Re: [Emc-users] Touch off / workpiece home coordinate
I don't know which version you are using, but judging from the message it appears that there is an interpreter bug. There is a table in the interpreter that contains pointers to the functions that implement the gcodes. The actual gcode number is multiplied by 10 to determine the index in the table. So, G5.2 goes in the 52nd slot and G5.3 goes in the 53rd slot. You can imagine how 5.3 and 53 might get confused with each other by a simple off by a factor of ten bug. That's just a (somewhat) educated guess about the problem. Ken Rob Jansen wrote: > Tom, > > The G53 command results in the following error: > > interp_error: Can use only G5.2 or G5.3 after G5.2 > > Is this a bug? - There is no G5.2 or G5.3, only a G53 and the manual does > not mention any dependencies on G53. > > I also read the information on G92 - it sets global offsets and affects all > coordinate systems. That's why I had problems understanding the touch off > ... > > G53 not working is too bad, but for now I'll use coordinate system 1 (G54) > as absolute system. That still gives me 8 fixtures to define which should be > just enough ;-) > > Regards, > > Rob > > > On Thu, Apr 30, 2009 at 9:07 PM, Tom wrote: > >> In MDI: >> >> Move to the machine origin. G53 G0 X0Y0Z0 (A0B0C0) >> >> Clear the G92 coordinate offset.G92.1 >> >> Use the G54 coordinate system. G54 >> >> Set the G54 coordinate system to be identical to the machine coordinate >> system.G10 L2 P1 X0Y0Z0 (A0B0C0) >> >> (watch the screen (in Axis) when you do this and you'll see the work >> offsets >> move to the machine home position.) >> >> Turn off tool offsets. G49 >> >> Turn on Relative coordinate display from the menu >> > -- > Register Now & Save for Velocity, the Web Performance & Operations > Conference from O'Reilly Media. Velocity features a full day of > expert-led, hands-on workshops and two days of sessions from industry > leaders in dedicated Performance & Operations tracks. Use code vel09scf > and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf > ___ > Emc-users mailing list > Emc-users@lists.sourceforge.net > https://lists.sourceforge.net/lists/listinfo/emc-users -- Kenneth Lerman Mark Kenny Products Company, LLC 55 Main Street Newtown, CT 06470 888-ISO-SEVO 203-426-7166 -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Touch off / workpiece home coordinate
Chris, I downloaded a version from cvs about two weeks ago - in the speed of EMC development this indeed is 'a while back' :-) Based on your mail I did a cvs update / compile and now G53 works. Regards, Rob Chris Radek wrote: > On Fri, May 01, 2009 at 09:39:07AM +0200, Rob Jansen wrote: > >> Tom, >> >> The G53 command results in the following error: >> >> interp_error: Can use only G5.2 or G5.3 after G5.2 >> > > This was a bug in TRUNK but I fixed it a while back. What version > are you running? > > > -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Touch off / workpiece home coordinate
Rob Jansen writes: > > Tom, > > The G53 command results in the following error: > > interp_error: Can use only G5.2 or G5.3 after G5.2 > > Is this a bug? - There is no G5.2 or G5.3, only a G53 and the manual does > not mention any dependencies on G53. As Chris R mentioned, check for which version of emc2 you are using. I was using a pre-release 2.3.0 Head recently and ran into a bug in an unrelated feature so I just installed the release version 2.3.0 and all was well. You can find more info on downloading / compiling / upgrading here: http://wiki.linuxcnc.org/cgi-bin/emcinfo.pl?Installing_EMC2 look at the following headings: 2.2. Getting the source with CVS 2.3. Getting the latest updates with CVS > I also read the information on G92 - it sets global offsets and affects all > coordinate systems. That's why I had problems understanding the touch off > ... Yes, that is why you must use G92.1 to clear them before touching off. > G53 not working is too bad, but for now I'll use coordinate system 1 (G54) > as absolute system. That still gives me 8 fixtures to define which should be > just enough > snip... That is a known bug, you should not have to go without the MDI G53 command... best, Tom -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Touch off / workpiece home coordinate
On Fri, May 01, 2009 at 09:39:07AM +0200, Rob Jansen wrote: > Tom, > > The G53 command results in the following error: > > interp_error: Can use only G5.2 or G5.3 after G5.2 This was a bug in TRUNK but I fixed it a while back. What version are you running? -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Touch off / workpiece home coordinate
