Here’s one.
At the top right, click on your name and go to preferences. Under General preferences set your “Default modeling orientation” to “Z up”. This will save loads of headache when setting up your stock in the CAM software.
Also, right clicking on the entry fields while setting up toolpaths will allow you to set/retrieve default values for various settings such as feed rate, plunge rate, stepover, etc.
Click on your name in upper right, select preferences -> General -> CAM, and check the “enable cloud libraries” box. Then when you go into the CAM workspace and manage your tools you can save your tool library in the cloud instead of on the individual machine. Makes working across multiple machines nicer, but just better in general.
You can type your measurements in as a decimal or a fraction say 2.125 or you can type 2 1/8 fusion will accept either.
Learn to use offset planes. These things are awesome; especially if you use them along with lofts.
A really good video on lofts…but it also shows the power of planes.
Something I’m only just now understanding (and isn’t well explained in the docs and is done wrong in the example videos, even the ones from AutoDesk):
A “Setup” is the concept of placing a piece of stock in the machine at a particular place - nothing more than that. There is no “history” of what’s already been cut out of the stock between two Setups. This means for example that you should not have multiple Setups where each Setup is named after the router bit in the machine because that breaks rest machining.
An Operation is using a particular tool to make a cut on that piece of stock.
There is also the idea of a Folder under a Setup which can contain Operations. It has become clear to me that the workflow should be:
Then you run Post Processing on each of the Folders to generate the nc file for that bit. This is how you set up a project that maybe uses one bit for roughing and then another for finishing. When your entire project uses just one bit you can skip the Folder, but it’s probably good practice. You can also select a subset of Operations directly within a Setup and Post Process them, but you lose the inherent documentation of having the operations grouped by tool bit.
I haven’t actually tried this workflow yet, just developed it as a result of trying to figure out how to get rest machining and multi-bit carves rationally set up in Fusion.
I have my roughing and finishing passes all in the same setup. It works fine.
It works very well. It is how I set up a lot of what I have been messing with.
Another use for setups is if you want to carve both sides of a piece. If you make a new setup and invert the Z axiss, you can use that one to create toolpaths for carving the other side once you turn the stock over.
That’s actually what I found out today is that Setups aren’t actually a good separator for bit changes. You can’t do rest machining between setups. That’s why I’m proposing Folders under Setups as that separator - it’ll work better.
Another use for setups is if you want to carve both sides of a piece.
Yes, that’s what I meant when I said that a Setup is the concept of placing a piece of stock in the machine at a particular place. It doesn’t have to be a virgin piece of stock, just that all history of what’s been done to it in the past is lost, in fact that’s kind of the only legitimate use of multiple Setups in a project. First I put a piece of stock in one machine, did stuff to it. Then I took that object out and put it in a new Setup - it’s put in the same machine in a new way, or a different machine entirely and had different operations performed on it. If you think about that way a Setup makes more sense.
Here’s a link to the Fusion 360 forum post I started about this
The folks who have automatic tool changers don’t care about their being a separator between bits and don’t care about folks (like us) with “toy” CNC’s that don’t have that capability. While we naturally try to use Setups as the collector of Operations using a given bit and that leads us into problems with rest machining because of the mismatch in concepts.
I’ve been trying more with Fusion’s Rest Machining function lately - it’s the feature that’s described as only milling in this operation what hasn’t already been done in a previous operation. It’s a big time saver, but there’s an important tip to know. The rest machining feature works totally differently in 2D operations than 3D. If you select a 2D pocket clearing and turn on rest machining, there will be a setting for the rest machining tool diameter which defaults to twice the bit diameter. For a 2D operation Fusion will assume that everything that can be cut with larger than that diameter has already been machined and skip it - it’s not actually keeping track of what has actually been machined, and there can be bad surprises.
3D Rest machining actually does keep track of what has actually been cleared by previous operations within the same setup (that part is important), so there is no rest machining tool diameter setting in the 3D operation - it doesn’t “cheat” that way.
So if you were previously using 2D pocket clearing and that worked, but you get a little more fancy with multiple bit carving and rest machining and don’t get what you expected, you need to switch to the 3D pocket clearing and things will start working more as advertised. This happened to me, I was carving a sign and couldn’t figure out why some material between letters wasn’t getting carved even when I had passes for 1/4, 1/8, and 1/16" bits, but when I switched to 3D pocket clearing it all started working and taking the least amount of time.
I’ve been using Easel to do the gcode sending, so Easel seems to send the command to turn on the spindle before it actually starts to send the actual gcode. It also puts the final move to home (which I could do without, but have worked around) and then shuts off the spindle. So I didn’t even notice the issue you’re mentioning. I’m guessing you are using UGS?
One reason I didn’t like UGS was that it isn’t aware of whether the spindle is manually or automatically controlled, so in the event of some weird error condition where it didn’t make it to the end of the gcode file the spindle would be left running.
It’s unfortunate that Fusion doesn’t have a native way to group operations under a setup, so I used folders in lieu of anything else. But one thing for certain is that 3D operations that use Rest Machining will not work across setups. Rest machining works differently with 2D operations and could work across setups, but then has a different set of problems which are worse.
Hi guys, I’m new here and new to xcarve. I’ve jumped in on the deep end and gotten straight into fusion 360 CAM. I use CAD and CAE, so it hasn’t been too bad. I’ve found this thread and some YouTube channels extremely helpful (look up NYCNC). One thing I can’t get my head around is how to lock the steppers for a tool change. I don’t have limits for g28, but will add soon, but would like to get stuck in first and the first part I want to make requires a tool change. Any tips on this ?
Re. steppers locking, I believe there is a setup to keep them locked when stationary, but that causes heat and wear and tear. Is there a way to code the lock into just one place in the sequence?
Tia for any help, I’m looking forward to getting stuck in.
Anybody able to help?
Thanks PhilJohnson.
i will do some reading and give it a try.
