Gentlemen,
I will try to explain how the fanuc control uses the G28 command
and then later I will look up the command in a fanuc manual to try to
corroborate my explanation.
Steve's description/quotation is accurate.
The G28 command is in essense a two part command. The axis
departure commands happen first and then the homing part of the cycle
is executed.
G90 G28 X0.0 Y0.0 Z0.0
will rapid move all axes to X0.0 Y0.0 Z0.0 in the current coordinate
system specified by a G54 group command and then all the axes will
rapid move toward home position. At a preset distance (a parameter in
the control) from the home position each axis will slow down to what
EMC calls home-latch velocity. Each axis will find the index pulse,
move to home position and turn on the axis homed light.
G90 G28 X1.5 Y2.0 Z2.5
will rapid move all axes to X1.5 Y2.0 Z2.5 in the current coordinate
system specified by a G54 type command and then all the axes will
rapid move toward home position. At a preset distance (a parameter in
the control) from the home position each axis will slow down to what
EMC calls home-latch velocity. Each axis will find the index pulse,
move to home position and turn on the axis homed light.
G90 G28 X0.0
will rapid move the X axis to X0.0 in the current coordinate system
specified by a G54 type command and then the X axis will rapid move
toward home position. At a preset distance (a parameter in the
control) from the home position the X axis will slow down to what EMC
calls home-latch velocity. The X axis will find the index pulse, move
to home position and turn on the axis homed light. This will only act
on the X axis. The other axes will do nothing at any time during the
execution of this line of code. If I then want the Y axis to home I
will use a second line of code specifying the Y axis instead of the X
axis.
G91 G28 X0.0 Y0.0 Z0.0
no axis movement will occur as in incremental mode a departure command
of zero does not move an axis. Then all the axes will rapid move
toward home position. At a preset distance (a parameter in the
control) from the home position each axis will slow down to what EMC
calls home-latch velocity. Each axis will find the index pulse, move
to home position and turn on the axis homed light.
G91 G28 X1.5 Y2.0 Z2.5
will rapid move the X axis 1.5 units in the positive direction from
the current X axis position, the Y axis will move 2.0 units in the
positive direction from the current Y axis postion and the Z axis will
move 2.5 units in the positive direction from the current Z axis
posittion. Then all the axes will rapid move toward home position. At
a preset distance (a parameter in the control) from the home position
each axis will slow down to what EMC calls home-latch velocity. Each
axis will find the index pulse, move to home position and turn on the
axis homed light.
G91 G28 X0.0
no axis movement will occur as in incremental mode a departure command
of zero does not move an axis. Then the X axis will rapid move toward
home position. At a preset distance (a parameter in the control) from
the home position the X axis will slow down to what EMC calls
home-latch velocity. The X axis will find the index pulse, move to
home position and turn on the axis homed light. This will only act on
the X axis. The other axes will do nothing at any time during the
execution of this line of code. If I then want the Y axis to home I
will use a second line of code specifying the Y axis instead of the X
axis.
I don't know how the specification defines the execution of this
line but I have never seen a control that would move an axis whose
departure command was omitted from this line. I have other controls
that will move the axis to the home position but will not go through
the homing cycle and will not turn on the axis homed light. If you do
not want to deviate from the standard I have no problem with that. I
would just like to have the option of choosing to deviate from the
standard at times.
My preference would be for EMC to move to home position and not
bother with the homing cycle.
thanks
Stuart
> >From the "CNC Programming Handbook" by Peter Smid (ISBN 0-8311-3158-6)
> and basically describing Fanuc behavior....
>
> G28 is NOT modal, the G28 must appear in each block where used
>
> G28 in a block by itself is not valid, one or more axis parameters
> must be supplied. Only those axes specified will move.
>
> Traverse rate will be rapid, like in a G00.
>
> The axis parameter must have a value specified (Fanuc behavior).
>
> The value will obey the absolute or incremental mode currently
> in effect!!!
>
> The value is used as an intermediate way point on the path to
> machine zero.
>
> If no intermediate way point is desired, the value should be such
> as to cause no motion away from the starting point. For example
> while in absolute mode the value should repeat the current
> position, or while in incremental mode the value should be zero.
> You MUST know what mode you are in before using a G28 command.
>
> The purpose of the intermediate way point is to avoid clamps etc.
>
> I do not know if some controls other than Fanuc will allow the
> value to be omitted and assume that no intermediate way point
> is desired, but this seems a reasonable behavior to me.
>
> Regards,
> Steve Stallings
>
> > -----Original Message-----
> > From: [EMAIL PROTECTED]
> > [mailto:[EMAIL PROTECTED] Behalf Of Chris Radek
> > Sent: Saturday, August 04, 2007 3:33 PM
> > To: Enhanced Machine Controller (EMC)
> > Subject: Re: [Emc-users] G28 return to home
> >
> >
> >
> > Hi Stuart, can you find for us a reference that explains how G28
> > typically works on non-EMC controls? If they all work the same except
> > for EMC, we could talk about breaking with ngc for this.
> >
> > In particular I want to know how it should behave when
> >
> > in G90 mode and all axes are specified
> > in G90 mode and some axes are specified
> > in G91, all
> > in G91, some
> >
> > Also is there a difference of behavior when axes are specified to be 0
> > and when they're nonzero? You said something about an intermediate
> > point/move that I didn't understand.
> >
> > Thanks
> >
> > Chris
> >
> > -------------------------------------------------------------------------
> > This SF.net email is sponsored by: Splunk Inc.
> > Still grepping through log files to find problems? Stop.
> > Now Search log events and configuration files using AJAX and a browser.
> > Download your FREE copy of Splunk now >> http://get.splunk.com/
> > _______________________________________________
> > Emc-users mailing list
> > [email protected]
> > https://lists.sourceforge.net/lists/listinfo/emc-users
> >
>
>
>
> ------------------------------
>
> -------------------------------------------------------------------------
> This SF.net email is sponsored by: Splunk Inc.
> Still grepping through log files to find problems? Stop.
> Now Search log events and configuration files using AJAX and a browser.
> Download your FREE copy of Splunk now >> http://get.splunk.com/
>
> ------------------------------
>
> _______________________________________________
> Emc-users mailing list
> [email protected]
> https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
> End of Emc-users Digest, Vol 16, Issue 11
> *****************************************
>
-------------------------------------------------------------------------
This SF.net email is sponsored by: Splunk Inc.
Still grepping through log files to find problems? Stop.
Now Search log events and configuration files using AJAX and a browser.
Download your FREE copy of Splunk now >> http://get.splunk.com/
_______________________________________________
Emc-users mailing list
[email protected]
https://lists.sourceforge.net/lists/listinfo/emc-users
