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.

Shortcut: d

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 dialog opens on the placement of the dimension.

    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.

Note that 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.

  1. Click Dimension tool icon.
  2. Click a line to dimension one line, or two lines to dimension the distance between them.

    When dimensioning between two lines, note that this will imply parallelism without a visual parallel constraint.

  3. Drag to visualize the dimension.
  4. Click again to access the numeric value field.
  5. Type value and press Enter.

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

  1. Click Dimension tool icon.
  2. Click corner points diagonal to each other.
  3. Drag to visualize the dimension.
  4. Click again to access the numeric value field.
  5. Type value and press Enter.

Example of how to find Diagonal distance

Example of length or height distance

  1. Click Dimension tool icon.
  2. Click the edge of the circle.
  3. Drag cursor into or away from the circle.
  4. Click to activate numeric value field.
  5. Type value and press Enter.

Example of how to find the Diameter

  1. Click Dimension tool icon.
  2. Click each line.
  3. Move cursor into angle.
  4. Click to activate numeric value field.
  5. Type value and press Enter.

Example of clicking each line to find the angle

You are also able to drag the label 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

Direct distance

  1. Click Dimension tool icon.
  2. Click each endpoint of the lines.
  3. Move cursor away at an angle to get shortest distance between the points.

Example of how to find the direct distance between two lines

Linear distance

  1. Click Dimension tool icon.
  2. Click each endpoint of the lines.
  3. Move cursor straight up for linear distance.

Example of how to find the Linear distance between two lines

  1. Click Dimension tool icon.
  2. Click the edge of the arc.
  3. Move cursor into or away from arc.
  4. Click to enter numeric value field.
  5. Type value and press Enter.

Example of how to find the radius of an arc

  1. Click Dimension tool icon.
  2. Click each arc endpoint.
  3. Move cursor to arc line.
  4. When arc line is highlighted, click to activate numeric value field.
  5. Type value and press Enter.

Example of how to find the length of an arc

  1. Click Dimension tool icon.

  2. Click a spline point.

  3. Click any other sketch point (including another spline point).

  4. Move cursor to position the dimension.

  5. Type a value and press Enter.

Example of spline dimensions

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. Start the dimension between the entity and the construction line, resulting in a distance dimension:

Example of starting to create a centerline dimension

  1. Move the mouse to the opposite side of the construction line to toggle the state to a centerline dimension.
  2. Enter the value and press Enter.

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 over-constrained, 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
  1. Tap Dimension tool.
  2. Select the entity (or entities) between which to dimension, and the location of the dimension.

    The dialog opens on the placement of the dimension.

  3. Enter a value and select the checkmark to accept the value.
  1. Tap to select a corner point.
  2. Tap to select the opposite corner point.
  3. The current value appears, tap on it to open the number pad.
  4. Use number pad to enter a dimension.

Example of diagonal distance dimension

  1. Tap to select a vertical or horizontal line.
  2. The current value of the length or height appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of length or height dimension

  1. Tap to select the edge of circle.
  2. The current value appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of diameter dimension

  1. Tap to select a line.
  2. Tap to select another line.
  3. The current value of the angle between the two lines appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of angle dimension

Linear distance / direct distance

  1. Tap to select a point.
  2. Tap to select another point.
  3. The current value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of Linear distance/direct distance dimensions

  1. Tap the edge of an arc to select it.
  2. The current value of the radius appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of radius dimension

Arc length

  1. Tap to select both points of an arc.
  2. Tap on the curve of the arc to select it.
  3. The arc length value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of Arc length/curve length dimension

Spline curve length

  1. Tap a spline to select it.
  2. The curve length value appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of spline curve length dimension

  1. Tap to select a point.
  2. Tap to select a plane.
  3. The current value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of dimension between sketch geometry and 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.

  1. Tap to select the point to dimension.
  2. Tap to select the construction line to create as the centerline.

    A dimension is set between the point and the construction line.

  3. Touch and drag the dimension across the construction line.

    Once the dimension crosses the construction line, the construction line becomes the centerline and the dimension adjusts accordingly.

    Example of using the centerline dimensions tool with the circle center point and construction line selected

    Example of centerline dimensions, showing the final result

  • 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. Tap to select a dimension, then two-finger tap to bring up the context menu. In the context menu you can tap to Toggle Driven/Driving dimensions.
  • Driving dimensions appear black and can be edited.
  • Driven dimensions appear light gray and are not able to be edited (toggle a driven dimension to driving and then edit, if necessary).

Example of driven dimensions

  • 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 dimensions; 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 over-constrained, 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.

iOS allows negative values for:

  • Distance dimension
  • Angle dimension
  • Line length

iOS does not allow negative values for:

  • Arc dimension
  • Spline dimension
  • Radius or Diameter dimension
  1. Tap Dimension tool.
  2. Select the entity (or entities) between which to dimension, and the location of the dimension.

    The dialog opens on the placement of the dimension.

  3. Enter a value and select the checkmark to accept the value.
  1. Tap to select a corner point.
  2. Tap to select the opposite corner point.
  3. The current value appears, tap on it to open the number pad.
  4. Use number pad to enter a dimension.

Example of using the diagonal distance dimension tool

  1. Tap to select a vertical or horizontal line.
  2. The current value of the length or height appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of using the length and height dimension tool

  1. Tap to select the edge of circle.
  2. The current value appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of using the diameter dimension tool

  1. Tap to select a line.
  2. Tap to select another line.
  3. The current value of the angle between the two lines appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of using the angle dimension tool

Linear distance / direct distance

  1. Tap to select a point.
  2. Tap to select another point.
  3. The current value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of using the linear distance/direct distance dimension tool

  1. Tap the edge of an arc to select it.
  2. The current value of the radius appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of using the radius dimension tool

Arc length

  1. Tap to select both points of an arc.
  2. Tap on the curve of the arc to select it.
  3. The arc length value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of using the Arc length/curve length dimension tool

Spline curve length

  1. Tap a spline to select it.
  2. The curve length value appears, tap on it to open the number pad.
  3. Use the number pad to enter a dimension.

Example of using the Spline curve length dimension tool

  1. Tap to select a point.
  2. Tap to select a plane.
  3. The current value appears, tap on it to open the number pad.
  4. Use the number pad to enter a dimension.

Example of using the dimension tool between the sketch geometry and 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.

  1. Tap to select the point to dimension.
  2. Tap to select the construction line to create as the centerline.

    A dimension is set between the point and the construction line.

  3. Touch and drag the dimension across the construction line.

    Once the dimension crosses the construction line, the construction line becomes the centerline and the dimension adjusts accordingly.

    Example of using the centerline dimensions tool with the circle center point and construction line selected

    Example of using the centerline dimensions tool, showing the final result

  • 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. Double tap a dimension to open the Number pad, then tap the Driven/Driving button to switch the dimension type. The button says what type of dimension you have selected. Tap the button to switch to the opposite type of dimension.
  • Driving dimensions appear black and can be edited.
  • Driven dimensions appear light gray and are able to be edited (toggle a driven dimension to driving and then edit, if necessary).

Example of driven dimensions

  • 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 dimensions; 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 over-constrained, 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.

Android allows negative values for:

  • Distance dimension
  • Angle dimension
  • Line length
  • Spline dimension

Android does not allow negative values for:

  • Arc dimension
  • Radius or Diameter dimension