Over the course of my 20+ year career with the SOLIDWORKS software, I have been exposed to a number of great tips, tricks and shortcuts. Today I’d like to review and share with you two of my favorites.
Two useful SOLIDWORKS tools: auto dimensions and the status bar.
Auto-Dimension in Sketches
Whenever I begin a new session of SOLIDWORKS, I examine my options to make sure that my sketch entities will automatically have dimensions added to them as I am sketching. This option can be found in Options > System Options > Sketch.
Figure 1. The option for auto-dimensioning sketch entities is found in Options > System Options > Sketch.
The setting I am looking for is shown in Figure 1 above. It is actually a selection of two settings: “Enable on screen numeric input on entity creation” and its sub-option, “Create dimension only when a value is entered.” With these two settings enabled, I will have the option to create a driving dimension automatically whenever I create the most common types of sketch entities: circle, line or rectangle.
To use this tool, start by enabling the options as shown above. Next, begin a new sketch. Let’s start with the Circle command and then review the other entity types.
Auto-Dimension When Creating a Circle
Figure 2. When in Sketch mode, click the circle command.
While in Sketch mode, click the Circle command on your Sketch toolbar (see Figure 2).
Figure 3. Single-click on screen for the center point of your circle and then move your mouse away (without clicking).
Move your mouse onto the screen and single-click to indicate the center point of the circle (see “b” in Figure 3). Be sure to use the single-click method and not the click + drag method of sketching a circle.
Move your mouse away from the center point of the circle to indicate the approximate diameter (see “c” in Figure 3). Do not click anything.
Figure 4. Let go of your mouse and move your hand over to the number pad.
Let go of your mouse and move your hand over to the number pad on your keyboard (see Figure 4). If you are using a keyboard without a number pad, you can use the numbers across the top of the standard keyboard. It is important to let go of your mouse. Moving your mouse will cause the numeric value of the diameter to update and we don’t want this number to change until we are done entering the desired value for our driving dimension.
Figure 5. Type the value for the diameter and press Enter.
Type the desired value for the diameter of the circle and then press the Enter key on your keyboard (see Figure 5).
You will now have a driving dimension on your circle.
A circle sketched with the driving diameter dimension automatically added.
Auto-Dimension When Creating a Line
When creating a driving dimension on a line, the process is very similar:
- Click the line command from the sketch toolbar.
- Single-click on the screen to indicate the start of the line.
- Move your mouse in the desired direction for the line without clicking anything.
- Let go of your mouse and move your hand over to the numeric input on your keyboard.
- Type the desired dimension to represent the length of the line and press the Enter key on your keyboard.
You will now have a driving dimension on your first line segment.
Figure 6. A single line sketched with the driving linear dimension automatically added.
As we can see in Figure 6, a line has been created with a driving SOLIDWORKS dimension automatically added. Since we created this line using the click-click method, we are still in the line command and ready to create a second line. This technique is very useful when creating polygons. We can immediately move to the next segment and create another driving dimension by following the steps shown above.
Figure 7. A completed polygon, fully defined, using automatic dimensioning.
In Figure 7, we can see that using the click-click method for sketching lines allows us to create a closed polygon where each line segment has a driving dimension automatically applied. We also notice that two of the dimensions are omitted from the sketch (shown in red ovals in Figure 7). This omission was intentional, since adding these two dimensions would have created an over-defined sketch. To understand how this omission occurred, let’s recall the two options from our system options that we enabled: “Enable on screen numeric input on entity creation” and its sub-option, “Create dimension only when a value is entered.” This sub-option means that if we don’t move over to the keyboard and enter a value, a driving dimension will not be added. This terrific sub-option was added in the SOLIDWORKS 2013 release and should always be enabled when using auto-dimensions in sketches.
Auto-Dimension When Creating a Rectangle
When working with the rectangle tool in Sketch mode, the process will be similar to the Circle command, with one additional step. You have to enter two dimensions to represent the height and the width of your rectangle.
