Sheet Metal Success in SOLIDWORKS
Oh, sheet metal, how one can love and be completely frustrated with the process at the same time! Sheet metal design is an intricate design process. It requires many skills, trade secrets, compromises of design intent, machine capability knowledge and, often, patience in a fast-paced design environment. The sheet metal designer is often wearing two or three hats to accomplish all of these tasks.
Regardless of all of those requirements, designers and engineers have to get the job done, and we have to get the job done fast in order to help our company succeed in producing new and innovative products. SOLIDWORKS has some great tools to help with these. Let’s go over a few.
First off, let’s start with selecting material and gauge. The gauge table tool (see Figure 1) should be used as much as possible. It is located in C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Sheet Metal Gauge Tables. I personally use the K-factor version, but many may prefer bend allowance or go with a bend table. Both can be found in a nearby folder.
Properly formatting the list of gauges is important. It must be done from thinnest to largest, and there can’t be duplicate thickness. One may have to create a few of these files to fully utilize the entire catalog of a company. But once it is done and in place, it makes life easier for everyone in the company, especially if they all work off the same controlled file set. This setup builds consistency and accuracy out on the shop floor, which means less headaches for the designer.
Figure 1. Filling this out with the help of your shop team really makes life easier. (All images courtesy of the author.)
Next, let’s look at the basics of creating a sheet metal design. There are many ways of doing this.
A common favorite is sketching out the profile and using the Base Flange/Tab tool (see Figure 2) that is usually located first on the Sheet Metal ribbon. Drawing a simple profile and using the Base Flange/Tab tool will open up the options that can be used. To use the gauge tables that were discussed earlier, one must check the “Use gauge table” box that opens up all selectable shop-approved gauges with their corresponding radii and the K-factor (or bend allowance), so that there is no worry of forgetting or mistyping anything. At any stage, these parameters can be overridden with drop downs and checkboxes that will correspond with input boxes to adjust for special cases. Not shown (scroll down in Property Manager) is an auto relief setting that controls how corners and relief cuts are handled.
Figure 2. Options in basic Sheet Metal Base Flange/Tab.
This same tool can be used to make a flat piece of sheet metal that one would use to add edge flanges and other useful sheet metal features.
Edge Flange (see Figure 3) can be used to add an attached wall to any sheet metal body. This flange will inherit the radius and thickness parameters of the base flange. Of course, these can be overwritten if required. Designers can even select multiple edges that can be adjacent (by creating a mitered edge between the two) or located anywhere else on the same sheet metal body during this one operation. Designers can select flange positions that can move the flange location to the inside, outside, offset or to other less commonly used options that should be explored at your leisure.
One thing that often gets missed in the Edge Flange option is the ability to edit the flange profile. It doesn’t necessarily have to be a rectangle. It can be any shape that is required as long as it is a closed profile that connects to the original edge. Some small rules apply here that most designers will figure out quickly.
Figure 3. Edge Flange with profile adjusted.
Another thing that I would like to point out on the Edge Flange is the ability to change the angle to match another surface. This comes in handy when trying to match up awkward angles. There are some rules to this as well but, once learned, it does become invaluable in tricky spots. The result is usually very appealing and is difficult for many other CAD programs to execute. SOLIDWORKS users are lucky to have this feature. Designers should get to know it before they have to try too many workarounds.
The last thing I will touch on for the Edge Flange function is that designers should be encouraged to use a relatively new tool called the “Up to Edge and Merge” option that is located in the Flange Length dropdown. The main purpose of this is that if there are two (3D) parallel flanges that are not part of the same body (it can be the same body, but this process is rarely practical), you can use this tool to create a connecting flange between the two and create one sheet metal body. This is a good trick to keep in your back pocket.
Convert to Sheet Metal
This is a very helpful tool, especially for concept and prototype work. Basically, designers can build a bunch of flat-sided boxes with flat or curved sections. The designer can then select one face and add adjacent edges (within reason) to create a quick parametric sheet metal part. All the previously mentioned controls are available to the designer. The Split Line command (in the Surfaces ribbon), or inserting holes and cuts, can be used to control profiles of each side prior to the Convert to Sheet Metal function (see Figure 4).
Figure 4. Convert to sheet metal, with split line to control one flange.
As shown in Figure 4, the checkbox for “Keep body” has been enabled in order to reuse the same body in case the bottom and back side need to be utilized for a multibody sheet metal design.
Multi-body Sheet Metal
Designers are not limited to only one sheet metal part per file. One part can be used for a combination of mutliple sheet metal bodies, CNC parts and weldment parts. This is very smilar to how an assembly would be constructed. This is a huge timesaver in prototype design and can be used for production if configurations and design tables are used with careful strategy. The possibilities are nearly limitless but could require some well thought out and disciplined processes for this workflow to work.
Unfold and Fold
The Unfold and Fold comands are very powerful tools. One often needs to add fillets to miter corners in order to gain extra clearance during the manufacturing process—or to accomplish something that can’t be more easily done in the folded view. All the designer has to do is to select the Unfold option from the sheet metal ribbon, select a face that will be stationary and click the “Collect All Bends” option.
The part should unfold if it is made of sheet metal features and has a uniform thickness. After this operation, the designer should realize that this part is not manufacturable because of the two flanges that are highlighted (see Figure 5). In this case, a correction would need to be made. This correction can be achieved by first using the Convert to Sheet Metal function and then by adding a replacement flange to a new body (see Figure 6).
Figure 5. Unfolded sheet metal, before correction.
Figure 6. Folded sheet metal, with bottom added, after correction.
There are many other tools that can be used with this software. Miter Flange, Lofted-Bend, corner controls, Sheet Metal Gusset and Rip are all very common tools that can make life easier for the designer.
These tools are valuable for different aspects of design, and all of them are very user-friendly once the designer is aquainted with them.
About the Author
Ryan Reid is a CAD administrator, PLM enthusiast, designer, GD&T specialist, lead, lean philosophy supporter, Microsoft Office expert, 3D printing hobbyist and manufacturing-focused professional with 17 years of combined experience in those areas. Reid has accomplishments in all aspects of manufacturing engineering, from cradle to grave plastics/mold to structural, systems, process and change management design.