Join Thom Tremblay for an in-depth discussion in this video Creating a solid from the T-Spline, part of Fusion 360: Designing for Plastics.
- [Instructor] With the freeform shape nearly complete, it's time to revisit some of the needs of the manufacturing process. In this video we will add the last touches to the overall shape and convert the body to a solid model. I'll return to the sculpt workspace by editing the form, and coming back to the nearly finished model. One of the things that I need to make sure of is that this model would drop out of a mold, that there's sufficient draft in the faces around the side to allow this part to be injection molded.
One thing that can help is an analysis tool. Under the inspect pull down, I'll select draft analysis, I'll select the body, and then set the direction. There are no sharp edges or flat faces on this body, so I'll turn on the origin and select the Z axis. This will represent green, or the cavity side, and blue for the core side. If there are colors in between, such as I see on the side and the corner, that means that the draft is inconsistent.
So I need to make modifications to the model. I'll click Ok to leave the draft analysis on the screen, and make note that it adds an analysis folder to the browser. We can actually have different draft analyses. I can turn this on or off just by simply switching the light bulb icon. For now, I'll leave it on so that I can use the edit form tool to make modifications. Let's start with this corner. Symmetry is still on, so any change made to one side will be made to the other.
And any defect on one side, will be on the other. So looking at this it looks like there's an undercut going on, and we can see that looks true. Let's first start by grabbing this point and maybe moving it out. And while that seems to help, it's creating problems elsewhere. So that's probably not the correct solution, so I'll cancel that edit, grab the point at the top corner and pull it back, and we start to see the defect disappear.
Now there will be a shadow of the defect that remains, to remind me of where there was a problem. So let's take a look at this lower edge, and using the view cube I can align my view and it looks like yes, this is tucking back underneath, which is not good. So let's grab this edge and maybe this edge, holding the Shift key, and pull them out and with a little bit of adjustment, maybe just grabbing this point, in no time at all, I'm able to make the modification.
Now, I can again use the view cube to align my view and see that this edge kind of has a little wobble to it, so we'll just clear this up because of course, the manufacturing consideration is always critical. We also want to make sure that we're able to maintain the aesthetic as well. All right, so now we have our part ready to be dropped out of a mold. But of course right now it's still infinity thin as well. To thicken this model there's a couple of different options. Let me finish the edit form tool and turn off my draft analysis and turn off my origins.
One option is to use the thicken tool inside of the sculpt workspace. I'll go to the modify pull down, and select the thicken tool. When I select the body I can drag which side I would like to thicken it to. What this will do is not create a solid model, instead it will create a series of parallel faces at a specific distance. This will create some interesting options. Since these are parallel faces they too can be modified using edit form, so you can create a unique interior shape to the exterior shape.
So there are designs where you want a very, very complex exterior and a very, very simple interior. This will make this easy to do. Some of the other options are to have the thicken type be sharp, so that it will create a face that creates a flat transition between the inside and the outside. You can also use a soft transition, which will create a round shape from the inside face to the outside face, or you can say no edge, which will just simply create a series of parallel faces that don't have a connection initially, so you can define it down the line.
The key with this model is that I'm not 100% sure yet how thick we want this body to be. So in all reality, having a parametric approach or the ability to change that design based on a dimension, would be better, so I won't use the thicken tool in the sculpt work space. Instead I'll finish my form and return back to the model workspace. In the model workspace, under the create pull down, I can find the thicken tool. Select the faces using a window, and set the thickness to minus two millimeters.
This will create a solid model, but the back face might not be completely flat because what it will do is create faces that are normal to the adjacent face. So it will be a series of faces with curves. This isn't necessarily a problem either. Taking a look at the right, I'll turn on my origin, and see this is very, very close to my XY plane. So I will create an offset plane based on the XY plane, bring this in maybe a millimeter, and now use this new plane along with the split body tool, under the modify pull down, selecting the solid and then using this new plane for the splitting tool.
It looks like it's going to cut off a portion of the entire shape, which is exactly what I want. I'll click Ok. And now it looks exactly the same except there's a line around it. This is where the use of bodies inside of Fusion 360 is important to remember. In the browser, I'll expand the body's folder, and see that there is the original T-spline body, which is hidden. There is this new body that was just created based on the old one.
That is this lip that has the uneven faces. And then the body that i want to maintain. So I'll give this a name and simply turn this body off. Now I have a flat face that I can build with. I could add a lip to it for a plastic feature, I can start creating the details around my solid model and complete the design using the hybrid approach, which allows Fusion 360 to use the best of freeform and parametric solid modeling.