Newbie G19 j and K explanation please


Results 1 to 9 of 9

Thread: G19 j and K explanation please

  1. #1
    Registered slowdigits2's Avatar
    Join Date
    Nov 2014
    Location
    canada
    Posts
    74
    Downloads
    0
    Uploads
    0

    Question G19 j and K explanation please

    Hi all I hoping someone could give me a good explanation of how you go about figuring out the j and K values when cutting an arc G19 I'm trying to create a small arc to follow the radius of a pipe im cutting out of, I have loaded the gcode for the part, when i get to the radius part i get an error incorrect arc data , if try to use just the R i get an error about using g41-g43 in g19 if i take out the radius the program runs fine, the other radius were written by another programmer they run in g17 . Thanks in advance all
    G17 G20 G40 G80
    G90 G54
    M6 T1 (scribe)
    G90 G0 X1.1 Y-0.625
    G0 Z1.0
    S1000 M3
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-0.9 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    M6 T3 (cut)
    M3 S930
    G90 G0 X6.25 Y-0.75
    G0 Z0.1 M08
    G1 G41 X5.625 Y-0.75 Z-0.950 F5.
    X1.9364 G1 F12.
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    G19
    G2 J0.75 K1.3 (this arc) (is moving to y0.75)(if i replace this line with G1 y0.75 no problems)
    G17
    G1 X-1.9364
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    G19
    G3 J-0.75 K1.3 (This arc)(moving to y-0.75)(if i replace this line with G1 y-0.75 no problems)
    G17
    G1 X5.5
    G0 Z10. M9
    G0 G40 X0 Y3.5
    G91 G28 Z0.
    G91 G28 Y0.
    G90
    M30

    Similar Threads:


  2. #2
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    You cannot change planes while cutter comp ( G41 or G42 ) is applied
    - comp is active on the XY(IJ) values when running G17, the Z value allows adjustment of the cutting tip ( which is not comped )
    - G19 uses the YZ(JK) plane, comp is not applied to the X values

    I suggest programming a tool centreline path, and remove the G41 ( what control ?..........some m/cs require a D address )
    - planes then can be switched from one to another

    Some controls may have a 3D option for cutter comp ( it could be a G43 to you, going by your comments ) .....make sure you have it before going too far into working this out.....as it does cost extra



  3. #3
    Member
    Join Date
    Jan 2009
    Location
    United States
    Posts
    103
    Downloads
    1
    Uploads
    0

    Default Re: G19 j and K explanation please

    Made changes to get the arcs to cut properly, cutter comp will be a problem as Superman stated.
    you could write a macro to calculate the center line offset geometry that will include tool dia. changes.
    If you do a lot of this shape in a family of parts then it will be worth the effort.

    G17 G20 G40 G80
    G90 G54
    M6 T1 (scribe)
    G90 G0 X1.1 Y-0.625
    G0 Z1.0
    S1000 M3
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-0.9 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    M6 T3 (cut)
    M3 S930
    G90 G0 X6.25 Y-0.75
    G0 Z0.1 M08
    G1 G41 X5.625 Y-0.75 Z-0.950 F5.
    X1.9364 G1 F12.
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    G19
    G3 Y0.75 J0.75 K1.3 (CHANGED TO G3, ADDED Y0.75)
    G17
    G1 X-1.9364
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    G19
    G2 Y-0.75 J-0.75 K1.3 (CHANGED TO G2, ADDED Y-0.75)
    G17
    G1 X5.5
    G0 Z10. M9
    G0 G40 X0 Y3.5
    G91 G28 Z0.
    G91 G28 Y0.
    G90
    M30



  4. #4
    Registered slowdigits2's Avatar
    Join Date
    Nov 2014
    Location
    canada
    Posts
    74
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    sorry for taking so long to get back to this I run a mazak 430 A vertical mill, so i assume you mean remove the cutter comp G41 and add half of the cutter dia which would be .250( its a .5 end mill) to all dimensions? the problem i have is not fully understanding the the I J formula for radius, i can and have used th R but it does not produce the proper results in this situation the 4 radius are .5" I have upload loaded what the part looks like x0 y0 is in the very center of the part the reduced section is 1" the ends are 1.5 any help would be great this part is ran 1 at a time from all diffrent materialG19  j and K explanation please-img_1857-1-jpg

    Thanks





    Quote Originally Posted by Superman View Post
    You cannot change planes while cutter comp ( G41 or G42 ) is applied
    - comp is active on the XY(IJ) values when running G17, the Z value allows adjustment of the cutting tip ( which is not comped )
    - G19 uses the YZ(JK) plane, comp is not applied to the X values

    I suggest programming a tool centreline path, and remove the G41 ( what control ?..........some m/cs require a D address )
    - planes then can be switched from one to another

    Some controls may have a 3D option for cutter comp ( it could be a G43 to you, going by your comments ) .....make sure you have it before going too far into working this out.....as it does cost extra




  5. #5
    Registered slowdigits2's Avatar
    Join Date
    Nov 2014
    Location
    canada
    Posts
    74
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    mcode i tried this but the g3 makes the arc cut in the wrong direction goes in the -z direction if i try to change it to g2 the arc becomes distorted



  6. #6
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    It looks like a tensile test piece ??

