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.

Creating Dimensions

Open the Brackets_views02.CATDrawing document.

1. On the Dimensioning toolbar, click the Dimensions icon.

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 toolbar).

creatingdimensions05NLS.gif (3126 bytes)

At this step, the command options in the Tools toolbar ( ) allows you to position the dimension using one of the modes below: Projected, Forced or True Length 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 command option from the Tools toolbar.

creatingdimensions06NLS.gif (3221 bytes)

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. 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 check Display Symbol 2 to display two-symbols dimension, or uncheck this option to display one-symbol dimension.

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

7. Create another dimension on a line.

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

9. Start creating another dimension: click the command icon

and select another circle:

Click in the drawing to validate the creation.

10. 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:

11. 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 until the center anymore.

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 move and then merged the it will generate an error and the dimension will be fuchsia:

Properties

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.

Associativity

If one parent element of the dimension is deleted or deactivated, as soon as you update the drawing (either 3D Generative or 2D Interactive drawing), the orphan dimension becomes purple on the condition you activated the Analysis Display Mode option from the Tools toolbar.

Ensure that if you key in "c: Force Update" to synchronize the drawing with the 3D, any non-associative dimension will disappear.

Colors can be customized using the Analysis Display Mode option from the Tools toolbar or via Tools->Options->Drafting, Dimension tab).

Driving Dimensions

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

	Go to `Tools -> Options` (`Dimension` tab) and activate the `Create driving dimension` option from the `Options` dialog box.
	Create and/or modify the desired dimension on the geometry. If needed, you can use the Tools toolbar and define the `Value` of the dimension you want to be driving.

For more information, refer to Creating Dimension Constraints.

True Dimensions

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

Before using true dimensions make sure that in tools->Options->Associativity on 3D, you have not set only create non-associative dimensions option, to work this functionality must be applied to an associative dimension.

Half-Dimensions

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, for 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):

If in Tools -> Options -> Mechanical Design -> Drafting -> Dimension, you have checked Dimension following the mouse option, then to move the extension line anchor you must hold on the crtl key before selecting the yellow symbol (to switch temporarily the option).