3dprintforums logo

CNCzone Network:  RFQwork :: 3Dprintforums :: Welderzone :: Google+ :: Our Facebook :: Twitter :: SiteMap



Page 1 of 2 12 LastLast
Results 1 to 12 of 13

Thread: Changing Radius To I And J Values

  1. #1
    Registered
    Join Date
    Aug 2007
    Location
    Australia
    Posts
    8
    Downloads
    0
    Uploads
    0
    Rep Power
    0

    Changing Radius To I And J Values

    I use mastercam v9. I do all my toolpaths then post them to get the g code, i find it alot quicker. Thing is in the g code all my radius's are in R values and id really prefer to use the I and J method for this. How can i change this when i post it? I read a thread about it but was all double dutch to me!

    CHRIS...

    Similar Threads:


  2. #2
    Registered
    Join Date
    Dec 2006
    Location
    usa
    Posts
    7
    Downloads
    0
    Uploads
    0
    Rep Power
    0

    post ij

    Hello
    In your post there is a line that give you the option of r or IJk . It will have a number associated with it Example(1) = r (2) =ijk
    It is in the first couple of pages. Change the number to refect the format
    you want. Save program out as another name.PST so if you make a mistake you still have the original.
    AL

    # --------------------------------------------------------------------------
    # General Output Settings
    # --------------------------------------------------------------------------
    sub_level : 1 #Enable automatic subprogram support
    breakarcs : yes #Break arcs into quadrants?
    use_rigid : 1 #Use Rigid Tapping?
    arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
    arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
    arccheck : 1 #Check for small arcs, convert to linear
    atol : .01 #Angularity tolerance for arccheck = 2
    ltol : .002 #Length tolerance for arccheck = 1



  3. #3
    Radius output is actually shorter code. Your machine doesn't care which format you use.

    Mike Mattera

    Tips For Manufacturing Training CD's, DVD's for Mastercam, SolidWorks, Inventor, G-Code Training & More
    http://www.tipsforcadcam.com


  4. #4
    Registered
    Join Date
    Aug 2007
    Location
    Australia
    Posts
    8
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    Quote Originally Posted by Mike Mattera View Post
    Radius output is actually shorter code. Your machine doesn't care which format you use.

    Mike Mattera

    We were talking about it at uni today and whilst the r or ijk values are the same thing, our teacher would prefer us to program with IJK. We lead in lead out with radius's but yeh cant use them.
    Id prefer to solid the part in master cam and gen the tool path that way, much quicker for me but we have to manual program also!

    CHRIS...



  5. #5
    Registered ObrienDave's Avatar
    Join Date
    Jun 2005
    Location
    USA
    Posts
    294
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    To quote a manual from a Cincinnati machine:

    "If the ENDPOINTS of the arc are more important, use R."
    "If the curvature of the arc is more important, use IJK."

    I had a problem when the R value was rounded off, using 180 degree arcs, the hole I was contouring came out of round by 8 to 10 thousanths.

    Switching the post to IJK or using "break arcs into quadrants" fixed the problem.

    Also when checking a contoured hole, I measure the hole at the 45 degree points.
    The reason for this is, if there is a following error in your lead screws, it will show up when BOTH axes are at MAXIMUM velocity.

    ObrienDave. MasterCam since V6. Gcode since 1983.
    The nose you punch today may belong to the butt you have to kiss tomorrow.


  6. #6
    Registered Shotout's Avatar
    Join Date
    Jun 2006
    Location
    USA
    Age
    40
    Posts
    439
    Downloads
    0
    Uploads
    0
    Rep Power
    8
    Quote Originally Posted by Mike Mattera View Post
    Radius output is actually shorter code. Your machine doesn't care which format you use.

    Mike Mattera
    Some controllers, like the Haas, do. With IJK you can cut a complete 360 degree circle with no X,Y,Z value while R requires these values. Also with IJK the circle tolerance is +/- .0005 for the radius while with R is +/-.001 for the radius. The latter reason is probably the only really compeling one when CAM/CADing a program.

    Suppose you were an idiot and suppose you were a member of Congress. But I repeat myself.
    Mark Twain


  7. #7
    Registered
    Join Date
    Sep 2007
    Location
    USA
    Posts
    8
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    Your machine may not care which one you use.

    BUT, if you use ijk it will care what ijk means.

    Fanuc treats ijk as arc tan. Most conversationals and at least one other

    control I have used - an Onsrud gantry router- treat ijk as arc center.

    With Fanuc code, R = the square root of (i squared + j squared) .

    With arc type switch set to arc center in your post, i(x) and j(y) are

    as the name implies, the arc center, as they are in a cad system.

    Some controllers have a parameter that controls how ijk is interpreted.

    ijk has more plane and directional information. K represents Z in G18(xz)

    and G19(yz) modes, and quadrant info by sign.

    R is portable across any control I've ever run ijk isn't.

    I've never heard of any difference in accuracy in modern controls though

    ijk is shorter for a circular spring pass ie j-1;j-1; or helical interpolation

    j-1 z-.01;j-1 z-.02;.

    millcat



  8. #8
    Registered ObrienDave's Avatar
    Join Date
    Jun 2005
    Location
    USA
    Posts
    294
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    It was not a problem in the control, as much as a math rounding error in MasterCam.
    And, the difference from IJK to R was only .00005.

    ObrienDave. MasterCam since V6. Gcode since 1983.
    The nose you punch today may belong to the butt you have to kiss tomorrow.


  9. #9
    Registered
    Join Date
    Sep 2007
    Location
    USA
    Posts
    8
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    At 45 deg the ball screws are moving at minimum velocity.

    At that moment they"re both moving at the same minimum rate.

    'x' ball reaches mv at 90 and 270, 'y' 0 and 180, when the other axis

    is stationary.

    millcat



  10. #10
    Registered
    Join Date
    Aug 2007
    Location
    Canada
    Posts
    2
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    Quote Originally Posted by anddsn View Post
    Hello
    In your post there is a line that give you the option of r or IJk . It will have a number associated with it Example(1) = r (2) =ijk
    It is in the first couple of pages. Change the number to refect the format
    you want. Save program out as another name.PST so if you make a mistake you still have the original.
    AL

    # --------------------------------------------------------------------------
    # General Output Settings
    # --------------------------------------------------------------------------
    sub_level : 1 #Enable automatic subprogram support
    breakarcs : yes #Break arcs into quadrants?
    use_rigid : 1 #Use Rigid Tapping?
    arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180
    arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.
    arccheck : 1 #Check for small arcs, convert to linear
    atol : .01 #Angularity tolerance for arccheck = 2
    ltol : .002 #Length tolerance for arccheck = 1
    Can someone help me to do this for mcx2?

    thanks



  11. #11
    Registered
    Join Date
    Aug 2007
    Location
    Canada
    Posts
    2
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    sorry double post

    Last edited by Bliss; 09-24-2007 at 05:43 PM. Reason: double post


  12. #12
    Registered
    Join Date
    Mar 2006
    Location
    United States
    Age
    34
    Posts
    153
    Downloads
    0
    Uploads
    0
    Rep Power
    9
    The technical term for the ijk is directional vectors. Now depending on the machine and the control the syntax for them are different. I have ran across older cnc/nc machines that won't use r so ijk is required. I have had to move that specific program from the older machine to a brand new haas mill and the control wouldn't accept the ijk as written. It was easier and quicker to go with r to get the program to run. So it all depends on the machine. I'm sure the instructor wants you to know how to use ijk if needed.



Page 1 of 2 12 LastLast

Posting Permissions



About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed