Join Thom Tremblay for an in-depth discussion in this video Adding internal features, part of Fusion 360: Designing for Plastics.
- [Instructor] On plastic components, you will often find the most complex geometry on the inside. Ribs, webs, and bosses can take on many dramatic shapes and remain unseen. With the model in a solid state, it's now time to start building the internal structures. There are two sketches, one that we'll use to create an opening for the screen and another that we'll use to create two bosses to support buttons. We'll start out just using the Extrude tool. I'll select the rectangle, and begin to drag the rectangle.
As I do, and it comes in contact with the model, it will switch the operation to Cut. I want this to go all the way through, and I want to make sure that it's not affected by any possible changes to the geometry of the housing, so I'll change the extent to All. Clicking OK to create the opening, I'll use the keyboard shortcut of E to restart the Extrude tool and select the two circles. I'll start to drag out their size, and it will be adding geometry until it makes contact again.
For this, I'd like to change the extent to Object and select the inside face of the housing. This will add geometry that comes in contact and takes on the shape of the inside of the housing. I'll click OK to generate these two new bosses, and then let's take a look at the timeline. In the timeline, the end marker is not all the way at the end. There are three features, an extrusion, a plane, and a sketch after the timeline marker.
I'll expand the Sketches folder so that we can see that there are currently four sketches. When I drag the timeline marker to the end, a fifth sketch will appear, as now it is part of the model. You'll also notice that an opening appears underneath the screen created by the extrusion in the timeline. We'll come back to these features in a moment. First, I want to build the internal support for the LCD screen. I'll turn the screen sketch back on, come to the Create menu, and start the web tool.
The web tool will create geometry based on a thickness using open or closed sketch geometry. When I select the rectangle, it will generate a thickness going a direction. I can drag the thickness, or set the value, and take a closer look, seeing that it's going the wrong direction. I'll use the Flip Direction option in the dialog and then take a closer look and see that the shape is now coming through the front of the housing.
This won't work either. If I look also, I can see that it's creating geometry on both sides of the sketch. I'll make sure the thickness option is set to one direction, and now the geometry is going to the inside of the sketch, and still coming out the front. That's because the sketch, which was used to create the opening, is allowing the geometry to come through instead of terminating on the curved face. To fix this, I'll change the direction that the geometry is being added based on the sketch by having it develop on the outside by using a negative value.
When I update this, there is no geometry coming through the curvature on the front of the housing, but it is still building the support structure on the inside. This is exactly what I need, so I'll click OK to add this geometry. Now I'd like to turn the grill sketch on, and I'll start the web tool again using the Marking menu. Making sure that I can clearly see what I'm working with, I'll use a window selection to grab all the lines in the grill sketch.
Upon grabbing them, you'll see a pretty dramatic preview. I'll set the thickness value to one millimeter, and this will update the grill, but still, it's clearly not right. I'll flip the direction, which will put the grill back through the opening, but now it's on the outside. So I'll change the depth option from To Next to the Depth definition. Then, I'll drag out the value to 1.5 millimeters.
This will create a complex grill using the web feature in simple steps. I'll create OK to generate this, and that will complete my webs. The next step I'd like to take is creating a rib. I'll turn on the rib sketch and take a closer look at it. When I look at the rib sketch, it's floating in space, not in contact with the boss or with this face. And that's fine. The rib feature will still work with it.
I'll start the rib tool, select the sketch, and make sure that the thickness is correct. You'll see that it's generating geometry that fills the space between the curved face of the boss and the curved face of the housing. I'll click OK to create the rib. Now, I need more ribs, so I'll go to the Create pulldown and under Pattern find the circular pattern tool. Make sure the Features option is set, and select the rib feature from the timeline.
Then, I'll set the curved face as the axis. I can change the number of features that are generated using the manipulator, but three is just fine. I'll click OK to create the ribs. Now I need ribs on the other boss, so I'll use a pattern again. I'll create a rectangular pattern this time, again making sure that the features is the pattern type, and then holding my command key to select the rib and the pattern of the rib.
I'll set the direction using the inside edge of the LCD panel opening, and drag out a value. I need two instances, 26 millimeters apart. When I click OK, it will generate the second set of ribs. It would've been acceptable to create one boss, add the ribs, and then pattern all the features, but I wanted to show that Fusion 360 could take an open-sided sketch, generate a rib, generate a pattern of that rib, and then pattern that pattern and still generate an intact, solid model.
This is a great sign of just how robust the modeling capabilities of Fusion 360 are. The last feature I'd like to add at this stage is Hole. I'll create a hole for the button in the top boss, centering it and making sure that it goes all the way through and that it is 13 millimeters in diameter. I'll repeat the Hole tool to add the hole to the second boss as well. Let's take a step back and take a look at all the detail that's been added in just a couple of minutes in Fusion 360.
And now, with all the internal structures in place, we can start to focus on the details required to manufacture the component.