Setting Up Your SOLIDWORKS System Files

In the past three articles, I have focused on how you create your template as well as your Property Tab files:

But once these files and other system files, such as BOMs, weldments profiles, etc., have been created, how do you access them?

I will elaborate in this article.

Basic Setup

If you have created your own templates, profiles, BOM tables and so forth, I highly recommend that you save them in a custom folder that is not part of the SOLIDWORKS installation. This way you will not delete it by mistake if you do a complete uninstall of SOLIDWORKS.

In this example, I have created a folder with different subfolders based on the type of file.

To ensure that I can access them I go to Tools > Options.

Within “General options,” click on “File Locations.”

Browse to the different locations based on the type of file. For instance, with the sheet format file, select Sheet Formats in the dropdown list.

Browse to the location you want.

Make sure that the unused file locations are deleted where possible. Note that not all file types allow for multiple file locations.

This procedure is usable with both local files, network files and PDM.

Setting Up in 3DEXPERIENCE

You should set up your system files in 3DEXPERIENCE because it will ensure that you will always have access to the latest version of the template. Even if you log on to another workstation, you are ready to go.

Previously you had to save the templates to 3Ddrive and use it much like a Dropbox or similar cloud storage. However, this new method saves the files in your collaborative space and, depending on your coworkers’ access, they can also use the same templates.

Before you start saving your files to your collaborative space, I recommend opening your bookmark editor and creating a new bookmark. I have called it SOLIDWORKS Resources.

Ensure that all users have access to the bookmarks, or they will not be able to use the system files.

This also requires ensuring that the bookmark is in a state where everyone can access the content.

Once the bookmark is created, you can drag your system files to your 3DSpace which you share with your coworkers.

If you drag a folder to your bookmark, this will be converted to a bookmark. This means that you can keep the Weldment Profile file structure.

Again, make sure that these files are in a state that ensures that your coworkers have access.

To use these newly created files, once again go to Tools > Options and within the System Options tab go to the File Locations tab and select the Sheet format drop down selection, then press the Add Button. This will show the latest selected folder, as previously shown.

However, if you have the SOLIDWORKS Connected or the 3DEXPERIENCE add-in installed on your computer, you will have an additional button called “Select from 3DEXPERIENCE.”

If you press this button, a new pop-up will appear and give you access to the bookmarks of your collaborative space.

Within this you can change the workspace and select the bookmark you want to look at.

Once selected, the system will, in the case of the Sheet format files, locate all the files with the extension and download them to your system, making them available at all times.

There are some exceptions to what system files that can be located this way.
Among these are template files (see next section on how to handle this), inspection system files and defeature rule sets.

If there is an update to the files, you must update the files (almost) manually. This is done to ensure that your system does not have to download the system files every time you start your SOLIDWORKS product.

To update the files, select one of the file types that are on the platform and the path, and press Update.

A window will appear and allow you to check for updates and, of course, update any files that are out of date.

Tinkering with Templates

I went into depth on templates in my previous article but it’s worth touching on templates here.

Everything with templates starts when you save the template. Unlike previous versions of SOLIDWORKS, you no longer use Save As and find the file extension (SLDDOT). Instead, go to File, and press Save As Template.

This will open a command, which allows you to save the files directly on the platform.
Again, you need to decide if you want the file to be available for all users or only to you.

I recommend saving the final version for all users and saving draft versions for yourself.

Save as Draft allows you to test and see if everything works as intended before rolling it out to the rest of the company.

After the file is uploaded and put in a Released state, it will automatically be added to the templates that others can use.

Bonus info from the train

Revision tables are an important part of your drawings as they give you information about what changes have been made to a drawing.

Creating a Revision table is a manual process in SOLIDWORKS and can be quite tedious. However, it is possible to automate the process and use the revision that you use on the 3DEXPERIENCE platform on your SOLIDWORKS drawing.

To do this, open your SOLIDWORKS drawing template (for more information on creating templates see: Setting up Your SOLIDWORKS Template for Drawings), go to Document Properties and select Tables > Revision.

At the bottom, you will find a section called Type. By default, this is set to SOLIDWORKS Revision Table, which is how revision tables have been handled for the past 25 years in SOLIDWORKS. However, if you select “3DEXPERIENCE driven Revision Table,” you will now use the revision scheme on the platform.

All you need to do now is to select the number of rows you want on your table. This will ensure that you always have access to the latest revision from the platform. Once this is set, you are good to go, and you can insert your revision table and let that take care of itself.

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