How to Model a Precise Mechanical Part in Fusion Using Sketch Constraints and Parametric Design
If you're transitioning to Fusion from another CAD platform, you're in for a streamlined modeling experience. In this tutorial, we'll design a precise mechanical part using Fusion's sketching tools, construction geometry, and full parametric control. You'll also learn how to move smoothly from 2D sketching to a 3D solid model, then into the drawing workspace—all in one powerful platform.
Step 1: Starting with the Sketch
Begin your design on the horizontal construction plane. We’ll place a center diameter circle right at the origin of the Fusion canvas. Set the diameter to 24 mm, or customize it to fit your project.
Next, add a second circle with a 42 mm diameter to create a closed, blue profile between the two.
Step 2: Add the Right-Side Geometry
Now sketch a third circle—this will define the larger end of the 3D part. Set its diameter to 36 mm, and then add a 100 mm distance between the centers of this and the original circle. You’ll notice the left circle becomes black (fully constrained), while the right one stays editable for now.
Add a final right-side circle and set its diameter to 64 mm. Reposition your dimensions to keep the sketch clean and readable.
Use the Fix constraint on the right-side circles to lock them in place as you build the next features.
Step 3: Connect the Circles with Tangent Lines
Draw a straight line between the two right-side circles. Apply the Tangent constraint to each circle. If Fusion adds an unwanted horizontal or vertical constraint, delete it first to avoid conflicts.
Mirror the line to the opposite side using a construction line and the Mirror tool. This symmetrical setup ensures that parametric updates are smooth—edit one side, and Fusion automatically updates the other.
Constrain the last blue line using another Tangent constraint to fully define the sketch.
Step 4: Creating the 3D Body with Extrude
With the sketch complete, go straight into the Extrude tool:
Extrude the first part to 24 mm
Extrude the second circle to 36 mm
Use the Join operation for the connecting middle section
If the sketch auto-hides, just turn its visibility back on from the browser.
Step 5: Strengthen the Model with a Central Support
Sketch on the vertical construction plane—no need to hide existing geometry. Just press and hold the left mouse button and select the plane from the menu.
Use Project to bring in the outline of the existing 3D geometry. Projected lines appear in purple and will auto-update if the model changes.
Sketch between the projected endpoints to create a fully constrained closed profile.
Set the Extrude Direction to Symmetric and choose Half Length. A 6 mm setting gives a total thickness of 12 mm. Keep the operation set to New Body, then Join the part with the main geometry. Repeat the process on the other side.
Step 6: Add a Cut Feature
On the top face of the solid, sketch a center rectangle using the point where the red axis intersects the body.
Set the rectangle dimensions to:
Length: 10 mm
Width: 6 mm
Then, use Extrude Cut to cut through the body. This ensures the cut adapts if you modify the thickness later. Pro tip: fully constrain the sketch before extruding to keep the model robust.
Step 7: Save and Move to the Drawing Workspace
Now’s a great time to save your project.
In the Drawing workspace, Fusion gives you manual and automated options to generate professional drawings.
Create a Base View of your model. Fusion keeps your design and drawing in separate files, which makes things easier to manage. Once placed, scale and reposition the view as needed.
Add a Projected View and adjust its position. Use Auto Dimension to let Fusion suggest dimension sets. You can customize these for density and clarity.
Final Thoughts
You’ve now modeled a precise mechanical component from sketch to solid, then translated it into a clean technical drawing. This workflow demonstrates the power of Fusion's parametric modeling and sketch constraints—tools that help you build parts that are adaptable and production-ready.
Chapters:
00:11 Create your first sketch
00:21 Start your sketch with a circle
00:53 Use a dimension to position your sketch
01:08 Why the sketch is black
01:35 Constrain your sketch
01:45 Add a tangent constraint
02:15 Trim and mirror your sketch
02:56 Fully define your sketch
03:17 Extrude your sketch to a 3D model
03:32 Turn on the visibility of your sketch
03:39 Extrude the section between the circles
04:03 Create the support structure between the circular bosses
04:13 Select behind an object
04:24 Project a sketch from a solid body
05:11 Make a symmetrical extrusion from a sketch
05:28 Choose measurement setting extrude command
05:48 Connect the support structure with the circular bosses
06:09 Change from Extrude Cut to Join
06:34 Create a sketch on a body
06:44 Create and dimension a center rectangle
07:08 How to make an extrude cut operation
07:36 Create a drawing
08:12 Place a Base View
08:27 Change the scale of your view
08:44 Place a projected view
09:08 Adding dimensions to a drawing
09:18 Adding auto dimensions to a drawing