Using the Extrude Intersect command
- Brad Tallis
- 3 days ago
- 5 min read
Creating complex parts in Fusion does not have to be a tedious process. This guide shows you a faster way to build a radial clip part by using simple shapes and the Extrude Intersect command. You will learn how to stack layers like a cake and use clever tricks to keep your designs easy to change.
The Wedding Cake Method for 3D Modeling
When you look at a part that is round but has different widths, you might think of using a revolve. However, there is a simpler way called the wedding cake method. In this method, you stack cylindrical primitives on top of each other. This keeps your design clean and avoids complex sketches.
Using primitives is a fast way to work. You do not have to create a sketch, draw a circle, and then add a dimension. You simply pick the cylinder tool and type in your numbers. This saves several steps for every section of your part.
Starting Your Design
Before you begin, make sure your settings are correct. This part uses inches. You should also create a new component to keep your work organized. For this example, name the component "long axle."
Select the cylinder primitive from the create menu.
Pick the side plane to start your first shape.
Click the center point and enter a diameter of 0.48 inches.
Type in a length of 0.83 inches.
This is the first layer of your "cake." It sits on its side, but you can imagine it as the base of your part.
Stacking the Layers
Now you will add more layers to the ends of the first cylinder. This builds the length of the axle quickly. Use the Cylinder Primitive command again.
Second Layer: Select the face of the first cylinder. Use a diameter of 0.35 inches and a length of 0.67 inches.
Third Layer: Select the new end face. Use a diameter of 0.5 inches and a length of 0.14 inches.
Once you finish one side, move to the other end of the main axle. Repeat the process with the remaining dimensions from your drawing. On the other side, add a section that is 0.35 inches wide and 0.44 inches long. Finish that end with another section that is 0.5 inches wide and 0.14 inches long. You now have a rough 3D model of your axle without drawing a single sketch line.
Why You Should Chamfer Early
It is often better to add chamfers before you cut flat sections into a round part. If you wait until after you make the part flat, you will have more edges to select.
When the part is perfectly round, the edge is a single continuous loop. If you click that edge and add a 0.1-inch chamfer, it happens in one click. If you cut the top and bottom of the part first, that single loop breaks into four different edges. You would have to select each one separately. This little detail saves you a bit of time.
Using the Extrude Intersect Command
The Extrude Intersect command is a powerful tool that many people may not know about. Most people know how to join two shapes or cut one shape out of another. Intersect is different. It only keeps the material where two shapes overlap. Everything else is removed. This is perfect for creating a part that is round on the sides but flat on the top and bottom.
Creating the Flat Section
To make the flat faces, you need a new sketch. Use the front plane for this sketch.
Open the rectangle menu and choose the center rectangle.
Click the center point of your axle.
The drawing shows the part thickness is 0.234 inches. Type this into the height box.
The width of the rectangle does not matter as long as it is wider than your part. Type in 1 inch to fully constrain the sketch.
Applying the Intersect Operation
Once your sketch is ready, select the three profiles inside the rectangle. Right-click and choose the Extrude command.
Instead of cutting through the part, look at the Operation menu in the extrude window. Change the operation to Intersect. As you drag the arrow through the part, you will see the top and bottom of the cylinders disappear. Only the middle section inside your rectangle remains.
For the distance, do not type a number. Choose All from the extent type menu. This ensures that if you ever make the axle longer, the flat cut will always go through the entire part. This is a key part of parametric design.
Adding Slot Features
The next step is adding slots to the flat faces of the axle. These slots are 0.2 inches wide. They sit 0.7 inches from the end of the part.
Projecting Geometry
Start a sketch on the top flat face. Before you draw the slots, use the Project tool. This brings the edges of your 3D model into your 2D sketch. You will see purple lines and dots. This allows you to snap your slots perfectly to the existing part.
Drawing the Slots
Use the center-to-center slot command. Pick two points on the face and set the diameter to 0.2 inches. To make sure the slot is perfectly centered, use the midpoint constraint. Click the midpoint of the slot arc and then click the center line of your part.
Dimensioning to Arc Tangents
Dimensioning the slot according to the drawing can be tricky. Usually, Fusion wants to measure from the center of the circle. However, this drawing measures from the very edge (the tangent) of the slot.
Pick the Dimension tool.
Click the end point of your axle.
Right-click and select Arc Tangent.
Click the arc of the slot.
Now the dimension goes to the edge of the slot instead of the center. Set this to 0.7 inches.
Linking Dimensions for Faster Updates
When you have two slots that need to be the same, you can link them. Create your second slot just like the first one. When it is time to add the 0.7-inch dimension, do not type the number. Instead, click on the dimension you created for the first slot.
Fusion will now reference that first number. If you change the first slot to be 1 inch long, the second slot will change automatically. This saves you from having to update two different numbers every time you make a change.
Final Finishing Touches
The final step is adding small 0.02-inch chamfers to the edges of the slots. This removes sharp corners and makes the part look professional.
Select one edge of a slot.
Right-click and select Chamfer.
Type in 0.02.
Hold the Control key on your keyboard.
Select the other three edges while holding the key.
This lets you apply the same chamfer to all four edges at once. It keeps your timeline clean because all four chamfers stay in one single feature.
Conclusion
Using the Extrude Intersect command is a smart way to handle complex geometry. By combining it with the wedding cake method, you can build parts much faster than using traditional sketching. This workflow is cleaner and easier to manage when you need to make changes later.
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