587,006 active members*
3,202 visitors online*
Register for free
Login
Results 1 to 15 of 15
  1. #1
    Join Date
    Sep 2005
    Posts
    276

    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..

  2. #2
    Join Date
    Feb 2006
    Posts
    992
    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
    Join Date
    Feb 2005
    Posts
    78
    What machine? What control? What cad cam software? Face? Cross milling?
    If you use Mastercam I may be able to help.

  4. #4
    Join Date
    Sep 2005
    Posts
    276
    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
    Join Date
    Nov 2005
    Posts
    274
    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
    Join Date
    Nov 2005
    Posts
    219
    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
    Join Date
    Mar 2016
    Posts
    2

    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
    Join Date
    Jun 2015
    Posts
    4156

    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 ?
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  9. #9
    Join Date
    Jul 2016
    Posts
    8

    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.

    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


  10. #10
    Join Date
    Mar 2017
    Posts
    314

    Re: How do you use polar interpolation

    do you have a part drawing ?

  11. #11
    Join Date
    Jul 2016
    Posts
    8

    Re: How do you use polar interpolation

    @generaldisarray, Hows this?

  12. #12
    Join Date
    Mar 2017
    Posts
    314

    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.
    #

  13. #13
    Join Date
    Mar 2017
    Posts
    314

    Re: How do you use polar interpolation

    with .15 lead in
    Have you indicated you tool, so you know its on center?

    G0 C0. Y0.
    M68
    G0 X.9228 Y0. Z.25
    G97 S800 M13
    G12.1
    G1 X.9221 C.0177 F500.
    Z.05
    Z-.5906 F15.
    X0. F10.
    X-.3662
    C-.0177
    X0.
    X.9221
    Z.25 F500.
    G13.1

  14. #14
    Join Date
    Jul 2016
    Posts
    8

    Re: How do you use polar interpolation

    Hi @generaldisarray, thanks for your time in this. Sorry for the late reply I've been extremely busy (not a bad thing) and had to stop this project for now (about to restart it though) I've bought a 7mm cutter and have decided to plunge cut it. The tool is on centre too :/ I have come across a page in the manual looking for something else saying I will get better accuracy performing it as a sub routine dunno really what the difference would be but i will also try that for the experience. Thanks again for your time

  15. #15
    Join Date
    Sep 2018
    Posts
    10

    Re: How do you use polar interpolation

    From memory:

    G112
    G42 G0 X60. Z-5. C0. F.1
    G01 X40.
    C20.
    X-40.
    C-20.
    X40.
    C0.
    G40 X60.
    G113
    G0 Z10. M05


    Tool offsets c axis enabling and disabling chuck clamping, and speeds needed but that's the general idea for milling a 40x40 square on the face with x,z and c axis.
    I'll update this after I check my code reference.

    Direct reference to 3d quadratic equations.

  16. #16

    Re: How do you use polar interpolation

    G112 (some machines use G12.1)
    Rules:
    no G00 within G112
    cutter comp must be off when entering (G112) and exiting (G113) the cycle
    Behaviour:
    within G112 X works as normal, Z works as normal, C becomes a pseudo Y axis (parallel to X and Z) and is RADIAL not diametrical like X, so to program a 10x10 square the code would be:

    G112
    G01G41(cutter comp)X20.(diametrical)C10.(radial, pseudo Y axis not C axis)
    C-10.
    X-20.
    C10.
    X20.
    G40X30.
    G113

    Note: when G112 is invoked it doesn't care where the C axis is, so that cycle above if called at C0(true C) then called again at C45.(true C) Will result in the second square being 45 degrees rotated from the first.

Similar Threads

  1. Polar Interpolation
    By alps01801 in forum G-Code Programing
    Replies: 1
    Last Post: 02-18-2012, 01:11 AM
  2. Polar interpolation on 10T
    By guhl in forum Fanuc
    Replies: 7
    Last Post: 05-18-2009, 12:26 PM
  3. Replies: 0
    Last Post: 11-11-2008, 02:35 AM
  4. Polar Interpolation
    By jackson in forum Daewoo/Doosan
    Replies: 2
    Last Post: 05-20-2008, 09:17 PM
  5. G12.1 Polar cordinate interpolation
    By theemudracer in forum G-Code Programing
    Replies: 11
    Last Post: 03-27-2008, 03:27 AM

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
  •