How would you make this part?
- Brad Tallis
- 3 days ago
- 6 min read
This blog post breaks down the process for creating a detailed mechanical model in Autodesk Fusion. By using smart features like the pattern and hole commands, you can speed up your design process. The key focus is on keeping all sketches fully constrained. This lets you change the model later and get predictable results. We will build a complex part by breaking it into three simple shapes and using powerful tools.
Beginning with a Fully Constrained Sketch
The first step is to draw the part's side profile for a revolve. Always start a new component and check your units. In this case, the design uses millimeters.
Create your first sketch on the front plane. Start with a center line from the origin. The overall height of this part is 63 mm. Type this in first to set the main dimension.
A good tip is to keep your sketches folder open. This lets you see if your sketch is fully constrained. You should always tell Fusion exactly how you want your sketch to behave. Do not assume lines you drew are horizontal or vertical. Add constraints manually to verify lines are horizontal or vertical.
After drawing the basic shape, you must add dimensions from your reference drawing. A helpful trick is to click the center line first, then a point. This creates a diameter dimension instead of a radius.
Dimension Type | Value |
Overall Height | 63 mm |
Top Diameter | 50 mm |
Lower Step Height | 6 mm |
Interior Notch Height | 11 mm |
Base Diameter | 106 mm |
Middle Diameter | 40 mm |
Lower Diameter | 36 mm |
Sometimes you need to add fillets directly in the sketch. Usually, you add fillets in the 3D model. However, if your design needs a specific offset from a fillet, it may be easier to sketch it.
Use the offset command on that single sketched fillet. Then, trim away the extra geometry. Trimming can remove constraints and/or dimensions. You will need to add them back. You can check your sketch by dragging blue lines. This shows what is still unconstrained.
Creating the Main Body with Revolve and Hole Commands
Once your sketch is fully constrained, use the revolve command. Because you drew a center line, Fusion will automatically select it as the axis. Revolve the profile 360 degrees to create the main 3D shape.
Next, create the large hole through the center. Use the hole command for speed and power. It is much faster than sketching circles and extruding.
Select the top face and drag the blue dot to the white center snap point. The drawing calls for a 24 mm diameter hole going all the way through. It has two counterbores.
Top Counterbore: Diameter 30 mm, Depth 10 mm.
Bottom Counterbore: Diameter 28 mm, Depth 8 mm.
You cannot make a "counterbore on both sides" in one step. Create the top counterbore first. For the bottom, run the hole command again on the bottom face. Set the termination to "To" and pick the face of the top hole. This ensures the hole always goes all the way through, even if the part height changes.
Finally, add the 1 mm chamfers shown on the drawing at the top and bottom edges.
Adding Tapped Holes with a Circular Pattern
The next major feature is three M4 tapped holes on the top flange. According to the drawing, they are on a 40 mm diameter circle. The holes are drilled 12 mm deep, with threads 10 mm deep.
Create a sketch on the top face.
Draw a 40 mm construction circle.
Place a point at the 3 o'clock position. A good tip is to place the point above the circle line. Then, add a horizontal constraint between it and the circle's center. You will see it snap into place visually.
Use the hole command on this point. Change the settings to create a tapped hole.
Hole Type: Countersink
Tap Type: Tapped
Thread: ANSI Metric, Size M4
Total Depth: 12 mm
Thread Depth: 10 mm (use the "Thread Offset" option)
Now, use the circular pattern command. Select "Features" and pick the hole you just created. Select the central cylinder as the axis and set the quantity to three. The pattern creates all three holes instantly.
Designing Side Notches with Extrude and Pattern
The part has four indentations around its base. The drawing shows they are 12 mm wide on a 90 mm diameter circle. They are 2 mm deep and have a 6 mm hole through their center.
Create a sketch on the flat face of the base. Draw a 90 mm construction circle. To place a feature at 45 degrees, draw two construction lines from the center to the circle. Then, dimension the angle between them to 45 degrees.
Draw a 12 mm circle centered where one line meets the 90 mm circle. Draw two lines tangent to this small circle that touch the part's outer edge. Make these lines parallel to your construction line. This creates the notch profile.
A common problem is selecting the profile when a large fillet is in the way. Click and hold on the face for a second. This lets you "probe through" and select the sketch profile underneath.
Extrude this profile 2 mm into the part. To avoid leaving a thin "sliver" of material from the fillet, use the "Two Sides" extrude option. Cut 2 mm in one direction, and in the other direction, extrude "To" the top of the part. This cleans up the geometry.
Then, use the hole command to add the 6 mm diameter hole through the center of the notch.
Finally, use the circular pattern command. This time, select both the extrude cut feature and the hole feature. Pattern them around the central axis with a quantity of four.
Building Offset Features on the Cylinder
The part has a cylindrical boss offset from the main body. The drawing shows its front face is 36 mm from the center. Use the Offset Plane command to create a construction plane at this location.
A new Fusion feature lets you "extend" this plane after creation. This makes it easier to see and sketch on.
Create a sketch on this new plane. You need to project geometry from the main cylinder. Use the "Project" command with the "Bodies" option. This projects the body's silhouette, giving you vertical edges to reference.
From this sketch, you will create the main boss and four smaller screw bosses. A good method is to pattern the small bosses within the 2D sketch. While 3D patterning is usually better, pattern-in-sketch ensures the features properly intersect with the curved geometry.
After sketching, use the extrude command. Select all the small boss profiles. Instead of a set distance, choose "To" and select the cylindrical face of the main body. Set the operation to "Join." This makes the extrusion wrap neatly around the cylinder.
You can then delete any leftover sliver faces. Fusion will heal the geometry automatically.
Using the Rule Fillet for Speed
The final step is adding fillets. The drawing calls for many radius 1 mm fillets on the offset boss. Selecting each edge by hand would take a long time.
Use the powerful Rule Fillet tool. Click on a face from the boss extrusion. Look in the timeline to see which "Extrude" feature created it. In the Rule Fillet dialog, select "Faces or Features." Then, pick that extrude feature from the list.
Set the radius to 1 mm. Under "Topology," choose "Fillets Only." This applies the fillet to all interior edges created by that feature at once. It saves many mouse clicks.
The Power of Parametric Design
The entire model is built to be changed easily. Every sketch is fully constrained. Features like holes and patterns are used heavily.
You can go back and edit any dimension. For example, you can edit the first sketch and change the overall height from 63 mm to 70 mm. Because the hole terminates "To" a face, it updates correctly.
You can also use parameters. In a later sketch, instead of typing "36 mm," you could set the dimension to be Height / 2 + 5. If you change the "Height" parameter, the boss location updates automatically. This is the true power of parametric modeling in Fusion.
Conclusion: Streamlining Your Fusion Workflow
This walkthrough shows how to tackle a complex part by breaking it into pieces. The most important practices are to fully constrain every sketch and use the right tools for the job.
The hole command saves massive amounts of time over sketching circles. The pattern command lets you build one perfect feature and repeat it. The rule fillet can apply many edge treatments in one click.
By building your model this way, you create a smart design. You can update dimensions and know the rest of the part will adjust correctly. This makes your design process faster and more flexible for future changes.
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