How to Use Save As with References
How to use Save As with References
If you have an assembly that you want to re-use, modifying some or all of the component assemblies and/or parts, the Save As with References workflow is worth considering. SOLIDWORKS is great for giving us multiple ways of accomplishing tasks, and this scenario is no exception. Many SOLIDWORKS users are familiar with the Pack and Go utility, but Save As with References provides a few advantages that may make it a better choice in specific circumstances.
Note For PDM Users
If you use PDM you can use the Copy Tree or Move Tree functions within PDM which behave in a similar manner. See our articles on PDM Copy Tree and PDM Move Tree for more information.
Differences Between Pack and Go and Save As with References
In most cases Pack and Go is the preferred method to duplicate an assembly including all sub-assemblies, parts and drawings. With the ‘Include drawings’ option selected, you can create an exact duplicate of the existing file set, including drawings for all referenced subcomponents.
Let’s take a look at the results of the Pack and Go operation including drawings on a sample file set. In this case we have a top-level drawing as well as a drawing of one of the sub-assemblies.
Save As with References provides a little more control over which files get copied to the new location, but does not include drawings for sub-components. In some cases this may be preferable rather than creating new versions of all files. In our example, the file set is contained in a single folder which is easy enough to manage, but in the real-world we often have documents stored across many folders, so duplicating the entire assembly with all of its referenced documents is not always the best option.
When to use Save As with References
A good example of a use-case for this method would be if you have a top-level assembly that you want to make a new version of along with its drawing, but you want to also create modified versions of some, but not all, of the sub-components.
In our example, we are going to use the top-level assembly drawing ‘Simplified Assembly’ to create a new version of the assembly as well as a new version of the arm. All other components in the new assembly will continue to reference the original files in their original locations.
How to use Save As with References
The mechanics of using this workflow are fairly simple:
- With the top-level drawing or assembly open in SOLIDWORKS, choose ‘File’->’Save As…’
- Browse to the destination folder for the new drawing/assembly if you wish to save it in a different folder
- Modify the ‘File name:’ field to the appropriate name for the new document
- Check the ‘Include all referenced components’ option
Note: At this point if you click ‘Save’, the behavior will be identical to the default behavior of Pack and Go with the ‘Include Drawings’ option unchecked. - Click the ‘Advanced’ button
- Note that the top-level document displays the name that you entered in step 3 and the ‘Folder’ for that document reflects the folder chosen in step 2, but all other files and folders are still displaying the original filenames and locations
- Rename documents (repeat steps 7a-7c for all documents that you wish to create a new version of)
- Double-click on any document you wish to rename and enter the new document name
- To save the change, single left-click on any other field and the edited text will display in green to indicate that it has been modified
- Update the ‘Folder’ location if needed
- Copy the ‘Folder’ location from the top-level document
- Single left-click into the ‘Folder’ field of the modified filename, select the existing path and Paste the new folder path to replace it
- To save the change, single left-click on any other field and the edited text will display in green to indicate that it has been modified
- Click ‘Save All’ to complete the process
If you open the target folder you will see that the result of this operation is a renamed version of the top-level document along with any of the documents that were renamed.
When we open our new drawing and assembly we can see that it is referencing the ‘Version 2 Assembly’ and ‘Version 2 Arm’ while all other components are referencing the original files, avoiding unnecessary duplication of parts which could become confusing
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