SOLIDWORKS design tables offer an easy way to create multiple configurations using Microsoft Excel worksheets. Basic design tables allow for simple data entry to bypass hours of modeling time. For advanced Excel users, rules and formulae can be used to create hundreds of unique model configurations. Dimensions, suppression states and configuration properties can all be controlled using design tables. This tutorial focuses on using designing tables to configure parts, but design tables can also be used to configure assemblies. Here we have an existing studied plate model with three pre-defined configurations created in the usual way. Extra instances of the stud and tube features are created on larger plate sizes using the fill pattern command in the existing two by two configuration. The tube pattern features been suppressed because that's going to add more instances of the tube feature in cases where the part is wider than two studs. In the one by one configuration, the stud pattern, tube and tube pattern have been suppressed because only one instance of the stud feature and no tube features are required. We want SolidWorks to automatically generate configurations of the plate with several more stud combinations, and this is where the design table comes in. Rather than creating individual parts or configurations which could take hours or days, we can simply use an Excel spreadsheet to generate these new configurations in seconds. Oh and while it's always good practice to name your features and dimensions, it's especially useful when using configurations and design tables. As named features are so much easier to identify. So to create a new design table we’ll head up to the insert menu, table and then Excel design table. You'll see in the property manager that we've got three source options here blank, auto-create and from file. We'll start by demonstrating the blank source method. A blank table will only contain a table name, default configuration name and any parameters which are manually selected upon creation. The edit control options allow the design table to update if parameters are changed in the model. For example, if a new material or feature is added, you'll be prompted to add this to an existing design table when you go to edit it. We'll use this option. When you finish creating your model and you don't want anyone to be able to change the parameters which are controlled by the design table. Then we could block model edits, which will update the design table. We'll also leave all the default options at the bottom ticked to add new parameters or configuration information to the table. Warn us when we're editing the design table and enable dropdown lists which make certain properties such as materials easier to modify. The green tick can then be clicked to create a new blank design table. A pop up will then appear asking which existing configurations and parameters we'd like to include in the design table. Here we're only going to modify dimension values and suppression state to features in this design table. So we'll select the three existing configurations by holding the control key and to add parameters to the table. We can either select them here or double click on features once the table is open. Here we'll click on the named width and length dimensions before pressing okay. Once the table is open, we can still add additional features if needed. This is easiest when the table is opened initially in its embedded form, but will come onto editing design tables later on. For now, we'll click on the stud pattern, tube and tube pattern to add them as columns. When creating a blank design table, an additional row is added called the first instance. This can have values assigned to be treated as a default configuration, or you can delete it if you don't need it. To return to SolidWorks from an embedded design table. Simply left click in the graphics area. But taking a step back, we’ll look at the resulting table. If the auto create method is used. Notice that once we've clicked the green tick, the design table will automatically populate with any parameters that have already been used for configurations. This may include certain parameters that are actually unwanted. In this case, the colour column can be removed. Column syntax controls a link to the SolidWorks model. That's these headers here, and they're usually created automatically when selecting a parameter to include. But you can also add the manually. And this is where the power of design tables really shines, as you can include custom properties to automatically populate. For example, if a configuration specific vendor needed to be added, you’d type $PRP@Vendor and this will create a new configuration specific property called vendo. But if you're looking to automate processes like configurations, then it's worth checking out DriveWorks for design automation. DriveWorks removes those repetitive tasks and even powers an online configurator that you can build into your website. So anyone buying your product can choose exactly what they want and see how it will look without you needing to create any prototypes. It's a great tool to consider and you can get started today for free with the DriveWorks Express tool that's included within your SolidWorks already. Just hit the subscribe button below and head to the tools menu to get started. For checking in on the custom properties. We can see that a new configuration specific property has indeed been added for each of the existing three configurations. At this point you can add formatting and new rows to your design table to create new configurations. Once you've created a design table, then you can of course edit it. It's easiest to edit a design table after creating it by opening it in a new window. When you're in the configurations tab, expand the tables folder and right click on the design table. Then you can click on opening a new window. Here we've edited the original design table to include some extra rules and formulae. These will determine the suppression status and dimensions for each configuration as it's just a standard spreadsheet. Any excel formulae work. Here we have IF and VLOOKUP functions which are going to apply the correct values to each cell. We won't go into detail on these here, but we will include the formulae in the video description. In simple terms, a U or S is added to feature columns to determine if they're suppressed or unsuppressed while numbers can be added to columns which are controlling dimensions. With these rules in place, new rows can be created by dragging cells and the formulae will automatically update. Each new row represents a new configuration. The part number column can be used to show part numbers as document names, configuration names or any other text according to the syntax in this table. In this example, $C ensures that the configuration name is used for the part number. Once complete, we can close the design table and the SolidWorks model will update. All of those new configurations have been added and they can be organised by right clicking on the part at the top of the configuration manager before clicking tree order and numeric. To save our finished design table, right click on the table in the configuration manager and click save table. This table can then be sent to colleagues as an Excel file to be checked without the need to open SolidWorks. And remember that third option when we created the design table? Yeah. This is where it comes into play. So if you already have an existing design table file, then we can use the from file source method when creating a new design table to pull through that data and save us even more time. Since you've made it this far, why not go a step further and advance your SolidWorks skills with our professional training courses? Head to our website and discover a whole range of courses led by the SolidWorks experts. With courses running online and in our classrooms. There's always one near you. So let us know in the comments what tutorials you want to see next. And don't forget to subscribe for more SolidWorks tips, tricks and solutions.