Path: File | Save Management
Use this to ...
- Save several documents at once.
- Save component parts, assemblies, and drawings independently.
- Save a file and all its related files to a new file location.
- We recommend using Save Management as a best practice for saving files instead of the Save, Save As, or Save All commands. This command is particularly appropriate for new users to learn when CATIA designates files to be automatically saved.
Save Management allows you to see which files CATIA will save, and where CATIA will save the files. The function also lets you override CATIA's default of automatically saving related documents.
- Actions you assign to files (Save, Save As, or Save Auto) don't actually occur until you click OK. Changes are not made to the files when you click Cancel.
Process: Using Save Management
1. Select File | Save Management. The Save Management dialog displays.
2. To set a file to save with its current name and location, select it from the list and click Save.
3. To set a file to save with a new name or location, select it from the file list and click Save As. The Save As dialog displays.
In the Save in list, select a location. In the File Name box, enter a new name, and click OK to return to the Save Management dialog.
4. If you used Save As on a .CATProduct document, click Propagate directory to assign the new location to all the assembly components.
5. Click OK to execute the defined actions.
Open File List
Shows all the documents you currently have loaded.
Indicates whether the file is new, has been modified, or is read-only.
Shows the current name of the file. If you assign a new name using Save As, the new name displays.
Shows the current path for the file. If you assign a new path, the new path displays.
Shows the action CATIA performs on the file when you click OK. The Save action displays when you click Save or Save As. By default, CATIA also assigns the Save Auto action to all the dependent files that have been modified. For instance, when you save an assembly, components that have been modified automatically receive the Save Auto action. CATIA also assigns the Save Auto action to the parent file (assembly or drawing) when the component file is saved with a new name or new path.
Designates that the file will be saved with its current name and in its current location. This command is only available if you have modified the file and it is not read-only.
Displays the Save As dialog, allowing you to assign a new name and location to the file.
Lets you assign the new directory to all of the parent's dependent files, if you move the location of a parent document (using Save As).
Removes the action assigned for the selected file only.
Enable Independent Saves
Stops CATIA from assigning the Auto Save action to any dependent documents. The default setting is disabled, meaning all dependent files receive the setting Save Auto.