Defining a Multi-Instantiation

This task shows you how to repeat components as many times as you wish in the direction of your choice.

The option "Automatic switch to Design mode" is now available for this command. For more about this option, refer to Access to geometry.

Open the Multi_Instantiation.CATProduct document.

Select the component you wish to instantiate, that is CRIC_BRANCH_3.

Click the Define Multi-Instantiation icon

The Multi-Instantiation dialog box is displayed, indicating the name of the component to be instantiated.

The shortcut Ctrl + E calls the command too.

The Parameters option lets you choose between the following categories of parameters to define:

Instances & Spacing

Instances & Length

Spacing & Length

Keep the Instances & Spacing parameters option and enter 3 as the number of instances and 90mm as the value for the spacing between each component.

To define the direction of creation, check x axis.

There is another way of defining a direction. You can select a line, axis or edge in the geometry. In this case, the coordinates of these elements appear in the Result field.

Clicking the Reverse button reverses the direction.

The application previews the location of the new components:

Make sure the option Define as Default is on. If it is so, the parameters you have just defined are saved and will be reused by the Fast Multi-Instantiation command.

Click OK to create the components.

Three additional components are created in the x direction. The tree displays them as well.

The Apply button executes the command but the dialog box remains open so as to let you repeat the operation as may times as you wish.