Updating Your Design

This task explains how and when you should update your design.

The point of updating your design is to make the application take your last operation into account. Indeed some changes to geometry or a constraint may require rebuilding the part. To warn you that an update is needed, CATIA displays the update symbol next to the part name and displays the corresponding geometry in bright red.
To update a part, the application provides two update modes:
automatic update, available in Tools -> Options -> Shape, General tab. If checked, this option lets the application update the part when needed.
manual update, available in Tools -> Options -> Shape, General tab, it lets you control the updates of your part. You simply need to click the Update icon whenever you wish to integrate modifications. 

  1. To update the part, click the Update icon .

A progression bar indicates the evolution of the operation.

You can cancel the undergoing update by clicking the Cancel button available in the Updating... dialog box.
Keep in mind that some operations such as confirming the creation of features (clicking OK) do not require you to use the update command. By default, the application automatically updates the operation.
The Update capability is also available via Edit -> Update and the Update contextual command. 

To update the feature of your choice, just select that feature and use the Local  Update contextual command.
Besides the update modes, you can also choose to visualize the update on the geometry as it is happening by checking the Activate Local Visualization option from the Tools -> Options -> Shape, General tab.
In this case, as soon as you have clicked the Update icon :
  1. the geometry disappears from the screen
  2. each element is displayed as it is updated, including elements in No Show mode. Once they have been updated, they remain in No Show mode.

Interrupting Updates
This task explains how to update a part and interrupt the update operation on a given feature by means of a useful message you previously defined.
Open any document containing geometric elements.

  1. Right-click an element from the specification tree and choose the Properties contextual menu item.

The Properties dialog box is displayed. 

  1. From the Mechanical tab, check the Associate stop update option.

  1. Enter the text to be displayed when the updating process will stop when reaching this element.

  2. Click OK to confirm and close the dialog box.

The Stop Update.1 feature is displayed in the specification tree, below the element for which it was defined.

  1. Whenever it is needed, click the Update icon to update the whole part.

The updating process stops after having updated the element selected above, and issues the message as has been defined earlier:

  1. Click Yes or No, depending on what you intend to do with the geometry created based on the selected element.
Would you no longer need this capability, you can:
right-click the element for which the stop was defined, choose the Properties contextual command and check the Deactivate stop update option from the Mechanical tab: the update will no longer at this element.
You notice that when the capability is deactivated, the Stop Update icon changes to: in the specification tree.
right-click Stop Update.1 from the specification tree, and choose the Delete contextual command.

 
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