For many users, their first introduction to design tables in SOLIDWORKS occurs when they are preparing for the Certified SOLIDWORKS Associate (CSWA) or Certified SOLIDWORKS Professional (CSWP) exam. That’s because the exam requires you to link your dimensions to a design table. Figure 1 shows a sample.
Notice how the sample question shown in Figure 1 lists variables A, B and C. Those are dimensions that will change. If you link your dimensions to a design table, then all you have to do is update the values in the design table and the part will automatically update. This saves time because you won’t need to go searching through the browser for the correct sketch, open up the sketch, change the dimension, and then move on.
In this article, I am going to walk you through all the different ways you can use design tables, starting with linking dimensions—that way, you’ll be ready to take that certification exam—all the way through using it for assembly configurations.
I’m going to start with a very simple part—a serial number label (see Figure 2). I use serial number labels all the time in my work. They are a standard size—usually 0.625 in x 1.5 in.
I drew a center rectangle and applied the dimensions. I added a 0.05 radius fillet at each corner of the label. To make it easier to identify which dimension was length and which was width, I modified the dimension names from “D1” to “Length” and “D2” to “Width” (see Figure 3).
You can change a dimension name from “D#” to a name you choose either in the Properties panel or when you edit the dimension. Note that you should keep the “@Sketch#” as part of the name you use, or you will get an error message.
Next, I extruded the serial number label to a thickness of 3 millimeters.
Once I had my basic part, I could bring in the design table. It’s always best to start with the basic geometry already defined because you can then work from that geometry to create your design table.
To add a design table to a part, go to the Insert menu→Tables→Design Table (see Figure 5).
The design table is placed inside the part or assembly file, so you don’t have to worry about losing the link, unless you opt to use an external Excel spreadsheet. I will discuss that option later in this article.
I like using the Auto-create option because then the design table automatically pulls any existing dimensions from the part into the design table. That said, I have had students who forgot to add dimensions to their sketch. If there are no dimensions in the sketch, then the design table will have no data to import.
Before you click the green check icon shown in Figure 6, I want to go over some of the options in the dialog box, so that you’ll understand how they work. The first option under Edit Control is pretty important (see Figure 7). If you select Option 1 (Allow model edits to update the design table), then you can edit the model and the design table will automatically update. If you select Option 2 (Block model edits that would update the design table), then you can only make changes inside the design table to make changes to the model. This becomes important if you are designing a part to meet a specification. For example, I use design tables to keep track of dimensions that are controlled by a specification. I don’t want the model dimensions to change because then the model would be conflict with the required specification. So, do you want the model to drive the design table or vice versa?
The bottom list of options (New parameters, New configurations, etc.) will automatically update the design table when you add dimensions, colors, materials and configurations. You also will get a warning when the design table changes, so you can check to see if you are happy with any updates that were made.
A list of dimensions will appear, and you can select which dimensions you want to add to the design table. This is where naming the dimensions can be very helpful. You can see the Length and Width dimensions that I placed. The “D1@Sketch1” dimension is the fillet radius dimension, which I failed to name because I wasn’t planning to change it or control it with the design table. The “D1@Boss-Extrude” dimension is the thickness of the label. Again, I wasn’t planning to change the label thickness or control it with the design table, so I didn’t bother assigning a name to the dimension. I highlight the dimensions I want to bring into the design table (see Figure 9), and then press “OK.”
The design table auto-fills with the dimension values I selected (see Figure 10).
Instead of using “Default”—or some other word that is pretty meaningless—I like to use the company’s part number to identify the part. In the example shown in Figure 10, I added two additional part numbers along with their sizes. This means that this part file now has three configurations (see Figure 11).
To exit the design table, just left-click anywhere in the display window.
You should see a confirmation dialog box indicating that the three part configurations have been created. Press “OK.”
Now, switch over to the Configuration Manager tab on the Browser palette. The default configuration is still there and has a green check mark next to it. The green check mark indicates that this is the active/current configuration. Notice that there is a dash/hyphen next to the other configurations. This means that those configurations have not been generated or activated yet.
Select the part name at the top of the Configuration Manager palette and right-click. You will see a list of menu options (see Figure 13).
Adding a configuration attaches an additional row to the design table. When I have different configurations of a part, I set the Properties as shown in Figure 14. I enable “Use in bill of materials.” And I set the “Bill of Materials Options” to use the “Configuration Name.” If I have set the configuration name as the part number, then my bill of materials will automatically fill in with the part number and description as I defined them in this dialog box. If I suppress new features and mates, this ensures that no changes are made to this specific configuration unless it is active. I can also assign a specific color to a configuration to make it easier to identify or because it is the color that will be used in production.
The Configuration Publisher allows you to take your part one step further and upload it to the SOLIDWORKS 3DContentCentral portal. I normally do not do this with any models or assemblies I create in my job simply because anything I create at work—even if it is a connector based on a vendor’s spec—may be considered proprietary, either by my employer or by the vendor. It just isn’t worth the legal liability. That said, if you are working for an employer that wants their content on 3DContentCentral, figuring that if their parts are incorporated into a design that will translate into sales, then this is where you would do that.
The Rebuild All Configurations selection will automatically compile the geometry for all the configurations.
Depending on how complex your model is, there is a slight pause while SOLIDWORKS runs through the compile. You will then see a green check mark next to each configuration. This also increases the file size of your part. If you plan to email or upload the part, you may want to purposely forgo compiling all the configurations to keep the file size smaller. The configurations will still be available to the end user.
To reduce the file size prior to emailing or uploading it, you can use the Remove Mark and Purge Data for All Configurations option. If you choose this option, you will see the green check mark removed from all the configurations except for the active configuration (see Figure 17).
To see or activate a configuration or part version, simply select that configuration, right-click, and select “Show Configuration” (see Figure 17).
Because it is easy to close the design table by simply left-clicking in the display window—and if your part has a lot of parameter values—you may want to use the Edit Table in New Window option. Highlight the Design Table in the Configuration Manager tab, right-click, and select “Edit Table in New Window.”
Any parameters or configurations that have been added since the previous time you opened the design table will be displayed to give you the option of adding them to the design table. I am going to select the “LBL-004” configuration as well as all the parameters to add to the design table, and then press “OK.”
The advantage of using the “open in new window” option is that it opens the design table in Excel, making it much easier to edit and move around (see Figure 20).
SOLIDWORKS uses an equation based on the RGB values to determine color (see Figure 21). If you know the RGB values, you can calculate the color. Many companies use custom colors for their products, so it can be useful to create a sheet in your design table just to designate the color and then link the color back to the configuration (see Figure 22).
The formula to designate the color code is = MAX(MIN(B3,255),0) + MAX(MIN(C3,255),0)*16*16 + MAX(MIN(D3,255),0)*16*16*16*16.
Note that the B3, C3 and D3 values in the above formula are cell values. Because they are blank in the spreadsheet, the resulting color code number is 16777215, indicating white (see Figure 22).
When you insert a part using a design table or configurations into an assembly, you can select which configuration to place in the Open dialog box. You can change which configuration you want to use after the part is placed.
Once you have placed the part inside the assembly, you can switch the configuration using the right-click menu (see Figure 25).
To locate the part in the assembly browser, right-click, and select “Configure Component.”
In this case, my assembly has several configurations, and I can specify which label I want to use for each assembly configuration.
To select a different label configuration, use the drop-down list to identify the preferred configuration (see Figure 27).
Note that having different configurations does not mean that you are using a design table. A design table will automatically create configurations, but adding configurations does not automatically add a design table.
I also want to discuss how you can use a design table to suppress features in a part.
In this first version of a front chassis panel, I have several cuts-out for various connectors. I would like to create a version that has an opening for an HDMI connector and a version that does not have the opening.
It is useful to name your features to make it easier to identify which features you want to suppress/unsuppress.
Note how I have named the cut-out openings to make them easy to identify.
I now switch over to the Configuration Manager to add another version of the front panel.
Once again, I always set up my configurations to use the corresponding part numbers so that my bill of materials can leverage this data.
I then suppress the panel cut-outs that I don’t want to use for this configuration.
Next, I place the cut-out that I want to use for this version of the panel and name the feature.
Once I have created the basic features I need for each configuration, I can insert the design table.
Notice that I can select the “$STATE” of a feature to add to the design table. The state determines whether the feature is suppressed or not.
Once you have created the basic design table, you can modify it in Excel to control which features you see for each version.
If you have two (or more) versions of the front panel, you will also need to create the same number of versions/configurations in the assembly.
Once you have completed your preliminary setup, you can insert a design table. Keep in mind that the larger the assembly, the larger your design table may become and this can slow down your system a great deal.
Each version of the assembly should be assigned to the corresponding version of the front panel.
In conclusion, design tables can be used to control the size of features, whether or not the features are suppressed, colors, and versions of parts and assemblies. They can be a powerful tool to boost your productivity.
About the Author
Elise Moss has worked as a mechanical engineer for more than 20 years in Silicon Valley. She owns her own consulting firm, Moss Designs. She is a Certified SOLIDWORKS Professional (CSWP) and a Certified SOLIDWORKS Instructor. She has taught SOLIDWORKS on a part-time basis as a member of the adjunct faculty at Laney College in Oakland, Calif., for eight years. She is a regular presenter at SOLIDWORKS World. Moss holds a BSME from San Jose State University.