G13 Circular Milling on FANUC


Results 1 to 13 of 13

Thread: G13 Circular Milling on FANUC

  1. #1
    Registered
    Join Date
    May 2012
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default G13 Circular Milling on FANUC

    Hello all,

    Attached is a scanned diagram from our HAAS milling machine manuals showing the G13 command, which is an incremental circular pocket milling command.

    This G13 command does not exist on our newer Fanuc 16i-M controller for our horizontal boring mill.

    Using the macro found here:
    Circle Milling A Bolt Hole Pattern : Modern Machine Shop
    I have been able to circular mill in a bolt hole pattern but in a single cut.

    There must be a way to take multiple cuts as in this G13 haas cycle?

    Any thoughts? Thank you in advance.

    Similar Threads:
    Attached Thumbnails Attached Thumbnails G13 Circular Milling on FANUC-g13-jpg  


  2. #2
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Yeah. A custom macro.

    Are you wanting to know how to write one?



  3. #3
    Registered
    Join Date
    May 2012
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by txcncman View Post
    Yeah. A custom macro.

    Are you wanting to know how to write one?
    thank you, yes i am. i have a custom macro book here, that i have looked through and have used for minor changes in the past...but i am not very familiar at all with macros.

    does this macro already exist somewhere to be seen? i imagine this has been asked for many times, but still cant seem to find it.

    appreciate any insight.



  4. #4
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    I am sure someone has a macro to do this already in their library. Maybe they will upload it here. Until then, if you have the Haas macro, you can modify/rewrite it to work with Fanuc.



  5. #5
    Member
    Join Date
    Feb 2007
    Location
    USA
    Posts
    592
    Downloads
    0
    Uploads
    0

    Post

    There are 2 existing threads on this.

    In one I posted my G13 (yaznaq formatted) macro I use on a Mori Seiki with the MSC-518 ( Fanuc 18M) control.

    Others built on it and those results were in a later thread.



  6. #6
    Registered
    Join Date
    May 2012
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by skullworks View Post
    There are 2 existing threads on this.

    In one I posted my G13 (yaznaq formatted) macro I use on a Mori Seiki with the MSC-518 ( Fanuc 18M) control.

    Others built on it and those results were in a later thread.

    thanks, unfortunately 'G13' is not a searchable word on this forum...

    i've found one of the threads...
    http://www.cnczone.com/forums/fanuc/...g13_fanuc.html

    happen to have a link to the other? thank you



  7. #7
    Gold Member
    Join Date
    Aug 2011
    Location
    Fordaville
    Posts
    2517
    Downloads
    0
    Uploads
    0

    Default

    hehe! I suspect that thread went over your head ;-)

    you can't use G13. it only cuts a single pass. you need a full blown pocket roughing macro.

    I have not seen anything useful like this on the net so I'll release one from my archives for the community :-)

    Here's a circle pocket milling macro I wrote about 25 years ago.

    This will mill a 50mm x 24.5mm deep circular pocket taking 5mm deep rough cuts with center X0 Y0.
    the explanation of the variables is at the bottom. just change the numbers on the G65 line to something simple in inches.
    for example....
    G65 P9205 A2. B0 E0.2 F0.01 H0 I2. J10. K2. Q40. R0.5 T-1. X0 Y0 Z-2.
    it should be relatively easy to understand what its doing but unless you're an expert dont try to understand the macro.
    just try it on the machine above the job/table to see the movements.



    %
    O0001 (MACRO-CIRCLE POCKET MILLING)
    G40 G49 G90 G92 X-200. Y200. Z0
    G0 X0 Y0 G43 H1 Z100. S500 M3
    G65 P9205 A50. B0 E5. F1. H0 I50. J150. K50. Q40. R3. T-1. X0 Y0 Z-24.5
    G0 G49 Z0 M5
    G27 X-200. Y200. Z0
    M30
    %


