Fear Not! Custom Properties to the Rescue in SOLIDWORKS

Many users avoid custom properties but lately I have come to see their advantage. This is mostly because I am currently working for a company that uses the PDM software Agile to manage their inventory. My workflow goes like this:

  1. I create a conceptual design of a part or an assembly.
  2. I meet with a couple other mechanical engineers, as well as the project lead.
  3. We review my design. If it gets greenlighted…
  4. I fill out a form and submit it to the engineering change control team.
  5. They send me back an email with the assigned company part number, the description of the part/assembly using the preferred nomenclature and the ECO number.
  6. I do a Save As of my part into the SOLIDWORKS ePDM Vault.

When I do that last step, the fields that come up are the same as the fields in Agile. If I have filled out my custom properties, the dialog box will automatically fill with all the values in my custom properties. If I haven’t filled out my custom properties, I have to manually type everything in and my SOLIDWORKS file does not have the matching custom properties imported.

Luckily, we have an efficient CAD manager who has created a custom properties file for each file type in SOLIDWORKS – one for parts, one for assemblies and one for drawings. If I import the custom properties file and enter the correct information prior to checking into ePDM, then all the fields will automatically fill in. Instead of having to type the same information multiple times, I enter it once in my file’s custom properties and it will carry through the rest of the process, even filling in fields in the title block of my drawing. It feels a bit magical.

You can create custom properties using a text value, a list, a checkbox, or material properties. Once you define the custom properties for each file type, you can save them as an external file. Store the external file on a shared drive and have your users link to that file.

If your company uses Agile or similar PDM software, start by creating a list of all the fields used by the PDM software. Those are the custom properties you want to create.

Custom properties are defined on the Custom Properties tab on the Task panel located on the right side of your screen. You can also create custom properties using the Property Tab Builder available on the Start menu under your SOLIDWORKS release.

If you don’t see the Custom Properties tab on your resource panel, right click on the Task panel and enable Custom Properties.

To create a custom property, click the Create Now button.

A dialog box appears with several controls. Each of these controls can be used to create a custom property.

Drag the desired custom property control from the far-left panel into the Groupbox in the middle panel.

Fill in the definition for the custom property in the right panel.

To create a drop-down list, drag and drop the List control into the Groupbox in the middle panel.

To add values to the list, just click in the Values field. The list starts with about five items but you can add as many items as you like to the list.

A checkbox can be used for a custom property that has a Yes/No definition. For example, if you want to designate whether it is a purchased or fabricated part.

You can even leverage existing properties, such as material or mass, by adding a text custom property and linking the value to the existing SOLIDWORKS property in the list.

Once you are done, simply click the Save button located at the top of the Property Tab builder dialog.

The custom properties will be saved to a properties template.

Next, you need to load the custom properties into your file.

Go to Tools > Options.

Highlight File Locations.

Select Custom Property Files from the drop-down list.

Delete the default SOLIDWORKS folder and add the location where you stored the custom property template you created.

The properties will automatically appear in the Custom Properties tab.

If you go to File Properties and select the Configuration Specific tab, you will see the custom properties that you created.

Once you have set the file location for your custom properties, any time you start a new file the custom properties for that file type will automatically be loaded into that file.

This becomes even more useful when you create a drawing. If you have set up your title block to link to custom properties, the title block will automatically fill in with all the values you have entered.

Let’s say I have designed this aluminum plate. I fill in the custom properties for the plate. Note that the weight of the plate is automatically calculated by SOLIDWORKS based on the plate’s mass and the material designated.

Next, I want to create a drawing for the plate.

This is the revision block in the drawing. These also can be custom properties for my drawing.

When creating the title block, I will add notes and link it to the desired custom property. Then I will save the drawing as a template that will auto-fill in with the values of the custom properties that have been defined.

To link the column values in the revision table to the custom properties, click in the cell to be edited and then type $PRP:”<CUSTOM PROPERTY>”. For example, $PRP:”ECO Description.”  When you press Enter, you will see the value stored in that custom property.

Unfortunately, when you save the revision table, it only stores the column headers, not the data rows, so you can’t create a revision table that links to your custom properties.

If you want to modify the custom properties you have created, you have to open the Property Tab Builder. Go to your Start menu and locate the tool under your SOLIDWORKS installation.

Use the Open tool to open the desired template file and then make the desired changes.

To set up the title block to use custom properties, right click anywhere on your drawing sheet and select Edit Sheet Format.

You can also select the Sheet Format tab and select Edit Sheet Format.

To link a text note to a property, click in the text note and select the Link Property tool on the far left.

Select the desired property from the Property name drop-down list. Notice that all the custom properties are automatically available.

If you want to use one of the properties in the part or assembly shown in the drawing, enable Model found here and select File Properties.

Then select the file property you want to link.

The property name and the current value will be displayed.

If you hover over the text note, you will see the linked property.

If you want to set the order of the text notes in your title block to be filled in, you can use the Title Block Fields tool available on the Sheet Format ribbon. If you have linked all your text notes to custom properties and filled in the values of the custom properties, you will not need to do any typing at all. As soon as you place a view on the sheet, all the fields in the title block will immediately be populated.

To exit Edit Sheet Format mode, right click and select Edit Sheet or toggle the Edit Sheet Format icon on the ribbon.

Save the drawing as a drawing template. Remember to delete any drawing views you placed before saving as a template.

You now have a drawing template set up that will use the custom properties you defined.

To recap the process:

  1. Start with the Property Tab Builder.
  2. Create custom properties for part, assembly and drawing files. Save each template type.
  3. Set the file location under Options for custom properties to the folder where the custom property templates are stored.
  4. Now, when you open or create a file, the custom properties will be added to that file.
  5. When you save the file to ePDM, the fields will be filled in with the values from the custom property fields.
  6. Create a title block with notes that link to the custom properties.
  7. Save the drawing as a template.
  8. Use the template for new drawings.

It sounds like a lot of work, but you can get everything done in less than half a day and it will save you hours in the days ahead. If your company uses a PDM system, it saves even more time. You have nothing to fear and only precious time to save.

About the Author

Elise Moss is a mechanical design engineer, currently working in Silicon Valley. She has been using SOLIDWORKS since 1998 and uses it daily in her current work. She holds a BSME from San Jose State University. She has written articles for Autodesk’s Toplines magazine, AUGI’s PaperSpace, DigitalCAD.com, Tenlinks.com and EngineersRule.com.  She has taught CAD classes at Laney College, DeAnza College, Silicon Valley College and for Autodesk resellers.  Laney College has recently named her as Professor Emeritus. She is currently teaching CAD at Laney College in Oakland.  Autodesk has named her as a Faculty of Distinction for the curriculum she has developed for Autodesk products. She is a Certified Autodesk Instructor as well as a Certified SOLIDWORKS Educator. 

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