In my opinion, one of the better file management features in SOLIDWORKS 3D CAD is Pack and Go, which was introduced around 2007. Included in every release of SOLIDWORKS since then, this feature is still very useful today. I’ve been providing SOLIDWORKS tech support for nearly 14 years and it’s fun to show unsuspecting users Pack and Go.
In this blog, I’ll take you through two scenarios:
- Duplication of a data set for sharing or repurposing
- Organizing a data set by renaming multiple files simultaneously
It’s true that these tasks can be done outside of Pack and Go, but I think you’ll find that through the use of Pack and Go, these processes will be completed faster and you will have fewer problems with mixed up file references.
Scenario 1: Duplication of a data set for sharing or repurposing
How many times have you asked for, or received an assembly file from another user and you see the dreaded message regarding missing files in Figure 1?
It’s important to note that there are multiple ways to launch Pack and Go.
First Way to Launch Pack and Go
I typically launch the Pack and Go feature from within a SOLIDWORKS session (I will list an alternate method below). This is found under File > Pack and Go…
Figure 2: First Way to Launch Pack and Go
A view of the default interface settings is shown below. If I’m going to share data with another user and it’s important to include all assemblies, parts and drawings, I’ll check the box in the upper left to “Include Drawings” and I’ll hit the radio button to “Save to Zip file”. I also typically leave the box checked for “Flatten to single folder”. If the flatten option is deselected, the resulting zip will contain sub-folders similar to the original folder locations for each respective part and subassembly. By default, the zip file will take on the name of the assembly or drawing that was chosen for the Pack and Go. We can rename this zip file to any name we choose.
Figure 3: Pack and Go User Interface
The resulting zip file that is generated includes all of the files along with their updated references. If this file is opened in a fresh SOLIDWORKS session on my system, it will not reference the original files, so long as they are not already resident in memory and as long as I left all of the boxes checked for each component name along the left hand column. The file can also be sent via FTP or email to another user with the same results.
Looking more closely at the contents of the zip file, we can see that all of the associated assembly and part files are included. If this data set had drawings, they would be included as well (Figure 4 below).
Figure 4: Zip file contents
Second Way to Launch Pack and Go
Some people prefer to launch Pack and Go from the Windows file explorer right-click menu. This might save time from opening the assembly in a SOLIDWORKS session, but it does make it a bit more difficult to see which files were resolved or lightweight in the last save of the assembly. For this reason, I’m not a big fan of this method. Why is the lightweight/resolved setting important? See the drawbacks in the next section.
Figure 5: Launching with the Right-Click
Alas, there are some drawbacks
Historically, there are a couple of things to watch for. First, make sure the assembly is loaded with all of the components fully resolved. A lightweight component most likely will not make it into the pack and go and you’ll receive a call for missing files from the customer. Beware if you see the blue lightweight feathers below in your feature tree (Figure 6 below).
Figure 6: Lightweight Symbols
Second, if you selected the option to “include drawings”, double check that they are present in your zip file as they don’t always carry over as expected.
Finally, and maybe most importantly, if you are using SOLIDWORKS Workgroup PDM, SOLIDWORKS PDM Standard, or SOLIDWORKS PDM Professional, be very careful. When using Pack and Go in one of these environments, it is all too easy to place the incorrect revision or version of the file back into your vault on your next check-in.
Scenario 2: Organizing a data set by renaming multiple files simultaneously
Use Pack and Go to your advantage if you have a large quantity of files that to be renamed. Again, this is not really intended for SOLIDWORKS PDM users.
- Add prefix or suffix
- Adjust the save to folder
- Adjust the save to name
Add prefix and add suffix to all files
For non-PDM users, Pack and Go might be used to add a revision name or letter to every file in the data set. Note in the image below, how we have selected the box for “Add suffix” and specified “-Rev B” as our custom text. This results in changing all items in the “Save To Name” column to a green color and the text is updated to reflect the “-Rev B” for each individual item. The “Add prefix” functions the same way, but it places the desired text at the beginning of each file name. No changes are final until the “Save” icon at the bottom is selected.
Figure 7: Bulk Change the Filenames
Change the “Save To Folder” for all files
To make this bulk change, simply modify the text string at the bottom of the dialog to include the new destination. In this case, I’ll create a sub-folder called “Rev B”. This should turn the column green, but at least we can see that the Rev B is now present in the folder path in the screenshot below.
Figure 8: Bulk Change the Folder Path
Modify the “Save To Name” and “Save To Folder” attributes individually
Sometimes it’s handy to rename one or two files in the Pack and Go dialog or specify a unique path for just a couple of files. As shown in the screenshot below, we have a green Save To Name cell and a blue Save to Folder cell. These have been manually edited by double clicking on the cells themselves and modifying through a Rename dialog.
Figure 9: Individually Adjust Filename and Folder Path
Select/Replace is useful in situations where we want to take common text in a family of files and replace it with a new set of common text. For example, in our previous sections, we added a –Rev B to all of the files. Let’s go through the process for changing these to a –Rev D.
Again, I’m going to open the main assembly file called READING LIGHT-Rev B.SLDASM and perform a Pack and Go function. As shown in the screenshot below, I’ll pick on the “Select/Replace…” icon. The Select/Replace dialog comes up. Next, I’ll key in the characters “-Rev B” in the top cell and “-Rev D” in the bottom cell. Finally click “Replace All”.
Figure 10: Select/Replace
This changes all of the “Save To Name” labels to a green color and adjusts each name to include –Rev D as a suffix, replacing the old –Rev B. The Select/Replace dialog can be closed at this point. I’m going to adjust the Save to Folder at the bottom of the Pack and Go dialog to the Rev D folder.
Figure 11: Adjusting Save to Folder Path
The final screenshot below reveals a new Rev D folder which contains a fully independent assembly with each file reflecting a –Rev D suffix.
Figure 12: Rev D Folder and Rev D Suffix
As you can see, Pack and Go is a handy tool to help users manage groups of SOLIDWORKS files and repurpose data without impacting existing projects. Like many SOLIDWORKS tools, there are multiple ways to gain access to the application and a wide array of results can be obtained and tailored to your specific project needs.
For more involved file management and revision control options, SOLIDWORKS PDM should be investigated. Users should exercise caution while using Pack and Go if they already have an existing SOLIDWORKS PDM setup established and seek advice from at SOLIDWORKS PDM specialist.
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About the Author
Matt Haywood has a Bachelor of Science in Mechanical Engineering from Western Michigan University. After several years of experience in the automotive and office furniture industries, he joined Fisher Unitech in 2003 as an Application Engineer. Fisher Unitech created a dedicated SOLIDWORKS support group shortly thereafter, and Matt was one of the founding members of the support team. As a Senior Support Engineer today, Matt enjoys working with customers to resolve SOLIDWORKS technical issues and teaching SOLIDWORKS training classes.