Sketch Dimensions

Overview#

A sketch dimension is a numeric constraint. It tells the solver the exact length, diameter, radius, distance, or angle of a piece of geometry. Together with geometric constraints, dimensions make a sketch fully defined and give the design its parameters: change a number, and the geometry (and everything built on it) updates.

Fusion has a single smart tool, Sketch Dimension, that picks the right kind of dimension from what you select. This page covers how it behaves, how to enter and edit values, how to use expressions and named parameters, and the difference between driving and driven (reference) dimensions.

Where to find it#

• Panel: Sketch tab > Create panel > Sketch Dimension.
• Shortcut: D.
• Edit a dimension: Double-click the dimension in the canvas, then enter a new value or expression.
• Right-click options: Before you place a dimension, right-click for contextual options such as Radius or Diameter, Driven or Driving, and Pick Circle/Arc Center or Pick Circle/Arc Tangent.
• Parameters: Design > Modify > Change Parameters (opens the Parameters dialog with User Parameters and Model Parameters).

Step by step#

1. Press D to start Sketch Dimension.
2. Select the sketch geometry. What you select determines the dimension type (see the table below).
3. Define the value: enter a specific value, click an existing dimension to reference it as a parameter, or enter an expression made of values, parameters or both. Press Enter to accept.
4. Move the pointer away from the geometry, then click to place the dimension.
5. Repeat for more dimensions. Press Esc or start another tool to end.
6. To change a value later, double-click the dimension and enter a new value or expression.

Geometry constrained by a dimension turns black.

What each selection gives you#

These are the selections listed in Autodesk's help. Before placing a dimension you can right-click to switch between Radius and Diameter, Driven and Driving, or to pick a circle/arc center or tangent.

Note: not confirmed in Autodesk's documentation: dimension types for a point and a line, two circles or arcs, ellipse axes, spline points, and arc length or sweep angle. Try them in your build and check the result.

Entering values#

The input box accepts:

• Specific values, with or without units (the Parameters unit types list abbreviations such as deg and rad for angles).
• Expressions containing values, parameters, or a mix, such as 20 + 5 or Width / 2.
• References: click an existing dimension to reference it as a parameter, or type a parameter name.

Pressing Enter accepts the value or expression.

Note: not confirmed in Autodesk's documentation: how plain numbers without units are interpreted (they follow the document units in practice), the available math functions, and the use of Tab between dimension fields.

Naming dimensions#

Dimensions create Model Parameters automatically, and you can create and name parameters in context as you add dimensions. You can also edit a parameter's name in the Parameters dialog; renaming updates every expression that references it. Meaningful names such as Width or HoleDia make expressions readable, and an expression can reference another parameter (for example Width / 4).

Note: not confirmed in Autodesk's documentation: default names such as d1, d2 and typing name = value into the dimension box.

User parameters#

User Parameters are created in the Parameters dialog and referenced in features and other parameter expressions. You can favorite parameters and filter the list by Favorites or User Parameters. A classic use is one Thickness parameter used by an extrude distance, a hole depth, and a sketch dimension.

Managing parameters in the Parameters dialog#

The Change Parameters tool (Design > Modify > Change Parameters) manages every parameter in one place. There are two types: User Parameters, which you create and then reference in features and other expressions, and Model Parameters, which drive the dimensions and values of timeline features. A model parameter is created automatically when you create a feature or define a dimension (an Extrude, for example, generates one for its distance). When you create and name a model parameter in context, Fusion adds it to your Favorites list at the top of the table.

You can filter the table by Favorites or User Parameters, sort by Name, Unit, Expression, Value or Comment, and use Sort in Timeline Order to list parameters in the order they were created. Editing a parameter updates every place it is referenced, and renaming one updates the expressions that use it. Export Parameters saves User Parameters as a CSV file you can edit and bring back with Import Parameters; each parameter needs a unique name, and the unit type produced by its expression must match its assigned unit type.

From the Parameters dialog you can also reference the parameter name of driven or driving dimensions in other sketches, modeling features and parameter expressions. To reference a sketch's dimensions while working in another sketch, right-click the sketch in the Browser and choose Show Dimensions.

Driving versus driven dimensions#

A driving dimension controls geometry; changing it moves things. A driven dimension only measures and never constrains.

• Driving to driven: right-click the dimension and choose Toggle Driven. If its expression references only driving dimensions, it becomes a static value that cannot be recovered by toggling back.
• Driven to driving: right-click and choose Toggle Driving.
• Referencing a driven dimension: click it while defining another dimension, or use its parameter name in an expression. You cannot reference driven Tangent or Offset dimensions.

Driven dimensions are ideal for reading values you want to check without influencing the sketch.

Note: not confirmed in Autodesk's documentation: an automatic prompt to make an over-constraining dimension a driven one.

Dimension placement and tidy sketches#

The location of the dimension text has no effect on geometry, but it affects readability, so keep it clear of the shape when you place it. If you do not want to see dimensions while working, turn off Show Dimensions in the Sketch Palette; they still constrain the sketch. To reference a sketch's dimensions from another sketch, right-click the sketch in the Browser and choose Show Dimensions.

Options reference#

Tips and pitfalls#

Tip: Dimension from fixed references (the origin, projected edges, or construction lines) rather than from a chain of neighboring features. A chain makes your sketch fragile: change one link and the rest slide.

Tip: Put design intent in the numbers. If a hole should always be a quarter of the width from the edge, use an expression with a named parameter rather than a constant.

Tip: If you want to know a value without constraining it, create a driven dimension.

Warning: General guidance: dimensioning a small sketch to a very large value in one step can flip geometry. Make large changes in steps and check arcs and fillets.

Warning: Dimensions over-constrain quickly on symmetric or tangent geometry. If a new dimension conflicts, make it a driven dimension or delete the conflicting constraint.

Warning: If a dimension jumps by a factor of 25.4, the value was interpreted in the wrong unit (mm versus in). Check the document units.

Practice exercise#

1. Open the Parameters dialog and create a user parameter named Width with the value 60 mm and another named Height with 40 mm.
2. Draw a 2-Point Rectangle from the origin. Dimension its width with the expression Width and its height with Height.
3. Draw a circle. Dimension its diameter as Height / 4, and position its center from the left edge as Width / 2 and from the bottom edge as Height / 2.
4. Create a dimension on the rectangle's diagonal and right-click > Toggle Driven to read its length.
5. Change Width to 100 mm in the Parameters dialog and watch everything update.

Expected result: a fully dimensioned rectangle with a centered circle whose size and position are driven by two parameters, and a diagonal measurement that updates automatically.

Related#

• Constraints (02-sketching/constraints)
• Fully constrained sketches (02-sketching/fully-constrained-sketches)
• Sketch palette (02-sketching/sketch-palette)
• Troubleshooting sketches (02-sketching/troubleshooting)