So generally speaking, there are a few differences between g28 and g53. On fanuc and mits controls, g53 is merely machine coordinate position, you can put g53 anywhere in the stroke of axis travel. G28 is reference return position 1, g30 is reference return 2, g30 p3 is position 3, g30 p4 position 4. G30 positions are all programmable, via parameters, for where to go. The major difference is g28 and g30 both indicate back to the machine that it has reached a "home" position, where g53 does not. If i say g53 z0, the machine will not tool change, g91 g28 z0 will enable the reference status indicator and allow the tool change, even though it's the exact same spot.
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, 1:09 PM John Dammeyer <jo...@autoartisans.com> wrote: > 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:theferalengin...@gmail.com] > > 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 <jo...@autoartisans.com> > 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 > > > Emc-users@lists.sourceforge.net > > > https://lists.sourceforge.net/lists/listinfo/emc-users > > > > > > > _______________________________________________ > > Emc-users mailing list > > Emc-users@lists.sourceforge.net > > https://lists.sourceforge.net/lists/listinfo/emc-users > > > > _______________________________________________ > Emc-users mailing list > Emc-users@lists.sourceforge.net > https://lists.sourceforge.net/lists/listinfo/emc-users > _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