    Just trying to picture the actual path you want the tool to perform
    - why not just break the path into 2 contours ... not having the tool do a vertical arc "jump" on either end ??

    or
    - insert a Z move at Y0 ( this would create a vee type movement) - LH end
    - have the tool come right out of the part, move to next point before going back in ) - RH end

    Question.....What codes do you use for tool length compensation ( normally G43 H<tool #> )
    - & how do you call in tool radius from the offsets ( normally G41 D<tool #> )....I've put both in in the correct placement, and edited a little

    Code:
    G20  ( units check code, is m/c in inch setting? )
    G0 G17 G40 G80 G90 G94  (safety codes = rapid, XY plane, comp OFF, cancel canned cycle, absolute, feed per minute )
    G54 ( work co-ord system )
    ()     (<--- use empty comments for separating sections )
    M6 T1      (scribe)
    G90 G0 X1.1 Y-0.625
    S1000 M3
    G43 H1 Z1. ( goto Z1 while ADDING the value in H1 to the "distance of spindle to part origin" ) (G54 Z<value> is a -ive, tool length "H"<value> is +ive)
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-1.1 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    G0 Z1. M9
    M5
    G91 G28 Z0. ( retract to Z home )
    G90
    M1
    ()
    M6 T3      (cut)
    G90 G0 X6.25 Y-0.75
    M3 S930
    G43 H3 Z.1 M8
    G1 Z-0.950 F5
    G41 D3 X5.625 Y-0.75 F12. ( G41 actually forces a line move )
    X1.9364
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    Y0. Z0.  (<----- lift Z while going to centre)
    Y0.75 Z-0.950 (<--- line going back to depth )
    X-1.9364 
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    Z0.1 ( <--- lift out of part)
    Y-0.75 ( go to other side )
    Z-0.950 ( descend down to depth )
    X5.5
    G40 Y-1.2 ( cancel comp, while moving away from part )( move must be larger than comp value in the machine )
    G0 Z10. M9
     ( G0 G40 X0 Y3.5 ) (<--- not required )
    G91 G28 Z0. ( retract to Z home )
    G91 G28 Y0. ( move to Y home )
    G90
    M30




  7. #7
    Member
    Join Date
    Jan 2009
    Location
    United States
    Posts
    103
    Downloads
    1
    Uploads
    0

    Default Re: G19 j and K explanation please

    Superman has the right idea, Also If your cutting on the top of the pipe then you should
    cut the 2 long contours first then just cut the ends last. you can rough out the ends leaving
    a small amount of material that can easily be finished in a another op. you can also cut the
    whole contour using strait lines on the ends instead of arcs since your just cutting through the pipe
    which will allow you to use cutter comp.

    I changed the program to cut the arcs the other way by reversing the k values and arc direction.
    I would also insert changes that Superman referred to using G43 H, and G41 D.

    G17 G20 G40 G80
    G90 G54
    M6 T1 (scribe)
    G90 G0 X1.1 Y-0.625
    G0 Z1.0
    S1000 M3
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-0.9 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    M6 T3 (cut)
    M3 S930
    G90 G0 X6.25 Y-0.75
    G0 Z0.1 M08
    G1 G41 X5.625 Y-0.75 Z-0.950 F5.
    X1.9364 G1 F12.
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    G19
    G2 Y0.75 J0.75 K-1.3 (CHANGED TO -K, ADDED Y0.75)
    G17
    G1 X-1.9364
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    G19
    G3 Y-0.75 J-0.75 K-1.3 (CHANGED TO -K, ADDED Y-0.75)
    G17
    G1 X5.5
    G0 Z10. M9
    G0 G40 X0 Y3.5
    G91 G28 Z0.
    G91 G28 Y0.
    G90
    M30

    just as in cutting an arc in G17 XY IJ, in G19 J is the distance in Y from the start of the arc to the center
    and K is the distance in Z from the start of the arc to the center. the arc direction is determined by looking
    from the positive X

    hope that helps



  8. #8
    Registered slowdigits2's Avatar
    Join Date
    Nov 2014
    Location
    canada
    Posts
    74
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    I will try this see what happens im very new to all this trying to teach myself as i go with the help in the fourms for everyone thanks again ( I always run it above or with no material in the machine i just do my touch off well above the vise
    Quote Originally Posted by Superman View Post
    It looks like a tensile test piece ?? yes it is

    Just trying to picture the actual path you want the tool to perform
    - why not just break the path into 2 contours ... not having the tool do a vertical arc "jump" on either end ??

    or
    - insert a Z move at Y0 ( this would create a vee type movement) - LH end
    - have the tool come right out of the part, move to next point before going back in ) - RH end

