Ah. Ok. I'll try that to see what happens on my system. Sent from my Samsung
S10
-------- Original message --------From: Feral Engineer
<[email protected]> Date: 2021-06-25 10:36 a.m. (GMT-08:00) To:
"Enhanced Machine Controller (EMC)" <[email protected]> Subject:
Re: [Emc-users] G28 behaviour So generally speaking, there are a few
differences between g28 and g53. Onfanuc and mits controls, g53 is merely
machine coordinate position, you canput g53 anywhere in the stroke of axis
travel. G28 is reference returnposition 1, g30 is reference return 2, g30 p3 is
position 3, g30 p4position 4. G30 positions are all programmable, via
parameters, for whereto go. The major difference is g28 and g30 both indicate
back to themachine that it has reached a "home" position, where g53 does not.
If i sayg53 z0, the machine will not tool change, g91 g28 z0 will enable
thereference status indicator and allow the tool change, even though it's
theexact same spot.Phil T.The Feral EngineerCheck out my LinuxCNC tutorials,
machine builds and other antics atwww.youtube.com/c/theferalengineerHelp
support my channel efforts and coffee
addiction:www.patreon.com/theferalengineerOn Fri, Jun 25, 2021, 1:09 PM John
Dammeyer <[email protected]> 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:[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
[email protected]https://lists.sourceforge.net/lists/listinfo/emc-users
_______________________________________________
Emc-users mailing list
[email protected]
https://lists.sourceforge.net/lists/listinfo/emc-users
