I’ve been running into a problem accurately zeroing the Z axis when I use UGS. Before issuing the gcode I home the machine (standard limit switches, no noise eliminating mods), then I lower the Z down to the surface of the stock and hit “reset zero”, and then issue the start. When I issue, the bit initially raises all the way to the Z limit, instead of the retract height established in the code, moves to the position of the first cut and goes to work. For the rest of the job the retract height that I define in Fusion is used and everything is good. The problem is that the initial full retraction adds anywhere from 1/16" to 1/8" of error in the Z position, so my first cut ends up being too deep or not cutting at all (leading to too shallow a final cut). I think the error is coming from the switch, and if I could modify the Gcode to make that very first retraction stop at a specific point rather than hitting the limit switch it should solve the problem - but I dont know which command is responsible for the retraction. Alternatively maybe I could set a “soft limit” but it’s not clear to me on the Z if the soft limit is intended to limit downward movement or the retraction height (what I’ve read makes it seem like people use them on Z to keep the bit from cutting in to the backer)?
Just because of the way that G-code reads I would guess that the G28 line is being inserted by his post processor. If so, it should be removed from the post processor or he will have mysterious problems from time to time which will be very difficult to track down.
The Z0 ending doesn’t make any sense.
G28 Z0 G91 would make more sense, but is definitely not what he wants as that says go to the G28 position passing through Machine position Z = 0.
[Edit] ********* correction -> passing through Work position Z = 0
what i do is home he machine, reset all the axis’s, he jog to the surface of the material at my origin (X0,Y0) and write the number down. Then I load it in the program as the work offset with the G10 command.
Pretty consistent so far, with no strange moves.
With generic post processors, you always have to edit the g code. I see a lot of things that you can remove ( M6, M8, etc.) and you can do it by hand -editing the text, or dice in to the post and tweak it, once and for all.
There is no need to edit the code by hand every time. In the post processor options (comes up when you press ‘post process’) you can tell 360 to not use the g28 command.
You can also tell it to not send tool change commands somewhere too I think. I use chillipeppr to send the code to the x carve and it has an option to not pause on tool changes so I’ve never had to set it up in 360.
If you have limit switches though, why not set up the g28 location using the G28.1 command? You can set the location to be somewhere at the back of the machine so the work surface will always be clear for you when not carving.