Tom, The G53 command results in the following error: interp_error: Can use only G5.2 or G5.3 after G5.2 Is this a bug? - There is no G5.2 or G5.3, only a G53 and the manual does not mention any dependencies on G53. I also read the information on G92 - it sets global offsets and affects all coordinate systems. That's why I had problems understanding the touch off ... G53 not working is too bad, but for now I'll use coordinate system 1 (G54) as absolute system. That still gives me 8 fixtures to define which should be just enough ;-) Regards, Rob On Thu, Apr 30, 2009 at 9:07 PM, Tom wrote: > In MDI: > > Move to the machine origin. G53 G0 X0Y0Z0 (A0B0C0) > > Clear the G92 coordinate offset.G92.1 > > Use the G54 coordinate system. G54 > > Set the G54 coordinate system to be identical to the machine coordinate > system.G10 L2 P1 X0Y0Z0 (A0B0C0) > > (watch the screen (in Axis) when you do this and you'll see the work > offsets > move to the machine home position.) > > Turn off tool offsets. G49 > > Turn on Relative coordinate display from the menu > -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
Re: [Emc-users] Touch off / workpiece home coordinate
Rob Jansen writes: > > I'm lost. > I thought that the touch-off feature was for setting the workpiece home snip... > After homing my machine, giving machine coordinates, how do I manually > set the home coordinates of my workpiece to 0,0,0 ? > > Currently I search the sides of my workpiece and do a G92 X -5 / G92 Y > -5 but that's not really a good and solid way to work. > > Regards, > > Rob Hi Rob, After homing your machine you will still have the previous values stored from touching off even though you may have turned your machine & emc off. I cut and pasted some info from the Emc wiki below - and you can research more at: http://wiki.linuxcnc.org/cgi-bin/emcinfo.pl?CoordinateSystems In MDI: Move to the machine origin. G53 G0 X0Y0Z0 (A0B0C0) Clear the G92 coordinate offset.G92.1 Use the G54 coordinate system. G54 Set the G54 coordinate system to be identical to the machine coordinate system.G10 L2 P1 X0Y0Z0 (A0B0C0) (watch the screen (in Axis) when you do this and you'll see the work offsets move to the machine home position.) Turn off tool offsets. G49 Turn on Relative coordinate display from the menu now touch off on the workpiece using your edgefinder. Remember to add/subtract the radius of your edgefinder to your touchoff value so that the (X/Y) axis zero is position on the workpiece is equal to the spindle centerline. When you touchoff the Z, Emc will not add a tool offset unless a toolchange command is given M6 T1 G43 H1 so if you are using a toolchange and tool number (like above) then you should enter a reference tool in the tool table with an offset value of 0.0 and use that tool for touching off in Z. Now you can move where you want and G0 X0Y0Z0 will always return you to your workpiece home, and G53 X0Y0Z0 will always return you to the machine home position. Tom -- Register Now & Save for Velocity, the Web Performance & Operations Conference from O'Reilly Media. Velocity features a full day of expert-led, hands-on workshops and two days of sessions from industry leaders in dedicated Performance & Operations tracks. Use code vel09scf and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf ___ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
[Emc-users] Touch off / workpiece home coordinate
I'm lost.
I thought that the touch-off feature was for setting the workpiece home
position.
So I search for the side of my workpiece with one of these LED feelers
("kantentaster" in Dutch, don't know the English term) and perform a
touch-off with 5mm. I thought this should set my coordinate (X or Y) at
-5, but i get real strange results.
After homing my machine, giving machine coordinates, how do I manually
set the home coordinates of my workpiece to 0,0,0 ?
Currently I search the sides of my workpiece and do a G92 X -5 / G92 Y
-5 but that's not really a good and solid way to work.
Regards,
Rob
--
Register Now & Save for Velocity, the Web Performance & Operations
Conference from O'Reilly Media. Velocity features a full day of
expert-led, hands-on workshops and two days of sessions from industry
leaders in dedicated Performance & Operations tracks. Use code vel09scf
and Save an extra 15% before 5/3. http://p.sf.net/sfu/velocityconf
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
