# 2021 Equations in Properties

SOLIDWORKS 2021 now includes the ability to use equations in properties. By having equations to use to calculate physical aspects of your designs will greatly enhance communications to downstream stakeholders. It will also enhance the accuracy of the annotations and tables you apply to drawings.

First off we need to know where we can use equations and how to access them. Equations can be used in the following instances:

• Custom Properties
• Configuration Specific Properties
• Weldment Cut List Properties
• Sheet Metal Cut List Properties

Property Equations are available in the Type column in Properties Summary Information Dialog as shown here. Equation operators, functions and constants are listed here and can be found in Help under SOLIDWORKS Fundamentals > Equations. Let’s take a look at a few examples how equations can be used. In this first example we’ll set-up 2 equations to keep track of how much material I’ll need to order for this welded frame and what the material cost will be. Using File Properties>Configuration Specific Properties add a new property or select from the pulldown list. In this case I added Material Cost as the new property. Next change the Type to Equation. For the Value/Text Expression we are going to use Global Variables to calculate the cost. From the pulldown menu I’ll select the cost per pound variable. Next, we’ll multiply the cost variable with the mass of the frame. Notice the “ * ” used to multiply the cost per pound with the mass of the frame which returns \$429.88 for the material cost for this frame. The next example will calculate the length of material needed for the 4 plates used at each corner of the frame. Here we’ll use a Cut-List Property for the plates to capture the total length needed. From the Cut List Summary tab a new Property called Total Length was created as an equation. The cut list property “QUANTITY’ was added to the Value/Text Expression column. That quantity variable will be multiplied by the bounding box length cut list property to give us the total length of material for the 4 plates. I’ll add a half inch to the length to account for the three cuts between the plates making the overall length 21.02”. So a piece of material 21” long will work. The next example is a brake air duct for our race car. This duct transitions from a circular opening to an elliptical opening and is used to direct air to the brake rotors for cooling. The round end is fixed at 4” because of the hose we use for air ducting, much like a dryer vent hose but fireproof. The elliptical end is open and directs the air to the brake rotor. The operating confines for the duct allow a bit of freedom to experiment. The objective is to have the largest opening possible. Defining the equation for the area of an ellipse was easy and now gives me instant feedback on the opening size as I make changes to the elliptical opening size. The equation for the area of an ellipse is: The initial size of the ellipse is: The equation for the area of the ellipse in the Configuration Specific Properties is: 3.14*”D1@Sketch3@@Default@Part3.SLDPRT”*”D2@Sketch3@@Default@Part3.SLDPRT To populate the dimension names is easy. In the Value/Text Expression row click on a dimension and it will automatically populate the dimensions name in the row. Here’s a short video on how that works. I’ll add a callout to show the area of the ellipse while I make changes giving me instant feedback when changes to the dimensions are made. Having equations to use in properties opens up a lot of possibilities. No longer will we have to resort to using static notes or callouts and having to remember to update them when changes are made. With equations everything will be kept up to date. #### Mike Sabocheck

Mike Sabocheck is a Technical Sales Director with Dassault Systemes SOLIDWORKS. Mike has been with DS SOLIDWORKS for 21 years. Prior to SOLIDWORKS he worked for Xerox for 17 years and then for Intergraph. His specialties are applying SOLIDWORKS to different design and manufacturing processes. 