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Where are SOLIDWORKS templates stored?

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When you create a new part, assembly or drawing in SOLIDWORKS, you are really just opening a template file. These template files control units, drafting standards, title block references, custom properties and many other document settings.

By default, SOLIDWORKS stores its standard document templates in a hidden Windows folder similar to C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\templates. However, the effective location of your templates is driven entirely by the paths defined in System Options > File Locations and the choices you make in System Options > Default Templates. Managing these paths correctly is the key to reliable, predictable templates across upgrades and across a team.

What are SOLIDWORKS templates?

In the context of this article, “templates” primarily means document templates that you select when you start a new SOLIDWORKS file:

  • Part templates – files with the extension .prtdot
  • Assembly templates – files with the extension .asmdot
  • Drawing templates – files with the extension .drwdot

Each of these template types can store settings such as:

  • Units (MMGS, IPS, etc.) and dimensioning standard (ISO, ANSI, DIN, …)
  • Document properties (fonts, arrow styles, precision, line thicknesses)
  • Predefined layers, custom properties and annotations
  • Which sheet format or title block a drawing should use by default

There are also other “template-like” files controlled by File Locations (for example BOM templates, revision tables, hole tables and sheet formats). They are stored in different folders, but they are managed in exactly the same way as document templates.

Default Templates

The Default Templates settings tell SOLIDWORKS which document templates to use automatically when a new file has to be created behind the scenes – for example when importing a STEP file, mirroring a part, or saving bodies out as separate parts. They also control whether you are prompted to pick a template every time you create a new file.

To review or change these settings:

  1. Go to Tools > Options (or click the Options gear icon).
  2. Under the System Options tab, select Default Templates.
  3. Choose one of the two behaviours:
    • Always use these default document templates – SOLIDWORKS will silently use the specified part, assembly and drawing templates whenever it needs to create a file.
    • Prompt user to select document template – you will be shown the New SOLIDWORKS Document dialog and can pick the template each time.
  4. For each of Parts, Assemblies and Drawings, browse to the required template file in your template folders.

Use the Reset button on this page to clear the paths and return the default behaviour. Choose Reset this page only unless you intend to reset all of your SOLIDWORKS system options.

If the desired templates are not available in the browse dialog, it usually means the Document Templates path in File Locations is not pointing at the folder where your templates are stored. Update the path in File Locations, click OK to save, then return to the Default Templates page and select the correct templates.

“The default templates are not valid” error

If SOLIDWORKS shows the message “The default templates are not valid. The problems can be resolved by correcting the default templates under the Options dialog.” when you import a file or create a new document, it means that the part, assembly or drawing template specified here cannot be found or opened.

Typical causes include:

  • The template folder was moved, renamed or deleted.
  • SOLIDWORKS was upgraded or an older version was uninstalled, and Default Templates still points to the old version’s C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\templates folder.
  • Templates were stored on a network or PDM location that is currently not accessible.

To fix the error:

  1. First, go to System Options > File Locations and confirm that Document Templates points to a valid folder that actually contains your template files.
  2. Then return to System Options > Default Templates and re-browse to valid templates in those folders.
  3. If you are upgrading between major versions, the Edit All button under File Locations can be used with Find/Replace to update all paths from one version folder (for example 2024) to the next (for example 2025) in one shot.

Once both the File Locations and Default Templates settings point at real, accessible template files, the error will stop appearing.

File Locations

The File Locations settings are the master list of where SOLIDWORKS looks for templates and many other reference files. This is where you can see, and control, where your templates are actually stored.

To review these locations:

  1. Go to Tools > Options.
  2. On the System Options tab, select File Locations.
  3. Use the Show folders for drop-down to choose the item you want to inspect (for example Document Templates or BOM Templates).

Selecting BOM Templates from the list, for example, will show you where the Bill of Materials templates are stored.

Typical default locations

On a standard installation, some important template-related items are stored in locations similar to the following (the exact version folder will depend on your installation):

  • Document Templates: C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\templates
  • Tutorial templates (used for training examples): C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Tutorial
  • BOM Templates: C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english
  • Sheet Formats (.slddrt): C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\lang\english\sheetformat

The C:\ProgramData folder is hidden by default in Windows, so you may need to enable “Show hidden items” in File Explorer if you want to browse to these locations directly.

Using custom template folders

If any of these items are customized, it is good practice to create a dedicated templates folder rather than editing the out-of-the-box files in the default installation locations. The custom templates folder can be:

  • Local – for a single user or test environment.
  • On a network share – so multiple users on the same site can always access the latest standard templates.
  • Inside a PDM vault – if you use SOLIDWORKS PDM, templates can live in a controlled folder with revision history and permissions.

Point File Locations > Document Templates (and, if applicable, BOM Templates, Sheet Formats, etc.) to these custom folders so that they are used instead of, or in addition to, the defaults.

Use the Add and Delete buttons to add or remove paths for the selected file type. The Move Up and Move Down buttons control the order in which folders appear as tabs in the New SOLIDWORKS Document dialog.

You can also click Edit All to see all file locations in a single table and edit them in bulk. This is especially useful when:

  • Changing from one SOLIDWORKS version to another and updating all versioned paths.
  • Moving templates from local folders to a network or PDM location.
  • Standardising paths across a team after a new deployment.

Although you can use both the built-in SOLIDWORKS folders and your own custom folders at the same time, it is usually best to phase out the default installation folders over time. Once all of your templates live in a single controlled location (network or PDM), any missing items become obvious because they simply will not appear in the template tabs.

Creating or recreating templates

Sometimes the easiest way to solve template problems is to generate fresh templates and then build your company standards on top of them. A common workflow is:

  1. Let SOLIDWORKS recreate clean default templates:
    1. In Windows Explorer, browse to your existing template folder (for example C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx\templates).
    2. Rename the folder (for example to templates_old).
    3. Start SOLIDWORKS and choose File > New. SOLIDWORKS will regenerate a fresh set of default templates in a new templates folder.
  2. Create a new part, assembly or drawing using these clean templates, adjust all required Document Properties, custom properties and sheet formats, then save them as new .prtdot, .asmdot and .drwdot files into your custom template folder.
  3. Point File Locations and Default Templates to these new, company-standard files.

This approach gives you templates that match the current SOLIDWORKS version and removes old settings that may have accumulated over many years of upgrades.

Template update schedule

In many companies, templates are created once and then carried forward for many years by simply saving them in each new version of SOLIDWORKS. While this usually works, it can gradually introduce performance issues or inconsistent behaviour as new features and options are added to the software.

Resellers and SOLIDWORKS-focused consultants commonly recommend creating brand new templates when you move to a major new release of SOLIDWORKS, then reapplying your drafting standards and title blocks. This ensures that the templates contain the latest internal settings and document properties expected by that version.

To make this manageable, consider a staggered refresh schedule rather than trying to rebuild everything at once. For example:

  • Year 1 – recreate and verify all part and assembly templates.
  • Year 2 – recreate and verify all drawing templates and sheet formats.
  • Year 3 – review other template-driven items such as BOM templates, revision tables and weldment templates.

Whichever schedule you choose, the key points are:

  • Keep your templates in a single, well-documented location (ideally under PDM or regular backup).
  • After each major SOLIDWORKS upgrade, plan time to verify that the correct folders are set in File Locations and Default Templates.
  • Retire very old templates so that users always start from clean, consistent standards.

With a little discipline around where your templates are stored and how they are updated, you can avoid many common “missing template” errors and keep SOLIDWORKS performing reliably from one version to the next.

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