How SOLIDWORKS Design Tables work and why they are still relevant.

Article by Joe Medeiros, CSWE updated April 14, 2020

For those who have been using SOLIDWORKS for a while you may remember how Design Tables were used to create configurations. Of course this can now be done more efficiently using Modify Configurations in SOLIDWORKS. But there are situations where Design Tables are still required or work best.

Design Tables are Excel spreadsheets which are embedded in a SOLIDWORKS part or assembly.

The layout of a Design Table is very similar to that of a Configuration Publisher, in that features and components can be suppressed, dimensions changed and Configuration Specific Properties set.

As mentioned earlier, in some cases Design Tables are required. A good example of this is SOLIDWORKS Routing components. The Routing specific information contained within these tables, needs to be shared between connecting components (pipes, elbows flanges etc). At this the time the most efficient way of doing this, is with Design Tables. Design Tables are also when using the SOLIDWORKS Configuration Publisher.

Beyond those SOLIDWORKS applications that require Design Table, since Design Tables are created in Excel, all of the wonderful tools in Excel, are also available to Design Tables. These include formulas, linking cells and easily performing calculations.

Design Tables can be accessed from the Insert pull-down in SOLIDWORKS, under Tables.

Inserting Design Table

When launched, the user has various options to create a table. I prefer to use Auto-create, but if an existing Design Table has been saved externally, it can be reused. Keep in mind that Design Tables are embedded in the SOLIDWORKS  document, not linked. There is the option though, to link the embedded Design Table to an Excel spreadsheet. I also like to set the option ‘Block model edits to update the design table’. This prevents changes in SOLIDWORKS from updating the Design Table. I usually want the Design Table to drive changes. Of course this applies to only items specified in the Design Table.

Design Table Options

If there are existing configurations, these can be added to the Design Table on creation and dimensions can also be added automatically to the Design Table.

Selecting Items to Add to Design Table

It is good practice to give dimensions meaningful names, so that is easier to understand what the Design Table is controlling.

The Excel spreadsheet that the Design Table will be created from, may initially be shown within the SOLIDWORKS window and because of the limited room, this can make it hard to input information . Once the initial Design Table is created, I’ll close the Design Table and reopen it using the option Edit Table in New Window.

Edit Design Table

Edit Design Table

This will launch Excel in it’s own window. In this window I will define my configurations and add values to the items I want to configure (dimension value, suppression state etc). In column A I enter the configuration names I want to create and in all the other columns I enter values for the configurable items.

In the example below, different configurations of the SOLIDWORKS Slip on Weld Flange are shown in column A. Columns B through J control values for the configurable items. Some columns, such as Diameter of Hub X@Hub Diameter, control a dimensions value for each configuration. Columns starting $prp, control property values. The text after the @ is the property name. If the property does not exist, it will be created as a configuration specific property.

Design Table in Excel

Design Table in Excel

Once Excel is closed, all the configurations created. All configurations created by a design table will have an X as its icon.

Completed Design Table

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Joe Medeiros, CSWE

Joe Medeiros is a SOLIDWORKS and PDM Certified Expert. He has been helping SOLIDWORKS users with training, mentoring and implementations since 1998. He combines industry experience with a thorough understanding of SOLIDWORKS products to assist customers in being successful. He shares his experience and expertise through blogs; one of which has been incorporated into the SOLIDWORKS Essentials training manual.