The Change Parameters Dialog#

Overview#

Every driving number in a Fusion design is a parameter: a sketch dimension, an extrude distance, a pattern count, a fillet radius. The Change Parameters dialog lists them all in one table so you can read, rename and edit them in one place, instead of hunting through the timeline.

There are two kinds, and the dialog separates them:

• Model parameters: created automatically by features and dimensions (named d1, d2, d3 ... by default). They belong to a specific sketch or feature.
• User parameters: ones you create and name, such as wall, hole_dia, length. They hold values or expressions, and other parameters or dimensions can reference them.

A parameter has a name, an expression (what you type), a value (the evaluated result with units), and an optional comment.

Where to find it#

• Solid tab > Modify > Change Parameters in the Design workspace.
• The tool-search shortcut: press S and type "Change Parameters".
• Any dimension or feature field that accepts expressions also lets you pick parameters from a list while editing, and typing a new name there can create parameters on the fly (these are added to Favorites automatically per Autodesk's help).
• Help topics: Autodesk's help has "Parameters in Fusion", "Create or edit parameters" and "Parameters reference" pages. The menu path in the help is Design > Solid > Modify > Change Parameters.

Step by step#

Open and read#

1. Open a design with a few features.
2. Choose Modify > Change Parameters.
3. The dialog shows Favorites at the top, then User Parameters, then Model Parameters, grouped by component and feature. Expand arrows reveal each group.
4. Columns per Autodesk's reference: Parameter (identifies the parameter and the operation it belongs to), Name, Unit, Expression, Value, Comments.

Edit a model parameter#

1. Find d3 (a sketch dimension). Click the Expression cell.
2. Type a new value, for example 45 mm, or an expression referencing another parameter.
3. Press Enter. The model updates behind the dialog.
4. Click OK to close. If Automatic Compute is checked, the design updates in the background as you edit and you can use Apply to push changes; unchecking it pauses updates while you make several edits, which saves compute time on heavy models.

Rename a model parameter#

1. Click the Name cell of d3.
2. Type a meaningful name such as flange_width. Names must be unique. Autodesk's reference lists the allowed symbols as underscore, double quote, dollar sign, degree sign and micro sign. Avoid names that match unit symbols (like m, in, s) or function names.
3. All expressions using the old name update automatically.

Create a user parameter#

1. Click + User Parameter (the Autodesk help calls it Add User Parameter).
2. Fill in a unique Name, an Expression (the value is calculated automatically) and an optional Comments note, then expand the unit list and choose a Unit (mm, in, deg, No Unit, Text and so on).
3. Click OK. The parameter now appears in the list and in field dropdowns when you edit dimensions.

Use it:

1. Edit a sketch dimension and type wall in the field instead of a number.
2. The dimension is now driven by the user parameter. Changing wall changes the dimension.

Favorites#

1. Mark a parameter as a favorite (the table has a Favorite column).
2. Favorites display in a list at the top of the parameters table, for both user and model parameters.

Filter and sort#

1. Use the Search field to type part of a name. Filter User Parameters shows only user parameters, and Filter Favorite Parameters shows only favorites.
2. Sort In Timeline Order restores the list to the order features were created.

CSV export and import#

Autodesk's help documents Export Parameters and Import Parameters buttons in the dialog. They work on user parameters only.

1. Click Export Parameters, enter a Name and Location, and click Save. The user parameters are written to a CSV file (optionally check Save to a project in the cloud to save it to a Fusion project).
2. Edit the CSV in an external table editor. Export a set first and use it as a template so the header format is correct (columns: Name, Unit, Expression, Value, Comments, Favorite). Keep each name unique, make sure the expression's resulting unit matches the unit column, and enter unit syntax correctly.
3. Click Import Parameters, select the CSV and click Open. In the Selected Parameters dialog, uncheck any you do not want, then click Import. For a family of variants, Configurations is usually the better route.

Options reference#

Tips and pitfalls#

Tip: Rename model parameters you care about. flange_thk tells you what you are changing; d27 does not.

Tip: Short names speed typing and autocomplete (e.g., t for thickness), but do not use names so short they collide with units or become ambiguous. A middle ground such as wall or hole_d is safer.

