Hi everyone, I'm new to this forum, so I apologize if I'm not posting to the correct discussion group. Here's my issue. Once in a while, when I launch a program on my CNC, the Z-axis will decide to go down into my waste board instead of going up... obviously, this is causing me a lot of grief. Anyone else seeing this? Thanks, Fred
Hi @Fred Roy, it's probably going to help if you give us a lot more information:- what machine, what controller are you using, what software for CAD/CAM/CONTROL. Does this sometimes happen with a file that works at other times, or does it happen with some particular files? If it happens with files that have worked at other times then check for bad connections to your stepper motors and make sure you haven't got any mains leads or spindle drive leads near low power leads. Alex.
Good point @Alex Chambers ! The machine is one I built myself using components from Openbuilds. The controller is the xPro V4 using software version 1.0.174. I use Fusion 360 for the CAD and CAM. Yes, it will happen sometimes to a file that works at other times. Sometimes, disconnecting and rebooting fixes the issue, but sometimes it doesn't. I think I partially found the issue. I don't have homing switches on my machine (yet), but I noticed Fusion adds the G28 command to the G Code. If I understand correctly, G28 is a homing command. If that's what's happening, then why isn't it doing that every time? Yesterday, I was working with a new file and disabled that line (G28 G91 Z0) and had no issues. Maybe that will be solution. Thanks!
What post processor are you using with Fusion 360? This one is highly recommended: sharmstr/GRBL-Post-Processor G 28 will, I believe, return to a pre-defined point (G28.1) so could cause problems if you haven't consciously defined one. I would, though, given the symptoms, have a look at how leads are routed to keep noisy mains leads away from low voltage ones. Alex.
Your Xpro is running GRBL firmware. GRBL sets the G28 position to 0,0,0 (same as machine home) if you don't set it yourself. So the question is, "where is home". Without a homing cycle, home is where you turned it on. You should turning it on with Z as high as it will go. This is easiest to do if you park it there before turning off. If you do this, then G28 is a valid and safe default, safety moves like 'G53 G0 Z0' will be useful and safe, and you will not be surprised by seemingly random moves. On my machine I always turn it on with the Z up and the gantry at the far right corner (positive ends of travel). This is the industry standard and Gcode generators expect this. This basically 'fakes' a home cycle, you always know where machine home is and this means that your most recent set of work offsets all still valid after a power cycle. This came in handy last night when the power went off in the middle of a cut. I turned the drivers off and pushed the gantry back and right, wound the Z up and then reset the controller when the power came back on (my controller stays on because the laptop powers it). I then double checked the Z height which was spot on and continued the cut. There is no visible restart point in the cut. So, assuming you are doing something like the above then the other thing it could be is interference on the Z direction pin. However, I would not expect this to last longer than a step or two so a prolonged move is probably not this.
