CHAPTER 10

Using Equations

Parametric sketch relations are not the only way to drive dimensions with intelligence. You can also use equations, link values, and global variables. Equations help you create simple or complex mathematical relations between dimensions. Link values are essentially a quick way of making two dimensions equal. Global variables can be used in equations like other dimension names. These three techniques are all very similar and related to one another in the interface, but are used in different ways in different situations.

Equations can cause problems if used incorrectly, but if you are familiar with how they work, you can avoid the common pitfalls and get maximum benefit by adding intelligence to your designs.

Understanding Equations

You can use equations to create mathematical relations between dimensions. You can find the Equations tool on the Tools toolbar or by choosing Tools Equations from the menu. Equations are stored in a folder at the top of the FeatureManager. Figure 10.1 shows the Equations main interface along with the Add Equation window. As I have noted with other areas of the interface, Equations still uses a floating dialog box. SolidWorks has put most functions in the PropertyManager, but equations tend to be more horizontal than vertical, while the PropertyManager is more vertical than horizontal.

FIGURE 10.1 The Equations interface

Using the Equations interface, you can turn off individual equations temporarily by deselecting the Active check box to the left of the equation. Equations can also be deactivated by a design table. I will discuss design tables in more detail in Chapter 11, where I also discuss configurations.

Creating equations

Equations are easy to create and useful for many purposes. A common situation where you would use an equation is to space a pattern of holes evenly along an edge, including the gap on both ends, where the gap at the ends is half of the regular spacing. Before you write an equation, you need to take care of a few organizational details.

Naming dimensions

It is not necessary to name every entity in every SolidWorks document, but you should get in the habit of naming important features, sketches, and even dimensions. Named dimensions become particularly important when you use them in equations, configurations, and design tables. Under most circumstances, you do not use or even see dimension names, but with equations, you do.

Named dimensions make a huge difference when you want to recognize the function of an equation by simply reading it. A most obvious example would be the difference between D3@Sketch6 and Length@WindowExtrusionSketch. The first name means nothing, but the second one is descriptive if you are familiar with the part.

To name a dimension, click the dimension and go to the PropertyManager. In the Primary Value panel shown in Figure 10.2, type the new name for the dimension in the Name text box. You cannot use the symbol @ in dimension names because it is used as a delimiter between the name of the dimension and the feature or sketch to which it applies. Also, be aware that even though the software allows you to change the name of the sketch or feature in the Dimension PropertyManager, it will not accept this change.

FIGURE 10.2 Renaming a dimension

FIGURE 10.3 Using the FeatureManager Filter to filter dimension names

Building the equation

When creating an equation in SolidWorks, it is often a good idea to write it out on paper first to make sure you have the concept correct. Examine the part shown in Figure 10.4, where the relevant dimensions have been named and displayed. The number of holes — called Instances here — is the driving variable. From that number, the spacing of the holes is calculated over the length of the part. There is also a gap on each end of the pattern of holes. This gap (measured between the center of the last hole and the end of the part) always needs to be half of the spacing between the holes. The sigma symbols to the left of the dimensions indicate that an equation is driving it. Dimensions driven by equations cannot be directly edited.

FIGURE 10.4 Variables for the hole pattern

In this case, a more sophisticated equation has not been implemented to account for the diameter of the holes possibly interfering with one another when there are a large number of holes. In other words, because there are two values that need to be calculated (the spacing and the gap), you need to create two equations. Because the gap dimension is always half of the spacing, the spacing needs to be calculated first, as follows:

Spacing = Length / ((Instances-1)+1)

The Instances –1 term stands for the number of spacings. If you have two holes, then there is only one spacing. The +1 term stands for the two half-spacings for the two ends. The second equation is simpler and looks like this:

Gap = Spacing / 2

The order of the equations is important. SolidWorks solves the equations in the order in which they are listed in the Equations dialog box. Because the gap is dependent on the spacing, the spacing must be calculated before the gap. If it is done the other way around, you can get into a situation where it takes two rebuilds to finalize a set of equations, or even a situation where in every rebuild all the numbers change. This is called a circular relation, and is a common error in order or history dependent functions, not just in SolidWorks but in many CAD applications. Figure 10.5 shows the resulting set of equations.

FIGURE 10.5 Equations for the hole pattern

Before beginning to build the equation, you should first display the dimensions that you need to use to create the equation. You can add dimensions to the equation by clicking them from the graphics window. To do this, right-click the Annotations folder at the top of the FeatureManager, and select Show Feature Dimensions, as shown in Figure 10.6. You should also select the Display Annotations option if it is not already selected. When you have done this, all the dimensions that you need to create every feature are displayed. Also, be sure to turn on the Show Dimension Names option by choosing View Dimension Names.

