Configurations#

Overview#

A configuration is a named variant of a design. Instead of saving five copies of a bracket (short, medium, long, with and without holes), you keep one parametric model and a configuration table. Each row of the table is a variant; each column is something that varies.

Per Autodesk's documentation, configurable aspects include:

• User parameters (from the Parameters dialog).
• Feature parameters: sketch dimensions, extrude distances, hole diameters, pattern quantity, fillet radii and so on.
• Suppression of timeline features or components.
• Visibility.
• Physical material and appearance, handled through theme tables.
• Sheet metal rules and plastic rules, also through theme tables (a Custom theme table type exists too).
• Properties (for example part number or description), on a Properties tab of the table.

Theme tables combine several aspects into one choice. Autodesk's example is a cabinet with or without a door; one "door" column suppresses the door, hinges and handles together.

A design with two or more configurations defined in a Configuration Table is a configured design. When you convert a Standard Design, its latest version becomes the first configuration; the configured design's history starts over, and the Standard Design's earlier history stays reachable through the Data Panel.

Note: Autodesk's Configurations pages mark Configuration Rules as part of the Fusion Design Extension. The core Configuration Table pages do not state any license requirement, and Personal-use entitlement is not confirmed in Autodesk's documentation; check Autodesk's current feature comparison.

Where to find it#

• Design workspace toolbar: Configure enters Configuration Mode and displays the Configuration Table. Display Configuration Table shows the table without entering Configuration Mode, and Create Configuration Rules opens the Configuration Rules dialog.
• Rows are configurations, columns are aspects. A Configured Design icon appears on the document tab and in the Data Panel, and the Browser lists the Configurations.
• In Configuration Mode, features in the Timeline and objects in the Browser are highlighted; click one to open its Configure dialog and check the aspects to add as columns. Outside Configuration Mode, right-click a feature or object and choose Configure. While creating a feature you can also use the contextual Configure tab.
• The table's Parameters tab holds the top table and the theme tables; the Properties tab holds Part Number and Description. The first row is the Default Configuration; it cannot be deleted or moved from the top row.
• To activate a configuration, double-click its name in the table (or right-click > Activate), or select it in the Browser's Configurations list.

Step by step#

Create the table#

1. Open a parametric design with user parameters (for example length, hole_count).
2. Click Configure on the toolbar to open the table in Configuration Mode.
3. Use Add Configurations to add the rows you need. Each row is one configuration; you can add a specific number at once.
4. Name each row clearly, such as Short, Medium, Long.

Add parameter columns#

1. Click Add Parameters (opens the Parameters dialog in Configuration Mode) and pick length, or configure a feature parameter from the feature's Configure dialog.
2. For each row, click the cell and type a value, a parameter name, or an expression.
3. Activate each row (double-click its name) and check that the model matches.

Feature parameter columns can reach into the timeline: for a hole, fillet, extrude or pattern, add the specific feature's parameter (for example, extrude distance). This works without making user parameters for everything.

Add suppression columns#

1. Select a feature in the Timeline (in Configuration Mode click a highlighted feature; otherwise right-click > Configure), check Suppression and click OK. A Suppression column is added; groups can be configured the same way.
2. For each row, click the Suppression button to set the state (suppressed or unsuppressed).
3. Choose features at the right level: suppress the cut that makes the hole, not the later fillet that depends on it.

Add material, appearance, properties#

1. Select the component or body in Configuration Mode (or right-click > Configure) and check Physical Material or Appearance. The aspect is managed in a theme table, and you pick a value per row from a list.
2. Use the Properties tab of the table to set part number and description per configuration when you want BOM-friendly data.

Use a theme table#

1. Create a theme that groups several columns (door suppress, hinge suppress, handle suppress).
2. Give the theme options such as With door and No door.
3. Reference the theme in the main table. One choice now flips several aspects.

Convert and save#

1. To convert a Standard Design, open it, click Configure, add two or more configurations, configure at least one aspect and click Save.
2. The latest Standard Design version becomes the first configuration and the design history starts over. The Standard Design history stays available through the Data Panel. To keep a pristine copy, copy the Standard Design first and convert the copy.

Use configurations in assemblies and drawings#

1. Insert a configured design into another design as an external component and choose a configuration; this is a Configured Component.
2. To switch the inserted configuration per row of a destination table, configure the component's Insert aspect; the result is a configurable assembly.
3. A drawing can document one or more configurations of the same configured design. Use Table > Configuration Table on the Drawing toolbar to place a table of configurations, and Switch Configuration to change the configuration of a view set.
4. To derive from a configuration, open the configured design and use Create > Derive, choosing the configuration to derive (see Derive).

