Modify Dimension

You can change a dimension in a part, sketch, assembly, or drawing in the Modify dialog box.

To change a dimension:

  1. Double-click a dimension.
    The Modify dialog box appears.
  2. Change the dimension value with the arrows, thumbwheel, mouse wheel, or by typing in the dimension box.
    The Modify dialog box displays a slider instead of a thumbwheel when the numeric value is bounded, such as an angle that must be greater than 0 and less than 90 degrees.
    Thumbwheel Slider
    Up arrow, Thumbwheel/Slider right, Mouse wheel up Increases value by length increment set in Spin Box Increments.
    Down arrow, Thumbwheel/Slider left, Mouse wheel down Decreases value by length increment set in Spin Box Increments.

    Ctrl + Arrow

    or

    Ctrl + Thumbwheel/Slider

    or

    Ctrl + Mouse wheel

    		 Increases/decreases length increment by 10 times the length increment set in Spin Box Increments.

    Alt + Arrow

    or

    Alt + Thumbwheel/Slider

    or

    Alt + Mouse wheel

    		 Increases/decreases length increment by the length increment set in Spin Box Increments divided by 10.
    You can use the dimension box as a calculator by entering values and arithmetic symbols directly. You can also assign units of measurement to a value by using the type-ahead list or by typing the unit directly.
  3. Choose from:
      Option Description
      Add Equation If a dimension is driven by an equation, appears in the Modify dialog box.
    If you specify different units of measurement to each value in an equation, the dimension will use the unit of measurement defined in the document.
      Add a Global Variable If a dimension is assigned as a global variable, appears in the Modify dialog box.
    This Configuration Applies the value to the active configuration only.
    All Configuration Applies the value to all configurations in the model.
    Specify Configuration Applies the value to the active configuration and any other configurations you select.
    Link to Parent Configuration (Available only in derived configurations.) Maintains the link between the value in the parent configuration and the derived configuration. If the dimension was previously overridden in the derived configuration, re-establishes the link and sets the value to the value from the parent.
  4. Use the buttons as follows:
      Option Description
    Save the current value and exit the dialog  
    Restore the original value and exit the dialog  
    Regenerate the model with the current value  
    Reverse the sense of the dimension  

    Reset spin increment value

    		 Launches the Increment dialog box, where you can change the increment used by the spin box arrows. After you enter a value, press Enter to accept the value. Select Make Default to make your new specification the default spin box increments in System Options.
    Mark dimension to be imported into a drawing Available only in part and assembly documents. When you Insert Model Items into a drawing, you can insert all dimensions or only those marked.