Updating Parts

The point of updating a part is to make the application take your very last operation into account. Indeed some changes to a sketch, feature or constraint require the rebuild of the part. To warn you that an update is needed, CATIA displays the update symbol next to the part's name and displays the geometry in bright red.

To update a part, the application provides two update modes:

	automatic update, available in `Tools -> Options -> Mechanical Design`. If checked, this option lets the application update the part when needed.
	manual update, available in `Tools -> Options -> Mechanical Design:`lets you control the updates of your part. What you have to do is just click the Update icon whenever you wish to integrate modifications. The Update capability is also available via `Edit -> Update` and the `Update` contextual command. A progression bar indicates the evolution of the operation.

Note that you can cancel or interrupt updates.

What Happens When the Update Fails?

Sometimes, the update operation is not straightforward because for instance, you entered inappropriate edit values or because you deleted a useful geometrical element. In both cases, CATIA requires you to reconsider your design. The following scenario exemplifies what you can do in such circumstances.

Open the Update3.CATPart document.

The part is shelled in this way:

Enter the Sketcher to replace the circular edge of the initial sketch with a line, then return to Part Design.

CATIA detects that this operation affects the shell. A yellow symbol displays on the feature causing trouble i.e. the shell in the specification tree. Moreover, a dialog box appears providing the diagnosis of your difficulties and the preview no longer shows the shell:

To resolve the problem, the dialog box provides the following options. If you wish to rework Shell.1, you can:

edit it

deactivate it (for more about deactivated features, refer to Feature Properties)

delete it

For the purposes of our scenario that is rather simple, click Shell.1 if not already done, then Edit.

The Feature Definition Error window displays, prompting you to change specifications. Moreover, the old face you have just deleted is now displayed in yellow.

The text "Removed Face" is displayed close to the face, thus giving you a better indication of the face that has been removed. Such a graphic text is now available for Thickness and Union Trim features too.

Click OK to close the window. The Shell Definition dialog box appears.

Click the Faces to remove field if not already done and select the replacing face.

Click OK to close the Shell Definition dialog box and obtain a correct part. The shell feature is rebuilt.

Cancelling Updates

You can cancel your updates by clicking the Cancel button available in the Updating...dialog box.

Interrupting Updates

This scenario shows you how to update a part and interrupt the update operation on a given feature by means of a useful message you previously defined.

Open the Update1.CATPart document.

Right-click Hole.1 as the feature from which the update will be interrupted and select the Properties contextual command.

The Properties dialog box is displayed.

Check the option Associate stop update. This option stops the update process and displays the memo you entered in the blank field.

This capability is available in manual or automatic update mode.

Enter any useful information you want in the blank field. For instance, enter "Fillet needs editing".

Click OK to confirm and close the dialog box.

The entity Stop Update.1 is displayed in the specification tree, below Hole.1, indicating that the hole is the last feature that will be updated before the message window displays.

Edit Sketch.1, which will invoke an update operation.

When quitting the Sketcher, the part appears in bright red.

Run the Update operation by clicking the

icon.

The Updating... as well as the Stop Update message windows are displayed. The Stop Update windows displays your memo and lets you decide whether you wish to stop the update operation or continue it.

Click Yes to finish.

The part is updated. You can now edit the fillet if you consider it necessary.

If you decide not to use this capability any longer, you can either:

	right-click Hole.1, select the Properties contextual command and check the Deactivate stop update option: the update you will perform will be a basic one. To show that the capability is deactivated for this feature, red parentheses precede Hole.1 in the specification tree.
	right-click Stop Update.1 and select the Delete contextual command to delete the capability.