What's the right way to design in Fusion?

Do you often wonder about the "best" way to design in Fusion? Should you use the Hole command or use a sketch with a circle? The truth is, there isn't a single right way; many methods work effectively. This guide shares practical tips and thought processes to help you model more efficiently with Fusion. We’ll explore how breaking down complex shapes, choosing the right features, and using constraints can significantly improve your design workflow.

Designing with Intent: The Foundation of Efficient Fusion Modeling

Breaking Down Complex Shapes into Simpler Forms

When approaching a new design, it's helpful to break it down into its most basic geometric forms. This simplifies the initial modeling process. Think about the core profiles that define the overall shape. For example, when designing the "rod guide" model as shown in the video, we can see three distinct rectangles: an 80x15, an 80x20, and a 30x16. Starting with these foundational shapes allows you to build the model’s structure before adding finer details.

Understanding Design Changes and Feature Selection

Consider what happens if you change the width of the model from 60mm to 80mm. If you used a standard fillet with a 30mm radius, Fusion will try to maintain that radius. This can result in an unwanted flat segment appearing where you expected a smooth curve. It’s crucial to select features that inherently adapt to future design modifications.

Implementing Full Round Fillets for True Roundness

The "Full Round Fillet" command offers a better solution. When applying it, you select the faces that should be tangent to the rounded edge. This ensures the fillet remains perfectly rounded, regardless of changes to the model's dimensions. You don't even need to input a specific radius value. This method maintains true roundness, preventing those awkward flat sections and keeping your design looking clean and intentional.

The Hole Command: Speed and Precision for Standard Holes

Choosing between the Hole command and creating a hole via a sketch can significantly impact your workflow speed.

Leveraging the Hole Command's Snapping and Positioning

The Hole command offers intelligent placement features. You can click near your desired location and then use manipulator arrows to precisely position the hole’s center. Snapping to reference geometry, like the center of a fillet, makes alignment effortless. This avoids the need for extra sketch lines and constraints to locate the hole accurately.

The "To" Object Option for Intelligent Extents

A common mistake is using the "Through All" option for hole extents. If your part's geometry changes later, a hole set to "Through All" might cut through unintended areas. Instead, using the "To" object option and selecting a target face ensures the hole respects the part's boundaries. This makes your design more robust against future modifications.

When to Use a Sketch for Holes (and Why the Hole Command is Often Better)

Creating holes with sketches involves more steps and can be less efficient than using the dedicated Hole command.

The Manual Process: Sketching, Dimensioning, and Extruding

To create a hole with a sketch, you first create a sketch on the desired face. Then, you draw a circle, add dimensions and constraints to position it correctly, and finally use an extrude cut. This process involves more mouse clicks and a higher chance of introducing errors compared to the streamlined Hole command.

Understanding Constraints vs. Fixed Dimensions for Adaptability

If you use a fixed dimension, like setting a hole 30mm from an edge in a sketch, it can cause problems if that edge’s position changes. You would then need to manually update the dimension or use constraints. The Hole command automatically handles these positional relationships, keeping your holes centered and correctly placed without extra effort.

Advanced Sketching Techniques: Constraints and Equal Relationships

The Power of Constraints Over Redundant Dimensions

Using constraints is a powerful way to link geometric elements and reduce the need for repeating dimensions.

Employing the "Equal" Constraint for Simplicity

Instead of duplicating dimensions for similar features, use the "Equal" constraint. For instance, when creating notches, apply the "Equal" constraint to link their dimensions. This way, you only need to edit two dimensions, and both notches will update simultaneously. It makes your sketches cleaner and editing much simpler.

Avoiding the Mirror Command for Cleaner Sketches

While the Mirror command can be useful, it often adds extra construction lines and symmetry constraints to your sketch. This can make the sketch look cluttered and harder to manage. Using the "Equal" constraint is often a cleaner and more efficient method for creating symmetrical features, requiring fewer clicks and resulting in a simpler sketch.

Streamlining Your Workflow: Workflow Tips for Fusion Users

Prioritizing Features from Largest to Smallest

A good modeling strategy involves tackling the most significant features first. Build the overall form of your model, then progressively add smaller details like holes or chamfers. This top-down approach ensures the foundational structure is solid before you get into the fine details.

Using Right-Click Context Menus for Faster Access

Get into the habit of pre-selecting geometry and then right-clicking. This brings up a context-sensitive menu with relevant commands, like "Extrude" or "Hole." It’s often quicker than searching through the command ribbon, allowing you to access the tools you need more directly.

Extrude Cuts: "Through All" for Open-Ended Features

When creating cut features with the Extrude command, consider the "Through All" option. This is particularly useful for slots or holes that should pass completely through a part. It’s a safe choice for cuts as long as there’s no other geometry that could be unintentionally affected. For example, applying a "Cut" with "Through All" to the notches ensures they remain open, even if the part’s overall length is later modified.