Similar to the benefits offered by near-net shape in the Cartesian coordinate system, parts that were created with a rotary printing operation can also benefit from CNC milling or post-processing. There are some critical differences between the setups for printing and milling that should be understood before proceeding:
In order to take advantage of mesh bed levelling during printing (keeps the printing tool at the same height above the mandrel at every point of rotation), the rotational axis is defined as 'Y', and the print surface is defined as Z=0. In CAD operations, the rotational axis is defined as 'A' and the axis center is defined as Z=0. Macros and workpiece offsets will take care of this, as detailed below.
To set up the model in Fusion360, set the slit of the model oriented down, in -Z, as shown below. This may differ from how the printable model was oriented, and that is because the model is always "centered" in Simplify3D - so the ends of the model (where it is slit) will be at +180 and -180. The center of the model (opposite the slit) is at 0.
The model origin is on the center axis of the part. The X position of the original will depend on how the part was setup in Simplify3D during printing. Most often, the part is centered in Simplify3D, and so should the origin should be centered relative to the part.
If you did not 3D print your stock, then this matters less. You can define the position of the part wherever you want, and then ensure that the machine WCS is set so that stock is physically present where Fusion360 expects it to be.
Generate your toolpaths by selecting 2D Pocket or 2D contour, and select "Wrap Toolpath" in the Geometry tab.
Post-process the toolpath and make sure that the "Caxis is installed" option is set to "no" (it is off by default).
Machine Setup - 3D printed stock
If you just 3D printed the model, then you will need to change the rotary axis to be defined as A instead of Y by running the attached "RotaryToA" macro. The beginning of this macro send the rotary axis to 0, and should move the seam to -Z, as shown below.
Next we will select our Workpiece offset. Everything should be the same as the WCS used for printing, except the Z position needs to be -R (negative of the mandrel radius). This is the simplest way to tell the machine that Z=0 is at the A center axis (which we defined above in Fusion360).
For example: if your mandrel is 38mm in diameter (19mm radius), and the machine is configured to be at Z=0 at the surface of the mandrel, then a WCS offset of Z=-19mm will put the effective Z=0 at the mandrel center axis. Because of the axis limits, the machine will never be able to reach the Z=0 position, but that is not a problem (unless you want to mill into the mandrel, in which case a different setup method is required). Below is what the offset would look like if using G59.
Machine Setup - from other stock
If you are starting with stock, then no changes are required to the machine axis. Simply clamp your stock (most commonly in the ER32 collet, but perhaps in the rotary vise), and press the Home A button.
To set the WCS, it is easiest to measure off of the axis drive body. Probe the top surface and set the Z value of the WCS to the current position minus 41mm. You want the Z=0 position to be at the axis center, which is 41mm below the probed surface.
Then probe vertical surface of the body with the "-Y(↑)" button and set the Y value of the WCS to the current value plus 26mm.
In both cases, it may be useful to do a sanity check by jogging away from the rotary drive and mandrel, and jogging to Y=0, Z=0. The tool tip should align with the A center axis at this position. If it does not, check that the WCS is correct and that the offsets were set correctly.
As a general-purpose sanity check, it is often helpful to "air cut" first. This is often done easily by moving away from the rotary drive in the X-direction. Jog the machine in -X until the turret is clear of the mandrel and set the WCS X position to current. Then run the CNC file and confirm that both the Z and A positions are where you expect them to be, and the speeds are appropriate.
Once you are satisfied with the CNC file, set your WCS back to the original position over the stock, and start the file again.
As always, feel free to post comments or questions on the forums.