Greg, 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 \(EMC\)" > <emc-users@lists.sourceforge.net> > 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. >
Correct! > 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. The above line would cause the Z axis to first move to the z0 of coordinate system in effect and possibly crash a tool (pragrammers responsibility) into the workpiece with no tool length in effect. > > G91 G28 Z0. ( will ignor a tool offset ) The above line specifies an intermediate point that equals the current point since it is incremental and the intermediat point is 0 distance from the current point. This is proper behavior. > > I do not know if having a cutter comp ( G41 | G42 ) has any affect on a > > G90 G28 X0. Y0. Cutter comp should be exited before using a G28 again the above lin being in absolute will cause the machine to move to program zore point and then to machine home. A possible crash! And again that's the programmer's responsibility. > > 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. > It should be based on the coordinate system in effect at the time, G54, G55, etc. with an incremental G91 G28 (z.x,y) the coordinate system is irrelevant since the intermediate point is 0 distance from the current point. > 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 > Emc-users@lists.sourceforge.net > 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 Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
