Jon, Also notice that when you "touch off" it asks you what coordinate system you want to set via the touch off.
For some reason I tend to use G55 on my lathe. Then after I am all setup. I have a G55 near the top of my program to get into that coordinate system and run the program. As you can see there are a number of ways to do this... Dave On 3/25/2010 7:07 AM, Andy Pugh wrote: > On 25 March 2010 11:19, John Guenther<[email protected]> wrote: > >> At any rate, I out of habit use machine coordinates all >> the time. >> > I think that is the problem. The machine coordinates are fixed to the > axes and can only easily be relocated by a homing process. > The machine will refuse to move outside these limits. > I think you said that you have no home switches? In that case I can't > remember what happens when you home the axis, I think that the current > physical position becomes the point at which the machine absolute > numerical position takes the value from the ini-file axis home > position. > > >> Perhaps a better example of what I would like to be able to >> do is this. I use a manual tool height setter. I put it a new tool, >> then jog Z down until the tool height setter shows 0 on its dial. Now I >> need to be able to tell EMC that the Z axis is at 2 inches above the >> work. How can I do this in EMC? I have tried the work offsets as >> suggested and that is not working for me. In Mach3 I just click on the >> Z axis DRO and enter 2.00 and I am ready to go. >> > This is exactly what the working coordinate systems are for. If you > change the view to "Relative" either from the menu or by pressing "#" > then you will see the current working coordinate values. > > Note that you are _always_ on one of the working coordinate systems. > You have to use special G-codes to move in the absolute machine > coordinate space. The distinction might not be clear in cases where > the working coordinate system has no offset from the machine > coordinate system, and this will often be the case for a machine with > no home switches. > > However, any G0, G1, G2, G3 etc move will always move in the current > (probably G54) coordinates. > > So, for a machine with no home switches the start-up process would be: > Select Absolute coordinate view > Move to the extreme limits of travel of each axis. Home the axes from > the GUI with the "home" button. I think you will see the machine > coordinates take on the home position values from the INI file, but I > could well be wrong. To save time and trouble you could set the home > position to be mid-travel and set the axes limits symmetrical about > this point. > Change the view to Relative Coordinates > Jog to where you want X=0 and Y=0 to be, set them to zero (or some > other value) with the touch-off button. > Bring your tool down to the height setter, select Z, press the > touch-off button and type in your 2" tool height value. > > You should now be good to go. > > Clicking the DRO in Mach sounds to be doing exactly the same thing as > EMC touch-off. > > There is also the option of touching-off into the Tool table, which > can be useful for machines with multiple tool holders, less so for > single collet machines. > > There is a lot more info on the Wiki, > http://wiki.linuxcnc.org/emcinfo.pl?CoordinateSystems > > Bear in mind that my understanding of this issue is incomplete, and I > don't have a machine here at work to experiment with. I still > sometimes find myself in a bit of a tangle with offsets and > "programmed move would exceed machine minimum...." when there is > clearly lots of space left. > > ------------------------------------------------------------------------------ Download Intel® Parallel Studio Eval Try the new software tools for yourself. Speed compiling, find bugs proactively, and fine-tune applications for parallel performance. See why Intel Parallel Studio got high marks during beta. http://p.sf.net/sfu/intel-sw-dev _______________________________________________ Emc-users mailing list [email protected] https://lists.sourceforge.net/lists/listinfo/emc-users
