Many people are aware of the use of design tables in SOLIDWORKS to allow for quick changes to models. Just add the feature or dimension to the table, and in a few quick clicks you can change design parameters from one convenient spot. However, what is less known is that it is also possible to use the many built-in equations in Excel to create a table that will be “smarter” than just a spread sheet of numbers. Let’s look at a basic example to illustrate how easy it is to get some extra intelligence in your tables.
In this example I am creating a flywheel. I know that in the end, my Center of Gravity (CG) must be at the center axis of rotation. I want to add a sensor to my table, making my Design Table a one stop shop for modification and alerts. While you may be familiar with the ‘Sensor’ tool available in SOLIDWORKS, it is not currently possible to add the sensor output to a Design Table. However, this is not a problem because it is possible to add some simple conditional formatting in the table to act like a sensor.
The first step is to create the actual table: Insert>Tables>Design Table
The dialog will then give you options on how you would like to create your design table. In this case, I chose to “Auto-create”.
Now that a design table has been created you can open the table in a new window or chose to modify it inside of SOLIDWORKS.
I want to be alerted if a change I have made will move the CG from the center (0,0) of the part. To get the CG data into a table, you simply need to add it in the ‘Configuration Specific’ properties of the part. To add the properties go to File>Properties then select the ‘Configuration Specific’ tab.
Once you have added the desired properties, the next time you open your design table you will be prompted to add the newly created properties to the table. Now it is just a matter of adding some conditional formatting to the newly created cells:
In this case I selected the two table cells for the CG I added in the previous step, and then added conditional formatting that turns the cells red when the output of the CG does not equal 0 and green when it does.
Now if I was to create a new feature, say an extrusion around the outside of the part, and if I accidentally missed and didn’t quite make it concentric about the center…
…it would be easy to accidentally miss this mistake, but when I go to update my design table.
The CG cells have turned red giving an alert that there is currently a problem with the model.
I have also created a video on how to add conditional formatting here:
Using similar conditional equations, the table can also be used to turn on or off an entire feature. In this example, when the flywheel grows above 17.5 inches in diameter a clearance cut will need to be added. To accomplish this, the new feature is added to the design table by opening the table, then double clicking on the item in the design tree to be added to the table. This was done both for the new extrude feature, as well as the dimension for the overall diameter that will be used to determine if the clearance cut needs to be turned on or off.
Then the conditional statement is added based on the overall diameter of the part. In this case the equation was =IF(AD5>17.5,0,1)
This equation means that if the overall diameter exceeds 17.5 then the extra cut will be turned on.
Note: you may need to reformat the cell to be “general” for Excel to accept the equation.
Now when I change the overall diameter (D1@Sketch1) either in the sketch or in the design table, the clearance cut will be turned on or off accordingly.
Though this is a simple example, any time you have a part that you are going to be reusing and modifying, don’t forget about making your design table smarter so you don’t have to work harder.
I also created a video on how to make a feature turn on and off using a conditional statement here:
And if you want even more automation in your parts, check out DriveWorks!