Tip: Put a comment on every user parameter: units, source, and reason. Future you will be grateful.

Note: Renaming a parameter updates every expression that references it in this design (per Autodesk's help). Behaviour in derived designs or external references is not described there, so check those designs after a rename.

Warning: Typing a value with the wrong unit (for example 25 deg into a length) is an error. Break the expression up and inspect each Value to find the culprit.

Other behaviours:

• Parameters are per design; to reuse them elsewhere, export them to CSV or see Derive.
• Equation chains are allowed (b = a * 2, c = b + 1). Circular references cannot be evaluated, so avoid them (general guidance; not spelled out in the parameters help).
• The parameter's Unit column controls how its Value is displayed.

Creating parameters without opening the dialog#

When a tool is active (Extrude, a sketch dimension, Fillet), click any parametric text field and type Name=value or Name=expression, for example Width=50 or Length=Width*2. Fusion creates the parameter and adds it to Favorites automatically. This is the fastest way to build a parameter set while you model: you dimension the first sketch with box_l=80, then reuse box_l everywhere else. The parameter's unit is taken from the field, so a length field yields a length parameter.

In a parametric text field you can click the parameter icon to switch between the expression and its evaluated value, and any favorite can be reused by typing its name and picking it from the suggestion list.

Text parameters#

Setting the Unit to Text lets a parameter hold text instead of a number, for example part_label = "REV A". Inside the Expression box wrap other parameters in curly braces: "Bracket {box_l} x {box_w}". Text parameters are used where a field accepts text (sketch text, for instance), so you can drive a label from the dimensions it describes.

Reading the table efficiently#

Model parameters are named d1, d2 and so on in creation order, grouped under the feature or sketch that owns them. If a sketch has 14 dimensions, only rename the five that carry intent; the rest can stay as they are.

Worked example: converting a bracket to a parametric table#

You have a 50 x 30 x 10 mm plate with a 6 mm hole 8 mm from each edge.

1. Open Change Parameters and rename the sketch dimensions: d1 to length (50), d2 to width (30), d3 to hole_d (6), d4 to hole_edge (8). Rename the extrude distance d5 to height (10).
2. Add user parameters tol = 0.2 mm and hole_clear = hole_d + tol. Edit the hole sketch dimension to use hole_clear (6.2 mm).
3. Star length, width, height, hole_d, tol. Filter Favorites and you see five lines that control the part.
4. Uncheck Automatic Compute. Change length to 80 and width to 40, then check it and click Apply; the model rebuilds once, not twice.
5. Check the Value column: the hole center should now be at hole_edge = 8 mm from each edge, which is 80 - 16 = 64 mm apart in X.

Common errors in the dialog#

Practice exercise#

Convert a plain design to a parameter-driven one and test the dialog features.

1. Draw a 50 x 30 mm rectangle and extrude it 10 mm. Draw a 6 mm hole 8 mm from two edges and cut it through.
2. Open Change Parameters. Rename the five dimensions to length, width, height, hole_d and hole_edge. Confirm that each is listed under its sketch or feature.
3. Add user parameters: margin = 5 mm, tol = 0.2 mm, hole_clear = hole_d + tol, and plate_label as a Text parameter whose expression is "{length} x {width} x {height}".
4. Edit the hole dimension to hole_clear. Draw a second rectangle inside the plate offset by margin and check the dimension.
5. Create a parameter on the fly: start a new extrude and type boss_h=4 mm in the distance field. Confirm it appears in Favorites.
6. Star length, width, height, margin, tol. Use Filter Favorite Parameters and Search to find them.
7. Uncheck Automatic Compute, change length to 90 and margin to 8, then check Automatic Compute and click Apply.
8. Break something: type 25 deg into width, note the error, and fix it.
9. Click Export Parameters, save the user parameters as CSV, edit margin in a table editor, and bring it back with Import Parameters.

Expected result: a design whose sizes are edited from one table, with parameters created on the fly, text parameters and an understanding of Apply behavior.

Related#

• User parameters and equations
• Units and expressions
• Configurations