SolidWorks – Custom templates

Custum SolidWorks templates are very handy. You always have one layout for your drawing which matches the style of your company. But how do you create your own custom templates? What is possible? What do you need?

First of all, you need a nice basic template. For this tutorial I’ve used the standard/default templates that are used by a fresh SolidWorks installation.

You’ll have to change three templates.

• Part – *.prtdot
• Assembly – *.asmdot
• Drawing – *.drwdot

You can find the SolidWorks template files in:

C:\Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks 2008\templates

Copy the default templates (just for a backup) to a new folder and let’s get started with your own templates!

Part template

When you open the part.prtdot file in SolidWorks you see an empty file.

Go to file -> Properties

And a popup window appears. Choose the custom tab.

You can pick one of the variables in the ‘Value / Test Expression’ column, put static text into the boxes or pick one of the variables in the list below to add automatically the info to your title block in the lower right corner.

• $PRP:”SW-Author”
  I’ve fount this one on the internet but it doesn’t work – yet!?
  I’ve used a manual Author
• $PRP:”SW-Comments”
• $PRP:”SW-Created Date”
• $PRP:”SW-File Name”
• $PRP:”SW-Folder Name”
• $PRP:”SW-Keywords”
• $PRP:”SW-Last Saved By”
• $PRP:”SW-Last Saved Date”
• $PRP:”SW-Short Date”
• $PRP:”SW-Subject”
• $PRP:”SW-Title”

After I’m finished I’ve got this result:

Note!
You can change the order of the properties by clicking on the number and drag it to the preferred position.

Change all the preferences to the part. For example: show the origin and the standard planes.

Click on the ‘OK’ button and close the part after you’ve saved it.

Assembly template

Do the same for the Assembly template. Open the file ‘assem.asmdot’ and change all the properties to your preferences. My result:

Set all your preferences and click on the ‘OK’ button. Close the assembly after you’ve saved it.

Now we only have to create a drawing template!

Designing a title block

First you’ve got to think about the layout of your drawing layout and title block. Make several sketches on paper. Notice all the default variables you’ve added to the properties in the part and assembly templates. All of this information has to be in the title block, but there is more important information that you has to show.

• Projection type
• Sheet scale
• Standards
• Tolerances
• Material
• Quantity
• Etcetera…

I’ve translated my final sketch to a design in Adobe Illustrator. You can also start drawing in the Drawing template.

Export the layout to a *.dwg file. For example:

Open the file with the SolidWorks DWGeditor or AutoCAD. Let’s see what the end result is. Images are not exported to the dwg file.

Ajust the titleblock to your own preferences.

Move the block to the origin of the file. Type ‘move’ in the command line and select the entities. Hit enter and click on the bottom left corner of the rectangle.  Type ‘0,0′ to specifie the base point and the block is moved to the origin of the drawing.

Save the file and exit the program.

Drawing template

Open the drawing template from your templates folder and the default templates is shown. Rightclick on ‘Sheet1′ in the feature tree and select ‘Edit sheet format’

Delete the existing title block.

Insert a a block.

Adjust the scale

Add some images to add more style to the titleblock and than we go adding the variables to the titleblock.

Add notes to all the fields where you’d prefer the information. Insert a variable to the note. Use the following Syntax:

$PRPSHEET:”propertiename“

Note that you enter the property name between “” and not the {}. This syntax will be recognized as a variable and will be converted to a syntax with accolades.

Good

Wrong

You can also add some variables which refers to the sheet.

• $PRP:”SW-Current Sheet”
• $PRP:”SW-Sheet Format Size”
• $PRP:”SW-Sheet Name”
• $PRP:”SW-Sheet Scale”
• $PRP:”SW-Template Size”
• $PRP:”SW-Total Sheets”

This is my result:

Go back to ‘Edit Sheet’

You’ll notice that none of the variables are displayed in the title block. Great!

Go to Sheet1 and properties to change the sheet format and choose another paper format. Style all the paper formats you use in your company. I’ll choose A4, A3 and A0.

Save all the templates under a different file name. This is easier to use.

Now save the drawing template and let’s start making a drawing!

Don’t you love the result? Read more about making a drawing in 1. Solidworks basics

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