How to Define the MBD Data of Sheet Metal Parts
Previously, we discussed “How to Define a Shaft Using SOLIDWORKS MBD” and “How to Present the MBD Data of a Shaft.” Aside from shafts, sheet metal parts are also widely used in our daily lives, including computer enclosures, heat radiators, doors and windows. Figure 1 shows a sheet metal mounting structure example downloaded from the National Institute of Standards and Technology (NIST) website.
To improve the communication clarity and reduce the 2D drawing maintenance overhead, many manufacturers are looking for ways to communicate sheet metal product and manufacturing information (PMI) in 3D using model-based definition (MBD) as an alternative to the traditional 2D drawings. In this article, we will walk through the key dimensions, notes and tables using the NIST example.
Figure 1. A sheet metal part example. (Image courtesy of NIST.)
First of all, it’s important to emphasize that you can define a sheet metal part or assembly in a way similar to other 3D models using PMI tools such as DimXpert and reference dimensions. Despite several specific requirements that we will address shortly, sheet metal models are only one type of 3D model. Therefore, typical PMI capabilities can support sheet metal models well. Figures 2 and 3 illustrate several examples. The geometric dimensioning and tolerancing (GD&T) definitions not only satisfy the NIST test case requirements, but also recognize manufacturing features such as the slot shown in Figure 2. This was discussed in more detail in “Design for Manufacturing: How to Define Features Directly.”
Figure 2. DimXpert GD&T definitions on the sheet metal main body.
Furthermore, the DimXpert feature control frames automatically create and visualize the coordinate systems according to the datum references to ease the design interpretation as shown in Figure 3. Please refer to the “PMI Enhancements in SOLIDWORKS MBD 2016” for more details.
Figure 3. DimXpert GD&T definitions on the sheet metal flange.
After these general 3D PMI definitions, let’s dive into the specific sheet metal requirements. Bend line locations are often needed to indicate where to fold a sheet during fabrication. Figure 4 shows the flat pattern with bend lines and their location dimensions. The key is to use the reference dimension tool to pick up the bend lines, which are sketch entities, rather than features. In this case, the reference dimension tool is more flexible for handling sketch elements than DimXpert. DimXpert can also call out these dimensions, but you’ll just need to create some reference geometries associated with the bend lines for DimXpert to pick up, as explained in “What’s New in SOLIDWORKS 2017: MBD.”
Figure 4. Use the reference dimension tool to define the bend line locations in a flat pattern.
As shown in Figure 5, the same reference dimension techniques can be applied to define the bounding box to estimate the raw sheet material sizes.
Figure 5. Use the reference dimension tool to define the bounding box in a flat pattern.
As you may have noticed, Figure 5 also shows two bend notes indicating that “90 degree up” is the appropriate bend angle and direction, which will be useful for fabricators. These can be added using the notes command as shown in Figure 6.
Figure 6. Use a leader note to specify the bend angle and direction in a flat pattern.
In 2D drawings, a bend table is often inserted to group the key bend parameters, as shown in Figure 7. However, in MBD, an automatic bend table function is not yet available, but here are some workarounds that require a bit more steps.
Figure 7. An automatic bend table per the flat pattern on a 2D drawing.
First, you can insert an automatic bend table on a 2D drawing as shown in Figure 7. Then save this table as a Microsoft Excel table rather than a bend table template, as shown in Figure 8.
Figure 8. Save a 2D drawing’s automatic bend table as an Excel table.
Now open this Excel table and copy all the cells with the bend parameters, as shown in Figure 9.
Figure 9. Copy the bend table cells from the Excel spreadsheet.
Finally, inside SOLIDWORKS, paste these cells as shown in Figure 10. This is actually an embedded Excel table and you can double-click to edit it using the Excel commands.
Figure 10. Press the Ctrl+V key combination to paste the bend parameters.
With one more step, you can also insert the data as a general table, as shown in Figure 11. Just make sure the numbers of columns and rows are larger than the Excel table in order to carry over all the cells. Now you can edit this general table using the table commands. Another benefit is that you can save this table to be reused in the 3D PDF template editor later.
Figure 11. Copy and paste the cells into a general table.
Although these workarounds are less than ideal and don’t maintain the associations with the existing bend notes and sheet metal parameters, they can collect and present the key fabrication requirements in a well-organized table for the shop floor to execute. I hope the software can add a more automatic bend table command in the future.
Before concluding this article, I’d like to share several free resources for you to better understand the sheet metal support in the software. Here is a tutorial to walk you through defining the 3D PMI on a sheet metal part. Similarly, a sheet metal assembly tutorial is also available. They are part of an online series of 12 free learning modules including videos, click simulations, quizzes and sample data sets. I highly recommend this series to anyone new to MBD. To learn more about how the software can help you with your MBD implementation, please visit the product page.
About the Author
Oboe Wu is a SOLIDWORKS MBD product manager with 20 years of experience in engineering and software. He is an advocate of model-based enterprise and smart manufacturing.