Have you ever been working in SOLIDWORKS software and thought to yourself: “Why do I have to change my units from millimeters to inches every single time I start a new part document?” Have you ever wondered why you have to keep changing the precision of your units from two (x.xx) places to three (x.xxx) places? Have you ever been working in a drawing and wanted to set the driven dimensions to exclude the parentheses every time?
If you answered yes to one or more of these questions, I encourage you to continue reading for an overview of how to configure, use and re-use templates in the software.
Figure 1. Sample of templates that use different units of measurement.
Out-of-the-Box Templates
When first installing the software, you will be presented with a choice of three templates, Part, Assembly or Drawing, as shown in Figure 2.
Figure 2. The three default out-of-the-box templates.
These three templates provide you with out-of-the-box settings. To get the most out of the software and accelerate the completion of your projects, you can create and save customized templates containing your desired custom settings.
What is a Template?
A Template is a special file type that helps users begin a project with the desired settings. Let’s take a quick look at a screen shot of a Windows Explorer folder containing customized SOLIDWORKS 2016 templates (Figure 3).
Figure 3. Windows Explorer folder showing template files.
As you can see in Figure 3, a template has been created for both inches (INCH) and millimeters (MM) for each of the three file types (Part, Assembly and Drawing). By setting up our templates in inches and millimeters we can save a lot of time. Depending which units the current project is in, we can select the appropriate template and save ourselves having to change the option for units. Similarly, we might want our inches projects to use three-place precision (x.xxx) while our millimeter projects could use two-place precision (x.xx). This setting may also be saved into our templates.
You may also notice in Figure 3 that the file type is different from a standard document. A SOLIDWORKS part document is an .sldprt file and a part template is a .prtdot file. Similarly, Assembly and Drawing templates use special extensions. Let’s take a look at how to create, save and re-use a part template.
How to Create and Save a Part Template
Let’s start by clicking the icon for a New document (Figure 4).
Figure 4. Click the document icon to create a new document.
After clicking this button you may switch between the Novice and Advanced template selection window. Click this button until it says Advanced, which indicates that you are looking at the Novice screen, and then double click the default Part template (Figure 5).
Figure 5. Toggle the Advanced/Novice button and then double click the default Part template to begin a new part.
Customizing the Settings for a Template
There are four main items that may be configured and saved into a new part template:
- Names of planes and origin
- Custom file properties
- Hide/show state of Origins, Planes, Sketches, etc.
- Document settings and options
You can also create new geometry to use in your template. For example, you could create a block with four counterbores in the corners to use as a common fixturing plate. This could then be saved as a template so that whenever you begin a new part and select this template, the geometry is already created. (This is a bit on the advanced side of things, though.)
For today’s article, we’ll focus on the four main items you can configure and save into a template.
Names of Planes and Origin
The names of the three default planes and the origin may be changed. These changes will be saved with the new template. Let’s change the default plane names to XY PLANE, ZX PLANE and YZ PLANE. We will also change the name of the origin to ORIGIN – 0,0,0 (Figure 6).
Figure 6. You may change the names of the default planes and the origin. These changes will be saved with your template.
Although this is an option, I typically stick to the default names of the planes: Front Plane, Top Plane and Right Plane.
We’ll next take a look at Custom File Properties.
Custom File Properties
Custom File Properties are fields of data that can be saved into the file header as “metadata.” This means that the data can be read by other files, without needing to open the actual part file. An example of this would be a PDM system reading the metadata for Revision, or a drawing file reading the metadata for Description to be used in the drawing title block or the bill of materials.
The custom file property fields are often the same from one part file to the next, so they may be set up ahead of time by saving them into a template. Some examples of the most common custom file properties fields are:
- Part Number
- Description
- Manufacture
- Cost
- Revision
We’ll add these custom file properties to the part template we are creating. First, click on the icon for File Properties (Figure 7).
Figure 7. Click on the icon for File Properties in the menu bar.
Next, click on the tab for Custom properties (Figure 8).
Figure 8. Click on the tab for Custom properties.
Now in the Property Name column, we may either type in the new property names or we may choose the desired name from the drop-down menu (Figures 9 and 10).
Figure 9. You can manually type a name into the Property Name box.
Figure 10. You may also use the drop-down menu to select a property name.
For our template we will add the custom properties shown in the list above. We will set the Type column to Text for each of these fields. We will leave the Value/Text Expression column blank. (Figure 11.)
Figure 11. Create each of these five custom property fields.
Click OK at the bottom of the dialog box.
By creating these custom properties and saving them into the template, you save yourself the time needed to create them each time you make a new part. You will also ensure consistency across all of your part files, as you will avoid accidently setting one part file to use the custom property field for Part NO and another to use the custom property field for Part Number. Since the correct filed name is Part Number, and this field will be saved into your template, it will be the same for every new part file you create.
Hide/Show State of Origins, Planes, Sketches, Etc.
Whenever working on a part document, you may set the option to hide or show all planes. You may also set the option to hide or show all sketches, and hide or show all origins. This option is available from the “Heads Up” toolbar, and the settings will be saved with the template. We will set our options to show all Planes, Axes, Origins, Curves, Sketch Dimensions (SOLIDWORKS 2016 and newer), Sketch Relations and Sketches.
