530,019 active members*
3,473 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 35
  1. #1
    Registered
    Join Date
    Jun 2006
    Posts
    48

    Talking MACRO FOR HOLE SPIRAL MILLING

    HI ALL.
    I'M MAKING a FANUC 0M MACRO FOR HOLE SPIRAL MILLING .
    ANY SUGGESTION?

  2. #2
    Registered
    Join Date
    Feb 2007
    Posts
    592

    Cool G13

    I wrote a quick and dirty macro to give partial compatability with a Yaznaq G13 on our 518MSC (Fanuc 18M) Mori Seiki.

    I say partial because Yaznaq uses an "L" as one of the optional augments. This is not possible on the Fanuc as "L" is not normally supported in Macro B.

    You would need to look up several machine parameters and change the variables to match your 0m.

    I can stop by the shop and get a copy to post here later if there is interest.

    Note again this is the Yaznaq type which does not have ANY Z axis movement. You must use a G01 Z before the G13 and a G00 Z after...

    Someday I will "Upgrade" the Macro to be more like the HAAS usage of a G13. But at the time I was handed a cart with all preset tooling and ready to run Yaznaq code that I had to edit into something we could run today and it was full of G13's.

    You might also try the G65 Pxxxx method if you don't want to add a G13 command.


  3. #3
    Member
    Join Date
    Jan 2005
    Posts
    11558
    Hi alexcomo

    This is easy to do just right the Gcode that you need you don't need a macro

    T5M6
    M8
    G54
    S2850M3
    G90G0X-1.0985Y.3569
    G43Z.2H5
    G1Z0F20.
    G3X0.Y1.55Z-.16I1.0985J-.3569
    Z-.36J-1.155
    Z-.56J-1.155
    Z-.76J-1.155
    J-1.155
    G0Z.2
    M9
    M5
    G0Y5.5
    M30

    This will do a spiral down .200 per pass on a 2.56 dia hole x .760 deep .250 cutter centre
    being X0Y0
    Mactec54

  4. #4
    Registered
    Join Date
    Jun 2006
    Posts
    48

    Grazie!

    WERY WELL!!Thank you all for help!!!Grazie!

    First of all ....sorry for my english!!!!!

    Specification:for spiral i mean work an hole with archimede spiral. I think is the more efficent way for empty a round hole.

    Skullworks please post it when you can.

    G13 is the native way to do this on fanuc 18, isn't it?

    Hi all!!!

  5. #5
    Member
    Join Date
    Jan 2005
    Posts
    11558
    Hi ALEXCOMO

    The Gcode in my post is a archimede spiral & will work fine on your Fanuc 18 control
    you don't need to have a G13 to make a spiral
    Mactec54

  6. #6
    Registered
    Join Date
    Jun 2006
    Posts
    48
    Thank you mactec54 I'll try your code next day.

  7. #7
    Registered
    Join Date
    Oct 2008
    Posts
    11
    Hi,ALEXCOMO

    for mactec54's program,please check attached pic.
    Attached Thumbnails Attached Thumbnails SPIRAL.gif  

  8. #8
    Registered
    Join Date
    Jun 2006
    Posts
    48

    Talking ANTEPRIMA

    Hi all.

    Thank you Luky...Which program you have used for make the pic?

    Here is what I mean for archimede spiral
    http://www.math.it/spirale/spirale-archimede.htm

    The native Gcode for Fanuc 18 archimede spiral is only G2 or G3 but you
    need to put into the command line the adress L (number of revolution) or Q( radius increment for spiral revolution).This function is not available on the fanuc 0i-mc(absurdity!!!!!!!!!!!!)

    Tomorrow I'm going to test my dirty macro in my shop!

