[fignoggle]

hi all-

two questions i hope you can help get through my head

one i think may be more mori sl-2h specific the other, perhaps so as well...

1. i have a piece of code where i've stated G28 X0. Z0. when executed from zero return, the turret moves in the X-(turret goes up) and Z+(turret goes away from spindle). given my newfound fear of crashes, i've feed stopped the movement before it hits the hard limits. is this G28 supposed to do this? when the turret is in the safe travel zone, and G28 appears, it does go back to zero return at X0.Z0 which makes sense. what am i doing wrong here?

2. G50 is completely escaping me. i've read the online articles, my cnc programming book, and i generally understand the concept, but can't seem to wrap my head around how to employ this given in pages 80-83 in my mori sl-2 manual (B-121601-E). i guess my main question is, what in fact are my G50 values? how do i know what my "dimensions of cutting tool starting point (programmed G50)" value is?

thanks!
david

[underthetire]

G28 is return to first reference return position. I usually use G0G28U0W0 on a lathe. Seen some horrific crashes from people not specifying an incremental move like G91 or the U and W. In fact, at my old job, a applications engineer was teaching a customer how to run his BRAND NEW Mori horizontal. Hadn't even cut a chip yet. Well, it was look how fast this thing is. Boy was it, he forgot the G91 command with the G28, X and Y bounced right off the pallet. Bent the spindle, destroyed the X axis linear guides. At that kind of rapid speed, things to go very wrong with steel to steel contact.

[mfgbydesign]

I'll give this a shot although I'm a little rusty on lathes.
G28 is a "Zero return" command. The X & Z values are an intermediate move location and tell which axis are to be moved home. As you have written, the first move would be to absolute X0Z0 (assuming you are currently in G90 mode). Usually this code is:
G28 G91 X0 Z0
G90
if you want no intermediate move before the zero return. The zero return position is usually at the travel limit and sometimes called "home" or "reference" or "grid" position.
I've done a G28 G91 X1. Z0 to retract in X then move to "home"
Usually this is used for an ultra safe tool index position or at the end of the program.
I think you can use G30 (don't take my word for it, check your manual) for a user defined return or safe index position.
The G50 is a work coordinate shift and is the distance from home to part origin + any tool offsets. So if your tools were set to the chuck face and centerline, and your workpiece zero were 6.000 off the chuck face you would have a G50 Z6.000 at the beginning of the program.

[mfgbydesign]

good point, if you use U & W the result is an incremental move (or none with U0W0) without the risk associated in changing absolute to incremental then back again as in my example..