How do you use polar interpolation


Page 1 of 2 12 LastLast
Results 1 to 12 of 14

Thread: How do you use polar interpolation

  1. #1
    Registered positiverake's Avatar
    Join Date
    Sep 2005
    Location
    United States
    Posts
    179
    Downloads
    0
    Uploads
    0

    Default How do you use polar interpolation

    I was wondering if anybody can tell me how to mill on a live tool lathe with no Y axis, G112 polar interpolation, it looks like it ties the X and C togther ? is there a formula to figure this out,you know hex,square, raduis around the corners ect..

    Similar Threads:


  2. #2
    Registered CNCRim's Avatar
    Join Date
    Feb 2006
    Location
    usa
    Posts
    949
    Downloads
    0
    Uploads
    0

    Default

    If you look at the program XC closer it is milling program, but instead XY coordinate now it is XC(where Y used to be now it is C), and X location is double.
    That's it is.

    The best way to learn is trial error.


  3. #3
    Registered oldjohn's Avatar
    Join Date
    Feb 2005
    Location
    Sydney Australia
    Posts
    78
    Downloads
    0
    Uploads
    0

    Default

    What machine? What control? What cad cam software? Face? Cross milling?
    If you use Mastercam I may be able to help.



  4. #4
    Registered positiverake's Avatar
    Join Date
    Sep 2005
    Location
    United States
    Posts
    179
    Downloads
    0
    Uploads
    0

    Default

    Mori seiki Z1000 and dawoo puma, both have fanuc controls, no cad-cam, programing at the machine, just trying to understand how the G112 works, newtexas2006 post sounds good, have'nt tryed it yet, thanks for the reply



  5. #5
    Registered
    Join Date
    Nov 2005
    Location
    USA
    Posts
    274
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by positiverake View Post
    Mori seiki Z1000 and dawoo puma, both have fanuc controls, no cad-cam, programing at the machine, just trying to understand how the G112 works, newtexas2006 post sounds good, have'nt tryed it yet, thanks for the reply


    Just look at the "C" axis as if it were "Y". Program it as a 3 axis machine using X,C and Z do not try to think to much about how it works the G112 does all the thinking for you.
    I have programmed Mori MC's fpr years and it is pretty far out how it works. Just remeber that oce the G112 is on you now have a 3 axis machining center and not a 2 axis lathe

    Bluesman



  6. #6
    Registered
    Join Date
    Nov 2005
    Location
    Only the USA
    Posts
    219
    Downloads
    0
    Uploads
    0

    Default

    Like they said, Dont think to hard, its easy after you get thru the brain strain..

    Just remember to program C in Radius dimenision's and X in Diameter dimenision's....
    you also have to turn cutter comp on and off outside the G12 thru G13 programming..

    Its fun....



  7. #7
    Registered
    Join Date
    Mar 2016
    Location
    Mexico
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    Hi, I know your post is really old. but I was wondering if you could help me with the same issue. Thanks



  8. #8
    scaring mice @ north pole deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    2173
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    hi / 2 do list :
    ... cartesian coordinate system ( x , y )
    ... polar coordintate system ( r , alfa )
    ... transition between each other ( x = r cos alfa , y = r sin alfa )

    when milling with a live tool, on a nonY lathe, it may be possible to use both cartesian and polar systems ( swicthing between them with a G code )

    imagine a toolpath made of a line + arch :
    ... line between point A and B
    ... arch between point B and C

    coordinates :
    ... A ( xa ,ya ) and ( ra, angle_a )
    ... B ( xb ,yb ) and ( rb, angle_b )
    ... C ( xc ,yc ) and ( rc, angle_c )
    ...... first paranthesis is cartesian, 2nd is polar; if you know one of them, you may determine the other, by using the transformation ( x = r cos alfa , y = r sin alfa )

    kind of pseudocode for cartesian :
    Code:
    G00 XA YA ( rapid at 1st point )
    G01 XB YB ( line to 2nd point )
    G02 XC YC ( arc to 3rd point )
    kind of pseudocode for polar :
    Code:
    G00 rA uA ( rapid at 1st point )
    G01 rB uB ( line to 2nd point )
    G02 rC uC ( arc to 3rd point )
    core G-code sample for cartesian :
    Code:
    G... ( activate cartesian system )
    G00 X... Y... ( rapid at 1st point )
    G01 X... Y... ( line to 2nd point )
    G02 X... Y... parameters_for_arch ( arc to 3rd point )
    *coordinates should be inserted where the dots are : X=x , Y=y
    * those parameters_for_arch are required, so to identify a single arch between point B and C ( otherwise, there will be an infinity of arches between those 2 points )
    core G-code sample for polar :
    Code:
    G... ( activate polar system; it may be default, so no need to specify it )
    G00 X... C... ( rapid at 1st point )
    G01 X... C... ( line to 2nd point )
    G02 X... C...  parameters_for_arch  ( arc to 3rd point )
    * coordinates should be inserted where the dots are : X = 2 * r , C = alfa
    at this point i may share a complete G-code, but ... well, your move now


    it helps to undersand all these
    if you don't have time, than is good to have a nice postprocessor, that will do the work for you ...


    if you have neither, than you may be floating for a while in between any questions ?

    Last edited by deadlykitten; 04-17-2018 at 03:52 AM.
    if you wish to be famous, first you have to succeed
    ... where is Sid ?



