Figure 1. Sample CSWA question.

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.

Figure 2. A serial number label sketch.

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).

Figure 3. Assigning a name to a dimension.

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.

Figure 4. Serial number label—extruded.

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.

Figure 5. Insert menu.

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.

Figure 6. The Auto-create option.

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.

Figure 7. Design table options.

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.

Figure 8. List of values for the design table.

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.”

Figure 9. An auto-created design table.

The design table auto-fills with the dimension values I selected (see Figure 10).

Figure 10. Modifying the design table.

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.

Figure 11. Confirmation dialog box showing three configurations.

You should see a confirmation dialog box indicating that the three part configurations have been created. Press “OK.”

Figure 12. The Configuration Manager.

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.

Figure 13. The right-click menu on the Configuration Manager.

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).

Figure 14. Adding a configuration.

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.

Figure 15. The Configuration Publisher.

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.

Figure 16. After a Rebuild All Configurations process.

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).

Figure 17. Showing a Configuration.

To see or activate a configuration or part version, simply select that configuration, right-click, and select “Show Configuration” (see Figure 17).

Figure 18. Edit Design Table in New Window.

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.”

Figure 19. Adding to the Design Table.

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.”

Figure 20. The design table as an Excel spreadsheet.

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).

Figure 21. The SOLIDWORKS color numbering system.

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).

Figure 22. Creating the Custom Colors sheet in Excel.

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).

Figure 23. Inserting a design table part into an assembly.

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.

Figure 24. Placing the serial number label inside an assembly.

Once you have placed the part inside the assembly, you can switch the configuration using the right-click menu (see Figure 25).

Figure 25. Right-click menu to set the configuration.

To locate the part in the assembly browser, right-click, and select “Configure Component.”

Figure 26. The Modify Configurations dialog box.

In this case, my assembly has several configurations, and I can specify which label I want to use for each assembly configuration.

Figure 27. Selecting a configuration inside an assembly.

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.

Figure 28. Front panel Version 1.

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.

Figure 29. Feature browser.

Note how I have named the cut-out openings to make them easy to identify.

Figure 30. Adding a Configuration.

I now switch over to the Configuration Manager to add another version of the front panel.

Figure 31. Configuration options.

Once again, I always set up my configurations to use the corresponding part numbers so that my bill of materials can leverage this data.

Figure 32. Suppressing features with the Configuration Manager.

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.

Figure 33. Design table showing features suppressed and unsuppressed for different versions.

Once you have created the basic design table, you can modify it in Excel to control which features you see for each version.

Figure 34. Switching configurations.

Figure 35. Front panel in the assembly.

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.

Figure 36. Assigning part configurations to assembly configurations.

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.

Figure 37. Using the design table to control configurations.

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.

Those of us who are engineers know we can’t let them down. We have to produce products quickly—and perfectly—just like we did the first time. That means we have to reuse all the existing models to be efficient. As anyone in the trade knows, when dramatic changes in variation happen, engineers rarely get to use the same exact models twice. We may take one model and stretch and pull, save as, revise and reassemble into a new model that has no real connection to the original design that everyone loved.

Enter the SOLIDWORKS world of configurations.

With configurations, we turn parts on and off, change sub components, dimensions, part numbers, revision levels and pretty much anything that is CAD-related and can be controlled in configurations. If designers are unaware of configurations, they should really start studying up to better increase their time to market. The Help page on Configurations explains this very well.
One of the problems that configurations have is that they are difficult to tightly control from the general interface at a macro level. SOLIDWORKS does offer very intuitive controls for this, but as the design complexity and sheer amount of variations grow, these tools become increasingly difficult to maintain.

Design tables are the saving grace for these situations.

By inserting a design table into the configurations that are already in place, the software takes nearly every variation throughout that level of component and places it into an Excel spreadsheet. The spreadsheet is natively embedded into the file and formats so that any Excel-literate user can easily make hundreds of new configurations in a matter of minutes. It can become as easy as copying and pasting rows into Excel followed by a simple find/replace command. Of course things can get more complex than that, but if the design table is setup with substantial forethought, it can actually get even simpler than that.

Let’s walk through the basics first.

In my early days, when I was designing mining equipment, I would always need motors to drive various aspects of the mining equipment system, including conveyors, crushers, screeners and various other smaller components. I would always have to find a model from the manufacturer, or someone would share one in an online repository such as 3D ContentCentral. I was rarely lucky enough to find anything accurate for my specific needs. The models were often sketchy at best, and very time-consuming to track down. The total number of usable motors that I needed climbed to over 200. I also needed to be able to play with many of those options while I was designing. To solve this problem, I decided to model one myself. It was very flexible and had all of the features available so that I could modify or suppress as needed. It took me one model and a couple days’ worth of research and data entry to get all of them into one accurate selectable model that I would never have to maintain again. I didn’t have to worry about a huge file management problem, and I didn’t have to worry about the inevitable mate problems associated with different modeling techniques for each model.

Figure 1. A view of the base model created by the author. On the left is a small selection of the configurations that were required for his shop. (All images courtesy of the author.)

Figure 2. A design table used to create all of the motors in the author’s shop. Users should name the features and dimensions that will be configured to make their processes easier and more understandable to future users.

As most can understand by looking at Figures 1 and 2, setting up this environment takes some forethought. But once it is created, it can save you a lot of time. By using design tables and equations built into the Excel design table in the upper level assembly, I was able to control which motor was used via traditional engineering calculations.

With design tables, I could use the option to save a design table to a standard Excel file that controlled my conveyor length, shape, types of rollers, belt guides, pulley sizes, guards and every piece of the bill of materials (BOM). All I would have to do is get my rough dimensions from design sketches of conveyor inputs and outputs. My sales group would provide requirements such as the weight of material and speed required to satisfy the mining equipment output. I was able to put all of those rules and equations into this external Excel file, fill in the requirements and open the assembly, and all of my modeling work would be done.

At the same time, the vast majority of my drafting work was done—except for the dimension location cleanup and double-checking everything. Then I would just simply “Pack and Go” that file to a new part numbering scheme and be done. What used to take at least three days to fully complete now only took a few hours—sometimes less.

Figure 3. An example of a conveyor that can be created using only a spreadsheet.

This process was exceptionally helpful in a custom design shop that focused on similar and commonly used types of components. The end goal is to allow marketing to input basic data of this type and speed things along.

Designers might debate the notion that they don’t work in a custom design shop and that this may not help them. However, I would strongly encourage them to think about how it can help them. I have used design tables in a wide range of engineering industries and have always found them to be useful. However, I would warn users that the first couple of times should be run through the BOM and file management process that their company uses and make sure that those processes are fully incorporated into their setup of design tables.

Education of all engineers associated with a project is well worth the cost. I would also suggest leaning on a reseller to help in facilitating this, or at least bounce some ideas off of them before going too far. File management, product data management and product lifecycle management can sometimes throw some curve balls at this process. When a company goes into this with its eyes wide open and plans to succeed by using design tables, time-to-market can be greatly reduced.

Visit the Dassault Systèmes SOLIDWORKS website to learn about all of the company’s time saving design tools.

About the Author

Ryan Reid is a CAD administrator, PLM enthusiast, designer, GD&T specialist, lead, lean philosophy supporter, Microsoft Office expert, 3D printing hobbyist and manufacturing-focused professional with 17 years of combined experience in those areas. Reid has accomplishments in all aspects of manufacturing engineering, from cradle to grave plastics/mold to structural, systems, process and change management design.