For alternative option learn how to prepare toolpath in Rhino
Now we should have all the pieces that we need to generate the toolpath.
Prepare Toolpath in Fusion360 (CAM)
Switch over to Manufacture environment (top left corner). In Fusion360 toolpath operations are contained inside Setup folders. Setup contains information about your machines coordinate system, workpiece model and material stock.
To modify setup right click Dental trimming setup and select edit.
This will bring up setup properties window.
First thing we need to do is make sure that our work coordinate system represents how our machine is setup so that our digital model matches our physical setup in the machine.
Then we need to set Model as Dental guide body
In the second tab Stock we need to set stock from solid and select dental guide body again.
Multi-Axis Contour setup
The type of operation that we are using for trimming toolpath in Fusion is called multi-axis contour.
To modify the preset toolpath right click on Dental trim and select edit. This will bring up toolpath properties window.
In Fusion360 all toolpath operations structured in a similar way. Toolpath properties are split in to 5 tabs (Tool, Geometry, Heights, Passes, Linking) that you need to fill in from left to right to complete the toolpath.
Starting with the first tab we need to select a predefined tool or create a new one. Pay attention to setting right feeds for your tool. (tip: run your toolpath in the air first time to see if your speeds look right)
Select the (Tool) (Select) box and add or modify your tool dimensions.
If youre creating a new tool make sure you describe its geometry accurately, particularly tool length. Body length and then overall length are both your total tool length, which is measured from spindle face to the tip of the tool (it is important to get this measurement accurate)
Curve Selection: In (geometry) and (Curve Selections) subheading Select the sketch curve. Look for a (red arrow) located on the curve>ensure this is outside of the curve (Select it to change it)
Geometry: In (Model Surfaces) select the (guide wall) body
In passes tab we control our tool inclination. In the sideways tilt we specify tool angle away from normal(perpendicular) to the Guide wall geometry. This tilt allows the tool and machine head to stay clear of adjacent workpieces and not collide with current workpiece as the cut is performed on internal part of the arch.
Click OK to generate trimming toolpath.
Simulate and amend toolpath
It is important to simulate this toolpath and pay close attention to the tool angle, and the way the shaft moves.
Notice the Yellow axis changes, if their are many bunched together, it may be recommended to revise the curve to create a much more smooth tool path,
Delete the existing (Guide Wall) insert more points or move existing points, In the image below I have drawn a representation on how I would begin to revise the curve.
Remember to rebuild the wall each time the curve changes.
Repeat this process until you feel confident that the tool path will run smoothly.
"If you are unsure, run the machine without the stock and monitor the tool behavior, this may provide a good visual representation, until becoming more acquainted with this process"
Images below are for a curve that represents a smooth and flowing toolpath.
Notice that the tool does not enter the mesh, meaning that it does not cut into the 3D Print.
Notice that Yellow axis lines are not largely bunched together. This indicates that the tool does not move sharply while trimming.
Export tool path into text file using Post-processor. Run G-code in Mach3.
To prepare toolpath for multi-aligners setup go to Next step