    here is a preview
    %
    :9019(INTERPOLAZIONE FORI)
    (X E Y POSIZIONE CENTRO CERCHIO #24 #25)
    (I RAGGIO #4)
    (W NUMERO DI GIRI DI SVUOTAMENTO #23)
    (D PREFORO #7)
    (E EVENTUALI GIRI D'ELICA #7)
    (K ALTEZZA DI INIZIO #6)
    (Z PROFONDITA CON SEGNO- #26 DISTANZA DAL PUNTO K)
    (F AVANZAMENTO #9)
    (#500=NUMERO UTENSILE A MANDRINO MEMORIZZATO DA MACRO CAMBIO UT)
    #501=#5003(MEMORIZZA ALTEZZA IN CUI SI TROVA UT PRIMA CAMBIO MACRO)
    #502=#6
    #503=#9
    #505=#4
    #506=#26
    #507=#23
    #100=#[13001+#500](RAGGIO FRESA)
    #106=[#502+#26](PROFONDITA IN Z)
    #107=#505-#100(RAGGIO FINALE INTERPOLAZIONE)
    #110=[[#107-#100]/#507]/360(INCREMENTO RAGGIO A STEP)
    #112=0
    #111=#100
    #114=0
    #113=360*#23(VALORE TOTALE DEGLI STEP)
    G0#24Y#25
    G52X#24Y#25
    Z[#502+2]
    G1Z#106F[#503*0.7]
    N1WHILE[#114LT#113]DO1
    #112=#112+1
    #120=#111*COS[#112]
    #121=#111*SIN[#112]
    #111=#111+#110
    G3I#120J#121
    END1
    G1X#107Y#25
    G3I-#107
    I-#107
    G0Z#501X0Y0
    G52X0Y0
    M99
    %

  9. #9
    Member
    Join Date
    Jan 2005
    Posts
    11558
    Hi ALEXCOMO

    I think luky is showing you is my program

    You don't need a call for how many ( revolution's ) the Z step & J keeps it going around
    change it to metric numbers & it will work in your control

    The link you have posted is a face milling spiral which you would have to go back to the centre for each Z step to make this work not really a good way to do it

    Just drill a hole & use like what I have done you only need ( I ) ( J ) ( Z ) & ( G3 ) moves to make this work I use this for roughing all the time it can have arc on arc off if needed when I'm running one I will take a movie of it it is very cool way to do milling
    Mactec54

  10. #10
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    These are the macros that I use for spinning a hole. You don't need to drill out the center of the pocket. This climb mills to depth. I have written this and run it on all my Fanucs. I have not run it on a OM series. However as long as you have macroB programming this will work.

    Q=pick in Z, W=starting depth, E=dia to spin, K=cutter dia, Z=final depth, T=tool number, M=coolant code, X=x-center of hole, Y=y-center of hole.

    O0001(MAIN PROGRAM)
    #500=3.(CLEARANCE PLANE)
    G65P8001Q.025W.1E.5K.25Z.9T10M8X0Y0
    M30

    O8001(C-BORE RAMPING ROUTINE)
    #2=10000(ROUNDING)
    #12=#17
    #13=#23
    M6T#20
    #8=#8/2
    #6=#6/2
    #1=0
    #15=[#8+#6]/2(ARC IN)
    N100
    IF[#6GE#8]GOTO260
    G0G90G55G80
    X#24Y#25Z#500
    Z[#23+.1]
    G1Z#23
    G91G1X[#8-#15]Y-[#15-#6]M#13
    G3X[#15-#6]Y[#15-#6]J[#15-#6]
    N150G3X0Y0I-[#8-#6]Z-#17
    #23=#23+#17
    IF[#1EQ1]GOTO400
    IF[ROUND[[#23+#17]*#2]/#2GE[ROUND[#26*#2]/#2]]GOTO300
    GOTO150
    N300#17=#26-[#23-#13]
    #1=1
    GOTO150
    N400
    #23=#13
    #17=#12
    #1=0
    G3X0Y0I-[#8-#6]
    G3X-[#15-#6]Y[#15-#6]I-[#15-#6]
    G90G1X#24Y#25M9
    G0Z#500M5
    N200M99
    N260#3000=10(CUTTER DIA. TO LARGE)

    Stevo

  11. #11
    Member
    Join Date
    Jan 2005
    Posts
    11558
    Hi Stevo

    Does your macro cut the dia of the cutter all the way down or the whole surface of the hole all the way down You don't need to drill a hole with my Gcode It is a place the chips can go when cutting steel it's a lot easer on the cutter to have a hole if you are going more than .500/12.7mm deep
    Mactec54

  12. #12
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    This will cut around the diameter of the tool. So it will spin the hole dia that you specify - the tool dia. This will move to the center of the hole above the part. It will arc to the diameter of the hole then spin all the way around the hole moving down in the Z the pick distance specified with Q value. It will do this until depth set by Z is obtained then it will make 1 idle pass at the bottom to remove the material left from previous pass. Then it will arc back to the center of the hole and retract to the R-plane.