    %
    O9205
    #7=#2064
    #10=#26+#9
    IF [[[#1/2]-[#2/2]] GT [#7*2]] GOTO 1
    #3000=64 (CUTTER LARGER THAN HOLE!)
    N1 IF [#20 GT 0] GOTO 2
    #12=3
    GOTO 5
    N2 #12=2
    N5 #13=#1/2
    #14=#2/2
    #15=#13-#9-#24-#7
    #16=#9+#7
    #19=2*#7*#17/100
    #21=#13-#14-2*#16
    #22=#21/#19
    #23=#21/#22
    #27=#13-#9-#7
    G0 X#24 Y#25
    Z#18
    X-#15
    #28=#11
    WHILE [#11 GT #10] DO 1
    #28=#28-#8
    IF [#28 GE #10] GOTO 3
    #28=#10
    N3 G1 Z#28 F#4
    G#12 I#27 F#5
    #29=1
    WHILE [#29 LE #23] DO 2
    G1 X-[#15-#29*#22] F#5
    G#12 I[#27-#29*#22]
    #29=#29+1
    END 2
    G0 Z#18
    X-#15 Y#25
    IF [#28 LE #10] GOTO 4
    G1 Z[#28+1] F[10*#4]
    END 1
    N4 #15=#13-#24-#7
    #21=#13-#14-2*#7
    #22=#21/#19
    #23=#21/#22
    #27=#13-#7
    G0 X-#15
    G1 Z#26 F#4
    G4 X.5
    G#12 I#27 F#6
    #29=1
    WHILE [#29 LE #23] DO 1
    G1 X-[#15-#29*#22] F#6
    G#12 I[#27-#29*#22]
    #29=#29+1
    END 1
    G0 Z#18
    M99
    %


    #1 A:OUTSIDE DIAMETER
    #2 B:INSIDE DIAMETER
    #8 E:DEPTH OF ROUGHING CUT (Z AXIS)
    #9 F:FINISHING ALLOWANCE (COMMON TO ALL AXIS)
    #11 H:TOP OF JOB (Z AXIS)
    #4 I:FEEDRATE DOWN (Z AXIS)
    #5 J:FEEDRATE IN X-Y PLANE
    #6 K:FINISHING FEEDRATE
    #17 Q:PERCENTAGE OF CUTTER USED TO TAKE CUT IN X-Y PLANE
    #18 R:RAPID POINT ABOVE JOB
    #20 T:CUTTING DIRECTION 1=CLOCKWISE, -1=ANTI-CLOCKWISE
    #24,#25 X,Y:CENTRE COORDINATES OF CIRCLE
    #26 Z:DEPTH OF CAVITY

    #2064 TOOL DIAMETER OFFSET 64 (2001 - 2064)
    If using D1 use #2001

    Last edited by fordav11; 10-28-2012 at 05:33 AM.


  8. #8
    Registered
    Join Date
    May 2012
    Location
    USA
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    fordav - thank you! i'm going to give this a try, looks like just what i need



  9. #9
    Member
    Join Date
    Jul 2010
    Location
    South Africa
    Posts
    118
    Downloads
    0
    Uploads
    0

    Default

    the last step, you want to create your own G-code call in Fanuc 18m, G13 g-code,
    insert 13 in parameter 6050.
    renumber O9205 to O9010 and your done.
    now G13 will call program 9010, replace "G65 P9205" in your code,



  10. #10
    Member
    Join Date
    Apr 2007
    Location
    USA
    Posts
    28
    Downloads
    0
    Uploads
    0

    Default G13 macro

    Here is a macro we use on all of our Fanuc controls. You need to position to center of feature, and move down to desired depth. This macro does "1" shot holes and also will spiral. You can also loop with L command. (G13 I.xxx Dx Fx Lx)

    Hope this helps.


    :9013(G13 SPIRALLING MACRO)
    #3003=1
    (FOR FANUC 15M AND 16M, 18M ONLY.)
    (15M PARAMETER 7053=13)
    (16M, 18M PARAMETER 6053=13)
    (G13,I,K,Q,D,F AND ALSO C)
    (ON SPIRAL I=START RAD, K=FINISH RAD)
    (Q=STEPOVER,D=DIAM OFFSET#,F=FEEDRATE)
    (EX. FOR 2 DIAM WITH START FOR 1/2)
    (G13I.25K1.0Q.1D1F25.0)
    (IF USED, I,K AND D MUST BE GIVEN IN)
    (THE SPECIFIC ORDER AS SHOWN ABOVE.)

