 images about the same thing, but they are a bit messy

    you still have a sensitive side with this rad comp

    program to chamfer a corner
    by the way, if chamfer is 0.25, don't cut it at 0.3mm/rot, because the tool will stay on it less then a spindle revolution; if you wish for esthethic chamfers, try to keep the tool on them for a few spindle revolutions, thus use a feed < chamfer / 4

    So it does matter which side of spindle you are on?
    do you have a 2nd spindle, or a 2nd turret ? even so ...

    I moved the G41 down to the first line of the contour where it rapids to the start of the actual contour/profile and it worked like a charm.Is this the accepted protocol?
    kind of, check attached image from igf

    stuff ( protocols if you wish, from basic to next-level ) about compensation :
    - basic compensation ( comp radius = tool nose radius, toolpath = part )
    - virtual compensation ( comp radius = 0, toolpath = offset part )
    - lead-in & lead-out movement ( aproaching & canceling compensation )
    - imaginary vectors
    - imaginary shapes
    - VNSR* & VNRPN
    - ctr

    kindly


    Attached Thumbnails Attached Thumbnails OSP7000- Cant get program to chamfer a corner-01-png   OSP7000- Cant get program to chamfer a corner-02-png   OSP7000- Cant get program to chamfer a corner-03-png  
    Last edited by deadlykitten; 02-07-2019 at 08:50 AM.
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg


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

OSP7000- Cant get program to chamfer a corner

OSP7000- Cant get program to chamfer a corner