Fusion 360?

what post processor is used for fusion 360 and how do i add it?

If you go into Easle, and then select Import GCode, there is a text window that pops up with a link to the Fusion360 post processor.

Thank you

I just use the stock GRBL post that is included with Fusion. Works just fine! :slight_smile:

I tried running the stock grbl and my machine did some crazy stuff. The easel processor is just safer, in my opinion.

You absolutely must have your G28.1 home position set correctly. I crashed it twice learning that. But once it’s set right, I have literally hundreds of runs under my belt using it. :slight_smile:

After I figure out the whole g28 then I will switch back

It’s worth learning. Saves bucketloads of time running parts in a fixture, etc.

The way I work it is extreme simplicity. I just home the unit, then jog it until it is exactly where I want X and Y zero. Then I home JUST the Z-axis again, so that it’s all the way up and clear of my part. Then send “G28.1” from the input window, without the quotes. Now, any time (regardless of the machine being turned off and on, the position is saved) that you have homed your X-carve, sending or calling “G28” will take the bit straight back to that position.

Where that is extremely handy is if you have a fixture attached to your bed, and run it repeatedly. That way, every time you power up again, you just home, send “G28” from the console, and your tool runs right to X0Y0. Zero, and you’ve already got them set, ten seconds after power up! :slight_smile: Plus, the GRBL post in Fusion uses G28 as the home position for the tool at the beginning and end of each run, so it starts there and returns there. Having it at 0,0,MAX is a really good spot for it, since it’s highly unlikely to strike anything up there.


In the Fusion 360 post processor properties (the little window that pops up after you press ‘post process’) you can turn off using G28. It’s a checkbox.

1 Like

So a question about this, since I’ve never used this approach, but I have a fixture locked down to the bed so I reference every square object in the same place …

You say you “home” the unit, I assume you mean you use the homing switches ? I don’t have any, so wondering if I am unable to use this process.

As I understand your post, you send the machine to your intended starting position, with X and Y at 0, but the Z well up and out of the way of the piece. Then you issue the G28.1 command which tells the unit that’s your starting position?

I assume without a “homing” sequence, there’s no point in me trying this, since the machine has no idea of X, Y or Z when I power up, right …

So if I tried this, without homing switches, I could crash the head if I manually moved the carriage while the machine was off?

Yes, you will need homing switches. Adding them is trivially easy, you will need either the switches from Inventables, or similar ones from Ebay, etc. They’re very easy to come by, and extremely inexpensive. I think I paid $5 for my ten-piece sack of replacement ones. Attaching them uses the existing header, so you don’t have to solder to your board or anything.

Adding homing makes the entire X-carve work much better, and enables you to use machine homes. And if you’re already using a fixture on the bed, you’ll save the time you spend wiring your homing switches in the first couple runs!

Yeah, I actually bought the homing switches, and they’re installed on the machine, just not wired. I didn’t see the need, since they’re not limit, just homing, but now that I have a fixed reference position bottom left they make a bunch of sense, especially in conjunction with the process you outlined above.

Yeah, if you have them set up, once your machine has homed the G28 function works. And with a fixed corner position, it removes 75% of your zeroing for a project, right there, with extremely repeatable results. Add a touch plate for Z length, and you can zero for an entire job in less than a minute. Even better, with G28.1 set on that corner, you can very easily swap parts through the fixture for repeated operations, even if you have to shut the machine down and walk away for a while. For instance, during a lot of my production runs, I’ll spend a whole evening running one operation on a batch of parts, then come back the next day, power everything up again, return to my G28 position and zero out, switch to my next tool, touch it off, and carry on working right where I left off. :slight_smile:

Yep, I’m sold. :slight_smile: guess its time to wire the switches…

So G28.1 is a “home” position relative to the homing switches 0? And is retained even after controller power off?

Do I set X and Y at zero, but move Z up out of the way before storing? I assume so, since piece thickness varies between job.

Z axis touch plate (Charley’s) Is something I use a lot, I assume I could just do Z and avoid X and Y since they’re stored with G28.1?

“G28” is the command to go to a specific position, relative to the machine home that is established by the limit switches. “G28.1” is the command you issue from the console that tells the machine to “store current position as G28 home.” That position is retained after power off, so if you power back up, home the machine, then issue “G28”, it will return to that exact position. Remember, this is relative to the homed position, so you will need to MAKE SURE you home the machine when you start up! If you don’t, results can be unpredictable.

Since G28.1 orders the machine to set an exact position, it will return there in X, Y, and Z each time. This is independent of your tool offset set with the touch plate. So you are correct about what you have to set.

I would suggest homing your machine, jogging until your tool is exactly at the 0,0 point of your fixture, then homing the Z, which will put it right up at the top of its motion range. Then zero it out, and issue G28.1. After that, each time you call G28, it will return to that exact position, at your fixture’s 0,0 with the Z up at the top of the range. That’s where it will go to at the beginning of every Fusion job, and it will end there as well. Which makes it really convenient for changing tools. Once it’s there and you hit the zero button to set your work coordinates to 0 relative to that spot, you can jog freely and run your z-probing cycle just like normal. It basically just gives a safe position for the tool to go to at the beginning and end of each run, as well as automatically zeroing your X and Y to your fixture between power-downs.

EDIT: For a really good write-up on it, check out this thread here: Learning About G28