    (OMIT K AND Q FOR REGULAR)
    (NON-SPIRALLING CIRCLE CUTTING.)
    (I=FINISH RAD)
    (EX. FOR 2 DIAM, G13 I1.0 D1 F25.0)
    (DECIMAL PT NOT NEEDED ON ARGUMENT D)
    (ALL OTHER ARGUMENTS MUST SHOW A DECIMAL PT)
    (C MAY ALSO BE USED FOR # OF FULL 360 DEGREE)
    (ROTATIONS BEFORE TOOL RETURNS TO CENTER.)
    (IF C IS NOT USED, #3 DEFAULTS TO 1.)
    (I=#4,K=#6,Q=#17,D=#7,F=#9,C=#3)
    #27=#5041
    #28=#5042
    #31=#4001
    #32=#4002
    #33=#4003
    IF[#3NE#0]GOTO1
    #3=1
    N1#3=ABS[FIX[#3]]
    #7=ABS[FIX[#7]]
    IF[#9NE#0]GOTO2
    #9=#4109
    N2#9=ABS[#9]
    IF[#4009EQ80]GOTO3
    #3000=150(NOT IN G80 STATUS)
    N3IF[#4007EQ40]GOTO4
    #3000=151(NOT IN G40 STATUS)
    N4IF[#4NE#0]GOTO5
    #3000=152(I VALUE NOT GIVEN)
    N5IF[#7NE#0]GOTO10
    #7=0
    N10#20=#[13000+#7]
    IF[[ABS[#20]]LT[ABS[#4]]]GOTO20
    #3000=153(TOOL RADIUS TOO LARGE)
    N20IF[#6NE#0]GOTO25
    #29=1
    #21=#4-#20
    #22=#21/2
    G17
    G91
    G3X#21Y0I#22J0F#9
    WHILE[#29LE#3]DO1
    X0Y0I-#21J0
    #29=#29+1
    END1
    X-#22Y#22I-#22J0
    X-#22Y-#22I0J-#22F#9
    GOTO40
    N25IF[#17NE#0]GOTO30
    #3000=154(Q VALUE NOT GIVEN)
    N30#17=ABS[#17]
    IF[[ABS[#6]]GT[ABS[#4]]]GOTO35
    #3000=155(I NOT LESS THAN K)
    N35IF[#4GT0]GOTO36
    #6=-[ABS[#6]]
    #17=-#17
    GOTO37
    N36#6=ABS[#6]
    N37#101=#5001
    #102=#5002
    #21=#4-#20
    #22=#21/2
    #16=#6-#20
    #15=#16/2
    #30=ABS[#16]-ABS[#21]
    G17
    G91
    G3X#21Y0I#22J0F#9
    X0Y0I-#21J0
    WHILE[#30GT[ABS[#17]]]DO2
    G1X#17F[#9/2]
    G3X0Y0I-[#21+#17]J0F#9
    #21=#21+#17
    #30=#30-ABS[#17]
    END2
    G90
    #29=1
    G1X[#101+#15]F#9
    Y[#102-#15]
    G3X[#101+#16]Y#102I0J#15F#9
    WHILE[#29LE#3]DO3
    X[#101+#16]Y#102I-#16J0
    #29=#29+1
    END3
    X[#101+#15]Y[#102+#15]I-#15J0
    X#101Y#102I0J-#15F#9
    N40G01G90X#27Y#28
    G#31G#32G#33
    F#9
    #3003=0
    M99



  11. #11
    Registered javier1's Avatar
    Join Date
    Mar 2014
    Location
    USA
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default Re: G13 Circular Milling on FANUC

    Are this is for fanuc 15? The reason I ask is because I am new on the trade and since some time I need to do some spot face of 2.250 inch on diameter I will like to know how to use this macro.
    Thank you

    Best Regards
    Javier


  12. #12
    Member
    Join Date
    Dec 2015
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Re: G13 Circular Milling on FANUC

    Sorry for the thread resurrection.

    I'm looking to build a macro for a y axis lathe that can helical mill to a depth in X (using the X, Y and Z axes) and then spiral mill out (using the Y and Z axes). I'm currently programming this longhand, which is fine, but it doesn't lend itself well to small changes. We also have manual guide on the machine but the fanuc cycles are not fit for purpose IMO

    Thanks in advance

    DB



  13. #13
    Member
    Join Date
    Jan 2008
    Location
    Canada
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: G13 Circular Milling on FANUC

    Quote Originally Posted by db1974 View Post
    Sorry for the thread resurrection.

    I'm looking to build a macro for a y axis lathe that can helical mill to a depth in X (using the X, Y and Z axes) and then spiral mill out (using the Y and Z axes). I'm currently programming this longhand, which is fine, but it doesn't lend itself well to small changes. We also have manual guide on the machine but the fanuc cycles are not fit for purpose IMO

    Thanks in advance

    DB
    Not a macro but this code generating Google Spreadsheet might work as well. I wrote it for a part with 2 diameters/depths. You just fill out the white cells on the lift hand side and it will create the code on the right hand side (? Copy the code below ?). It doesn't orientate the part in C (just add the C-value to the highlighted line in the code).
    I haven't tried it but I'm pretty sure it works.

    https://docs.google.com/spreadsheets...Hn6h4_9ousUFjI



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

G13 Circular Milling on FANUC

G13 Circular Milling on FANUC