Setting up Your SOLIDWORKS Template for Drawings

In my previous article, I wrote about how you could set up your model template in SOLIDWORKS.

Building on that, in this article I will go over some of the points on how you set up your drawing template as well as your sheet format.

But before I get too technical, I want to explain the difference between template and sheet format.

The template is everything that is not related to the title block, font type, unit, projection type, document properties etc.

Which is why I usually recommend that you only have one “person” (template) and multiple sets of clothes (sheet format: A1, A2 etc.), although it is possible to have a template with a sheet format attached.

With that, we can start with the basic setup rules for the template and then move on to the sheet format.

It’s What’s Inside That Counts

As with the part template, we start looking at the document properties and then we will also look at the custom properties. Yes, that is also a thing in drawings.

Document Properties

The Document Properties are the backbone of the template.

As with the model template, the Document Properties can be divided into two separate entities:
Drafting standards and Non-Drafting standards.

The drafting standards control the document’s fulfillment of the standardization requirements, which are given to define how your drawings are presented and interpreted. It is possible to deviate from these standards, but using them will ensure that your drawings will pass quality control.

As you will notice the drafting standard list is a bit more extensive than model properties.

As with the model properties, there are a number of predefined standards that you can use as a starting point.

If you change anything, the name of the standard is changed to “<Standard name>_MODIFIED” and it can be saved and used in other drawing if you want to.

After looking at the drafting standard, let’s focus on the non-drafting standard Items: the “units.” This is for the dimensions in the drawing, but it also captures the units (such as for weight in pounds) from your model as the system automatically translates from the model to the drawing.

This means that even if your model is set to pounds and your drawing is set to grams, the units used will be grams.

Also consider the “performance” selection. You will have the option to turn off the save model data for detailing mode.

Detailing mode was introduced in SOLIDWORKS 2020. It is a great way to open large drawings quickly. However, using it increases the file size, so you want may want to only use this mode only for larger drawings that can take too much time to load.

One thing I need to point out is that it is not possible to change a template once the drawing has been created. You can change the drafting standard and the sheet format but all non- drafting standard settings have to be changed manually.

Custom Properties

As with Model templates, you have an option to set up different custom properties, the main difference is that you are not able to use configuration-specific properties on drawings, only custom properties.

As a rule of thumb, I do not use custom properties on drawings. Instead, I prefer to have information in the model represented in the drawing.

It is possible to use predefined views in your template which will be populated with the model you insert in the drawing. Doing this can save you time when you are creating drawings.

Once your template is ready, press File > Save as > and select the .drwdot format, which is the drawing template format.

If you are using SOLIDWORKS connected, use the File > Save template. This will bring out a menu for the 3DEXPERIENCE platform.

I will go into setting up your SOLIDWORKS resource files in a future article.

Sheet Format

As I mentioned, Sheet Format is what you see when you open the drawing.

The format size, the title block which can contain information from the model, is all part of the sheet format.

Setting up your sheet format is not rocket science, and with a little bit of patience you can do it quickly and get started on what you really want to do: model in SOLIDWORKS.

If we start from the beginning, you first need to look at the size of the sheet. This is done by right-clicking on the Sheet Format on the left side of the screen and selecting Properties.

In here you can select some of the standard sizes or define your own.

Once you have found the correct size, it is time to start building your title block.

Before you begin, start off by doing a sketch (by hand) to see what information you want on the title block and the general layout of it.

Once that is done, we are ready to do the title block.

On the empty drawing (with the proper size set), press the Sheet Format tab and press “Edit Sheet Format.”

Now two more buttons have become active. We are going to look at the Automatic Border.

This command helps you ensure that you get a symmetric border for your drawing and gives you the option to create zones in your drawing, which can be helpful on larger and complicated drawings and you can also use them for reference later.

After pressing the button, you get the option to delete the lines you don’t want on the drawing. Since our drawing is empty, I just press Next.

First, I need to decide the number of zones and how they should be distributed.

In this A3 example, I just want them to be evenly spaced.

When selecting the margins, you can stick to the standard: 10 mm for right, top and bottom, and 20 mm for the left side. Having 20 mm for the left side is to account for the perforations in the paper.

Afterwards you can decide if you want to see the zone dividers or not.

You might just want to hide some of them for some reason. If so, you press Next and use the “Add Margin mask” command. There you can add and modify a mask that ensures that the zone dividers do not appear.

With the drawing border done, we are ready to move on to the title block itself.

On the title block, we want to grab information from the custom properties on the model that we set up in my previous template article.

To do this we start by filling out the information on a model and then inserting it in the drawing.

Next ensure that Edit Sheet Format is active. Insert an annotation note.

After this you have two options on how to proceed. The easy way is to choose the “Link to Property” icon.

Next, select “Model Found Here” and select the property you want to use. Then press OK and insert a new annotation box, and repeat for all your custom properties.

One thing you should note: The link will always try to read the configuration of the model instead of the custom property.

If you have a custom property and a configuration property with the same name, the value in the custom property will be ignored until the line is deleted in the configuration property.

The Nerdy Way

This method gives you full control of the value inserted.

Insert the annotation and press OK then right-click on the annotation and press “Edit Text in Window.”

This will open a window where you can refer to the properties. You can write to different commands to refer to it: “$PRP” and “$PRPSHEET,” where $PRP refers to properties within the Drawing document and “$PRPSHEET” will refer to the model properties.

If you want to get the property “Description” from the model, you should write “$PRPSHEET:”Description”.

The two methods can be combined. For example, if you have inserted the property “weight” using the easy way (no units), you can add the unit afterwards, by right clicking and pressing edit in the new window and adding “gram,” for example.

Once the property has been inserted and you have ensured that the textboxes are placed in the proper location, it is time to save the file. Press “Save” and “Save Sheet format.”

But what if Save Sheet format is not available?

That is because it was changed in SOLIDWORKS 2024, which means that you have to use the “Save As New” option.

Once the *.slddrt is selected, SOLIDWORKS will automatically select the sheet format location.

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