Andrew Ayre wrote: > Jon Elson wrote: > >> Andrew Ayre wrote: >> >>> Hi, I've been happily generating g-code files and cutting them with >>> AXIS. I'm using EMC2 pre-2.2 CVS HEAD. Yes, I know it's old but I have >>> everything working and I am reluctant to change it right now as I am >>> trying to get Christmas gifts made as quickly as possible. >>> >>> With a new g-code file I get "Joint 0 Following Error" at the same point >>> every time in the file. Line 161 I believe. The g-code file is here: >>> >>> http://files.britishideas.com/public/emc2/jointerror1.ngc >>> >>> On April 17th, 2007 Chris Radek said this about the error message: >>> >>> "It means the difference between the commanded position and feedback >>> position differ by more than the allowed following error." >>> >>> I am using a simple, HobbyCNC card with steppers, three axis, no >>> feedback. I have backlash compensation set in the emc2 ini file. I have >>> cut lots of g-code files without a problem until now. Can anyone give me >>> some hints on how to solve this? Is it a problem with the g-code? >>> >>> >> A following error in this case means that the commanded velocity >> required more steps/second than the step generator could produce, with >> the settings of your system. It may be possible to make the step >> generator run faster by decreasing the value of BASE_PERIOD in the >> [EMCMOT] section of your .ini file. Warning! If you make this value >> too small, your system will freeze up when you start EMC. A quick check >> would be to set your feed override to 50% and see if the program gets >> past this spot. I didn't see anything near line 161 that looked like a >> sudden fast and long move. I do notice some G00 moves at other spots, >> which would command the fastest motion permitted by the .ini file >> parameters. That would be where I'd expect to see a following error. A >> 50% feed override ALSO affects G00 moves, so all motion should slow to >> 50%, and it should get past the bad spot. If it is really tripping on a >> G00 move, then you need to lower the MAX velocity in your .ini file >> (unless speeding up the BASE_PERIOD is possible.) >> > > Thanks for the detailed reply. I set the feed override to 44% and it > works (slowly), but I would like to better understand this so I can > avoid this in the future. > > I've set the BASE_PERIOD based on the latency test, and it is the > maximum my machine can run at. It gives me a max speed of 71.6 IPM. I > can't decrease this value, unfortunately. > > OK, then you already know the limits, you just need to set EMC to never ask for more than that. > The g-code file is supposed to limit the speed to 30 IPM, and you can > see this when running the file in AXIS. > > But, it has G0 moves in it, which will go to the MAX_VELOCITY in your .ini file. > However I now notice that when the file is running in AXIS the velocity > occasionally and only for a split second displays a value of 71.6 IPM. > Yup, those are your G0 (as opposed to G1) moves. > This raises two questions for me: > > - why would a movement cause the velocity to go beyond the maximum of > 30 IPM that I set? Is that a problem with AXIS/EMC2 or the g-code? > > - is this a symptom of the problem or is it normal? > > It is what your G-code is commanding, with the G0 moves. Prove it to yourself by editing the G-code file to change all G0 to G1 and run again. But, the proper fix is to give you some headroom. In your .ini file, change MAX_VELOCITY in both the [TRAJ] section and in each [AXIS_x] section to be 1.0 (1 inch/second = 60 IPM) and try with the existing program. You should now see the velocity spikes up to 60 IPM, and hopefully that will not cause any further problems.
Jon ------------------------------------------------------------------------- This SF.Net email is sponsored by the Moblin Your Move Developer's challenge Build the coolest Linux based applications with Moblin SDK & win great prizes Grand prize is a trip for two to an Open Source event anywhere in the world http://moblin-contest.org/redirect.php?banner_id=100&url=/ _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