Figure 8. When in Sketch mode, click the Rectangle command.
Click the Rectangle command from the Sketch toolbar (see Figure 8).
Figure 9. Single-click on screen for the starting point of your rectangle and then move your mouse away (without clicking).
Single-click on the screen to indicate the starting corner of the rectangle (see “b” in Figure 9).
Move your mouse in the desired direction for the orientation of the rectangle without clicking a second time (see “c” in Figure 9).
Figure 10. Let go of your mouse and move your hand over to the number pad.
Let go of your mouse and move your hand over to the numeric input on your keyboard (see Figure 10).
Figure 11. Type the value for the rectangle height, press Enter, type the desired value for the rectangle width and press Enter again.
Type the desired value to represent the height of your rectangle and press the Enter key on your keyboard. Then type the desired value to represent the width of your rectangle and press the Enter key on your keyboard a second time (see Figure 11).
You will now have a sketched rectangle with driving dimensions for the height and width.
Figure 12. A sketch rectangle with driving dimensions created automatically.
In Figure 12, we can see that a rectangle has been created with driving dimensions representing the height and width.
The tool to dimension sketch entities automatically while they are being created is a huge time-saver in the SOLIDWORKS software. It can save two, three or four clicks per command, and these clicks add up quickly. The nice thing about this tool is that there is almost no downside, since if you decide that you want to omit the driving dimension from an entity, you can simply click without entering a value.
Pulling Dimensions from the Status Bar in SOLIDWORKS
One of the most underutilized areas of the SOLIDWORKS software is the status bar.
The Status Bar location in SOLIDWORKS.
The status bar is located in the lower-right corner and gives you some great feedback. By quickly glancing down into the lower-right corner, you can see if you are in Edit Sketch mode, whether or not your sketch is fully defined, what units your model is utilizing and, my favorite, dimensions from your model.
There are a number of different types of dimensions you can capture from the status bar.
Length of an edge—Single-click on an edge in your model and examine the status bar (see Figure 13).
Figure 13. Length of a selected edge shown in the status bar.
You can also hold the Control key and select multiple edges to get the total length of multiple edges.
Distance between two faces—Single-click one face and then hold the Control key and single-click a second face to view the distance between the two faces (see Figure 14).
Figure 14. Distance between two faces shown in the status bar.
After holding the Control key and selecting two faces, you can see that the distance between the two is shown in the status bar. This distance also indicates that the two faces are parallel. If the two faces were not parallel, the status bar would show the angle between these two faces.
Angle between two faces—Single-click one face and then hold the Control key and single-click a second face, similar to the method for viewing the distance between two faces. If the two faces are at an angle (and the angle is not a compound angle), the status bar will display the angle between the two faces (see Figure 15).
Figure 15. Angle between two faces shown in the status bar.
If the two faces selected are at a compound angle, the status bar will not display the angle. This shortcut is very helpful to determine quickly whether two faces are parallel, at a standard angle or at a compound angle based on the status bar feedback.
Diameter of an edge or face—Single-click on a circular edge or a cylindrical face to determine the diameter of the edge or face.
Figure 16. Select a circular edge to display the diameter of the edge in the status bar.
Figure 17. Select a cylindrical face to display the diameter of the face in the status bar.
As we can see in Figure 16, if we single-click on a circular edge, we will see the diameter of the edge displayed in the status bar. In Figure 17, we see a similar result when we single-click a cylindrical face.
The ability to see dimensions in the status bar is an awesome shortcut and time-saver in the SOLIDWORKS software. By simply selecting edges or faces we can quickly gather important information about our design so that we can move forward with the engineering process.
Conclusion
Over the years, SOLIDWORKS has added some terrific shortcuts to the software to help you save time and get your job done more efficiently. These shortcuts are two of my favorites, and I use them during every session of SOLIDWORKS. I hope you find these to be great time-savers too!
About the Author
Tobias Richard is a SOLIDWORKS elite applications engineer from Philadelphia. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.