Design Tables & Configurations to Validate Robust Models in SolidWorks

In this tutorial Design Tables are used to create multiple configurations of a simple model in SolidWorks.

  1. Step 1: Create the solid model

    The configurations can be easily created and activated to validate the robustness of the model. Though some significant changes would cause many down-stream features to fail, it is important to create a model that is as robust as possible because changes to the design are inevitable and fixing failures in the model are almost always time consuming.

    One of the goals of a good design engineer using a CAD system should be to create a robust model that when changes are made there are no failures in the model feature tree. Failures to features in the model may take valuable time to correct and slow the design process. If the design engineer understands the form, fit, and function of the design, he or she should be able to implement a strategy when constraining and dimensioning the model to accommodate changes to the model without causing errors to dependent features. Unless we are reverse engineering a proven design, then changes to the model will occur frequently throughout the design process and even into the production and support phases of the life cycle of the product.

    SolidWorks has a good tutorial on Design Tables if you would like to review that Tutorial before proceeding with this one, though it is not necessary. The SolidWorks Design Tables tutorial is in Third row in the third column of the Basic Techniques group of tutorials.

    A good Top down design strategy (see my tutorial on Top-Down Design) is critical in most design projects unless we are creating a single part rather than an assembly. Even in a single part design where there are a number of interdependent features, a good top-down strategy can usually allow modifications to the model without failures and therefore improve overall design productivity.

    In this tutorial, we will use a single part as our example from a Certified SolidWorks Associate exam (CSWA). The procedure on creating the model will not be given in this tutorial. There are a number of tutorials for beginners that will help you learn how to model this simple, theoretical part.

    When constraining and dimensioning the sketches that define the profiles and features of the model, it is important to think of how the model might react to changes to any of the dimensions. In this tutorial, we are going to test the robustness of your model by changing the three variable dimensions labelled A, B, and C which are the Height (A), Depth (B), and the Width (C). So, try to incorporate a strategy that will allow you to make adjustments to those dimensions without causing failures to features. We might think of limits that we can accommodate of the A, B, and C dimensions. In some parts we might want to or have size and location of features defined as functions dependent on the variable dimensions.

    In this part, let's maintain all the explicit dimensions as shown and vary only the three dimensions labelled as A, B, and C. Start with A = 63mm, B = 50mm, and C = 100mm. Also note where the origin is at the intersection of the axes. If you use a different origin, a user-defined coordinate system can be defined when the Center of Mass is calculated and compared at the end of the tutorial.

  2. Step 2: Show Feature Dimensions in the Model

    Once you have your part completely modeled, let's modify the three variable dimension names. First, turn on the feature dimensions in the model for all dimensions by Right-clicking on the 'Annotations' name in the Feature Manager Tree, and then Selecting the option, 'Show Feature Dimensions.'

    You may want to change the text height of the dimensions in Tool, Options, Document Properties, Dimensions, font....

    Find the dimensions that control the Height, Width, and Depth of your model and slide them out away from the model. Select the Height dimension and rename it with an appropriate name in the dialogue box that pops open when the dimension is selected. In the model below, the height dimension has been changed from D1@sketch1 to A Height@Sketch1 so it identifies that Dimension as the height of the part. Change the other two dimensions (Width and Depth) to an appropriate name.

    If the names are not showing on the model, from the Pull-down menus, Select, View, Hide/Show, Dimension Names:

    You can turn off the other dimensions or hide them if you would like by right-clicking on the dimension, and selecting the 'hide' option. To toggle the dimension back on, right-click on the various features in the Feature Manager Tree or in the graphics area and select 'Show All Dimensions.'

    Leave the three dimensions visible we are going to assign to the Design Table.

  3. Step 3: Create the Design Table

    From the Pull-down menus, Select Insert, Tables, Design Tables

    The dialogue box for the Design Table opens , leave the option to Auto Create.

    In the Edit Control, leave the option to 'Allow model edits to update the design table. In the Options section, make sure the options 'New parameters', New configurations, and 'Enable cell drop-down lists' are also checked.

    Then select OK (green check) in the open dialogue box.

  4. Step 4: Fill in the Design Table

    The Design Table is created and displayed in the graphics window.

    With the Design Table open and the Feature Dimensions showing, Double-click on each of the three dimensions on the model in the graphic window that are to be changed: the Height, Depth, and the Width from the graphics screen. As you double click on the dimension, the dimension variable name will appear in the columns of the Design Table and the default values will appear in the first row.

    Now, in the first column, type in three names (or more if you would like) such as Config 1, Config 2, and Config 3 and then in the corresponding column for the Height, Depth, and Width type in values larger or smaller than the default values given in the original drawing for those values.

    Once the Design Table has been filled out, pick anywhere in the graphics screen and the the Design Table will close and save.

  5. Step 5: Check the Configurations

    Notice, that when the Design Table closes the Configurations are automatically created and the names are displayed in a notice to the user.

    From the Feature Manager Design Tree, Select the Configurations Manager which will display the Tables Menu and the Configurations that were created.

    Double click on each of the configurations and notice that the dimensions for the Height, Depth, and Width update to the values in the Design Table. If feature errors or failures occur in your model, do some investigation into your model and find out where the errors occur and resolve them. A good practice is to place sketches on Reference Planes which are defined by the variable dimensions rather than sketching on faces of the geometry. Also, dimensions from axes are also more robust than dimensions from edges or faces of the geometry.

    In some designs, it is often helpful to set Reference Planes that define the Front, Back, and Profile Sides of the part. Then when creating an extrusion, extrude 'Up to Surface' rather than extruding a specified depth. This approach works well when multiple features terminate at the same plane but their individual extrusion depths are different.

  6. Step 6: Edit the Design Table

    In the Configurations Manager, Expand the Tables menu to show the Design Table. Right-click the Design Table, and Select Edit Table.

    Select OK.

    And the Design Table will open up for editing.

    Change the values for the three configurations to match the ones in this Design Table above.

    Pick anywhere in the graphics window and the Design Table will close and save the new values.

  7. Step 7: Set Material and Compare Mass Properties

    Be sure to set the material of the part to Copper. In the Feature Manager Tree, Right-click on 'Material' and pick 'Edit Material.' The Material dialogue box will open, then select Copper from the list of materials, and Apply, and Close.

    With the first Configuration selected (the one below is called Config 1), from the Pull-down menus, Select Tools, Evaluate, Mass Properties

    Or, From the Icon Menu, Select, Evaluate, Mass Properties:

    Compare the mass properties of your model with the mass properties of my model. They should be the same values. Look at the Center of Mass values. If you have an origin different than shown in the illustration at the beginning of the tutorial, you may create a User-defined Coordinate System on your model , from the Pull-Down menus, Select, Insert, Reference Geometry, Coordinate System:

    The pick the origin, and then each of the edges of the part so the axes align with the correct direction . Notice you may toggle the direction with the icon on the left of each axis window displaying the edge defining the axis.

    Now, set the origin in the Mass Properties dialogue box, and then Recalculate the values.

    For Config 1, the mass of my model is 1280.33 grams.

    So it is easier to read, the Mass Properties is displayed separately.

    Config 2 Mass Properties:

    Mass of Config 2 shows that it is 1662.17 grams. You should have the same value.

    Config 3 has a mass of 2201.32 grams.

    Check your Center of Mass and make sure your model has the same values.

    Here is a video of my example: