Most of the times a sheet metal product does not consist of just one folded sheet. Due to its size or complexity it has to be divided into multiple sheets, which are then bolted or welded. A common way of building such an assembly is by modelling the different parts and add these to an assembly. A challenge could be the connectivity between the different components, because you want to avoid big gaps between the parts. Model changes could be difficult also, because the change of one part will also result in changing the other connected parts. In this tech blog I want to tell you more about the Convert to Sheet Metal tool and how this can assist you by building sheet metal assemblies the easy way. Let’s take a look at how to approach this step by step.
1. Creating the shape
Start with modelling the basic shape of the final assembly in a new part. Do this by using standard SOLIDWORKS features (Boss-Extrude, Lofted Boss, etc.). The advantage is that you can focus on the main shape of the product and you don’t need to think about any sheet metal parameters. You could end up with a part as in the image below.
2. Create the first sheet metal component
Now we have the main shape, we can start converting to sheet metal bodies. Select Convert to Sheet Metal (Sheet Metal toolbar) or go to Insert – Sheet Metal – Convert to Sheet Metal. Look at the image below for an example of the definition of this feature.
In the PropertyManager, under Sheet Metal Parameters, you define the sheet thickness and bend radius. Also, a Fixed Entity must be selected, this is the entity from which the other bends start. Under Bend Edges, you select all the bend edges (marked with a pink color). Once you select a bend edge the next flange will be recognized based on the main shape. Do not forget to select Keep body in this stage of the process, because this will keep the main shape visible, which is important to create the following sheet metal bodies. After you hit OK, you will end up with the main body and one sheet metal body wrapped around it.
3. Create the second sheet metal component
Because the main body is still visible, we now can use the other faces of this body to create additional sheet metal bodies. So, as you can see in the image below, we now create a second Convert to Sheet Metal feature.
Notice the red faces, which indicate the faces used by the first Convert to Sheet Metal feature. Also, the Keep body option is deselected, since we don’t need the main body after this feature. After you hit OK, you will end up with the two sheet metal bodies.
The result of the performed steps is shown in the following image:
As you can see in the image, the two bodies are perfectly connected. This is because we create the sheet metal bodies from one main body. A big advantage is when the main body dimensions change, that all the sheet metal bodies will change accordingly. So, you can change your design with minimum effort.
All the bodies are saved in one part. If this is not desired, then use the Save Bodies feature (Insert – Features – Save Bodies…). This exports the bodies to individual parts, which can be necessary for unique document numbering.
If you are going to work with the multibody sheet metal part, and you want to create separate drawings for each sheet metal body, then don’t forget to use the Select Bodies option. This option can be found in the Drawing View PropertyManager by selecting a view on the drawing.
This option makes it possible to select a single body in the multibody sheet metal part, so this will be displayed on the drawing.
Finally, if you want to quickly create DXF files for cutting purposes, then use File – Save As and select DXF as file type. In the menu that follows, you will see that the sheet metal bodies are already selected. At the bottom of the menu you can specify if you want to create separate DXF files for each sheet metal body. This is a big timesaver, because you can generate all the cutting files for an assembly at once.
Written by Martijn Visser, Elite Application Engineer