    We do a lot of steel, SS, Inco, Hastaloy. I have never drilled out the center of the hole first. Althought it never hurts for chip removal and less tool wear. This program runs as smooth as a baby's butt, a lot of guys are very happy with running this mainly because of the versatility. You might find that you won't have to drill out the hole first.

    This macro just runs one hole. I have these macros set up for doing mutiple holes on a BC with a rotary axis and non rotary axis machines. I also have them set up to use the tool radius in the offset page so you can make adjustments on the fly without resetting the program. I have also set them up for holes not on a BC but with multiple holes at different locations. This way would be set up with a macro modal call then just specify the X,Y locations. Let me know if this would be an application that you could use the other macros so I can post them.

    Stevo

  13. #13
    Registered
    Join Date
    Oct 2008
    Posts
    11
    my used software is CIMCO Edit V5.

  14. #14
    Registered
    Join Date
    Aug 2008
    Posts
    15
    hi EVERYBODY


    you can do machinning by using following program

    T01 M06;
    G00 G90 G54 G95 X-5.0 Y0.0;
    G43 Z100.0 H01;
    M03S1200;
    M08;
    G00Z2.0;
    #2=50.0 (TOTAL DEPTH OF SPIRAL MILLING);
    N1WHILE [#1 GT #2] DO1;
    G91 G02 X0.0 Y0.0 Z-5.0 I5.0 F100.0;
    #1=#1-5.0;
    END1;
    G00 G80 Z100.0 M09;
    M05;
    M01;
    EXPLANATION
    Z:- SIMULTANIUS TRAVEL OF Z-AXIS WITH X-AXIS &Y-AXIS IN ONE COMPLETE CIRCLE
    I:- RADIUS OF CIRCLE

  15. #15
    Registered
    Join Date
    Nov 2006
    Posts
    174

    Hmmm!!

    Hi msantaji1....

    Sorry but your prog would not work. If it did work it would produce a helix,
    not a spiral

    T01 M06;
    G00 G90 G54 G95 X-5.0 Y0.0;
    G43 Z100.0 H01;
    M03S1200;
    M08;
    G00Z2.0;
    #2=50.0 (TOTAL DEPTH OF SPIRAL MILLING); ---typo? (-50, perhaps)
    N1WHILE [#1 GT #2] DO1; <--- what is the value of #1?
    G91 G02 X0.0 Y0.0 Z-5.0 I5.0 F100.0;
    #1=#1-5.0;
    END1; ---- would jump to here without machining!!
    G00 G80 Z100.0 M09; G80? No G90! (risky)
    M05;
    M01;
    EXPLANATION
    Z:- SIMULTANIUS TRAVEL OF Z-AXIS WITH X-AXIS &Y-AXIS IN ONE COMPLETE CIRCLE
    I:- RADIUS OF CIRCLE

    Explanation
    Bad programming

    Soz for being picky but felt it needed correcting. Don't want someone to crash!!!!

  16. #16
    Registered
    Join Date
    Jun 2006
    Posts
    48

    Talking ATTENTION!

    Hi guy ,
    thank you all for interesting

    plese attention :spiral is one thing ,helix is another one!!!.
    There are 2 good way for milling a hole ,in my case i'm doing a set of macro
    with multiple strategy.....one with spiral....one with helix....one with ramping approach....etc.,thats why my pieces are much various.
    Thats is for increase the programming speed ,in fact in one line i can define
    a complex way for milling a hole and decreasing error.
    I'm going to saving evry macro in a 9000 prog. and assigning a gcode(g200-g201-g202)

  17. #17
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Quote Originally Posted by ChattaMan View Post
    Hi msantaji1....

    Sorry but your prog would not work. If it did work it would produce a helix,
    not a spiral

    T01 M06;
    G00 G90 G54 G95 X-5.0 Y0.0;
    G43 Z100.0 H01;
    M03S1200;
    M08;
    G00Z2.0;
    #2=50.0 (TOTAL DEPTH OF SPIRAL MILLING); ---typo? (-50, perhaps)
    N1WHILE [#1 GT #2] DO1; <--- what is the value of #1?
    G91 G02 X0.0 Y0.0 Z-5.0 I5.0 F100.0;
    #1=#1-5.0;
    END1; ---- would jump to here without machining!!
    G00 G80 Z100.0 M09; G80? No G90! (risky)
    M05;
    M01;
    EXPLANATION
    Z:- SIMULTANIUS TRAVEL OF Z-AXIS WITH X-AXIS &Y-AXIS IN ONE COMPLETE CIRCLE
    I:- RADIUS OF CIRCLE