    Question.....What codes do you use for tool length compensation ( normally G43 H<tool #> ) the tool offset is already in the tool directory when the tool is called up it applies the .250 offset and the tool length
    - & how do you call in tool radius from the offsets ( normally G41 D<tool #> )....I've put both in in the correct placement, and edited a little

    Code:
    G20  ( units check code, is m/c in inch setting? )
    G0 G17 G40 G80 G90 G94  (safety codes = rapid, XY plane, comp OFF, cancel canned cycle, absolute, feed per minute )
    G54 ( work co-ord system )
    ()     (<--- use empty comments for separating sections )
    M6 T1      (scribe)
    G90 G0 X1.1 Y-0.625
    S1000 M3
    G43 H1 Z1. ( goto Z1 while ADDING the value in H1 to the "distance of spindle to part origin" ) (G54 Z<value> is a -ive, tool length "H"<value> is +ive)
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-1.1 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    G0 Z1. M9
    M5
    G91 G28 Z0. ( retract to Z home )
    G90
    M1
    ()
    M6 T3      (cut)
    G90 G0 X6.25 Y-0.75
    M3 S930
    G43 H3 Z.1 M8
    G1 Z-0.950 F5
    G41 D3 X5.625 Y-0.75 F12. ( G41 actually forces a line move )
    X1.9364
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    Y0. Z0.  (<----- lift Z while going to centre)
    Y0.75 Z-0.950 (<--- line going back to depth )
    X-1.9364 
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    Z0.1 ( <--- lift out of part)
    Y-0.75 ( go to other side )
    Z-0.950 ( descend down to depth )
    X5.5
    G40 Y-1.2 ( cancel comp, while moving away from part )( move must be larger than comp value in the machine )
    G0 Z10. M9
     ( G0 G40 X0 Y3.5 ) (<--- not required )this put the table back as close as possible to the door so we can load the next partG91 G28 Z0. ( retract to Z home )
    G91 G28 Y0. ( move to Y home )
    G90
    M30




  9. #9
    Registered slowdigits2's Avatar
    Join Date
    Nov 2014
    Location
    canada
    Posts
    74
    Downloads
    0
    Uploads
    0

    Default Re: G19 j and K explanation please

    superman that worked great i did take the G43 H1 Z1. and replaced it with g0 z.5 I dont think the mazak recognizes the the H1 I ran it both ways same results or am i missing something the the v move at the ends make things alot simpler and i would rather keep the program cutting the sample all at one pass we are very busy some times and minutes add up quick thanks again for your help if you have any other thoughts or ideas please feel free to share them as i said I'm very new we cut material from .125 to .750 adjusting feed rates for thicker material

    - - - Updated - - -

    Thanks for you help again MCODE
    Quote Originally Posted by mcode View Post
    Superman has the right idea, Also If your cutting on the top of the pipe then you should
    cut the 2 long contours first then just cut the ends last. you can rough out the ends leaving
    a small amount of material that can easily be finished in a another op. you can also cut the
    whole contour using strait lines on the ends instead of arcs since your just cutting through the pipe
    which will allow you to use cutter comp.

    I changed the program to cut the arcs the other way by reversing the k values and arc direction.
    I would also insert changes that Superman referred to using G43 H, and G41 D.

    G17 G20 G40 G80
    G90 G54
    M6 T1 (scribe)
    G90 G0 X1.1 Y-0.625
    G0 Z1.0
    S1000 M3
    G1 Z0.45 F25.
    X1.
    Y0.625
    G0 Z1.
    X-0.9 Y-0.625
    G1 Z0.45 F25.
    X-1.
    Y0.625
    M6 T3 (cut)
    M3 S930
    G90 G0 X6.25 Y-0.75
    G0 Z0.1 M08
    G1 G41 X5.625 Y-0.75 Z-0.950 F5.
    X1.9364 G1 F12.
    G3 X1.275 Y-0.5 I-0.6614 J-0.75
    G1 X-1.275
    G3 X-1.9364 Y-0.75 I0 J-1.
    G1 X-5.875
    G19
    G2 Y0.75 J0.75 K-1.3 (CHANGED TO -K, ADDED Y0.75)
    G17
    G1 X-1.9364
    G3 X-1.275 Y0.5 I0.6614 J0.75
    G1 X1.275
    G3 X1.9364 Y0.75 I0 J1.
    G1 X5.875
    G19
    G3 Y-0.75 J-0.75 K-1.3 (CHANGED TO -K, ADDED Y-0.75)
    G17
    G1 X5.5
    G0 Z10. M9
    G0 G40 X0 Y3.5
    G91 G28 Z0.
    G91 G28 Y0.
    G90
    M30

    just as in cutting an arc in G17 XY IJ, in G19 J is the distance in Y from the start of the arc to the center
    and K is the distance in Z from the start of the arc to the center. the arc direction is determined by looking
    from the positive X

    hope that helps




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

G19  j and K explanation please

G19  j and K explanation please