CAD Forum

Distinguishing between these two file types often confuses new users, and sometimes experienced ones. I know it took me a while to get straight. What it boils down to is this:

A drawing template is a blank drawing document (.drwdot) that is used to start a new Solidworks Drawing (.slddrw). You can have several, for different situations, clients, etc. It can, and usually does, contain a sheet format.

A sheet format (.slddrt) is the layout of a drawing sheet, and controls the title block (or at least it should), sheet orientation (landscape or portrait), border lines, and table anchor points.

Now I'll elaborate on them.

As I said above, sheet formats contain the title block and its notes, along with a few other things. To edit a sheet format, right-click on a blank part of the drawing sheet or the sheet name in the tree and choose "Edit Sheet Format" from the drop-down.

When you finish your edits exit the sheet format function. If this is a one-time edit that's all you need to do. If you want to save this for future use then go to File > Save sheet format... Save it at the location you're pointing to at Tools > Options > System Options > File Locations > Sheet formats. I'd suggest not saving them in the default location, but somewhere away from the Solidworks installation folders so they won't get lost when you upgrade to a new version of the software.

If you've made this edit on a multiple sheet drawing, only the active sheet will reflect the change. You can go to Sheet Properties and select the Reload button for the other sheets to update them. This doesn't always work, so if it doesn't update right away try a Ctrl+Q rebuild. If it still doesn't work, go back to Sheet Properties, select a different sheet format, select "Apply Changes", then repeat the process but select the original format. That should bring in the updated version.

Speaking of editing the sheet format, this isn't something you should be doing often. It's best to have any variable notes in the title block like project name/number, date, etc linked to custom properties. If you don't know how to do this yet feel free to ask below in a Reply and I'll be happy to explain. I go months without ever editing my sheet formats.

You can have multiple sheet formats saved for different situations. To access your sheet formats go to the same drop-down shown above, but choose "Properties" instead. That will bring up the table shown below.

Here you can select a different sheet format or reload the current sheet format, along with a few other options.

Now for more on drawing templates. When you get a drawing set up the way you want it, with the desired sheet format and settings at Tools > Options > Document Properties, but without any drawing views, do a "Save as" and select Drawing Template from the file type drop-down. Again, save it at a location other than the default so you won't lose it when you upgrade to a new version of the software. If you're in an organization with multiple users it would be a good idea to save these files on a server so the other users will be able to access them, and to keep the drawings from your organization uniform.

As I said above, a drawing template will usually contain a sheet format, but if you don't want it to then open a new Drawing, right-click on the sheet format in the tree, and select "Delete" from the drop-down. Save this Drawing Template with the method explained above. After doing this, when starting a new Drawing using this template you'll be prompted to choose a sheet format.

Now for the part that gets a lot of people. When a Drawing template is saved, whatever sheet format it contains at the time is how it's saved. Drawing templates don't maintain a link to the sheet format, so if you've edited a sheet format and saved it, and then open a new Drawing using this sheet format, the changes you made won't be in this new document. You'll need to Reload the sheet format (see Sheet Properties screenshot above). After doing that be sure to save your Drawing template so you won't need to reload the sheet format in the future.

The same is true for existing Drawing documents. If you open an old Drawing that contains a sheet format that's been edited you'll need to Reload the sheet format to update it.

I'm going to stop here for now. This is a complex subject, so I'll revisit this from time, and edit as needed, or when something else occurs to me. Please feel free to ask if you have any questions about any of it. I'll be glad to help.

I think this is exactly the kind of content we need to create to move forward in the google search ranking. Congrats, Glenn. Love it.

A note on drawing templates:

If you have "Show Sketches" turned off in your default drawing template, sketches for engraving (edit: etching) won't show up when you export sheet metal DXFs because (if I understand it correctly) when you export a DXF it actually opens a drawing using your default template creates a drawing view of it and exports it.

Thank you Glenn. For some reason this type of write up seams more "human friendly" than the help pages sometimes. I think you can present it from the perspective of "what do I do with this as the user?" so it flows nicley.

If I may ask here, if not I'll start another thread, what are the experiences of saving templates and sheet formats (tables too) in the vault vs network share if the users have PDM? We have ours in PDM, here's a few of my observations maybe you can correct or confirm them:
+ PDM can update local cache of the "Templates" folder when the user logs in, based on user/group settings.
+ version control is wonderful
+ both windows shares and PDM have file permissions, but I like them better in PDM for this.
- if for whatever reason the templates are not in local cache when needed Solidworks appears to default back to the installation path in the Setting->File Locations.

bnemec wrote: ↑Thu Apr 08, 2021 5:48 pm Thank you Glenn. For some reason this type of write up seams more "human friendly" than the help pages sometimes. I think you can present it from the perspective of "what do I do with this as the user?" so it flows nicley.

If I may ask here, if not I'll start another thread, what are the experiences of saving templates and sheet formats (tables too) in the vault vs network share if the users have PDM? We have ours in PDM, here's a few of my observations maybe you can correct or confirm them:
+ PDM can update local cache of the "Templates" folder when the user logs in, based on user/group settings.
+ version control is wonderful
+ both windows shares and PDM have file permissions, but I like them better in PDM for this.
- if for whatever reason the templates are not in local cache when needed Solidworks appears to default back to the installation path in the Setting->File Locations.

