How to make new templates?

[Dwight]

We are upgrading from 2018 to 2022. I have read here that it may be a good idea to modify new templates, rather than updating old templates, so I am trying that out. So where are those new templates?

I see a selection for part and assembly templates in ProgramData/SOLIDWORKS/SOLIDWORKS 2022/templates. What is the size choice about? Should I pick a scale close to what we usually work in?

I find drawing templates in an entirely different place - Program Files/SOLIDWORKS Corp/SOLIDWORKS/data/templates. I guess I pick our drafting standard.

Any insights into this process are welcome.

Dwight

[JSculley]

From the Knowledge Base:
========================================================
Solution Id:S-053149

Product:SolidWorks 2011 Beta

Created:12/10/2010

Technically Reviewed Date:5/9/2011

Area:

Sub-Area:

Question:After installing SolidWorks 2011, why is the default templates folder empty?

Answer:The templates are generated in this folder the first time a new file is created in SolidWorks 2011. However, if the Templates File Location setting includes paths to other template folders, SolidWorks will use those other templates instead of generating the new default templates in the new folder.

To generate the templates in this case, remove all other Template file location paths, keeping only the 2011 templates folder in the list. Create a new SolidWorks file, and see all of the templates get created in the folder.

==================

[Dwight]

I only saw my old templates when creating a new part. I'm asking what is the 2022 templates folder, or folders. Are they what I show in my original post? And which ones to use? And is that "need to use new templates" thing a real thing?

Thanks

[zwei]

And is that "need to use new templates" thing a real thing?

Thanks

Personally, i dont see a need of creating new template with each version // updating template to latest version.

We had been running different SW version, SW2016~2021, using the same template in SW2016 and so far i do not notice any issue that requires updating the template version

It might be a different story if your template is too "old" since solidworks experienced some fundamental change in the file format if i remember correctly. (I cant remember the exact timeline though)

[Glenn Schroeder]

Dwight,

First of all, while my templates are edited occasionally, they haven't been started from scratch since 2009. I know some people have reported problems with old templates, but I haven't seen it. My tentative advice would be "If it ain't broke, don't fix it."

However, if you want to make new ones any way, I'll try to help. Please keep in mind that I've never done this, so I'm not 100% sure it's correct.

What templates do you show when you go to Tools > Options > System Options > Default Templates? If it's still the Solidworks default templates, then when you want to start a new document, and you only have your custom templates to choose from, click on the "Novice" button in the lower left corner of the New Document dialog box. That will take you to a different dialog box where you only have one option for each file type. If you haven't changed the defaults at the location I mentioned above then it will be the templates that are loaded with SW. You can open new documents with these templates, make your changes to each, and save as new templates at the location you have selected at Tools > Options > System Options > File Locations > Templates.

Again, I think this is correct. If someone else chimes in and says it's all wrong, please disregard the above.

[JSculley]

And is that "need to use new templates" thing a real thing?

Here is what SOLIDWORKS has to say:

====================================
Solution Id: S-071805
Product: SOLIDWORKS Professional 2016
Created: 8/18/2016
Technically Reviewed Date: 9/2/2020
Area: Save/Open
Sub-Area:

Question: In the SOLIDWORKS® CAD software, how do I determine if I am using an old template?

Answer: Making sure that you use the correct template version for your version of the SOLIDWORKS® software is fundamental in avoiding unexpected behavior in the Sheet Metal, BOM, Cut List and other environments.

There is no tool available in the user interface to check the template version. One way that you can do this is as follows:

1. Create a new part or assembly.
2. Select the 'Top Plane' in the FeatureManager®.
3. Right-click and select 'Properties'.

The ‘Date created’ field provides information about the creation date. If the template is very old, consider replacing it with a new template from scratch.

SolidWorks Development staff from time to time redesigns entire areas of SolidWorks software for better performance and stability. SolidWorks will always use the code which features were created in to ensure data parity - to take advantage of the latest and best code SolidWorks Development has to offer, it is recommended to create new templates instead of migrating existing templates to the latest version if you are encountering any faults after a migration to a new version.
Additionally, the old templates which possibly exhibit poor function should be provided to your local VAR (Value added reseller) for submission to SolidWorks for review.
===========================================

And I have personally seen several problems over the years directly attributable to old templates.

When you install SW, it doesn't 'install' new templates anywhere. You have to remove all folders listed in 'Document Templates' under 'File Locations' in the System Options and then create a new Part (File...New Part). Then SW will generate part, assembly and drawing templates.

[Glenn Schroeder]

. . . it is recommended to create new templates instead of migrating existing templates to the latest version if you are encountering any faults after a migration to a new version.
Additionally, the old templates which possibly exhibit poor function should be provided to your local VAR (Value added reseller) for submission to SolidWorks for review.
===========================================

And I have personally seen several problems over the years directly attributable to old templates.

When you install SW, it doesn't 'install' new templates anywhere. You have to remove all folders listed in 'Document Templates' under 'File Locations' in the System Options and then create a new Part (File...New Part). Then SW will generate part, assembly and drawing templates.

There you go. I will stand by my recommendation above to not go through the hassle of making new templates if you aren't having problems with the old ones.

[jcapriotti]

Open the template and go to "File / Properties.... On the "Summary" tab there is a "Last Saved With" entry.

In general we have few issues with old templates but it has occurred. Mostly with some of our Sheet metal templates that have start geometry for common shape parts (L- bracket, U-bracket, etc.). One of the versions add multi-body support for sheet metal and legacy parts were left as is so we recreated the templates for those so they had the 'new' way of handling it.

[Dwight]

And I have personally seen several problems over the years directly attributable to old templates.

When you install SW, it doesn't 'install' new templates anywhere. You have to remove all folders listed in 'Document Templates' under 'File Locations' in the System Options and then create a new Part (File...New Part). Then SW will generate part, assembly and drawing templates.

I figure that some problems may not be obvious and are suffered in ignorance for years. I've been copying old templates every upgrade since 2006, so I think this time I will make them from scratch.

I suppose that what I found in the folders (as described in my original post) are not necessarily fresh for 2022. I will try forcing SW to generate the templates, as you describe.

EDIT: JSculley - that worked great! Easy peezy. And the date test you describe works quite nicely.

Thanks

Dwight

[Dwight]

Open the template and go to "File / Properties.... On the "Summary" tab there is a "Last Saved With" entry.

image.png


In general we have few issues with old templates but it has occurred. Mostly with some of our Sheet metal templates that have start geometry for common shape parts (L- bracket, U-bracket, etc.). One of the versions add multi-body support for sheet metal and legacy parts were left as is so we recreated the templates for those so they had the 'new' way of handling it.

The Summary tab shows what the last save was, not the original file creation date, which is the "issue" here.

Dwight

[AlexLachance]

If you are updating from one version to another and already have your templates created, the simplest method to create your new templates is to use the one that are created inside your program's folder, which I will provide possible links to later. These templates are supposed to be fresh templates from the version you are running, so you can take these, wipe them clean and then copy and paste all from your old template into this new one. Proceed to save them. A good practice that I've started using to ensure that I don't forget to update them, is to have the year in the name of the template. So for instance, Drawing(2019).slddrt would be a drawing template made for SolidWorks 2019.

Possible locations of default templates:

C:\ProgramData\SOLIDWORKS\SOLIDWORKS version \templates
C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Tutorial

Cheers!