To build the equation, first click the Equation button on the Tools toolbar to open the Equations dialog box. Then click the Add button to display the Add Equation dialog box. To add dimensions to the equation section, just select the dimension. You can use the keypad on the dialog box or on your keyboard to add operators and syntax. All standard rules of syntax apply for the order of operations, use of parentheses, and driving versus driven sides of the equation.

FIGURE 10.6 Showing all of the dimensions in a part

Using comments

Notice the comment to the right of the first equation in Figure 10.5. Comments can be very useful for annotating equations for yourself or others. Two important reasons to annotate are to remember the significance of variables or dimensions and to add special notes about the logic of the equation that may not be obvious.

You can make comments for equations by using a single quote after the end of the equation, or by clicking the Comment button in the Add Equation dialog box. In the following example, the comment, “This must be solved first,” is applied to the equation using the single quote before the comment.

“Spacing@LPattern1” = “Length@Sketch1” / (“Instances@LPattern1”)
   'This must be solved first

To expand on the earlier discussion about projected changes to the Equation interface, several standard selection functionalities do not work in the Edit Equation dialog box. These include triple-clicking to select all (although double-clicking works to select a single word) and pressing Ctrl+A to select all.

Using driven dimensions

Sometimes it is more convenient to use a driven (reference) dimension in an equation. This is particularly true when using geometry is the best way to calculate a number. For example, if you are manufacturing a helical auger in 90-degree sections from flat steel stock, then you need to design the auger in 3D but begin to manufacture it in 2D.

What is the shape of the auger when flat? The best way to figure this out (aside from lofted bends, which are discussed in Chapter 21) is to use a little high school geometry, a construction sketch, and some simple equations.

Figure 10.7 shows a 90-degree section of an auger blade. The outside diameter is 12 inches, and the blade width is 3 inches. The overall height is 4 inches. In this case, the auger is represented as a surface because the thickness is ignored. Surface features can be useful in situations like this (used as construction geometry) and are discussed in Chapter 20.

FIGURE 10.7 A representation of the auger

With this information, you can calculate the lengths of the 3D edges using a sketch and a simple equation. In Figure 10.8, the hypotenuses of the triangles represent the helical edges of the inside and outside of the auger. By making the triangles the same height as the auger section, and by making the horizontal side of the triangle the same length as a quarter of the inside or outside diameter by using simple equations, the geometry and sketch relations automatically calculate the flat lengths of the inside and outside edges of the auger (length of triangle side = diameter of circle × pi / 4). In this way, the triangle is used to simplify the calculation, and give it a visual result.

FIGURE 10.8 Triangles calculate the length of the helical edge.

From this point, you can calculate the flat pattern again, using SolidWorks' sketch-solving capabilities as the calculator. Think of the auger as being the cardboard tube inside a roll of paper towels. If you examine one of these tubes closely, you see that it is simply a straight and flat strip of cardboard that has been wound around a cylinder. What was the flat, straight edge of the original board is wound into a helix. This method simply reverses that process.

This example requires the little-used arc-length dimension to drive the size of the arc. The hypotenuse dimensions are shown by driven or reference dimensions, and these are used to drive the arc-length dimensions, as shown in Figure 10.9. Remember that you can create arc length dimensions by using the Smart Dimension tool to click both endpoints of the arc and then the arc itself.

The reasoning behind this example may be a little difficult to grasp, but the equations and the sketches are certainly simple.

Equations are listed in the Equations folder in the FeatureManager. You can edit, add, or delete them through the right mouse button (RMB) menu.

FIGURE 10.9 Figuring the flat pattern of the auger

Using equation tricks

Some functions that are permitted in SolidWorks equations are often viewed as parlor tricks, but they actually do have some practical applications. The two functions that fall into this category are IIF and SWITCH. If you are familiar with any programming language, you may already be familiar with these two functions.

IIF

In words, this is how an IIF statement is used:

If some relationship is fulfilled, then the IIF function returns a value. If the relationship is not fulfilled, then it returns a different value.

A more technical description is

IIF(expression, value if true, value if false)

In practice, you could use it like this:

IIF(x>5, x-1, x+1)

which reads, “if x is greater than 5, then subtract 1 from x; if not, then add 1 to x.” One of the reasons why this is considered a parlor trick is that this function causes the value of x to oscillate between two numbers (depending on the number that it starts with) with each rebuild. It may be difficult to imagine an application where this sort of behavior would be desirable, but when you combine it with a macro that simply rebuilds a model a number of times, you can use it to create a certain animation effect.

