Need Help!- Helical Mill

[QUALMACH1]

Guys,
I have a Mazak H-15 with a fanuc 6m series 901 version 13 controller. I need to know how to do a helical mill. Here is the code I am using...
G03 X0 Y2.75 I0 J-2.75 Z-4.5 Q.1 F1.5 M3 S1200; This gets me into position, but when it starts it does not step .100" per revelution (Q.1), it go's full Z depth in 1 revelution. I am using a 1.5" inserted cutter, and only want it going in Z .100" per rev untill it reaches full Z depth. Thanks,

[dcoupar]

There is no Q mentioned in the 6M-B manual. You can program a sub call with a repeat count (L).

G00 X0 Y2.75 Z0.1
G01 Z0 F1.5
M98 P101 L45
G00 G90 Z0.1
...
...
M30

O101 (HELICAL SUB)
G91 G03 I0 J-2.75
M99

[sld4121]

Since it is a fanuc controlled machine, helical milling will not step down. You have to program pass by pass or use a macro. I believe starting with the 18i and above you can do it with an option called spiral/conical interpolation. However, since that was around $1750, most people continue to use macros.

[QUALMACH1]

Originally Posted by dcoupar There is no Q mentioned in the 6M-B manual. You can program a sub call with a repeat count (L). G00 X0 Y2.75 Z0.1 G01 Z0 F1.5 M98 P101 L45 G00 G90 Z0.1 ... ... M30 O101 (HELICAL SUB) G91 G03 I0 J-2.75 M99

I never have used subs..not sure how to do this, but say I call out program O0001 write the program as above, then do I write another program for the sub say O0002? Or will the P tell it to look for the sub in this program O001? Thanks,

[sld4121]

As you correctly assumed, the sub program needs to be separate from the main program. Just remember to end with a M99 so it knows to return to the main program when it is done.

[QUALMACH1]

worked great except for this, when it finishes the G03 it go's up in Y...thats not a good thing. Here is what im doing. I have a part that is 4.5" thick, it has na hole burned in it that is 6.875" in dia. I am milling it out to 7" using a 1.5" inserted cutter, thenim gonna finish bore it to size. The program is starting Y2.5, then it G03's back to Y2.5, then for some reason it starts feeding on up in Y. Why is this...how do I get it to stop at Y2.5?

Program so far...
O1570;
G40G80G90;
G54;
M08;
M3S1200;
G0X0Y2.75;
G0Z.1;
G1Z0F1.5;
M98P0001L45;
G0G90Z.1Y0;
M05;
M09;
M00;
----------------
(HELICAL SUB)
O0001;
G91G03I0J-2.75F10.;
M99;

Any suggestions??

[dcoupar]

Originally Posted by QUALMACH1 worked great except for this, when it finishes the G03 it go's up in Y...thats not a good thing. Here is what im doing. I have a part that is 4.5" thick, it has na hole burned in it that is 6.875" in dia. I am milling it out to 7" using a 1.5" inserted cutter, thenim gonna finish bore it to size. The program is starting Y2.5, then it G03's back to Y2.5, then for some reason it starts feeding on up in Y. Why is this...how do I get it to stop at Y2.5? Program so far... O1570; G40G80G90; G54; M08; M3S1200; G0X0Y2.75; G0Z.1; G1Z0F1.5; M98P0001L45; G0G90Z.1Y0; M05; M09; M00; ---------------- (HELICAL SUB) O0001; G91G03I0J-2.75F10.; M99; Any suggestions??

I don't see how the program could stop at Y2.5 when the 6th block positions to Y2.75, and the G03 helix ends at Y2.75. Please re-check the program.

[sld4121]

Looks like your helical sub is missing a negative Z value.
Otherwise, it should only be able to go to Y0 at the end of the 45 loops.

If it still does not work, try the following,

(HELICAL SUB)
O0001;
G91G03X0Y-2.75Z-.05I0J-2.75F10.;
Y2.75Z-.05J2.75;
M99;

This should just break the arcs into segments

[dcoupar]

Oops... my bad.

(HELICAL SUB)
O0001;
G91 G03 I0 J-2.75 Z-0.1 F10.;
M99;

[QUALMACH1]

Originally Posted by dcoupar I don't see how the program could stop at Y2.5 when the 6th block positions to Y2.75, and the G03 helix ends at Y2.75. Please re-check the program.

Yea...my bad, I had it programmed to go y2.5 in the sub program i forgot it was in G91...It now has a Z-, and it working great!!!! Thanks, guys. This machine had not been used at all hardly in our shop, due to no one knowing how to correctly program it. we are now using it daily thanks to you good pepole! Godbless you ALL!

[dcoupar]

Originally Posted by QUALMACH1 Yea...my bad, I had it programmed to go y2.5 in the sub program i forgot it was in G91...It now has a Z-, and it working great!!!! Thanks, guys. This machine had not been used at all hardly in our shop, due to no one knowing how to correctly program it. we are now using it daily thanks to you good pepole! Godbless you ALL!

Glad we could help. Good luck.