Parametric dimensions

On the ribbon, click Sketch tab Constrain panel Dimension to add dimensions to a 2D or 3D sketch. Dimensions control the size of a part and can be expressed as numeric constants, as variables in an equation, or in parameter files.

In 3D sketches, you can add only linear and angular dimensions. Radial dimensions are created only when you create bends.

1. On the ribbon, click Sketch tabConstrain panel Dimension.
2. In the graphics window, click the geometry and drag to display the dimension. To add:
   • A linear dimension for a curve, click to select the curve.
   • A linear dimension between two points, two curves, or a curve and a point, click to select each point or curve.

     In a 3D sketch, you can also constrain the distance between a point and plane or planar face.

   • A radial or diametric dimension, click to select the arc or circle. Right-click and select Dimension Type Radius for an arc or circle, or Linear for a centerline.
   • An arc length dimension, click to select the arc, right-click and select Dimension Type Arc Length.
   • An angular dimension:
     • In a 2D sketch, select two curves or three points.
     • In a 3D sketch, select two points, one of which can be a work axis.
3. Click to place the dimension. In a 3D sketch, the dimension text is parallel to a plane created by the two selections.

   Click the dimension text and drag to reposition if needed. In a 3D sketch, you can drag the dimension text on the placement plane only.

   If the dimension overconstrains the sketch, you can accept it or cancel the dimension. If you accept the dimension, it is saved as a reference parameter.

4. Double-click the dimension value to open the Edit Dimension box.
5. Specify a value, use an equation to calculate the value, or click the arrow to measure the value, show dimensions, or set a tolerance.
   TipYou can also enter or edit an expression that defines a parameter. For example, enter HGHT = 5mm. The expression is parsed to create the parameter HGHT and assign it a value of 5 mm.

You can edit sketch dimensions before or after a sketch becomes part of a feature. If a sketch has not been consumed by a feature, its dimensions are visible and can be edited. After a sketch is consumed by a feature, select the feature in the browser and activate the sketch for editing.

To change the dimension display style, right-click in the graphics window and select Dimension Display. Choose Value, Name, Expression, Tolerance, or Precise Value.

1. On the Quick Access toolbar, click Select Sketch Features.
2. Right-click the dimension in the graphics window.
3. Select Delete from the menu.

1. On the ribbon, click Sketch tabConstrain panel Automatic Dimensions and Constraints.

   The Auto Dimension dialog box shows the number of dimensions and constraints required to fully constrain the sketch.

2. Accept the default settings to add both Dimensions and Constraints or clear a check mark to prevent application of the associated items.
3. Click Curves, then individually or multi-select geometry.

   If you prefer, click and hold the left mouse button, then drag to enclose desired geometry in a selection window, then click to select.

4. Click Apply to add dimensions and constraints to selected geometry.

   To automatically dimension and constrain the entire sketch, click Apply with no geometry selected.

5. If desired, click Remove to delete the automatically added dimensions and constraints from the sketch geometry. The Dimensions and Constraints check boxes must be selected for the Remove command to delete the dimensions and constraints, respectively.
6. When finished, click Done.