    Explanation
    Bad programming

    Soz for being picky but felt it needed correcting. Don't want someone to crash!!!!
    The only problem that I see for this not working is what you pointed out in the typo of #2=50(this should be -50). #1 does not need to equal anything at the beginning. With the start of this program #1=null but will add up through the rest of the program until it equals -50. The Z100 is a pretty safe move. Most VMC's are set to retract away from the part in the positive direction so given the fact that your in the hole, moving Z100 with a G91 is a safe move to come off the part and end the program. I agree however that I would not run my program like this. This is more of a down and dirty get you through 1 part type of program.

    I would be more concerned that there is no arc or move to the center of the hole before retracting. You will run the tool up the side of the hole. There should also be an idle pass at depth. The last pass spins down to depth but the material from the start of the spin to the end is still there.

    Alexcomo,
    The program I gave you in post #10 takes care of any issues that have been brought up. It has been proven and running for years now. It has a lot of flexability. The only difference in this is I choose to use my offset radius to set the tool data instead of setting it in the macro call. This gives you the flexability to adjust in the offset wear on the fly. If you choose to want it that way let me know we can add it in.

    Stevo

  18. #18
    Registered
    Join Date
    Nov 2006
    Posts
    174

    Down and dirty

    Stevo1..

    Maybe "bad programming" was a bit harsh. I do like your down and dirty explanation.

    I believe that Null is not greater than -50 so would presume the prog would jump to END1, as the statement was not satisfied. But I'll now try it to see for myself.

    Also the poster put in a feedrate of "F100.0" in G95 (feed per rev) mode. Sounds catastrophic to me.

    There a lots of newbies just learning the exciting skills of programming and may just copy and paste the programs posted here, straight into their machines. Posters must be careful of these possible faux pas.

    Your macro looks good (post #10). I'll be checking that one out when I get time.

    I'll stick with my first comment though for the other poster.....

    Bad programming!

  19. #19
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Chattaman,
    Bad programming wasn't harsh. I agree people have to be careful what they plug into there machines. I would hope that people have enough commonsense not to pull a program off the forum and push cycle start . I guess I have seen worse things.

    The IF statment still works when #1=null. I can't speak for all controls but it works on my Fanuc’s. I however do not choose to start my programs that way. I always set #1=0 before jumping in.

    I agree the G95 should be taken out. Should use the default G94.

    I think you will like the macro. Works great. I have my thread milling set up the same way. No problems thread milling down to ¼”. The guys love them on the versatility that they have. Like I stated in my last post I have them set up to run the tool in the offset page instead of driven off the macro call. Being able to adjust this on the fly is great because we do a lot of holes around a bolt circle and they can just option stop after a hole, check, adjust and hit cycle start. This macro however is just to do 1 hole unless you go modal. I don’t use modal. I have the calculations in the macro to run around until the # holes are satisfied.

    Stevo

  20. #20
    Registered
    Join Date
    Nov 2006
    Posts
    174

    Soz.

    Well....I've got to stand up and be corrected. I tried the DO/WHILE loop with #1 as null. And it worked!
    So, sorry to msantaji1 for saying his null variable part of the prog wouldn't work.

    Still wouldn't produce a spiral tho'

    That's what makes this job interesting. You can learn something new every day

Page 1 of 2 12

Similar Threads

  1. Fanuc bolt hole macro
    By Machinist3 in forum G-Code Programing
    Replies: 4
    Last Post: 05-23-2008, 04:43 PM
  2. spiral macro ?
    By cyclestart in forum G-Code Programing
    Replies: 4
    Last Post: 03-24-2008, 03:42 AM
  3. 400x330x12mm AL hole milling
    By fantasy2 in forum Employment Opportunity
    Replies: 0
    Last Post: 05-06-2006, 04:54 PM
  4. G12/G13 hole milling
    By JFettig in forum Mach Software (ArtSoft software)
    Replies: 14
    Last Post: 03-11-2005, 03:23 AM
  5. Milling a hole
    By igorko in forum Uncategorised CAM Discussion
    Replies: 25
    Last Post: 01-30-2004, 12:55 PM

Posting Permissions

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