Home » How to change dimensions of SolidWorks parts?

There are multiple ways to edit the dimension of a part. Dimensions of parts can be edited from the part itself, from the assembly, as well as from the drawing.

From a Part


Both sketch and feature dimensions can be edited through editing them, they can also be changed from the graphics area. In both cases, there are three ways this can be done.

  1. Single click on the dimension will allow the user to change the input.
  2. Double clicking the dimension will bring up the Modify window. Use this method for dimensions that use equations, they appear with a sigma in front of their value.
  3. Select the dimension line to show the dimension properties in the design tree. Do not override dimensions by deleting <DIM> from the dimension text box.

Editing dimensions from outside a sketch or feature may require a rebuild. Click the rebuild button from the edit menu or on the SolidWorks menu bar. Tip: use Ctrl+B for rebuild, Ctrl+Q to force rebuild, and Ctrl+Shift+B to rebuild all configurations.

Dimensions with links

Dimensions can be related to each other by a formula, by a global variable, or they can be linked to custom properties.


To create a dimension linked to another, enter the modify window and type “=”. Next, select the dimension to link to and complete the formula. Alternatively use the syntax shown below, for features use @”featurename”.

Global Variable

Global variables can be linked to a dimension. Begin by defining a global variable, select “Tools” – “Equations”. Create a global variable called width (“Width”) and set it to 400mm. Double click the dimension to enter the modify window, in the text box type “=”. Hover over global variables to expand the menu and select width from the list.

Custom Property

Begin by creating a custom property called Thickness, set type to number and value to 85. Units cannot be added to custom properties defined as a number, ensure the value used matched the units of the part. Double click on the dimension representing the thickness and type “=”. This time hover over file properties and select thickness from the list.

Parts with Configuration Tables

Edit dimensions directly from the configuration table. Overwriting a linked value results in all configurations using the value that was input, instead of the defined formula. To edit a design table, select the configuration tab of the design tree and expand tables. From there select “Edit Table in New Window” to open the design table in an instance of Excel.

From an Assembly

Use the same procedure as above to edit visible dimensions of a part directly from the assembly. Dimensions with formulas or links need to be edited at the part level. First select the part from the design tree and use “Edit Component” from the assembly tab of the CommandManager. Use the same button to return to the assembly.

Tip: Define a global variable “Hole Dia” in the assembly, set the value to 110mm. Sketch a circle on the front plane and link the dimension to the global variable. Edit the part, from within the assembly, and delete circle used to create the hole. While still in the same sketch, use convert entities to reference the circle sketched in the assembly. Repair the extrude to create a hole using the new circle, then return to the assembly. The hole position and diameter can now be controlled from the assembly.

From a Drawing

To edit dimensions of a part from a drawing, “Import Annotations” and “Design annotations” must be selected from the view properties. Dimensions will be imported directly from the model. Editing these dimensions updates their value in the model.

The radius dimension, in black, is not required. In the part, edit the sketch and deselect “Mark For drawing”.