[ALEXCOMO]

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

[skullworks]

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.

[mactec54]

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

[ALEXCOMO]

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!!!

[mactec54]

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

[ALEXCOMO]

Thank you mactec54 I'll try your code next day.

[luky]

Hi,ALEXCOMO

for mactec54's program,please check attached pic.

[ALEXCOMO]

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
%

[luky]

my used software is CIMCO Edit V5.

[mactec54]

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

[stevo1]

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

[mactec54]

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

[stevo1]

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

[jack.depasquale]

I am new to parametric programming and so have a lot of questions. I saw your macro for the spiral hole, and saw you had several versions. Can you post them also? Can you supply a sketch showing the input variables I am not sure what the 1st one is q= zpick?


Appreciate any help possible,
Jack D.
[email protected]

[gbowne1]

I was wondering if G33 was similar (nobody posted to my thread about G33 that I am using).

Will these programs run on the 15M?

[stevo1]

Will these programs run on the 15M?

The macro I posted in post #10 I wrote for my 15series Fanuc controls so yes it will work in yours. Obviously do some investigating on your control before just running. You want to make sure that the variables I am using in the program are not already being used in your control for something else.

Stevo

[samu]

in this Thread, helical milling seems to be confused with spiral milling. Take a look a this thread that is more about spiral milling.
http://www.cnczone.com/forums/showthread.php?t=110522

[msantaji1]

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

[ChattaMan]

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!!!!

[ALEXCOMO]

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)