HI ALL.
I'M MAKING a FANUC 0M MACRO FOR HOLE SPIRAL MILLING .
ANY SUGGESTION?
HI ALL.
I'M MAKING a FANUC 0M MACRO FOR HOLE SPIRAL MILLING .
ANY SUGGESTION?
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.
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
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!!!
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
Thank you mactec54 I'll try your code next day.
Hi,ALEXCOMO
for mactec54's program,please check attached pic.
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
%
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
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
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
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
my used software is CIMCO Edit V5.
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
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!!!!
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)
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
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!
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
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