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Welcome to Day #9 of Learn Fusion 360 in 30 Days. I’m Kevin Kennedy,
and today we’ll model the shape of an LED lightbulb while learning to use the Sphere and Thread tools.
Note that today we’ll focus on the overall visual appearance without considering the manufacturing or other aspects of a real light bulb.
There will be times you’ll need to quickly create a 3D model for Rendering or communication purposes versus 3D printing or manufacturing.
We’ll start by creating a basic cylinder and sphere shape that we’ll refine as we make the lightbulb shape.
Instead of starting with a new sketch, we’ll activate the cylinder primitive from the Create dropdown menu of the Solid tab.
Notice it prompts us to select an origin plane or planar face. Let’s select the bottom XY origin plane.
Select the origin point as the start of the circle. We’ll define the width of the circle as 30mm.
After clicking to place the circle, you’ll see that we immediately enter the Cylinder dialog where we can define the Extrude distance.
At its core, primitives use the same building blocks as sketching the overall shape followed by an Extrude or Revolve command. They package this process into a streamlined feature. However, there are some drawbacks to using primitives, including potential reference and parametric issues.
I recommend only using Fusion 360’s primitive shapes when working on small or quick models, such as this visualization. For more complex models, particularly ones that need to be fully parametric, you should instead utilize fully defined sketches and modeling features.
Let’s define the height of the cylinder as 40mm.
We’ll need to create reference lines on top of our cylinder so we can sketch our sphere in the desired location.
Create a new sketch on the XZ origin plane, as this plane is located in the middle of our cydliner.
We’re going to use the ‘Intersect’ command to project the existing corner edges. Intersect is used as we only want the locations that “intersect” our active sketch plane.
Select the topmost edge and click OK. Notice the two corner points are now purple, indicating that we’ve projected them into our existing sketch. We can now reference these two points, knowing they’re the exact edges of the cylinder.
Let’s connect the two dots with the standard line tool, creating our first reference line across the top.
To have a starting point for the center of our sphere, let’s also create a new line running 20mm up.
Make these two lines a construction line as they’re only for reference purposes. This is not required, but a great habit to form as it will avoid issues in more complex models.
We can now activate the Sphere primitive from the Solid menu.
Start by selecting the endpoint of our construction line.
The width of our Sphere will be 61mm. We’ll also make sure the operation is set to “Join” so the sphere joins the existing cylinder.
Now that we have the basic shape complete, we can use the Fillet command to add material to the inside edge. Remember, Fillets will remove material from outer edges and add material to inner edges.
Activate Fillet and select the edge where the two shapes meet. We’ll define this Fillet as 45mm. Let’s also add a new Fillet in the dialog, followed by defining the bottom edge with a 4mm Fillet.
Before we create the thread, I’ll take a minute to add some appearances.
Activate the Appearances command. You’ll find Fusion 360 offers some LED appearances that represents real light when viewed in the Render Workspace.
To apply this appearance to just the upper portion, you’ll first select that part of the model. Notice this area is highlighted. This will ensure that our appearance is not applied to the rest of the model, since we’re working with a single 3D body. Drag and drop the appearance within the highlighted area.
We can then find a Grey Glossy Plastic to apply to the bottom faces. Note that this time we’ll need to select all four sections, which includes the bottom face.
After dragging the appearance over, we can also right-click on the appearance located in the “In this design” section of the dialog, followed by “edit”. It’s here that we can adjust the color and other appearance settings.
Take a moment to adjust the shade of grey.
Fusion 360’s Thread command requires us to select existing faces to turn into threads. With that in mind, we’ll need to first create an additional cylinder off the bottom.
We’ll make the diameter 22mm and the height 15mm. We’ll also set the operation to “New Body,” as that will avoid inheriting the existing appearances.
With our cylinder complete, we’ll activate the Thread command from the Create menu of the Solid tab.
Start by selecting the face of the cylinder.
We must check the ‘modeled’ option to have real threads in our model. Otherwise, these threads default to images, which helps save on computing power if you’d ever like to represent lots of threaded parts throughout large assembly models.
Fusion 360’s Thread command includes many thread presets. In this case, we’ll select the ANSI Metric M profile for the thread type. Select m22x3 for the designation and uncheck the full-length option. With ‘Full Length’ turned off, we can drag the bottom direction arrow to define an offset. Let’s define this as 3mm, which will provide sufficient room to Chamfer the bottom of the thread.
We can now add a Chamfer to the bottom sharp edge. Let’s define this as 4mm.
I’ll also add a final Fillet to the transition of the remaining sharp edge. Make this 2mm.
Lastly, we’ll need to add the “electrical foot contact” to the bottom of the bulb. Use the Cylinder command once again. This time with a width by snapping to the edge of the bottom planar face.
We’ll make this cylinder a height of only 2mm and set the operation to “New Body”. Again, this is not required, but it will make it much easier to apply a different appearance.
Let’s use Chamfer one last time by applying a 2mm chamfer to the end of the “electrical foot contact.”
Experiment by adding a metal appearance to the threaded body, and another appearance to the foot contact.
You’ve successfully completed the light bulb! I’ll see you on Day 10 where we’ll 3D model a phone case.
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