In 1979 the Dynamic Machinery Sales Chicago class for a Miyano 7BC lathe with Fanuc 5T control taught me to use G91 G28 X0 Z0 at the end of every program to make sure the machine reference was always accurate. I can't tell you how many times I watched the reference lights come on in the next six years - a bunch. Regards Stuart
On Fri, Jun 25, 2021, 6:06 PM John Dammeyer <[email protected]> wrote: > 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 > _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
