Re: G92

["Peter Cook" <kf2qd-at-terraworld.net>]

G92 was a way of defining the current coordinates for the current tool. It
does not affect offsets.On a mill it might not be as necesary as on a lathe
where the location of the tool tip can vary quite a bit from turning tools
to boring bars. It is also a neat way to move patterns around - drill a
pattern after a line like G92X0Y0 and then run the same section of code
after G92X2Y0 and you have moved the pattern 2 inches in X. Back when
everything was manually programmed and on manually punched paper tape you
learned to do things like that to make life easier. Even simple tasks like
boring a set of holes is done easily this way G92X?Y? and call a subroutine
and then G02XsomethingelseYsomethingelse and you have moved it around. -
Just have to remember to have reset the G92 when you are all done to get
back to the correct origin - machines didn't have machine home back then...
or the ability to put more than about an inch in the tool offsets.

Pete Cook
----- Original Message -----
From: "Brian Pitt" <bfp-at-earthlink.net>
To: "Multiple recipients of list" <emc-at-nist.gov>
Sent: Thursday, July 18, 2002 12:51 PM
Subject: Re: G92


>
> thanks Dale
>
> I was wondering why I'd never used g92 and what all the hubub was about
>
> so from what I've seen on the CCED list some are using it to make up
> for a lack of offset setting and manipulation controls in the user
interface
> and there realy isn't a bug in the interpreter at all right?
>
> Brian
>
> On Thursday 18 July 2002 08:15, you wrote:
> > G92 - position register preset/position preload/load position or
> > whatever the Mfg. called it.
> >
> > G92 is NOT an OFFSET!!! It simply changes the value of the position
> > register. It was meant to be used within a part program, not from MDI
> > mode to set axis zero or program origin point.
> >
> > In my nearly 30 years of experience every machine I have ever dealt with
> > had a method of setting axis zero manually and it had absolutely nothing
> > to do with the G92 code. The earlier machines had no offsets at all, but
> > G92 was included in the G & M codes. Next came tool length and diameter
> > offsets, program origin was still established by manual setting of axis
> > zero. Then came Work Coordinate Offsets. The first machine I encountered
> > that used G54,55,... still had the button for setting an axis to zero in
> > manual mode. G92 was still separate from the offsets. As for the setting
> > of an axis zero point, with the addition of Work Coordinate Offsets I
> > found no reason to ever set axis zero the old way and used the Work
> > Coordinate Offsets.
> >
> > A Simple Example:
> <snip>
>
> > There can be many Right ways to do something, but Wrong is Wrong no
> > matter how you look at it! IMO to use the G92 code as an offset is wrong
> > and can lead to problems as have been described.
> >
> > Dale
>
>