I'm glad you liked it.

I'm afraid my experience with PDM is exactly zero, so I can't address any of those points. Feel free to do so if you want, or I can put a comment in the text above referencing your points.

bnemec wrote: ↑Thu Apr 08, 2021 5:48 pm - if for whatever reason the templates are not in local cache when needed Solidworks appears to default back to the installation path in the Setting->File Locations.

Yep, this one bites me in the a$$ every once in a while. Not me personally but the end users, they clear their cache which clears all SolidWorks configuration files we store in the vault. We need an option to prevent clearing certain files.....like a permanent cache that always maintains the latest versions, in real-time....or near to it.

jcapriotti wrote: ↑Thu Apr 08, 2021 6:03 pm

bnemec wrote: ↑Thu Apr 08, 2021 5:48 pm - if for whatever reason the templates are not in local cache when needed Solidworks appears to default back to the installation path in the Setting->File Locations.

Yep, this one bites me in the a$$ every once in a while. Not me personally but the end users, they clear their cache which clears all SolidWorks configuration files we store in the vault. We need an option to prevent clearing certain files.....like a permanent cache that always maintains the latest versions, in real-time....or near to it.

I kinda thought we were just doing it wrong. But it's not enough of a pain that you want to put them on a network share I assume.

bnemec wrote: ↑Thu Apr 08, 2021 6:15 pm I kinda thought we were just doing it wrong. But it's not enough of a pain that you want to put them on a network share I assume.

I think a network share is fine and maybe even preferred if all users are local to the server. We have users spread across 4-5 locations and on VPN at home(lately). The network latency can slow down SolidWorks user not close to the server for certain functions that need to read those file locations (templates, gauge tables, etc.). So we moved to storing all configuration files in PDM and caching the folder.

One thing that had been bugging me recently is the sheet format file location...
If we change a sheet format location, is there a quicker workaround instead of remapping the file path in the template one by one?
Also what is the [Sheet Format] under the file location setting do?

@Zhen-Wei Tee I think you answered your own question. That Sheet Format path in your second pic defines what should show up in the Sheet Format properties dialogue in your first pic.

Zhen-Wei Tee wrote: ↑Thu Apr 08, 2021 7:18 pm One thing that had been bugging me recently is the sheet format file location...
If we change a sheet format location, is there a quicker workaround instead of remapping the file path in the template one by one?

image.png

Also what is the [Sheet Format] under the file location setting do?

image.png

I don't know if it helps but I posted a macro to swap sheet formats at viewtopic.php?f=33&t=74
Just edit the location of your new sheet format in the macro.

Oh, also you can use a loop to cycle through all the files in a folder to fix all the drawings in that folder.

Zhen-Wei Tee wrote: ↑Thu Apr 08, 2021 7:18 pm One thing that had been bugging me recently is the sheet format file location...
If we change a sheet format location, is there a quicker workaround instead of remapping the file path in the template one by one?

image.png

Also what is the [Sheet Format] under the file location setting do?

image.png

I'm afraid I didn't understand your first question, but I can definitely help with the second one. The sheet format file location determines which sheet formats will be visible to easily select from when you go to sheet properties. As you can see, there's a Browse button in that dialog box that allows you to find a sheet format that doesn't show in the list, but having the location of your custom formats at Tools > Options > System Options > File Locations > Sheet Formats eliminates the need to Browse to them.

If you'll look at the screenshot I posted above of what I see when I go to sheet properties you'll only see my custom sheet formats, and none of the defaults. That's because I deleted the default location from my file locations and added my own folder.

Thanks Glenn, to be honest, this had me confused me in the past also - thx for the very useful info and post!

Thanks Glenn for a very helpful post.

Is there some reason why these two files cannot be combined by Solidworks into one file? Seems like it would save on clutter and steps.

Uncle_Hairball wrote: ↑Mon Apr 12, 2021 12:39 pm Thanks Glenn for a very helpful post.

Is there some reason why these two files cannot be combined by Solidworks into one file? Seems like it would save on clutter and steps.

Yeah, sometimes people use multiple formats in single template. For example, multipage drawings. A template doesn't have to have a sheet size, but a format does. It makes sense to have them separate.

Great screen name, by the way.

Uncle_Hairball wrote: ↑Mon Apr 12, 2021 12:39 pm Thanks Glenn for a very helpful post.

Is there some reason why these two files cannot be combined by Solidworks into one file? Seems like it would save on clutter and steps.

I don't think that would work. I've had a number of occasions where for one reason or other I have a multi-sheet drawing that uses more than one sheet format. I can also imagine a situation where a user would want to have multiple drawing templates that used the same sheet format.

We have templates A - D sized with sheets 1 and 2. Sheet 1 & 2 are different formats, so for 4 templates there are 8 different formats. Use a funky BOM layout (leftover from acad) so there's the BOM sheet format. There's no BOM template because its added to end of a assembly drawing and never used as a standalone drawing.