584,861 active members*
4,901 visitors online*
Register for free
Login

Thread: Radius??

Results 1 to 15 of 15
  1. #1
    Join Date
    Jan 2009
    Posts
    11

    Radius??

    I have a Heian Router 180im-b Fanuc Controller

    I am trying to take a standard downshear bit and do an x,y,z, movement while also following a specified radius. Then follow it back up the same way it came down.
    I have been told by a few different people it can't be done. But it seems so simple??
    I have come up with nothing but error messages though when trying myself.
    Help anyone??

  2. #2
    Join Date
    Feb 2008
    Posts
    267
    Not really sure about the control or machine put it sounds like you are trying something more complicated than you think. Especially if your control is erroring out.
    Sounds like you want to move from XYZ point A to XYZ point B, all the while generating a radius. If that is the case you either need to generate the path using CAD/CAM or author your own macro to calc the XYZ per any given step along the radius and interpolate to that point then calculate again.

  3. #3
    Join Date
    Jan 2009
    Posts
    11
    I want to go from X2.25 Y2.25 Z .3865 to X 2.444 Y 2.444 Z-.2615 while following a .219 radius then back again.

  4. #4
    Join Date
    Feb 2008
    Posts
    267
    What (G17-G19) plane are you in?
    Does your machine have Helical interpolation?

  5. #5
    Join Date
    Jan 2009
    Posts
    11
    g17.

    How can I tell if I have that option or not. I have some experience but not a whole lot.

    Thanks!

  6. #6
    Join Date
    Feb 2008
    Posts
    586
    If you want the radius to be in the XY plane and ramping up and down (straight line from the side) you need to have helical interpolation turned on. You just might. If you want your radius to be in a plane other than XY, XZ or YZ, then helical will still work, but you need to change panes (G17, G18 and G19) Any other planes, you need coordinate rotation (maybe it would work, never tried it) AND helical interpolation. Other than that, have someone write some code from their CAM system in pure linear that you could cut/paste in your program.

  7. #7
    Join Date
    Jan 2009
    Posts
    11
    tHE BOLDED PART IS WHAT I AM WORKING ON...

    N10G0G17G20G40G49G80G90Z0
    M211
    M400
    M401
    T3M6
    G08P1
    N20G54M91S20000X[#500-3.0]Y3.155
    N30G43H3Z.25
    G42D19
    G90G1Y2.155F150.
    N40G1G90Z-.3865X[#500/2]F243.75
    X2.155F325.
    N50Y[#501-2.155]
    N60X[#500-2.155]
    N70Y2.155
    N80X2.9175
    N90G40G49G0G64Z0M95
    M400
    M402
    T3M6
    N100G55M91S20000X[#500-3.0]Y3.155
    N110G43H35Z.25
    G42D51
    G90G1Y2.155F150.
    N120G1G90Z-.3865X[#500/2]F243.75
    X2.155F325.
    N130Y[#501-2.155]
    N140X[#500-2.155]
    N150Y2.155
    N160X2.5575
    N170G40G49G0G64Z0M95
    M400
    M401
    T4M6
    G54M91S20000X[#500-3.0]Y3.155
    N190G43H4Z.25
    G42D20
    G90G1Y2.155F150.
    N200G1G90Z-.125X[#500/2]F187.50
    X2.155F250.G61
    N210Y[#501-2.155]
    N220X[#500-2.155]
    N230Y2.155
    [B]G91G2X.194Y.194R.219Z-.2615
    G3X-.194Y-.194R.219Z.2615

    N240G1X2.2331
    Z1.0
    G0G40X6.Y6.
    N250G0G49G64Z0M95
    M12
    M22
    /G53Y0
    N260G08P0
    /M212
    M99

  8. #8
    Join Date
    Feb 2008
    Posts
    267
    Quote Originally Posted by Tuz View Post
    g17.

    How can I tell if I have that option or not. I have some experience but not a whole lot.

    Thanks!
    Run this code or something like it.

    G17
    G0X0Y0Z3.
    G1G91X1.F50.
    G2I-1.(THIS.SHOULD.RUN.FINE)
    G2Z-.1I-1.(THIS.WILL.ONLY.RUN.WITH.HELICAL)
    G1G90X0

  9. #9
    Join Date
    Jan 2009
    Posts
    11
    Thanks for your reply,what will this tell me when I run that code? What am I expecting it to do?
    I run can run a program like this: (Is this Helical?)

    N20G55M3S18000X3.75Y2.75
    N30G43H24Z0.25
    N40G1Z-0.4F100.
    N40G62G91G2J1.F200.
    G2J1.F400.
    G2J1.Z0.5F400.G61
    G90X3.75Y3.125
    G1Z-0.4F100.
    G91G62G2J0.625F200.
    G2J0.625F400.
    G2J0.625Z0.5

  10. #10
    Join Date
    Feb 2008
    Posts
    267
    Quote Originally Posted by Tuz View Post
    Thanks for your reply,what will this tell me when I run that code? What am I expecting it to do?
    I run can run a program like this: (Is this Helical?)

