One useful capability of the H-Series is printing up your own "stock" then milling it back to get a high-quality finished part. This allows you to print faster (since you don't care about finish quality) and stronger (high-temp overextrusion improves layer-to-layer adhesion). This is often referred to as "near net shape" manufacturing, as the initial printed part is not the exact final geometry, but only near it.
We will use a small puck as a demonstration project. In Fusion360 or other CAM software, you will need to model up both the printed object, which will be slightly larger than the final object, and the final object itself. See our flowchart of the Hybrid toolchain. They should have the same origin, and be coincident on the bottom. See our support article on aligning coordinate systems.
How much larger the printed object is will depend on your print settings. It is important that the printed object be solid where it is milled. If it is not, then you will have voids on the surface of your final part. Here is the printed part:
In the model above, blue is an "adhesion layer" (one layer of TPU which sticks to the bed and the part, but which can be easily removed), grey is support material (helpful when you want your milling tool to reach the bottom of the final part, but not contact the bed), and green is the object to be machined.
All these files can now be imported into Simplify3D (or similar) for slicing:
Note: in this example, we have modelled each of the printed parts. You could also start with your final model and use Simplify3D to accomplish all of this:
- Raise the part off the print surface (this needs to be accounted for when you generate your milling toolpaths later) and generate support structures
- Use a raft to generate an adhesion layer (again, you'll need to account for the increase in Z-position)
- Scale the part up in X, Y, and Z to allow milling back to net
Once the part is printed, we can start a "Manufacture" setup in Fusion360. The Stock will be "From solid" - select the body that was used for printing. (If you used Simplify3D to move and scale the model, this is where you would ensure the Work Coordinate System matches your actual setup)
Now we can generate toolpaths as we would in any CNC operation. The great thing about near net shape processing is we don't have to find and orient our stock in the machine coordinates - we know exactly where we created it in the first place.
To generate the toolpath, select the Setup you want to use (G55 in the example below), then click the "NC Program" icon in the upper-left. That will bring up the NC Program window:
Make sure the HSeriesPost1.1 is selected (install it if necessary), then click "Post".
Although you can run the resulting file at this point, it is always a good idea to do an "air cut", which means running the job above the stock to make sure everything is working as expected. We do this by setting the WCS to a more-positive number. In the above example, we selected the G55 setup. So in the machine configuration, we will go to Offsets -> Workplace Coordinate Offsets -> G55 -> Z, and change the value from "0" to "100". This will cause the file we just produced to try and cut stock at 100mm above the print bed.
Now we start the milling cycle by uploading and starting the .gcode file:
During this operation, verify that the machine:
- Brings up the correct tool
- Turns on the spindle
- Turns on the air jets
- Operates in approximately the correct XY position.
If all this looks good, reset the G55 Z offset to "0" and rerun the program. It should mill the printed piece.
You can find the Fusion360 file below which includes the models and milling toolpaths.