Mastering Surface and Solid Modeling in Fusion
Autodesk Fusion, formerly known as Fusion 360, offers powerful tools for blending surface and solid modeling. In this tutorial, we’ll explore a workflow that simplifies complex designs. If you watch the full video below, keep an eye on the keyboard shortcuts in the bottom left corner of the screen.
Laying the Foundation
We begin by creating a new component, followed by a sketch on a vertical construction plane. Using a circumscribed polygon ensures precise alignment. Starting at the origin keeps it centered on the horizontal construction plane, which will be useful later. A 5 mm distance results in a polygon with a total height of 10 mm.
Using a mouse with a scroll wheel makes zooming easier. Activate Construction Line mode and create two guide lines for the honeycomb pattern. Fusion helps snap the second line to the middle of the polygon’s side with a small symbol indicating the correct alignment.
Patterning the Design
Select Rectangular Pattern in the sketch environment—the option with unfilled symbols. Include the entire polygon and use both construction lines for direction. Set distribution to Spacing and direction to Symmetric for a balanced layout.
A small gap between polygons is necessary. Since half the polygon is 5 mm, the total height is 10 mm. Increasing the spacing slightly above 10 mm ensures the proper separation.
Rather than calculating the exact number of polygons now, we’ll generate more than needed and refine the design later. While it may seem excessive initially, this workflow ensures flexibility as the design evolves.
Creating the Base Shape
The key focus isn’t the polygons themselves but the space between them. A 2-point rectangle captures this space efficiently. Aligning with the grid allows for quick positioning, but dimensions can refine placement for precision.
If construction lines were left on, they appear as dashed lines. Simply select the rectangle and convert these to regular lines. Now, we have a closed profile forming the base of the pattern.
Setting Up Measurements
The height from the middle to the top is 22 mm, giving a total height of 44 mm. We then create a sketch on the horizontal construction plane and draw a center diameter circle at the origin. This circle forms a thin cylinder, defining the pattern’s structure. A 75 mm diameter maintains balance with the polygon pattern.
Use the Surface Extrude command on the circle. Set direction to Symmetric with a total height of 44 mm. The measurement setting can define either the full or half length—verify it matches your intent. A quick check with the ViewCube ensures the cylinder is correctly positioned.
Extruding the Pattern
Save your project regularly. Then, extrude the honeycomb pattern. Adjusting the rectangle’s size allows future scaling. In the timeline, this flexibility ensures seamless adjustments.
Extrude the pattern through the surface model, setting the operation to Intersect. This retains only the intersected areas, removing the rest and leaving an infinitely thin pattern.
Transforming the Design into a Solid Model
To convert this pattern into a solid, use the Thicken command. A 2 mm thickness provides structural definition while keeping the model lightweight.
A Circular Pattern replicates the design around an axis. Since the layout is centralized, the axis serves as a natural reference. Rather than complex calculations, we increase the count until pieces align—matching the blue original object with the grey patterned copies.
A quick ViewCube spin verifies alignment. A few tweaks may still be necessary.
Refining the Design with Additional Features
Sketching directly onto an existing body allows for the creation of top and bottom rings. If you have a better workflow suggestion, drop a comment below.
At this stage, the design remains flexible, though it lacks user parameters and constraints. While essential for controlled adjustments, these are outside the scope of this tutorial.
Using Fillets and the Mirror Command
Efficiency is key. Applying a full round fillet before mirroring the top saves time. A parametric fillet auto-adjusts if top dimensions change. This workflow highlights the importance of symmetry around the horizontal construction plane and the advantage of making the top a separate body.
Select the object, choose the Mirror plane, and set the operation to New Body. Mastering these tools makes achieving precision in Fusion second nature.
Applying Materials and Finalizing the Design
Now, we refine the appearance. Since we haven’t merged all bodies after the circular pattern, we can assign distinct colors to different parts.
If a single body is preferred, select all, activate Combine, and they merge instantly in the Browser.
Watch the Full Fusion Tutorial for Students
If you enjoy working with complex patterns, check out the full tutorial video below. You'll also find additional learning resources and exclusive deals in the video description. For more Fusion tutorials, subscribe to The Maker Letters!