    N20G55M3S18000X3.75Y2.75
    N30G43H24Z0.25
    N40G1Z-0.4F100.
    N40G62G91G2J1.F200.
    G2J1.F400.
    G2J1.Z0.5F400.G61
    G90X3.75Y3.125
    G1Z-0.4F100.
    G91G62G2J0.625F200.
    G2J0.625F400.
    G2J0.625Z0.5


    I'm not a mill guy so I'm not sure what the G61 and G62 are doing but...

    if these lines...

    G2J0.625F400.(cut a circle using XY)
    G2J0.625Z0.5(cuts the same XY circle while moving in Z)

    then you have Helical and you "should" be able to do what you want.

    Provided that the Sarting point A and Ending point B are valid starting and ending points along the selected plane at the given radius.

    Good Luck!

  11. #11
    Join Date
    Jan 2009
    Posts
    11
    If I start at X 2.155 Y 2.155 Z-.125 and I want to go to X 2.349 Y 2.349 Z -.3865 while following the .219 radius will this work??

    G91G2X.194Y.194J.194Z-.2615
    G3X-.194Y-.194J-.194Z.2615

    Where does the radius call out go?

    Sorry I am failry new to all this, and I have no cad software to work from. I learn as much as I can by writing them by hand. But I am running out of time to complete this project.
    Thanks for your help!!

  12. #12
    Join Date
    Mar 2003
    Posts
    2932
    If you use I and J to specify the distance from start to center, you don't need a radius call out. I'm pretty sure your above example will not work (it will create a 3/4 moon shape). J.194 in the G02 block puts the center +.194 in Y from the start point. J-.194 in the G03 block puts the center -.194 in Y from the start point.

    I would replace the J.194's with R.219's. I back plotted it and it worked fine with R's.

    What alarm are you getting?

  13. #13
    Join Date
    Jan 2009
    Posts
    11
    Thanks I will try it.
    The alarm I was getting was ARC out of tollerance

  14. #14
    Join Date
    Feb 2008
    Posts
    267
    Quote Originally Posted by Tuz View Post
    Thanks I will try it.
    The alarm I was getting was ARC out of tollerance
    that means that the starting, ending and center call outs do not "fit".


    follow dcoupar's advice and remove the center callouts and replace with radius.
    this will force the control to fit the commanded radius into the starting and ending points.
    Good luck

  15. #15
    Join Date
    Sep 2008
    Posts
    3
    hello

    i created a macro program tot mill a given radius on a straiht line
    in case you dont want to use a concave or convex mill
    the sub progr. calculates the distance of each step in y and z
    if it has to be a smooth surface you take a one degree step or
    more for faster results

    i start at the top of the workpiece and mill then from left to right
    calculate a new y and z and go from right to left and so on
    until i reach a rotation of 90 degrees

    start is at Z0 and finish is at Z-5
    it works without radius compensation!!
    i am using a 20 mm mill with 0.8mm radius on the edge

    and i work in mm not in inches, but that must be no problem

    is this wat you have in mind ??

    sorry for the bad writting:withstupi

    %
    O0310(PARAM.RAD 5MM)
    G1902B100D100H25I0J50K0

    G0G91Z0M19
    T17
    M6

    M03S1500
    G00G90G54X-20Y-10
    G0G90G43H17D17Z50

    Z0
    G01Y-10

    G65 P9060 A1 B5 (a= degrees B=radius)

    M09
    G0G91G28Z0M5
    G91G30X0Y0P3M9
    G90M37
    M12
    M30
    %


    here folows the subprogram



    %
    O9060(SUB310)
    #3=0+#1
    N1
    IF[#3 EQ #3]THEN#3=#3+#1
    IF[#3 EQ 90]GOTO10
    #25=#2*COS[#3]
    #24=#2*SIN[#3]
    #26=5-#24
    #27=5-#25
    G01X-20

    Y#26
    Z-#27
    X125
    IF[#3 EQ #3]THEN#3=#3+#1
    IF[#3 EQ 90]GOTO10
    #25=#2*COS[#3]
    #24=#2*SIN[#3]
    #26=5-#24
    #27=5-#25

    Y#26
    Z-#27
    G01X-20
    GOTO1
    N10
    M99
    %

    greetings fzr1000

Similar Threads

  1. Replies: 8
    Last Post: 11-15-2009, 01:35 PM
  2. Outside radius
    By Shibumi in forum G-Code Programing
    Replies: 1
    Last Post: 10-30-2008, 04:27 PM
  3. radius help
    By Scott Halstead in forum GibbsCAM
    Replies: 0
    Last Post: 06-12-2008, 01:27 PM
  4. big radius
    By Dembo in forum Mechanical Calculations/Engineering Design
    Replies: 10
    Last Post: 02-01-2008, 06:01 PM
  5. Zero Radius Arc
    By Xular in forum Mach Mill
    Replies: 4
    Last Post: 12-14-2006, 04:10 AM

Posting Permissions

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