Available in: Sketch

Shortcut: d

Add horizontal, vertical, shortest distance, angular, diametrical, arc length, or radial dimensions to sketch geometry, as well as between sketch geometry and planes. You are able to specify dimensions as driven (reference) or driving.

You have the ability to use the Measure tool to measure anything in the graphics area.

Some tools allow you to dimension as you sketch.

You can also use the Show dimensions command in the context menu (RMB) of a sketch to view existing dimensions.

Dimensions are a robust way to define sketch entities. Two methods are available for adding dimensions to a sketch. The first method involves adding dimensions while creating the sketch, while the second method involves creating sketch geometry first and then adding dimensions.

To add dimensions while sketching, type in a number and hit enter after sketching the geometry. For example, place a line. After selecting the second endpoint, a white box appears with the length of the line. Enter a value and press Enter to assign a dimension. This method applies to nearly all sketch tools.

When defining geometry that involves two dimensions, like a rectangle, start by entering the horizontal dimension and then press Enter. The input will automatically switch to the vertical dimension.

The second method for adding dimensions is to add them after the sketch geometry is finished. Select the dimension tool or use the shortcut D. Left-click on the entity or entities to apply the dimension. Move the cursor and left-click to place the dimension. Enter the value for the dimension and press enter. The sketch automatically scales to match the first dimension placed.

Onshape’s sketch dimension intuitively responds to the type of entity selected. This makes dimensioning to the outside or inside of an arc or circle seamless. Left-click close to the outside of the arc or circle to dimension to the outside. Left-click close to the inside of the arc or circle to dimension to the inside.Following the same intuitive theme, the dimension tool automatically places an angle dimension when dimensioning two non-parallel lines.

To edit a dimension, double-click the dimension in the graphics. Type a new value and press Enter to accept. Select the dimension from the graphics area to delete a dimension and press Delete on the keyboard. You can also use Dimension to display a value driven by other dimensions and relationships. Driven dimensions appear as gray in the sketch, whereas driving dimensions are black. Onshape automatically toggles new dimensions to driven if their placement will over-define a sketch. Manually toggle a dimension’s driving status in the right-click menu.

  1. Click Dimension tool icon or press the d key.
  2. Select the entity (or entities between which) to dimension and the location of the dimension.

    The selected entity or entities are highlighted (browser only), and the Dimension context dialog opens on the placement of the dimension. See Dimension context dialog for more information.

    A rectangle has been sketched in the Part Studio. Two corners are highlighted yellow and are connected with an arrow and dimension value.The value field in the dimension is active and ready for input

  3. Enter a value and press Enter to accept the value. You can also use a variable for a dimension, simply enter "=#" and the variable name, as in: =#d.

    A rectangle has been sketched in the Part Studio. Two corners are highlighted yellow and are connected with an arrow and dimension value.

You can enter negative values for dimensions (length, linear distance, and angles) to flip the direction of the entity.

The image below shows a positive dimension; notice the position of the rectangle relative to the bottom horizontal line:

Example of dimension with positive value

The following image shows a negative dimension value being typed into the active field:

Dimension with negative value in dialog

When the value is accepted, the rectangle flips direction:

Negative dimension flips the direction of the sketch

  • You can use expressions and trigonometric functions in numeric fields in Part Studios.

  • Delete a dimension by selecting it and pressing the Delete key, or select it and select Delete from the context menu.

  • To edit a placed dimension, double-click the value to activate the field, then enter the new value. Press Enter to accept the change.

  • Except for Diameter and radius dimensions, when a new dimension value is entered, both geometric selections being dimensioned are translated by half the new input value, so that both geometric selections are translated equally. For example, when dimensioning a single line, each endpoint is translated by half the dimension value, so that both endpoints are translated equally.

  • Constrained geometry may not translate. See Working with constraints.

Single line distance

  1. Click the Dimension tool (Dimension tool icon).
  2. Click the line.
  3. Drag to position the linear distance dimension.
  4. Click to simultaneously place the dimension and open its numeric value field.

  5. Optionally, enter a new dimension value.

  6. Press Enter to accept the dimension value.

Single line distance dimension

This is the method used to dimension length or height:

Example of length or height distance

Distance between 2 lines

  1. Click the Dimension tool (Dimension tool icon).
  2. Click the first line
  3. Click the second line
  4. Drag to position the linear distance dimension
  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press Enter to accept the dimension value.

Example of the linear dimension used to dimension between two parallel lines

When dimensioning between two lines, this implies parallelism without a visual parallel constraint.

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the first corner point
  3. Click the second corner point, diagonal to the first.
  4. Drag at an angle to position the diagonal distance dimension
  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press Enter to accept the dimension value.

