In this comprehensive tutorial, we'll begin constructing our base component while mastering one of Fusion 360's most powerful features: user parameters. Navigate to your Fusion 102 Parametric Modeling folder and open Step 1: Base to follow along with this essential workflow.
While this file contains no components or geometry initially, it serves as our foundation for establishing critical project preferences, including material properties and unit systems. Once your file loads, hide the data panel to maximize your workspace. Now, let's explore how user parameters can transform your modeling efficiency and design flexibility in Fusion 360.
Access the parameter management system by navigating to Modify > Change Parameters. This opens the parameter dialog box, your command center for all user-defined variables. Initially, you'll see an empty parameter list—we'll populate this strategically to create a robust, updateable model structure.
User parameters represent one of parametric modeling's greatest advantages: they allow you to assign meaningful values to specific design elements that automatically propagate throughout your entire model. When you reference these parameters instead of hard-coded dimensions, any subsequent changes to the parameter values instantly update all associated features—whether that's part thickness, widths, hole diameters, or any other critical dimension. This approach dramatically reduces design iteration time and minimizes errors in complex assemblies.
Create your first parameter by clicking the plus icon in the dialog. The Add User Parameter window presents several fields requiring strategic consideration. Name this parameter "T" for thickness, then set the expression value to 15.
Notice how Fusion 360 automatically applies your default units (millimeters in this case). In the comment field, enter "Part Thickness" for future reference. This naming convention—keeping parameter names to one or two characters—proves crucial for efficient workflow, as you'll discover when we begin applying these parameters to actual geometry.
Continue building your parameter library by creating additional variables. Add "W" for width with an expression value of 30. Remember, these expression values serve as your baseline—they'll evolve as your design develops, but establishing logical starting points accelerates the modeling process.
Add a third parameter: "D" with a value of 5, commenting this as "Hole Diameter." To demonstrate a critical workflow principle, temporarily create one more parameter with a longer name.
Create a parameter named "Part Width" with an expression of 30—identical to our "W" parameter—then observe what happens during parameter selection. This exercise reveals why concise naming conventions matter significantly in professional parametric modeling workflows.
With our parameter foundation established, let's begin creating the actual model geometry. Right-click to create a New Component and rename it "Base." Activate this component, then create a new sketch hosted to the bottom plane.
Select Sketch > Rectangle > Center Rectangle to begin defining your base geometry. Place the center point and draw your rectangle, then press D to access the dimension tool. Set initial dimensions of 235 × 125 for the outer boundary.
Now create a second rectangle using the same Center Rectangle tool. This is where our user parameters demonstrate their power. When dimensioning this rectangle, instead of entering a static value of 30 for the width, type "W" instead. Notice how both "Part Width" and "W" appear in the suggestion dropdown—this illustrates why shorter parameter names create cleaner, more predictable workflows.
Select "W" and press Enter. Fusion 360 now displays "Function: 30," indicating that this dimension links directly to your user parameter. This parametric relationship means future changes to the W parameter will automatically update this dimension throughout your model.
Apply the thickness parameter by typing "T." Again, notice that "Part Width" appears in suggestions because it contains the letter T. In complex models with numerous parameters, this overlap can create confusion and slow down modeling. Stick with concise naming conventions to maintain efficiency.
Select "T" and press Enter to see the function display "fx: 15." Now add a Horizontal/Vertical constraint between the center points of both rectangles to maintain their alignment relationship.
For the final dimension between these elements, manually enter 30 rather than using a parameter. This represents a static value that should remain constant regardless of parameter changes—demonstrating that not every dimension requires parametric control. Strategic use of both parametric and static dimensions creates models that update predictably.
Click Stop Sketch and return to your Home view to observe the completed geometry. Before proceeding, clean up your parameter list by navigating to Modify > Change Parameters and deleting the "Part Width" parameter using the X button. This maintains a lean, organized parameter structure.
Now witness the true power of parametric modeling. Change the thickness parameter from 15 to 12.5 and watch the rectangle automatically adjust. Similarly, changing the width from 30 to 40 immediately updates all associated geometry. This real-time updating capability extends throughout your entire model—every feature, component, and assembly that references these parameters will automatically adjust when you modify the source values.
Reset the parameters to their original values of 30 and 15. As we continue building this model in subsequent videos, we'll regularly test and refine these parameters to ensure our design remains truly parametric and updates predictably across all scenarios.
Save your model to preserve this parametric foundation. In our next session, we'll complete the base component while exploring advanced parameter applications and modeling techniques. This systematic approach to parametric design will serve as the backbone for all your future Fusion 360 projects.