  9. #9
    Registered Aly-Tek's Avatar
    Join Date
    Jul 2016
    Location
    Australia
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    Hi Folks,

    I know its easy for some but I am struggling with working this whole thing out. I've managed to get two outside flat edges parallel but I am really struggling with the same for internal flats. Any assistance will be greatly appreciated.
    Code was written by me (I'm certainly no machinist/programmer on a Nakamura TW-20) and is still in progress.
    How do you use polar interpolation-20180426_074109-1-jpg
    G80G40(TWO FACE MILLING externall 8mm endmill)
    G28U0.W0.
    G98G40G97T0707
    M91
    M08
    G0C0.
    M88S1000
    X40.Z-18.
    G112
    G98G01G40X40.C10.23F1000
    G1X-25.C10.23F300
    G1X-40.
    G1C-10.23
    G1X-25.
    G1X25.
    G1X40.
    G113
    M90
    G00Z2.
    M09
    G99
    M87
    M41
    G28U0.W0.
    M01
    G80G40(INTERNALL TWO FACE MILLING 6mm endmill)
    G98G40G97T1212
    M91
    M08
    G0C0.
    M88S800
    X25.Z-15.
    G112
    G98G01G40X25.C0.5F30 (I've had to slow the feedrate right down as it seems to make the chuck "fall over" if that makes sense and alarm out all over the place to where I have to shut the machine down and restart it)
    X-10.15F30
    C-0.5
    X30.
    G113

    How do you use polar interpolation-20180426_074109-1-jpg

    Attached Thumbnails Attached Thumbnails How do you use polar interpolation-20180426_074109-1-jpg  


  10. #10
    Registered
    Join Date
    Mar 2017
    Location
    United States
    Posts
    166
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    do you have a part drawing ?



  11. #11
    Registered Aly-Tek's Avatar
    Join Date
    Jul 2016
    Location
    Australia
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    @generaldisarray, Hows this?

    Attached Files Attached Files


  12. #12
    Registered
    Join Date
    Mar 2017
    Location
    United States
    Posts
    166
    Downloads
    0
    Uploads
    0

    Default Re: How do you use polar interpolation

    metric, I almost barfed up my breakfast.

    crossing centerline is a problem. I have never put alot of effort into using polar while crossing center as I have always had Y and just use that.

    O0000
    (PROGRAM NAME - TOE PEG)
    (DATE=DD-MM-YY - 27-04-18 TIME=HH:MM - 08:47)
    (MCX FILE - C:\USERS\xxxx\DOCUMENTS\TOE PEG.MCAM)
    (NC FILE - C:\USERS\xxxxxxMY MCAM2018\LATHE\NC\TOE PEG.NC)
    (MATERIAL - STEEL INCH - 1030 - 200 BHN)
    (POST DEV - IN-HOUSE SOLUTIONS INC.)
    (TOOL - 12 - 1/4 FLAT ENDMILL - OFFSET - 12 - DIA. - .2362205")
    G20
    (TOOL - 12 OFFSET - 12)
    ( 6mmFLAT ENDMILL)
    (MPLMASTER GENERIC 3/4 AXIS LATHE)
    (MACHINE GROUP-1)
    G54
    N1 T1212
    G17 G98
    M45
    M69
    G0 C0. Y0.
    M68
    G0 X.6231 Y0. Z.25
    G97 S800 M13
    G12.1
    G1 X.6221 C.0177 F500.
    Z.05
    Z-.5906 F15.
    X0. F10.
    X-.3662
    C-.0177
    X0.
    X.6221
    Z.25 F500.
    G13.1
    M69
    G30 U0. V0. W0. H0. M05
    M30


    here are notes present in the Mastercam/mpmaster post about g112 and crossing center.

    #Polar interpolation, G112 canned cycle:
    # Polar interpolation is active only for face cutting (Right or Left).
    # Use the Caxis/Face Contour toolpath. Create geometry for the lead in
    # and lead out with the start and end position on the View number 3 tool
    # axis. All paths must start and end at the 'C0'location for output to
    # be correct. Chain the entire geometry without using Mastercam leads.
    # Set mi4 to activate!
    #
    #Axis substitution:
    # View number 3 is the C zero location on the part and corresponds to the
    # Y zero position of the "Mill Reference View". Positions are wrapped
    # from and to the diameter of the part as CCW for the Y positive direction.
    # If geometry is drawn from View number 4 (Bottom), it is correct for the
    # wrap/unwrap on the diameter. The radius of the specified diameter is
    # added to the Z position in the post. The Y axis is the only axis to
    # be converted with mill/turn.
    #
    #Simultaneous 4 Axis (11 gcode):
    # Full 4 axis toolpaths can be generated from various toolpaths under the
    # 'multi-axis' selection (i.e. Rotary 4 axis). All 5 axis paths are
    # converted to 4 axis paths where only the angle about the rotation axis
    # is resolved. Use View number 3 for the toolplane with all 'multi-axis'.
    # 4 and 5 axis toolpaths are converted assuming cross machining only!
    #
    #Y axis output and machining over part center:
    # Output Y axis motion by setting 'Rotary axis/Y axis' in the NC
    # parameter page. This requires a valid Axis Combination in your machine defintion.
    # y_axis_mch is set from the axis combination.
    # Set 'Rotary axis/Y axis' in a machine with no Y axis (y_axis_mch = 0)
    # to force linear/circular position moves in the XZ plane (g18).
    # This allows machining over the part center.
    #Caution: The machining must stay in the XZ plane at a Y fixed value
    # when y_axis_mch = zero because no C (other than the Tplane) or
    # Y positions are output!!! This occurs when selecting C_axis/Cross
    # Contour without 'y_axis_mch'. Use Mill toolpaths for cross profiling.
    #
    #NOTICE: Milling through the part center with a linear move requires the
    # geometry be broken at the centerline. Milling through the part
    # center with an arc move in the G18 plane, no Y axis and on the
    # negative side of X, reverses only the arc direction and I sign.
    #



Page 1 of 2 12 LastLast

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 do you use polar interpolation

How do you use polar interpolation