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You can use the first and second techniques for the angled line shown in Figure 3.1 to create any of the three dimensions shown. To accomplish this task, drag the cursor while placing the dimension until the witness lines snap to the orientation you want.

Tip

To lock the orientation of a dimension while moving the cursor to place the actual dimension value, click the RMB. To unlock it, click the RMB again. The RMB cursor appears as a lock when the functionality is unavailable and an unlock icon when it is.

The third technique locks you into the horizontal orientation because of the orientation of the selected lines.

Note

In some situations, you may run into lines that appear to be parallel but are not exactly so. This will result in an angle dimension instead of a linear dimension. Here, you can select one of the lines and one endpoint. SolidWorks requires parallelism be precise, and situations where lines aren't exactly parallel happen if the angular measurement is off in the second or third decimal place, measuring in degrees. Imported 2D drawings and reverse-engineered 3D models can be particularly susceptible to this type of error.

Caution

When you select lines to establish a dimension instead of endpoints, both of the lines gain an implied parallel relation that prevents them from moving as you might predict. In the example shown in Figure 3.1, neither of the end lines can be angled unless you remove the dimension.

Another issue with adding dimensions to lines is that if you delete either line, the dimension is also deleted. This is not true for the first and second techniques, where as long as the endpoints remain, the dimension remains.

You can change Smart Dimension values several ways. The most direct way is to simply key in a value such as 4.052. The software assumes document units unless you key in something specific. You could also key in an expression, even with mixed units, such as 8.5 mm/2+.125 or 25.4+.625 in. You can also key in negative dimensions, which function the same as the Change Sense button in the Modify box.

Another way to put a value into the Modify box is to click the down arrow to the right of the value field, and select either to use an equation to calculate a value or a Link Value. A Link Value is like a variable name to which you can assign a value. You can link multiple dimension values to that Link Value. In sheet metal parts, the default Link Value of Thickness is used; if you change the thickness in one feature, it changes for all the sheet metal features.

To the right of the drop-down arrow is a pair of up and down spin arrows that enable you to change the value in the Modify box by a set increment amount. You set the increment in Tools⇒Options⇒System Options⇒Spin Box Increments. You can also store multiple increment values within the Increment Value icon on the Modify box.

The final way to change the value in the Modify box is by using the wheel underneath the value field. The wheel uses the default increment value. Pressing Ctrl while using the wheel multiplies the increment by ten, and pressing Alt while using the wheel divides the increment by ten.

Here is a look at the Dimension Properties interface.

• Radial. You create the dimension by selecting an arc and placing the dimension. If you want a radial dimension of a complete circle, you must right-click the dimension after you create it, select Display Options, and select the Display as Radius/Display as Diameter toggle, as shown in Figure 3.2. Alternatively, you could use the Radius or Diameter leader display options on the Leaders tab of the Dimension PropertyManager.

Figure 3.2

The Dimension Properties interface

• Diameter. You can create the dimension by selecting a complete circle and placing the dimension. If you want a diameter dimension for an arc, use the RMB menu or Dimension Properties dialog box and select the Diameter Dimension option.

Note

Along with the Radial and Diameter dimensions, you may also