Yeah I wondered about that. I initially tried it with positive and with it at machine zero still moved up 2" and then back down again. Totally contrary to logical since my machine zero is furthest from the tool and any motion towards the tool should be negative?
Thanks John > -----Original Message----- > From: Feral Engineer [mailto:[email protected]] > Sent: June-25-21 3:35 PM > To: Enhanced Machine Controller (EMC) > Subject: Re: [Emc-users] G28 behaviour > > That's exactly the behavior that g28 follows on industrial controls. Try > g28z2. (positive) and it'll move up without having to switch to incremental > > 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, 6:28 PM John Dammeyer <[email protected]> wrote: > > > 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 > > > > _______________________________________________ > 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
