Afternoon All. Firstly I hope you are all safe and well in this challenging time. I have a Workbee 1000 x 750 screw drive from Oooooznest. I recently updated the firmware etc and got the machine online. I now get limit errors on all my programs. I wanted to re-flatten the bed, so I have a really basic facing operation drawn in Fusion360. I get the following error: I have attached the g-code file and my config file. Is anybody able to offer some guidance? Thank you all very much for reading this far Best Regards Colin.
Hi @Colin Hart, on my phone and about to have lunch but will have a look this afternoon. Have you upgraded to V7 firmware? Did you install the version for your size machine? Did you install the new User Interface (it's a separate step and I overlooked it the first time I did it) Alex.
Hi @Colin Hart, as @Rob Taylor has pointed out, your g-code is a bit big for your machine. According to the default settings from Ooznest your M208 lines are correct for your machine, so you have gone wrong in your cad. Alex.
Hi Alex and Rob.. Indeed this seems to be the case, however, no matter where I set my orientation on the XYZ X always seems to go positive. In F360 I have this yields So Y looks ok, yet X seems to be on the wonk. My stock option in F360 is 1mm top 0mm sides. Am I being very silly missing the total obvious or have I done things correctly? Help is much appreciated... REgards Colin
Try getting rid of the "select x and y" thing, leave it as "model orientation" and just select your G54 WCS on the same corner as you have it, see if anything changes. Might just be Fusion getting confused.
Evening Alex, Rob. Thank you for your advice so far... seems i am going round in circles. I do know if you use F360, but if you do I have shared a link to my spoiler board. Fusion It seems no matter what setting I try the initial X movement seems to be a positive number. Time to shut down tonight... head hurts.....
Are you setting the origin close to/at home position? Getting a bit late to play with it tonight, but will have a look tomorrow. Alex.
Just glanced through the code again. I see what it's doing. Fusion is thinking that your machine travel exceeds your part dimensions (which is sensible) and therefore it has space to provide proper machine acceleration between each line of cutting. At the top you have an arc into the material in X-Z, and as you scroll and you see the alternating blocks at X0 and X-622, the rest of each of those blocks is just an X-Y arc to move to the next line. So you need to a) move your origin off the "part" and to roughly the home switch location, or b) at the machine, set your G54 origin where it is in Fusion 360 (ie. slightly in from the machine limits by a few mm) and make sure that your Fusion "stock" isn't actually as wide as the machine, to provide room for the linking moves. However, the fastest way to fix the problem, whilst being the least pretty, is in your Face1 op, go to "linking moves" (the last tab) and switch from "smooth" to "straight line" in the last dropdown. That said, it may still want to go off the sides, like in this part I'm testing on: So there may be some manual code editing here and there to make it work. Personally, assuming it uses a consistent radius for its "smooth" linking moves, I'd just reduce the size of the material and let it think it's milling something smaller.
Addendum: Played some more with Fusion, it'll actually let you manually pull in the linking moves. If you pull them in by half the diameter of your end mill or thereabouts, it should work well. Here's an example with the same 3/4" cutter as above: So that's nice. Depends how much you want to play with it, I guess, though technically you should be able to reuse the same file forever by just adjusting your Z-zero, so it's probably worth playing with to get happy with.
Evening All... Apologies for the delay... sadly the calls of looking after children and work, well mainly work got in the way of me testing. So all fixed.... First Error. Was totally me (well both issues were me, but this is a bit a blazing ooops), i was testing by setting the Z axis 0 in the fully retracted position, this clearly pushed the Z axis out of limits. Second: @Rob Taylor said, I changed the linking to straight, this stopped the overshoot of the X axis. Thank you @Alex Chambers and @Rob Taylor for your help. Off to prepare this evenings Clap. Best Regards Colin.