Figure 12. From the “Heads Up” toolbar, set these items to show.
After we have set these items to show, click in the background. These settings will be saved with the template.
Document Settings and Options
The final section we will cover is the most important: document settings and options. At the top of the main interface, click the icon for Options (Figure 13).
Figure 13. Click on the icon for Options.
Once you enter the section for Options, you will see that there are two tabs, System Options and Document Properties. The options under the tab for System Options will affect the entire setup. The options under the tab for Document Properties will affect the current document.
The options under the tab for Document Properties will be saved with the document template, so we will focus on this tab (Figure 14).
Figure 14. The Document Properties tab contains options that will be saved with the template.
We’ll start by changing the units for our template. We click on the options for units and set the unit standard to IPS (Figure 15).
Figure 15. Set the units for your template to IPS.
Next, we’ll set the precision of our dimensions to use a three-place precision by clicking on Dimensions and setting the Primary precision to .123 (Figure 16).
Figure 16. Set the precision for dimensions to three places.
Lastly, we’ll set the option for image quality. This option will help the display of curved features to appear more round and less tessellated. I like to set the slider bar to a little beyond halfway (Figure 17). Setting it too far to the right will increase the file size, so you have to find a good balance.
Figure 17. Set the image quality slider to a little beyond halfway.
We have set the three most commonly adjusted options, and will now click the OK button to exit the options page.
Keep in mind that any options that are stored on the Document Properties tab will be saved with your template, so feel free to examine any other options and set them to be saved with your template.
Saving and Using Your New Template
Now that we have adjusted all the options for our template, we need to save our template as a template file. We then need to tell the software where to look for this template, so that we may use it over and over again.
Let’s start by saving our template.
I like to create a dedicated folder for my customized templates. This folder should be easy to browse, and you should be able to quickly copy the entire folder to be used as a backup to share with your co-workers or to be used on a new computer. We’ll create a folder called C:\SOLIDWORKS 2016 TEMPLATES (Figure 18).
Figure 18. Create a new folder for your templates.
This will be the new default location for all of our templates.
Next, in SOLIDWORKS, we will choose File→Save as.
We will choose the file type Part Templates (Figure 19):
Figure 19. First, choose the Save as type for Part Templates.
Then browse to the C:\SOLIDWORKS 2016 TEMPLATES location and give the new template a file name. Here we are using the name PART-INCH (Figure 20). Click on the Save button to save your template.
Figure 20. Give your template a name.
You have now created and saved a part template. The final step is to tell the software where to look for this template, so that you may use and re-use it.
Configuring the Options to See Custom Templates
Within the system option there is a section called File Locations. In this section we can point to libraries of files. One of the most commonly used libraries is the library of templates. We’ll go into the Options feature and point to our new directory containing our new part template.
Start by clicking the Options button at the top of the screen (Figure 21).
Figure 21. Click on the Options icon in the menu bar.
Within System Options, click on the tab for System Options and choose the section for File Locations (Figure 22). Notice that the section on the right is currently showing folders for Document Templates, which is the library we wish to configure.
Figure 22. Click the System Options tab and then click File Locations.
Next, click Add to add a location for the software to look for your custom templates. Add the location we created (C:\SOLIDWORKS 2016 TEMPLATES) and then click OK (Figure 23).
Figure 23. Add a location for and browse to the location where you saved your template. This location should now appear in the list.
Click the OK button at the bottom of System Options and you will be prompted to “make the following changes to your search paths.” Select No when this dialog box appears (Figure 24).
Figure 24. Select No when this dialog box appears.
Using and Re-Using Your Custom Template
Congratulations! You have now created and saved a customized template, and you have pointed the software to the location of this template. Now we’ll see if it all worked.
Click the New icon on the menu bar (Figure 25).
Figure 25. Click the New icon on the menu bar.
Toggle the button in the lower left between Advanced and Novice until the button says Novice. You should now see a new tab called SOLIDWORKS 2016 TEMPLATES (Figure 26). This tab represents the file location you pointed the software to look at when browsing for a library of document templates.
Figure 26. You should now have a tab representing your new folder.
Double click the PART-INCH template to begin your new part document and examine the results.
- Does the tree show your newly named planes and origin?
- Do the custom file properties reflect the Part Number, Description, Manufacture, Cost and Revision fields we added?
- Do the options reflect the correct units and precision?
If so, then congratulations! You have successfully created, saved and re-used a new part template in SOLIDWORKS.
Conclusion
The process of creating a new document template in SOLIDWORKS always follows the same process. First you create a new document and configure the options and settings as desired. Next you perform a Save as command, and save the document as a template. Lastly, you tell the software where to look for this template so that it will appear whenever you choose the New command.
Now that you know how to create a template for a Part document, you may repeat these steps to create a template for Assembly and a Drawing. You could also create different templates representing different units and precision, or to be used for different customers or projects.
About the Author
Tobias Richard is a SOLIDWORKS Elite Applications Engineer from Philadelphia. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.