3D CAD modeling of sheet metal parts
Determining the design intent behind the part is a good place to start
The main variation in sheet metal modeling technique is when to let the 3D CAD system know that the part is to be treated as sheet metal. Columnist Gerald Davis walks us through three different ways to accomplish this.
The main variation in sheet metal modeling techniques is when to let the 3-D CAD system know that the part is to be treated as sheet metal. With the 3-D CAD tool that I use most often, I have three basic options: Create the part as sheet metal from the get-go, model a general solid and then declare it to be sheet metal, or import a solid from another CAD system and just add sheet metal features.
From the 3-D CAD software's point of view, a sheet metal model is just like any other solid model. Sheet metal models have some special limitations, however.
These limitations vary from one software package to another, so I'm going to write about the software that I know. The wall thickness must be uniform and equal throughout. Seams can be very close, but they must not touch. Bends cannot cross over each other.
With those limitations in mind, what is the best way to model a sheet metal part? Clearly, you want the model to be completed efficiently. You want the result to be visually realistic. You also want the part to be easy to fabricate.
The fuzzy aspect of how to model relates to the future. How will the model be used? How realistic does the model need to be? What is the confidence level about the design? What design features are most likely to change? Who is going to maintain the design?
Those fuzzy questions comprise the core of what I mean by design intent. Design intent is likely to change from project to project. Even within the same project, the design intent may change over time. Nonetheless, it is worth spending a few moments before launching into a modeling session to contemplate what the likely future of the part will be.
Our first example of a sheet metal part is a pedestal (see Figure 1a). We've been told that it will support a weight of less than 1 lb., but we're not sure what the tapered angle will be. In fact, all of the dimensions are likely to change, but we at least have a starting point.
To model this sheet metal pedestal with minimum fuss, I propose that we start with a simple, 3-D solid and then convert it into sheet metal. This will be a four-step process.
Step 1: The two-step. Modeling the solid will require two operations. First, sketch a rectangle 1.5 in. by 3.0 in.—or whatever favorite unit of measurement you want to use—and extrude it to a depth of 3.0 in. Second, create another extrusion that projects 1.4 in. and tapers at 45 degrees (see Figure 1b).
Step 2: The shell game. Next, you need to hollow out the solid so that it has uniform wall thickness. On my 3-D CAD system, I use a tool called "shell" that lets me select a thickness as well as faces to remove. Figure 1c shows the result: The interior has been hollowed out, leaving all of the walls 0.062 in. thick. Notice that the part does not really look like sheet metal yet. All of the seams are closed. No bend radii exist. The edges are oddly tapered.
Step 3: The ripper. Figure 1d shows where I've decided to create seams so the sheet metal part will be able to unfold. Other edges could have been selected instead, but this scheme seems pretty easy for manufacturing. My 3-D CAD system allows me to rip corners like this as a distinct operation or to combine it in a single step while defining the sheet metal, which is our next and final step.
Step 4: The bends. The final 3-D CAD operation is to insert the bends. This is done by selecting an arbitrary face that will remain stationary (everything else moves while processing the bends), an inside bend radius, a K-factor (to accurately predict the flat pattern), and the type of corner relief. In Figure 1e, I opted to "tear" the corners because all of my seams are butt-style. If this part were subject to vibration, it might be prudent to use round corner reliefs.
Figure 1f shows the flat pattern for this pedestal. The notes that indicate the bend direction can be a nice touch to help the press brake operators plan their work. It is easy to either include or exclude those notes from the generated flat pattern.
As a final thought, it took me three mouse clicks to modify the design to achieve the mess shown in Figure 2a shows our next modeling challenge. This is a basic aluminum sheet metal bracket. Our goal is to create a 3-D CAD model based on this design.
How might we get that done? We could use the same process that worked for making the pedestal, but that would not be my first choice. I'm kind of a lazy guy. What I think we should do instead is sketch a few lines that represent only one side of the bracket and then turn that sketch into sheet metal.
Four lines and five dimensions later, we have the sketch shown in Figure 2b. With another few mouse clicks, that sketch becomes a sheet metal part.
In Figure 2c you can see that the computer finished doing all of the detail work—inside and outside radii and all of the parallel lines that represent the material thickness. We merely specified a material thickness (0.100) and an inside bend radius (0.125). If you could have watched me do this, you would have seen me use a gauge table to make it easier to pick a standard thickness, radius, and K-factor.
Figure 2d is a screen capture of the final CAD model. I selected an aluminum material and a factory floor background. It looks very realistic on my computer screen.
The Imported Model
No, I'm not talking about French automobiles. As a final example of a 3-D CAD sheet metal modeling technique, I offer Figure 3a. On a printed page, this model looks just like any other CAD model. However, I created it by importing a STEP file. That STEP file could have been downloaded from a catalog Web site. The problem is that we want to modify this off-the-shelf part so that it fits our design goal. We need to add a bend.
Again, we could have re-created the model as a solid or as a sheet metal part, but that would require extra effort. All we need to do is sketch where we want the bend and then let the 3-D CAD system do the rest of the work (see Figure 3b).
If this were a tutorial on how to use a 3-D CAD system, I'd step you through the process of inserting bends (e.g., click on the "insert bends"icon, click on a face) in order to declare that the imported part is sheet metal. Then I'd show you how to make the sketch for the bend (e.g., click on a face, click on the "sketch"icon, click on an edge, click on the "offset"icon, select a distance). And, finally, I'd show you how to insert the bend (e.g., click on the "sketched bend"icon, click on a fixed face).
The result would appear as shown in Figure 3c. Without knowing or editing the geometry that defined the original model, we've added a sheet metal bend to the part. That can be pretty handy for quickly modeling components for finished product assembly!
In closing, I offer a bit of advice. Three-dimensional CAD software makes it relatively easy to model sheet metal parts. However, it requires training to master the software. Even with expert knowledge of how to design and using the CAD software, knowing the what and why of design requires additional study.
Engineers and designers who have worked in a shop and actually run machinery enjoy a greater advantage than less experienced colleagues in the industry, but that level of experience is somewhat unusual. More often than not, it requires teamwork to develop great designs. Engineering, CAD operation, and manufacturing all must cooperate and contribute to achieve success.
Gerald would love to have you send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to firstname.lastname@example.org.
The FABRICATOR is North America's leading magazine for the metal forming and fabricating industry. The magazine delivers the news, technical articles, and case histories that enable fabricators to do their jobs more efficiently. The FABRICATOR has served the industry since 1971.