Customize Drawing Template and Save Time!

Whenever you open a drawings document in SOLIDWORKS, you must choose a template and a sheet format to begin your drawings. Do you know you can customize drawing templates and sheet format to display all the information you require automatically? You can even add your company’s logo and define units for your measurements. In this article, you will discover how to customize your sheet format in an efficient manner. This will prevent you from wasting time filling in the title block information and avoiding any document inconsistencies.

Custom Drawing Template

First, let’s define the elements you can customize with your drawing templates and the sheet format.

Drawing templates:

• Drafting Standards
• Fonts and Styles
• Line Thicknesses
• Units

Sheet format:

• Sheet Size
• Title Block
• Sheet Borders

Create a customized sheet format

Now, let’s continue with the steps to create your customized sheet format.

Step 1:  Start a new drawing document, and when the sheet format/size window is displayed, uncheck the “Display sheet format” checkbox, select your desired sheet size and press OK, as shown in the image below.

Sheet Format/Size Options

Step 2: A blank new drawing sheet will be displayed. Right-click on the page to display the pop-up menu and select the edit sheet format option. Now we can proceed with making our title block and sheet border.

Edit Sheet Format option

Step 3: Select the sheet format tab on the Command Manager and click on the automatic border command. Now you can create the borders of your sheet and customize different settings such as margins, labels, zones and line widths. Moreover, even though the frame is black, it is not fully defined. So don’t forget to add a fixed relation to the border so that you don’t accidentally shift it in the future!

Automatic border command

Step 4: At this point, we will create our title block area. The title block area is designed as a regular sketch. Therefore, we need to add dimensions and relations to fully define it. After you have added all your desired dimensions, select and hide them from view, so they don’t interfere with the rest of our drawing.

Step 5: The lines from the created title block differ from the border lines. To solve this, we will activate the line format menu. This menu can be accessed by clicking on “View”, then clicking on “Toolbars” and finally clicking on “Line Format”.

There are two options for changing our line thickness. The first is to select all the lines from the title block, then click on the “Line Thickness” command from the “Line format” menu and select the desired line width.

The second option is to create a group of lines, defined in SOLIDWORKS as a layer, and provide specific properties to the layer, such as line thickness, colour, or style. We will click on the “Layer Properties” command from the “Line format” menu to achieve this. Consequently, a new menu will appear where we can create our layer. We will click on “New” and create a new layer titled “Title Block” with the desired layer properties. Finally, we will select the title block lines, pick the “Change Layer” command and choose the recently created “Title Block Layer ” from the drop-down menu.

Step 6:  At this point, we will input the desired information in the block title. To achieve this, we will click on the “Note” command in the “Annotations” tab. With this command, we can add the required information to each block.

To automatically fill a required property to a block, we can click on the “Link to Property” option from the “Note” menu and select the desired property from the drop-down bar. Since it is a linked property, the notes get updates, with changes.

Step 7: Finally, we can enjoy our personalized sheet format by selecting “File” from the toolbar menu and clicking “Save Sheet Format”. Every time you create a new drawing, select the recently saved file, and the exact information you need will be populated to your liking.

I hope these seven steps helped to understand how to customize drawing templates in SOLIDWORKS. To learn more with what you can do in SOLIDWORKS, contact TriMech today!