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Manufacturing

User Interface Tips

8 Apr, 2004 By: Greg Jankowski

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Tips and techniques make the SolidWorks user interface easier to navigate, saving time and boosting productivity.

The SolidWorks user interface features a number of time-saving tips and techniques that help you get your work done faster. Some of these tips are personal preferences I use and find effective. Little things can add up because you spend so much of your day working with the user interface.

Single Command Per Pick
To change the behavior of the interface, switch the default mode (leaving a function selected) to the Single Command Per Pick mode. The advantage of this method is evident when you use display functions (pan, zoom, scroll, and so forth). Without it, you need to de-select the function, start another command, or press the Esc key.

Single Command Per Pick mode accesses the command one time only, so it avoids this problem. The catch is, what happens if you want to use that command more than once without reselecting it? Do this by double-clicking the icon to start the command, which then acts as if it's in Multiple Commands Per Pick mode.

This setting and the input dimension value are defined in the Tools/Options dialog box under the General section, as shown in figure 1.

Modify Dialog Box

Figure 2. Enter dimension values directly in the Modify dialog box.

When you create a dimension, the Modify dialog box appears when the Input Dimension Value setting is selected (figure 1). This is the default; in most cases you'll need to change the dimension value. When the Modify dialog box appears, you can enter the dimension value directly (figure 2).

Use the up/down arrows on the right side of the dimension value to change it. The increment value is defined, by default, in the Tools/Options dialog box under the Spin Box Increments section. The +/- button adds a new value for the spin box. You can also change the default value in this dialog box.

The Rebuild button changes the dimension value and rebuilds the change without leaving the dialog box. This lets you review multiple variations before exiting the function.

The button on the bottom right side of the Modify dialog box is the Marked Dimension To Be Imported Into A Drawing function, which marks the dimension to be used with the Insert Model Items function within a drawing. This marks the dimension for re-use within a drawing. There is a selection within the Insert Model items function (Marked for drawing) that inserts the marked model dimensions.

FeatureManager
The FeatureManager design tree is a focal point of the interface. The first setting is Name Feature On Creation (off by default). This lets you create a meaningful feature name that describes your design intent. It's easier to understand a design if its name describes its key features.

Use folders to organize parts and assemblies the same way you use them in Windows Explorer. You can also act on (suppress) folders as a group. The features within a part must be sequential to be placed in a folder. This is also good practice because features should be functionally grouped (created in the same area of the design).

Arrow Key Navigation navigates and replays a design. Enable it within the Tools/Options dialog box under the FeatureManager section. To replay a design, select the rollback bar, as shown in figure 3, and use the up/down arrows to walk through the design.

The up/down arrows scroll up and down the design tree. Left/right arrows expand or collapse the item you select

Scroll Selected Item Into View and Go to Feature (in the tree) are two features that help relate the selected item between the FeatureManager design tree and graphics window. Scroll Selected Item Into View jumps to the icon of the item you select in the graphics window. Right-click on a feature selected in the graphics window and choose Go To Feature (in the tree) to jump to that feature.

All of these features are enabled within the Tools/Options dialog box under the FeatureManager section, as shown in figure 4.

Copy a Plane
The easiest way to create an offset plane is to select the plane you want to copy, press and hold the Ctrl key, and drag the plane to the desired offset (figure 5). You can also enter the value within the PropertyManager.

Sketch Options
There are two default sketch settings that you can override during a session. When you create a sketch entity, SolidWorks creates references automatically. Figure 6 shows that the end of the line will be attached to the midpoint of the indicated edge, as shown by the red end point. To temporarily override this, hold down the Ctrl key while you create the second endpoint for the line.

Override Dims on Drag/Move is an option that lets you change dimensions by dragging the geometry. Figure 6 shows that the endpoint of the line was dragged to the midpoint of the edge, even though the 0.67 dimension was constraining the line. If the option wasn't checked, the 0.67 would not be overridden, and the behavior would be different based on how the other end is constrained.

You can change both Override Dims on Drag/Move (off by default) and Automatic Relations (on by default) within the Tools/Options dialog box under the Sketch section.

Incremental Improvements Add Up
You can be more effective with the SolidWorks user interface in many ways. Small changes and improvements to the way you work and the way information is presented can add up to big productivity savings over time.