Options reference#

Tips and pitfalls#

Tip: Make a sound parameter strategy first. Configurations are far easier on a model with clean user parameters.

Tip: Test every row. A variant can break the geometry even though the base row works.

Tip: Use expressions in cells (for example base_length * 2) so variants relate to each other.

Warning: Do not mix manual timeline edits and heavy suppression carelessly; a suppressed feature that others depend on leads to errors in only some rows.

Warning: Large tables on large assemblies can slow switching. Keep variants per part, and assemble.

Warning: Converting starts a new design history for the configured design. Copy the Standard Design first if you want an untouched original.

When to use what:

Worked example: a spacer family with numbers#

A spacer is a hollow cylinder with an optional chamfer. User parameters: od, id, h, plus a feature for the chamfer.

Check each row mentally before you enter it: wall = (od - id) / 2 = 2.4, 2.9 and 3.4 mm. The ID values follow the clearance holes for M3, M4 and M5 screws (3.2, 4.2 and 5.2 mm are close fits). A chamfer of 0.5 mm on a 2.4 mm wall removes 21 percent of the face width; fine. Make id an expression of an m_size column (id = m_size + 0.2 mm) so one input controls both.

Mass changes with Physical Material. For the L row, a steel spacer has volume pi x (6^2 - 2.6^2) x 20 = 1,837 mm3 and mass about 14.4 g at a typical 7.85 g/cm3 for steel, compared with about 5.0 g at 2.70 g/cm3 for aluminum (general material densities, not Autodesk data); verify with Properties on each row.

Expressions in cells#

A cell can hold a number, a parameter name or an expression, and expressions can reference other parameters. So od in row M can be id + 2 * wall_min where wall_min is a user parameter, making variants relate to each other. Use if(cond; a; b) expressions in cells only when a single column must switch behavior; otherwise use a suppression column, which reads more clearly.

Suppression strategy#

• Suppress at the feature that creates the geometry (the hole cut), not at a dependent feature (the fillet on the hole's edge). If you suppress the cut but leave the fillet, the fillet will fail in that row.
• Components can be suppressed too. Use a theme with options such as Fasteners: Included/Excluded to toggle screws, washers and nuts in one step.
• When rows disagree about which features exist, test every row after every timeline change. A newly added feature that depends on a suppressed feature breaks only some rows, which is hard to notice.

Using configured designs downstream#

• In an assembly, insert the configured design and choose a configuration for each instance, so one file can supply S, M and L spacers.
• To derive a configuration, choose it in the Derive dialog (see Derive).
• The Standard Design's history stays available in the Data Panel after conversion, so you can recover if the table becomes unmanageable.

Failure modes and fixes#

Choosing between configurations, parameters and separate files#

Use configurations when you need several named, saved variants that you will hand to other people (BOM entries, assemblies, drawings). Use Change Parameters when you only need one live design that you tweak. Use derive when the second design has genuinely different geometry built around the first. If two variants differ by more than half their features, separate designs are easier to maintain than a 30-column table.

Practice exercise#

Build a configured spacer family and prove all rows work.

1. Build a spacer with user parameters od, id, h, an m_size parameter, and a 0.5 mm chamfer feature on both ends. Set id = m_size + 0.2 mm.
2. Click Configure. The first row is the Default Configuration; add configurations so you have rows S, M, L (the default row can serve as one).
3. Add parameter columns for m_size (3 mm, 4 mm, 5 mm), od (8, 10, 12 mm) and h (5, 10, 20 mm), and a suppress column for the chamfer feature (suppressed in S only).
4. Use Configure on the body to add Physical Material, then set it per row (Aluminum, Aluminum, Steel). Fill in part numbers on the Properties tab.
5. Switch rows and measure wall thickness for each: expect 2.4, 2.9 and 3.4 mm. Read the mass from Properties for each row and compare with a hand calculation.
6. Add an appearance configuration so each row has a different color.
7. Create a new design, insert the configured spacer three times, and assign S, M and L to the instances. Check the Bill of Materials (see Autodesk's Use the Bill of Materials in a Configured Design).
8. Break it: add a fillet on the chamfer edge and see which row fails; fix it by suppressing the fillet where the chamfer is suppressed.

Expected result: one file generating three distinct parts with different masses, colors and part numbers, plus a documented dependency fix.

Related#

• Derive
• User parameters and equations
• Design-for-change patterns