Use parameters to constrain sketch geometry

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In Fusion, you can use parameters to drive and edit multiple dimensions from a single named parameter.

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Once you create a predefined parameter with a specified value,

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you can assign that parameter to multiple dimensions, instead of setting values individually.

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Editing this parameter value will then propagate the changes across all dimensions with the same parameter reference.

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To access the Parameters dialog, on the Design workspace toolbar, click Solid > Create Sketch, if you are not already in Sketch mode.

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Then, click Sketch > Modify > Change Parameters.

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Favorites are commonly used parameters that you want to access quickly.

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For a more complex design, these can be particularly useful.

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User Parameters are created by you, and if you already have some known dimensions,

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you can start populating these even before creating a sketch.

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Model Parameters are automatically generated when you create any 2D or 3D geometry.

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If you expand this category, you see expression values that match the geometry created in your design.

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Press Esc or click OK to close the Parameters dialog.

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To edit a dimension placed on the sketch, double-click the dimension,

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type a new value, and press Enter.

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If you have dimensions that are specific to certain geometry, then simply entering values is a reasonable workflow.

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However, if you have multiple geometries that share a common value

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—even across multiple sketches—

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setting up named parameters may be more efficient.

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To open the Parameters dialog again, type “S” to open the Toolbox,

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type “Parameters”,

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and then select Change Parameters in the search results.

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In the Parameters dialog, click + User Parameter to open the Add User Parameter dialog.

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In the Name box, type “Radius”.

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Set the Unit to mm, and in the Expression box, enter a value of 20.

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You can also add a Comment to clarify the purpose of the parameter.

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Click OK to complete the setup.

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You can see the parameter now populated under User Parameters, and you can start using it in your design.

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You can also create a parameter while creating a sketch feature.

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Instead of entering a dimension, type a parameter name followed by the equals symbol and the value, and then press Enter.

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In this case, enter “L1=20”.

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Open the Parameters dialog, and you can see that this parameter is automatically added under Favorites.

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This is useful if you want to quickly set and name parameters while modeling.

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Close the Parameters dialog.

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To use the parameter that you set up earlier, double-click the radius value on the lower arc,

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and then start typing the parameter name—in this case, “Radius”.

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In the filtered list of suggestions, select the Radius parameter to reference it.

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The name appears in the box and turns black to indicate that it is a valid parameter.

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Press Enter to confirm.

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The dimension updates to match this parameter value.

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You can confirm that you are using a parameter if you see fx preceding the value,

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and if double-clicking the parameter shows the parameter name.

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To edit the parameter, open the Parameters dialog, double-click the Radius value, and enter a new value of 30.

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Click OK.

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The geometry updates without entering the dimensions on the canvas.

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To see how parameters can save you time, first delete a constraint on the canvas.

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The sketch turns blue, indicating that it is not fully constrained.

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On the toolbar, click the Dimension tool, then select the arc.

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Start typing “Radius”, select the Radius parameter, and press Enter.

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The Radius parameter is now referenced in two places in your sketch.

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Open the Parameters dialog and change the value to 25.

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Note that you only need to edit one value, and any dimensions with that parameter reference updates accordingly.

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Setting up and using named parameters is particularly useful with more complex assemblies,

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but it can save you time on nearly any design.