Example of how to find Diagonal distance

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the edge of the circle.
  3. Drag into or away from the circle to position the diameter dimension.
  4. Click to simultaneously place the dimension and open its numeric value field.

  5. Optionally, enter a new dimension value.

  6. Press Enter to accept the dimension value.

Example of how to find the Diameter

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the first line.
  3. Click the second line, at an angle to the first.
  4. Drag into or out of the angle to position the angle dimension.

    1. You can also drag the dimension to the quadrant for which you want to define the angle:

      Example of dragging the label to the quadrant for which you want to define the angle

  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press Enter to accept the dimension value.

Example of clicking each line to find the angle

Direct distance

This dimensions the shortest distance between 2 points.

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the endpoint of the first line
  3. Click the endpoint of the second line.
  4. Drag at an angle to position the direct distance dimension.
  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press Enter to accept the dimension value.

Direct distance example

Linear distance

This dimensions the linear distance between 2 points.

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the endpoint of the first line
  3. Click the endpoint of the second line.
  4. Drag straight up/down or left/right to position the linear distance dimension.
  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press Enter to accept the dimension value.

Linear distance between two points

  1. Click the Dimension tool ( Dimension tool icon).
  2. Click the arc.
  3. Drag into or away from the arc to position the radius dimension.
  4. Click to simultaneously place the dimension and open its numeric value field.

  5. Optionally, enter a new dimension value.

  6. Press Enter to accept the dimension value.

Example of how to find the radius of an arc

  1. Click the Dimension tool ( Dimension tool icon).

  2. Click the arc’s first endpoint.

  3. Click the arc’s second endpoint.

  4. Click the arc.

  5. Drag to position the arc length dimension.

  6. Click to simultaneously place the dimension and open its numeric value field.

  7. Optionally, enter a new dimension value.

  8. Press enter to accept the dimension value.

Example of how to find the length of an arc

This dimensions the distance between 2 points on a spline or a spline point and any other sketch point.

  1. Click the Dimension tool ( Dimension tool icon).

  2. Click the first spline point.

  3. Click the second spline point (or any other sketch point).

  4. Drag to position the distance dimension.

  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

  7. Press enter to accept the dimension value.

Example of spline dimensions

You can also get the direct distance between two points on a spline or a spline point and any other sketch point if you drag the cursor away at an angle to position the direct distance dimension. See Direct distance.

This dimensions the distance between a plane and any other sketch point.

  1. Click the Dimension tool ( Dimension tool icon).

  2. Click the sketch point.

  3. Click the plane.

  4. Drag to position the distance dimension.

  5. Click to simultaneously place the dimension and open its numeric value field.

  6. Optionally, enter a new dimension value.

    If a new dimension value is entered, the sketch geometry moves while the plane remains in place.

  7. Press enter to accept the dimension value.

Example of how to find the distance between a sketch geometry and a plane

Create a centerline dimension between a circle, point, or non-construction line to a construction line; for instance, to dimension a part for a revolve operation. Start a distance dimension between one of these sketch entities and then move the mouse to the opposite side of the construction line. Moving the mouse across the construction line toggles the state between distance and centerline dimensions:

  1. Click the Dimension tool ( Dimension tool icon).

  2. Click the circle or sketch point.

  3. Click the Construction line. This results in a distance dimension between the 2 lines:

Example of starting to create a centerline dimension

  1. Drag to the opposite side of the construction line to simultaneously toggle the state to a centerline dimension and position the centerline dimension.
  2. Click to simultaneously place the dimension and open its numeric value field.

  3. Optionally, enter a new dimension value.

  4. Press Enter to accept the dimension value.

Example of a centerline dimension

Driven dimensions are useful for maintaining design intent, such as keeping a clearance or wall thickness above a certain value.

  • Dimensions are driving by default. Right-click on a dimension value to select "Driving/Driven" from the context menu.
  • Driving dimensions appear black and can be edited.
  • Driven dimensions appear light gray and cannot be edited (Toggle it to 'driving' and then edit, if necessary.)

Example of the drop down menu used to change a dimension from driven back to driving

  • When a dimension added to a sketch over-defines the sketch, the dimension is automatically made 'driven'.
  • You are able to add driven dimensions anywhere a driving dimension can be added.
  • Driven dimensions reflect the value of the implied dimension; it does not change geometry.
  • When a dimension is switched from driven to driving, it changes the geometry; if changing a driven dimension to driving causes the sketch to be overconstrained, red indicators appear as usual.

Onshape allows users to enter negative values for some dimensions but not all. See below for which dimensions accept negative values.

Onshape allows negative values for:
  • Distance dimension
  • Angle dimension
  • Line length
  • Spline dimension
Onshape does not allow negative values for:
  • Arc dimension
  • Radius or diameter dimension