In effect the G91 incremental with a Z0 just cancels out the initial move to the Z position.
I did try it on the mill as G28 Z-2 All that really happens is the machine sounds like it stumbles as it heads toward Z0 stopping briefly at Z-2. Very strange. John > -----Original Message----- > From: Todd Zuercher [mailto:[email protected]] > Sent: June-25-21 10:17 AM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > I'm pretty sure all of our Fanuc machines use G91 for incremental G28 > commands and not U V W. (maybe some older Fanuc controls > or controls specialized for some manufacturers or maybe just T-series, I only > have worked with Ms.) > > But as to why the intermediate command, I have no idea, It's just how Fanuc's > G28 has always been. > > Todd Zuercher > P. Graham Dunn Inc. > 630 Henry Street� > Dalton, Ohio 44618 > Phone:� (330)828-2105ext. 2031 > > -----Original Message----- > From: John Dammeyer <[email protected]> > Sent: Friday, June 25, 2021 1:06 PM > To: 'Enhanced Machine Controller (EMC)' <[email protected]> > Subject: Re: [Emc-users] G28 behaviour > > [EXTERNAL EMAIL] Be sure links are safe. > > Thanks for the explanation but I'm still curious why the intermediate point. > > I suppose if I had a tool changer at the machine 0,0,0 position (or close to > that) and my A axis sitting on the left of the work I'd want > to move to a position that allows a clear path directly to the tool changer. > > But, why a special code for this? If I need Z to be at a specific machine > position doesn't a > G53 G0 Z10 > G53 G0 Z0 > do the same thing? Granted two lines but one doesn't have to look up what a > G28 does... > > > -----Original Message----- > > From: Feral Engineer [mailto:[email protected]] > > Sent: June-25-21 9:51 AM > > To: Enhanced Machine Controller (EMC) > > Subject: Re: [Emc-users] G28 behaviour > > > > G28 is a return to reference using an intermediate point > > > > G90 G28 z0 would bring the tool to absolute Z0 before returning to > > reference zero (machine zero in most cases). By using g91 g28 z0, you > > specify that the intermediate point is your current position and the > > machine will reference return from there. You can also use values such > > as > > g90 g28 z50. To use 50mm above your workpiece origin to be your > > intermediate point or you can use g91 g28 z10. To move 10mm up and use > > that as your intermediate. > > > > Fanuc g code system a does not use g91, it uses u v w as their > > respective incremental axes for x y and z, which is why on a lathe > > you'll usually see > > g28 u0 w0 or something of that nature. You could use absolute values, > > but they come from your workpiece origin, so you'd have to say > > something like > > g28 x100 z100 to move to the absolute intermediate position above the > > part to not have a crash. > > > > The posted code in fusion is just ugly, no real reason to keep > > flopping back and forth like that. Fusion posts are JavaScript, so > > they're not terrible to modify. > > > > Phil T. > > The Feral Engineer > > > > Check out my LinuxCNC tutorials, machine builds and other antics at > > www.youtube.com/c/theferalengineer > > > > Help support my channel efforts and coffee addiction: > > www.patreon.com/theferalengineer > > > > On Fri, Jun 25, 2021, 12:28 PM John Dammeyer <[email protected]> wrote: > > > > > A friend who uses MACH3 and Fusion360 (free version) found that > > > every G-Code file created by Fusion for the MACH environment added: > > > > > > G28 G91 Z0 > > > G90 > > > G28 G91 X0 Y0 > > > G90 > > > > > > He's since figured out how to tell Fusion not to do this but looking at: > > > http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g28-g28.1 > > > > > > I m curious why there are two moves involved in this G-Code. In > > > this case the G91 changes to relative so the Z0 moves exactly 0 > > > first and then to the machine coordinates Z0 position. Same with XY. > > > > > > If 5161-5166 have something other than 0 and the G91 is left out the > > > system makes some interesting moves. > > > > > > My question is why would anyone want this kind of behavior? Where > > > would a > > > G28 be used without the G91? > > > > > > Is it perhaps to move around an obstacle before it heads for 0,0,0? > > > > > > Thanks > > > John > > > > > > > > > > > > "ELS! Nothing else works as well for your Lathe" > > > Automation Artisans Inc. > > > www dot autoartisans dot com > > > > > > > > > _______________________________________________ > > > Emc-users mailing list > > > [email protected] > > > https://lists.sourceforge.net/lists/listinfo/emc-users > > > > > > > _______________________________________________ > > Emc-users mailing list > > [email protected] > > https://lists.sourceforge.net/lists/listinfo/emc-users > > > > _______________________________________________ > Emc-users mailing list > [email protected] > https://lists.sourceforge.net/lists/listinfo/emc-users > > _______________________________________________ > Emc-users mailing list > [email protected] > https://lists.sourceforge.net/lists/listinfo/emc-users _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
