Dimension

Use the Dimension tool (D) to define and/or constrain the dimensions of a sketch.

The dimension tool can capture:
  • Vertical, horizontal, or aligned distance between a point, vertex, or entity and the sketch origin. (The sketch origin is a projection of the global origin onto the sketch plane.)
  • Vertical, horizontal, or aligned distance between a point, vertex, or entity and the the red and green sketch axes
  • Vertical, horizontal, or aligned distance between one point or vertex and another
  • Distance between two parallel lines
  • Diameter of a circle
  • Radius of a fillet or arc
  • Angles

Driving Dimensions: These dimensions drive the design intent. They can be edited directly through a microdialog either by entering numbers or assigning variables. Changes to driving dimensions will drive changes to reference dimensions.

Reference Dimensions: These dimensions appear in parentheses and cannot be edited directly.

Tip: To find and open a tool, press Ctrl+F. For more information, see Find and Search for Tools.
  • Decide which dimensions you will want to edit and capture them first. This is easier than changing them from reference dimensions to driving dimensions later.
  • Once a rectangle sketch has been defined by two dimensions (e.g. length and width), additional dimensions will be captured as reference dimensions by default.
Note: Currently you can only use the Dimension tool on sketch curves.

Apply Dimensions to Sketch Entities

Capture the length of a line, the diameter of a circle, the radius of an arc, or the distance between two sketch entities.

  1. In an active sketch, open the Dimension tool:
    • On the Sketch ribbon, select the Dimension icon OR
    • On your keyboard, press the D key
  2. Select a sketch entity. Dimension previews appear as you move your mouse. If desired, select a second sketch entity to apply a dimension between the two.
    Tip: You can select the red and green sketch axes to apply dimensions.
  3. Left-click in the modeling window to position the dimension. For driving dimensions, enter the desired dimension in the microdialog.
  4. Optional: To apply a variable, click the icon on the microdialog and select a variable from the dropdown menu, or select Add Variable to create a new variable based on the driving dimension.
  5. Right-click and mouse through the check mark to exit, or double-right-click.

Create or Assign Variables to Parametrize a Model

Create or assign variables to parametrize a model. Variables can be created from a tool or the tool’s microdialog where f(x) is present.

You can create or assign existing variables via the microdialog or in various tools and contexts.

Fully Define a Sketch

A sketch is fullly defined when its dimensions and its position relative to the point of origin have been defined. A fully defined sketch will appear in black.

  1. In an active sketch, open the Dimension tool:
    • On the Sketch ribbon, select the Dimension icon

      OR
    • On your keyboard, press the D key.
  2. Apply dimensions to the sketch.
  3. Apply dimensions between the sketch and the point of origin.
  4. Right-click and mouse through the check mark to exit, or double-right-click.
    Tip: To find and open a tool, press Ctrl+F. For more information, see Find and Search for Tools.

    The easiest way to fully define a sketch is to start it from the global point of origin.



Edit a Driving Dimension

Reposition, change the value of, or delete a dimensional constraint.

  1. In an active sketch, select a dimension.
  2. In the microdialog:
    • Enter the desired dimension in the text field OR
    • Select the icon the assign a variable to the dimension
  3. Press the Enter key.
  4. Left-click to close the microdialog.

Edit a Reference Dimension

Convert a reference dimension to a driving dimension and edit it.

To edit a reference dimension, you must first convert it to a driving dimension. If a sketch is constrained by driving dimensions, converting a reference dimension to a driving dimension will overconstrain the sketch. You must convert at least one of the driving dimensions to a reference dimension before you can edit any dimension.
  1. In an active sketch, right-click the reference dimension you wish to edit.
  2. Deselect Reference on the context menu.

    The dimension will appear as a driving dimension (without parentheses), but the sketch may now be colored magenta, indicating that it is overconstrained.
  3. Right-click one of the other dimensions. Select Reference in the context menu.

    The dimension now appears in parentheses, indicating that it is a reference dimension. The sketch is no longer colored magenta.

  4. Select the dimension you wish to edit.
  5. In the microdialog:
    • Enter the desired dimension in the text field, OR
    • Select the icon to assign a variable to the dimension.
  6. Left-click to close the microdialog.