Sometimes, we encounter issues with our generated toolpaths and need to limit what we want to machine. Simply changing the boundaries on the radii tab does not help much since Fusion still calculates using the original model and stock from the setup.
In the example below, I want to use an ID boring tool to machine the remaining stock from the part shown.
Notice how we cannot remove all of the stock. This is because the inner hub (in green rectangle) is interfering with out tool path generation. Even though we have set the radial limits for the inner radius to much more than that of the centre hub, it still does not solve our problem.
Using multiple setups
In order to get clean nice toolpaths for the selected face, we can create new geometry from the body we already have, create a new setup and use that new body instead.
Here’s how I did it:
Creating new geometry from your model.
I want to machine just the two faces selected in figure 1. To do this, I will simply create a surface offset of these faces at 0mm and extrude/thicken to create a solid body. I need a solid body for machining purposes as Fusion 360 will not recognize surface bodies to machine.
Now thicken this surface body to create a solid. Be sure to thicken in such a way that the surfaces you want machined are not modified.
At this point you should have a new body to work with. From here, we can simply go back to manufacture and create a new setup using our new geometry. Easy as pie.
Creating new setup
Since we have already setup everything in our original setup, we don’t need to redo everything. we just need to change two things:
- Redefine the model we are using (select our new body)
- Redefine our stock to pick up from where we left off with the previous setup (rest machining)
So to begin, we simply right-click on our setup and select duplicate.
We should have an exact clone which we can edit as per our changes mentioned above. Remember, it will duplicate all the generated toolpaths as well, so we can delete those since we don’t need them.
Edit the duplicate setup and make the following changes on the setup and stock tabs:
Select the new body as the model.
Select “from solid” for mode under the stock tab.
This will give you the option for rest machining and you can choose the previous setup as the selected solid.
At this point, we pretty much have what we need to proceed. We can generate the desired toolpath as required and we will find that it calculates based only on this new geometry.
NB: Remember to make the new setup active by toggling the circle next to it!
To proceed with the rest of the CAM process, we can simply repeat the above steps and create yet another duplicate of that setup.
When you are happy with your toolpaths, you may generate you NC code. Click on generate NC program button and move to the Operations tab. Since we have multiple setups, we must include all setups and all operations to be included in the final NC code output.
And we’re done! This can be useful in a variety of situations, not just turning and not just to get around toolpath limitations.