Can you use fusion 360 without preset tools?
Typically using three tools, roughing end mill, finshing ball end mill and 45 degree chamfer.
They are modelled as Fusion tools.
All have zero Z offset in LinuxCNC.
1. Design part in fusion, generate toolpaths.
2. Do three POST runs in fusion , one for each tool.
3. Mount first tool, touch off to top of material.
4 Load first tool path into LinuxCNC and run it.
5. Change tool and touch off against a place on the workpiece you know the Z of.
6. Run second tool path
Dougefresh wrote: Thanks kornphlake, I was thinking that would be the only way... So do you just make multiple copies of your part In fusion and then If you have three tools you would just save three individual files with only one tool path per file?
No, no need for anything so complicated.
In the setup / operation tree in the CAM you can right-click anywhere in the tree and postprocess only that selection.
So, just pretend that you have preset tools, store tool types, diameters, feeds and speeds in Fusion in the normal way.
Then make your post-process selections in such a way that there is only one tool per file. Choose file-names that make it easy to figure out the sequence of ops.
Fusion will automatically put a comment on the top of the file about which tool is used. Read that when you load the file, load that tool, tell linuxCNC that you have done so with a manual M6TnG43 and touch it off to your work or setting plate. (Preferably into the tool table, but either ought to work with this procedure)
Then just run the file.
Practice with birthday candles for tools