Hi Greg, et al Ah! Now the intermediate point make sense.
As for an alarm with G28... I wouldn't know. I can comment that with G54 and G53 co-incident a G53Z0 does not cause an error when tool length offset is active. Because of this I've gotten in the habit of raising the spindle and then canceling the tool length offset. However, being the basic chicken I tend to: G53G0Z0M5 G49 G53G0(tool change position). (MSG, ...... HTH Dave On Aug 4, 2007, at 3:09 PM, Greg Bentzinger wrote: > Quote Date: Sat, 4 Aug 2007 17:41:19 -0400 > From: "Steve Stallings" <[EMAIL PROTECTED]> > Subject: Re: [Emc-users] G28 return to home > To: "Enhanced Machine Controller \(EMC\)" > <[email protected]> > Message-ID: <[EMAIL PROTECTED]> > Content-Type: text/plain; charset="us-ascii" > >> 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. > > End quote------- > > I must add that a move: > > G90 G28 Z0. > > Will generate an alarm if Tool offset ( G43 ) is not cancelled with a > G49. > > G91 G28 Z0. ( will ignor a tool offset ) > > I do not know if having a cutter comp ( G41 | G42 ) has any affect > on a > > G90 G28 X0. Y0. > > move. I have stuck with using G91 mode exclusively since it seemed > less > error (alarm) prone. > > Also G91 G28 is always based on the G53 native coordinate set. > > PGAB > > ---------------------------------------------------------------------- > --- > 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
