Creating Dimensions   

In this task, you will learn how to create dimensions. When creating dimensions on elements, you can preview the dimensions to be created. 

This task deals with:


Creating Dimensions 

Open the Brackets_views02.CATDrawing document.
  1. Click the Dimensions icon on the Dimensioning toolbar.

  2. Click a first element in the view. For example, a circle.

  3. If needed, click a second element in the view.
    The dimension type is automatically defined according to the selected elements ( or in the Tools Palette).

    At this step, the options in the Tools Palette (        ) allow you to position the dimension using one of the following modes: Projected or Forced modes. These options are also available in the contextual menu.

    This toolbar is situated at the bottom right of screen. If you cannot see it properly, just undock it.

  4. Click the Force Dimension on element icon from the Tools Palette.

  5. Right-click to access the contextual menu and select 1 symbol.
    The dimension becomes a one-symbol dimension.


    During the dimension creation step, you can switch between one-symbol or two-symbols dimension by selecting or deselecting 1 symbol in the contextual menu.

    Once the dimension has been created, you must use the Properties menu to specify whether you want to use one or two symbols. Right-click the dimension and in the contextual menu, choose Properties. Click the Dimension Line tab and then select Symbol 2 to display two-symbols dimension, or clear this check box to display one-symbol dimension.

  6. Click in the drawing window to validate the dimension creation.

  7. Create two other dimensions on a line as shown.

  8. Select the two dimensions with the Ctrl key (you can move them both).

  9. Start creating another dimension: click the Dimensions icon and select another circle.

  10. Click in the drawing to validate the dimension creation.

  11. Right-click the dimension you just created and in the contextual menu, choose Dimension.3 Object and select Swap to Radius.
    The diameter dimension has swapped to radius dimension.

  12. Right-click the dimension again, and in the contextual menu, choose Dimension.3 Object, and uncheck Extend to Center.
    The radius extension line is not extended up to the center anymore.


More About Dimensions

  • You can use this functionality through the Properties menu: right-click on the dimension and choose Properties. On the Dimension Line tab, select the type of extension you want from the Extension list: From standard, Till center or Not till center.

  • This functionality works with radius dimension and one-symbol diameter dimension.
  • When you create a dimension between a generated element in a broken view and a sketched element, the dimension value may be false to let the user set a fake dimension value.
  • When you create a dimension between an axis and another element, the dimension created by the software is automatically an half dimension. 
    To bypass this problem, during creation, uncheck Half Dimensions in the contextual menu (right-click). 
  • You can generate errors when refreshing the dimensions in the following cases:
    • In this drawing the dimension "80.14" is measured from the line B to the line C:

      If the corresponding part is modified and the chamfer removed, when the drawing is refreshed the dimension is colored in fuchsia because the line B was removed with the chamfer:
    • If the two elements separated by the dimension value are moved then merged, an error is generated and the dimension turns to fuchsia by default (or according to the color defined for Not-up-to-date dimensions in the Types and colors of dimensions dialog box available via Tools > Options > Mechanical Design > Drafting > Dimension tab, Analysis Display Mode area, Types and colors... button).
      Note that in this case, it is not possible to create a null value. Should you need to, you should create  a driving dimension and set its value to 0.


If you right-click the dimension before creation, a contextual menu lets you modify the dimension type and value orientation as well as add funnels. Using this contextual menu once the dimension is created, you can also access the Properties options.


If one parent element of the dimension is deleted or deactivated, as soon as you update the drawing, the dimension turns to the color defined for Not-up-to-date dimensions in Tools > Options > Mechanical Design > Drafting, Dimension tab (provided the Analysis Display Mode is active).

Driving Dimensions

You can create dimensions that will, by default, drive the geometry. For this:

  • Go to Tools > Options> Mechanical Design > Drafting, Dimension tab, and activate the Create driving dimension  option.
  • Create and/or modify the desired dimension on the geometry. If needed, you can use the Tools Palette and define the Value of the dimension you want to be driving.

For more information, refer to Creating Driving Dimensions.


True Dimensions

True Length dimensions can be created using the True Length Dimensions option from the Tools Palette or using the contextual menu. 

Before using true dimensions, make sure that you have not set the only create non-associative dimensions option in Tools > Options > Mechanical Design > Drafting, Dimension tab, Associativity on 3D.  In order to work, this functionality must be applied to an associative dimension.



You can create half-dimensions. For this, right-click the dimension as you create it and select the Half-dimension option from the contextual menu.


Extension Line Anchor

As you create a dimension between two elements, one of these elements being a circle, you can select the extension line anchor. To do tor this, you can :

  • use the contextual menu (positioned on the dimension) and select one of the available Extension Line anchor options.

You will thus position the extension line:

  • at one extremity of the circle (First Anchor)
  • at the center of the circle (Second Anchor)
  • at one extremity of the circle (Third Anchor)
  • drag the yellow symbol to the one of the anchors (anchors appear when the cursor is over the yellow symbol):
  Note that if you selected the Dimension following the mouse option in Tools > Options > Mechanical Design > Drafting > Dimension tab, then, to move the extension line anchor, you must press the Crtl key before selecting the yellow symbol (to switch temporarily the option).