Need Help!- using machine coodinates

[nc novice]

hi guys, im trying to machine some washers but bar will not fit through drawtube so i need to machine multiple rings off the one setting. i read another post about this but can't quite understand it. The control i use is a fanuc series oi-tc (range g54 to g59) i need to machine 10 rings off each bar. can you check my program see where i went wrong thanks
ps: this is just a test program i did to get it running(with no luck)


o0001;
m98 p0002 L10;
g00 w-5.0; the other post hand g00 w(5 x "cccc" dimension) ?
m30;
%

o0002;
g28 u0 g28 w0;
t0000;
t0707; (parting tool 2mm wide)
g00 z-5.0 x63.0;
s1200 m03;
g01 x48.0 f0.15;
g00 z2.0;
s0 m05;
g00 w-7.0;
g28 u0 g28 w0;
m99;
%

I did a dry run and all it did was moved -2.0mm after sub program, went home and restarted at z0.0 again. thanks again in advance

[Geof]

I did something like this on a Haas by incrementing the work offset using a G10 command at the bottom of the sub program.

You also need a G10 to set the work offset to a starting position and another at the end to cancel all the incremental moves.

[mfgbydesign]

1. one g28 per line
2. get rid of the last g28 move; it's starting out from home again.
3. why subroutine for only 10 parts?
4. there was a crash move at the end
o0002;
g28 u0 g28 w0;
t0000;
t0707; (parting tool 2mm wide)
g00 z-5.0 x63.0;
s1200 m03;
g01 x48.0 f0.15;
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
G0 W1.0
X63.0
W-6.0
G1 X48.
g00 z2.0;
s0 m05;
g28 u0 W0
M30;
%

[nc novice]

thanks mfgbydesign will give this sample a go. and thanks Geof for explaining the process of sub routines in my previous post, i put it into practice and got it working, now just need to get a bar puller.
1 more question, do i need to reset the start position on the work co-ordinate
after it has run ten parts, or can i just load another bar and cycle start again? because there will be like 50 bars same length, thanks again guys

[nc novice]

oh i forgot, the reason i sub routine is that the part will be a little more complicated with a radius on internal dia for a ball valve and a recess on the back side, all this will be done before parting

[Geof]

If you do like I suggested and have a G10 command to set work coordinate to the starting position before the sub program call you should be able to just pull out another length of bar and go.

I also suggest the G10 after the sub program call and before the end of the program to avoid leaving the machine with all the incremental moves still in the work coordinate.

[Jonnis]

why not use G66?

o0001;
g28 u0 g28 w0;
t0000;
t0707; (parting tool 2mm wide)
g00 z-5.0 x63.0;
s1200 m03;
G66P0002
Z-5.
Z-10.
Z-15.
Z-..
...
G67
g00 z2.0;
s0 m05;
g28 u0 W0
M30;
;

O0002
G1X48.F.15
G0X63.




OR:

o0001;
g28 u0 g28 w0;
t0000;
t0707; (parting tool 2mm wide)
g00 z-5.0 x63.0;
s1200 m03;
M98P0002L10.
g00 z2.0;
s0 m05;
g28 u0 W0
M30;
;

O0002
G1X48.F.15
G0X63.
W-5.

[mfgbydesign]

For setting the end on a bar feed I use the side of a toolholder, or if manually moving the bar send the tool to Z0 at the end then pull the bar out to touch the tool. For a new bar you might load the bar, start the program to send the tool to Z0, M0 (program stop), pull the bar out and clamp the chuck, then start.

[sinha_nsit]

Repeating a subprogram/macro (L-count) in absolute mode or without coordinate/offset shift is meaningless.

Yes, G66 also can be used. But it does not simplify programming.

[nc novice]

I think i got it guys(I think). i created a test facing program to run, facing 0.5 each time(x3) after program finished i cycle start again, it cut air until last cut which was feathery. is this the correct procedure? thanks

o0001; (main)
m98 p0002 L3;
g10 L2 p1 w1.5;
g28 u0 w0;
m30;
%


o0002; (sub)
g28 u0 w0;
g00 z0.0 x68.0;
s1200 m03;
g01 x0.0 f0.5;
g10 L2 p1 w-0.5;
m99;
%

so in theory i could cut any shape and part off before the g10 line on sub routine and just have to change the w- value to correspond to how much material i have removed then change the w value on main program to go back to start position?

[sinha_nsit]

It is ok.
But you love G28 too much.

[nc novice]

when the machine installer showed me he used g28 u0 g28 w0 at the start and end of program so i kind of adopted that style, should i remove g28 from sub program?