We use cookies to personalize content, interact with our analytics companies, advertising networks and cooperatives, and demographic companies, provide social media features, and to analyze our traffic. Our social media, advertising and analytics partners may combine it with other information that you’ve provided to them or that they’ve collected from your use of their services. Learn more.
However when I tested carving my fusion object, it worked perfectly untill right before the end, when suddenly it started drilling right over my material in a path I never had. the bit was completly down in the whole material of 1.9 cm. Looking at fusion simulatio I see something called “rapid collision with stock” and I wonder if that’s the reason. I have tried to eliminate these collisions, but i can’t seem to shake them off. any ideas?
Ah, I’ll bet it made something that looked just like this! All the way done, pulls up from the last move, then BRAAAAAAAAWP, right across the stock on a straight-line path, in a direction you didn’t specify, to a depth you didn’t order.
It took me a darn long time to figure this one out! I’d bet money that your G28 home is set somewhere random. The last move in a Fusion program, by default, sends your machine back to G28. That move is regardless of safety height and everything else, it’s a direct move.
To make my suggestions more useful, do you have homing switches on your X-Carve?
Ah, then I know what’s going on, to about 95% certainty, I’d guess!
You need to set your G28 home. There’s a ton of good information on the forum here about what comprises G28 and different ways to use it. To simplify for you into just what you need to do to make it stop doing horrible things to your projects:
Fire up the Carvey, and send your homing command. When it’s homed, go to the console of whatever G-code sender you are using (easel, UGCS, CP, etc) and send “G28.1” without the quotes. That will set your G28 home to the same spot as your machine home. After that, each project you run from Fusion will move to that spot at the start of each run, and return to that spot at the end of the run.
It is critical for this that you home your carvey each time you start it up, before you run a project. You will only have to do that once each time it is power cycled. When you start the run, don’t be alarmed when your first move is not necessarily in the direction of your first cut! It will go to the spot you set as G28 home (the same spot Carvey homes to, if you use the steps outlined) THEN it will move to start the first cut. At the end of each run, it will return to the spot you set as G28 home and turn off the spindle.
Congrats on getting going with a new machine, man!
Hey, that’s coming out nicely! I’ve had my best luck with V-Carve using a 60-degree bit, myself. Seems a good blend of fine-line and wide-line capability, without getting too crazy deep. I’ve had little to no luck engraving in Fusion with the engraving paths, it just doesn’t work well for me. Or, rather, I haven’t figured out how to MAKE it work properly yet. Generally, I use Fusion for all my functional machining, and V-Carve for machine engraving.
Glad that worked out for you, and congrats on a mostly-successful project! That’s 95% of the way there!
I hadn’t thought about using G30 that way, I’ve always just jogged it back a couple times with the 10" setting. I’ll have to set that, that’s a great idea!
Makes sense. My G28 is always set at the X0Y0 of whatever fixture I’m using, with Z homed (all the way up), then backed down ~5mm just to make sure it doesn’t go into the switch at the end of the job if the motor has somehow lost a couple steps.
Seems like that’d be an easy thing to add to the post-processor, just a last two lines to go to G28, then G30.
