The SOLIDWORKS Design Table feature allows spreadsheet-driven configuration of parts and assemblies. This enables you to build several different configurations of a part by varying the values in the table cells. Each cell is linked to a parameter and configuration of the part or assembly.
Getting Started
Many times, parts have similar features and generally vary a few dimensions to create a unique configuration of that part. One example is piping and piping components that have common features and are scaled to particular sizes to create families of parts and configurations.
We will start with such a component, a piping weld neck flange. Figure 1 below shows the general geometry and configuration of this part.
Figure 1. Weld neck flange.
This is a nominal 2-in-diameter pipe flange with a flange thickness of 0.69 in. We will begin by creating a design table that will modify the flange thickness. During this process, we will be selecting dimensions from the graphics window. To make the dimensions visible, right-click on the Annotation folder in the Feature Manager Design Tree and select “Display Annotations.”
Feature Manager Design Tree
The model will then appear as in Figure 2.
Figure 2. Part showing dimension annotations.
The parameter to modify will be named to better identify it further in the design table. Click the 0.69 dimension on the model. Change its name to FlangeThickness in the properties window as shown in Figure 3.
Figure 3. Dimension properties.
Creating the Design Table
The design table is inserted by navigating to the following menu item: Click Insert > Tables > Design Table.
The Property Manager window shown in Figure 4 appears.
Figure 4. Property Manager.
Under Source in the Property Manager, select “Blank” to insert a blank design table.
The remaining options can be left at default. It should be noted that design tables are bidirectional with the model dimensions and an inadvertent change to the design table from a model dimension change can occur. The Options section of the Property Manager controls this and other model associations with the design table.
A Microsoft Excel worksheet (Figure 5) appears in the part document window. Excel toolbars replace the SOLIDWORKS toolbars. By default, the third row (cell A3) is named “First Instance” and column header cell B2 is active.
Click the FlangeThickness (0.69) dimension value in the graphics area. The dimension name is inserted in cell B2, and the dimension value is inserted in Cell B3. Figure 5 shows the result.
Figure 5. Design table embedded in part.
Click anywhere outside the table window to close it and return to the normal SOLIDWORKS interface. Our configuration pane now looks like Figure 6 with the additional configuration “First Instance” added.
Figure 6. Configuration Property Manager.
We now have the base configuration and the design table–generated configuration (“First Instance”). The power of the design table is being able to generate configurations without having to navigate the Feature Tree. To demonstrate, we will create thicker and thinner versions of the flange as separate configurations. Right-click on the design table feature in the Configuration Manager and select “Edit Table” to bring up the spreadsheet. In Cell A4, enter “ThickFlange” and 0.75 in cell B4. In cell A5, enter “ThinFlange” and 0.60 in cell B5. The table should look like Figure 7.
Figure 7. Design table with additional configurations.
Click outside the window and the message in Figure 8 should appear, confirming that the additional configurations were properly recognized.
Figure 8. Alert window for design table modification.
Our Configuration pane now looks like Figure 9.
Figure 9. Configuration Manager.
When the design table is open, the menu items become the Excel menu items. Any cell operations that Excel allows can be done in the design table. A family of part configurations can quickly be made, for example, by copying equally spaced values down one column.
As one starts using custom Excel spreadsheets to drive the configurations, a word of caution is necessary. The cell in the top-left corner of the table must maintain the reference name “Family.” This is defined by default by SOLIDWORKS, and if there is manipulation of the spreadsheet, this cell must maintain this reference name. Figure 10 shows the yellow highlighted cell demonstrating the “Family” cell location after inserting several blank rows above the original design table region. The design table becomes all cells to the right and below this “anchor” cell.
Figure 10. Design table illustrating location of the “Family” cell.
Additional parameters can be added to the design table by following the same editing procedure that we did previously. When the design table is visible and the dimension of interest is visible in the graphics area, selecting the dimension will add it to the table as another column. For example, to add the bolt hole diameter as an additional configurable property, click on its 0.75 dimension value. The design table then appears as shown in Figure 11.
Figure 11. Adding additional paramters to the design table.
The user interface can be expanded to a full Excel window by right-clicking on the design table item in the Configurations Feature browser and selecting “Edit Table in new Window.” The result is shown in Figure 12.
Figure 12. Design table with additional parameters.
As discussed previously, any operation that is available in Excel can be used in a design table. We can enter a formula in any of the cells holding fixed values. For example, we can set the bolt hole diameter for the ThinFlange configuration to be 80 percent of the size for the ThickFlange configuration by entering the formula “=0.8*C4” for the ThinFlange bolt hole diameter size (cell C5). This has many advantages over the SOLIDWORKS Equations feature for linking dimension values to other dimensions in a part and for advanced mathematical relationships in parts.
Conclusion
SOLIDWORKS allows great flexibility in creating parts with different configurations. In addition to creating manual configurations, design tables allow configurations to be made in a familiar Excel spreadsheet template. This allows part configurations to be made rapidly using Excel tools in conjunction with the SOLIDWORKS graphics window.
About the Author
Attilio Colangelo has more than 25 years of experience in engineering and project management in the chemical, process, ceramic and advanced-materials industries. His specialties include CAE, with an emphasis on FEA, high-temperature and heavy industrial design. His software skills include SOLIDWORKS Simulation, NASTRAN, Caesar II, ANSYS and iOS programming.