FIGURE 10.10 An equation using IIF

You can use an IIF statement to control the suppression state of features and components. This function is described in detail later in this chapter.

SWITCH

The SWITCH function enables you to have a list of relationships with associated values. The value of the first relationship in the list that is satisfied is returned by the SWITCH function. For example,

switch (x>2, 1.5, x>1, .5 x<1, 2.5)

reads as follows: “if x is greater than 2, then the answer is 1.5; if x is not greater than 2 but greater than 1, then the answer is .5; if x is less than 1, then the answer is 2.5.”

As you can see, this function does not cover all situations, but it does create a condition where the value cycles through three different numbers in a specific order. Is this useful? Possibly. Again, the main application for this function would be a simple animation for changing the size or shape of SolidWorks components that cannot be changed in other more conventional ways.

Using Link Values

Link values are simply a way to link several dimensions together, making them equal. A link value is not exactly like an equation that sets the dimensions equal, because it does not depend on order like an equation does. All dimensions are set to the same value simultaneously.

A special relationship and overlap of functionality exists between Link Values and Global Variables. I cover this relationship in this chapter.

Link values are available by right-clicking on a dimension. You can also get to link values by clicking the down arrow on the right side of the Modify dialog box. Unfortunately, they are not available from the RMB menu when the dimension tool is active. To apply a link value to a new dimension, you must place the dimension, exit the dimension tool, right-click the dimension, and select Link Value.

Link values are listed under the Equations folder in the FeatureManager. Figure 10.11 shows the link values in a listed part, and the drop-down list from which you can select them or type them. Notice again that the Link Values feature also operates from a dialog box instead of the PropertyManager.

FIGURE 10.11 Link values listed in the FeatureManager, and the Shared Values interface

You must type in the first link value that is assigned in a part. After you add the first one, you can link other dimensions to this link value by using the drop-down arrow shown in Figure 10.11. You cannot edit link values directly, which means that you cannot change a dimension from linking to a value called “height” and instead link it to a value called “length.” In order to change the value to which a dimension is linked, you must first unlink the value and then relink it. The Unlink function is available from the RMB menu in the same way that you assign link values. Dimensions that have a link value have the small chain symbol displayed to the left of the dimension. Figure 10.12 shows the Unlink option in the RMB menu.

FIGURE 10.12 Unlinking a link value

To link several dimensions to the same value at the same time, you can Ctrl+select multiple dimensions and then right-click one of them and select Link Value. It will link all the dimensions selected at once. (Thanks to Brian McElyea for this suggestion!)

Link values of different types are not necessarily interchangeable. You cannot use angular dimension link values on radius, diameter, or linear dimensions. You can use linear and diameter link values interchangeably, but not angle link values.

Using Global Variables

Global variables are assigned in the Equations dialog box as simply the variable name equaling an expression or a value. Figure 10.13 shows a list of equations, link values, and global variables. When you type in a variable name, you do not need to add the quotation marks; they are added automatically. The global variable named “multiplier” uses an expression to calculate its value. The global variable shown in Figure 10.13 called “global variable” is simply assigned a value directly.

FIGURE 10.13 Equations, link values, and global variables

Global variables can be used as values in other equations, or they can be used as link values. The link value functionality has been available since SolidWorks 2007. Figure 10.14 shows the Shared Values dialog box enabling the user to select either global variables or link values when assigning a link value. Note that link values cannot be assigned through the Equations interface; they must be assigned through the Shared Values dialog box, while global variables can only be assigned in the Equations interface, not in the Shared Values dialog box. Notice that the items with the $VAR syntax are the global variables.

FIGURE 10.14 Assigning a link value or a global variable as a link value

You can use custom and file properties to drive equations. If you right-click your Equations folder and select Show Properties, you see that the default file properties already exist in the list, shown in Figure 10.15:

Global Variable

Custom Property

Default File Property

FIGURE 10.15 Equations and properties

In the equation editor shown on the right in Figure 10.15, you can expand the list of global, custom, and default properties for easy selection and placement into equations. Any custom properties you add that are of the type “number” are automatically added to this list and can be used in equations. Notice that the custom property “cost” is a property saved in my template and gets picked up for use here.

Note that you can assign both a custom property and a global variable with the same name. The global variable will take precedence over the custom property to evaluate an equation.

Starting in SolidWorks 2011, global variables are now configurable. Chapter 11 covers this feature in more detail, but the syntax for using a design table to drive a global variable is as follows:

$VALUE@global_variable_name@equations

Using Expressions

Expressions, unlike all the previous variables, values, and equations, can be entered directly into dimension dialog boxes in the Modify dialog box and PropertyManager value boxes. The expressions have to be composed of numbers and mathematical operators. An expression such as

2.375+(4.8/3) −1.1

is perfectly acceptable, as is

1+1/2

or

1 1/2

In the second case in this example, the plus symbol is understood.

Other types of operations are also available, such as ones for changing units in a dimension box. For example, if you are editing a part in inches, and enter 40mm, then SolidWorks does the conversion for you. You can even mix units in a single expression such as 4.875+3.5mm, where the inch part is assumed as the document units.

SolidWorks does not remember the expression itself, only the final value. Expressions can be entered into any place where you enter dimensions for SolidWorks features.

Controlling Suppression States of Features

You can use the IIF statement described earlier in this chapter to control suppression states of features and components. An example of the syntax is:

<feature name> = iif(expression, value if true, value if false)

Figure 10.16 shows this type of equation in use. Keep in mind that the quotes are important.

You can also use this equation in assemblies to control suppression states of components (parts and subassemblies).

FIGURE 10.16 Using IIF to control suppression states

Linking to External Equations

You can use externally saved equations to share equations between models. To export an equation, click the Export button in the lower-right corner of the Equations dialog box, as shown in Figure 10.16. To link the current model to the externally saved equation, make sure the Link To File option is checked at the bottom of the Equation Export dialog box, as shown in Figure 10.17.

FIGURE 10.17 Saving an equation to an external file

The equation is saved to a simple *.txt file. The default name for the external equation text file is equations.txt. You can change the name if you like, but remember that if you use Windows Explorer to change the name or change it with the referencing file closed, SolidWorks will not know that the filename has been changed. At the bottom of the Equations dialog box is a path for a linked equation file. You can only link to one equation file at a time.

To link to an existing equation from a SolidWorks model, use the Import button in the Equations dialog box.

Also be aware that only equations and global variables can be shared in this way. Link values cannot be shared.

Tutorial: Using Equations

Follow these steps to get some practice with using equations:

1. Start from the part on the DVD with the filename Chapter10 Tutorial Start.sldprt, shown in Figure 10.18.

   FIGURE 10.18 Starting the Equations tutorial

   

2. Show the dimension names. Choose View Show Dimension Names to find this setting.
3. Double-click the Circular Pattern feature to display the angle and number of instances of the feet and related features. You may have to move the angle dimension to see the pattern instance number.
4. Click the instance number. Change the name of the dimension to # (pound or number sign) in the Dimension PropertyManager. Make sure that Instant3D is unselected when doing this.
5. Double-click the first feature, which is the revolve, and rename the 3.60-inch dimension CapRad, again by selecting it and using the PropertyManager.
6. Write an equation that drives the number of legs by CapRad/7.
   1. Open the Equations dialog box by choosing Tools Equations.
   2. Click Add to add an equation.
   3. Double-click the Circular Pattern and click the # dimension. Make sure that the name of the dimension is listed in the equation box, and type an equal sign.
   4. Double-click the Revolve feature and select the CapRad dimension; then type the characters /1.5.
   5. Add a comment to the equation to reflect which dimension is driving which dimension.
7. Click Rebuild, press Ctrl+B or Ctrl+Q to rebuild the model, and observe whether any update takes place.
8. Rename the 6.00-inch dimension for the height of the revolved feature to DomeHt.
9. Create a second equation that drives the DomeHt dimension at the current ratio of the height to the radius.
   1. Create a global variable called Ratio = 6/3.6 (1.66667) in the Equations dialog box.
   2. Create the equation. The equation will take the form of DomeHt = (Ratio) × CapRad. You can use the drop-down list under the calculator pad to select the Ratio variable from the list.
10. Use a link value to make the radii of Fillet1 and Fillet2 the same.
11. Double-click the revolve feature. Change the CapRad dimension to 5 and rebuild. You should observe 3 feet. Change it again to 6 and you should see 4 feet.
12. Give the part a new name, including your initials or the date, and save and close it.

Summary

SolidWorks equations and related dimension-management tools are powerful but often leave you wishing for a little more flexibility and control. The interface is not up to date with the rest of the SolidWorks interface, and so I would look to see an updated equation interface soon that integrates dimension input, link values, and global variables.

Be careful about crossing SolidWorks native equation functionality with configurations; you may end up with dimensions that are controlled by both tools. Remember that the calculation capability of Excel is far greater than what is found in SolidWorks equations.