When creating solid models, you are no longer limited to creating them in a contiguous manner. This means that, when the features are created, they no longer need to form a single enclosed body. Modeling more than one non-continuous solid body is referred to as multi-body modeling. This ability to manipulate bodies with the same command set as features leads to more flexible design approaches.

Examples of typical applications of multi-body modeling in SolidWorks include

• bridging, which means you model the most important features first to drive the design and bridge a feature in between the bodies;
• local modeling, which means you model only one portion of the part;
• symmetry/patterning, which means you use multiple bodies for symmetrical or pattern shapes;
• combining, which means you derive part geometry based on Boolean functions to combine, subtract, and intersect multiple bodies.

Bridging. As shown in Figure 1, you can define two different bodies and use a loft feature to bridge the bodies to create a contiguous solid part. The design is driven from the two blue bodies, and the bridging features are based on the geometry created by the two original bodies. Without multi-body design, a surface, a reference, or assembly techniques would have to be used to create the contiguous solid model. Bridging allows the designer the freedom to model the part in a more logical manner.

Figure 1. For this object, a loft feature is used to bridge the bodies to create a contiguous solid part

Local Modeling. Let's say that you want one body that has a shell and another that doesn't. In a contiguous solid model, the entire part would be shelled. Here, after the shell is created, a feature connecting the two bodies can be designed to combine the two bodies. With this technique, the connecting feature between the two cups remains solid, as shown in Figure 2. Otherwise, the shell feature would not allow the connecting feature to remain solid.

Figure 2. With the local modeling technique, you can get the connecting feature between the two cups to remain solid.

When modeling in a multi-body environment, the scope of a feature (for instance, a fillet or shell) is limited to a single body. The shell in Figure 2 can only affect the body on the left. An additional feature can be created to the second body or the shell can be added to the combined feature. Multi-body part modeling offers the flexibility to choose based on the needs of the design and what is known.

Combine. The Combine function gives you the flexibility to modify different multiple bodies. This function allows for Boolean operations within the part. As shown in Figure 3, there are three different options: Add, for merging contiguous multiple bodies into one single body (the bodies must intersect to be merged); Subtract, for removing the volume defined by another body; and Common, for defining a feature by the shared volume between multiple bodies.

Figure 3.

To use the Combine feature, hold down the Ctrl key and select the bodies from the Solid Bodies folder within the Feature Manager design tree. After the features have been selected, press the right mouse button and select Combine.

When creating a new feature using the Extrude function, the option Merge Results is checked by default. If this option is checked, the feature remains part of the body that it contacts. In other words, SolidWorks will try to attach the new feature to an existing body, if possible. If the option is unchecked, or the feature is not continuous with an existing body, a new body will be formed. The new body will appear in the Solid Bodies folder using the feature name used to create the body.

Figure 4. The symmetry/patterning technique allows you to pattern or mirror a body to create the desired geometry.

Symmetry/Patterning. You can use the symmetry/patterning technique to pattern or mirror a body to create the geometry. As shown in Figure 4, there is one body that defines the original set of features, a mirrored feature of the body for the opposite end and a linear pattern of the original body for the geometry between the mirrored bodies.

The bodies are then combined to produce the final part. Without multi-body part modeling, creating this design would require the use of an assembly to create the part using the Join function. This can all be done inside a part file using multi-body features such as pattern or mirror.

Visual Clues
SolidWorks allows a graphical, flexible approach to displaying, identifying, creating, and modifying multi-body parts. Figure 5 shows a part comprising two solid bodies. The number shown in parentheses next to the Solid Bodies represents the number of solid bodies within the part. The Solid Bodies folder will display a body icon for each solid non-contiguous body within the part.

Figure 5. The number in the parentheses next to Solid Bodies displays the number of bodies within this multi-body part.

The default name of the body is the last feature added to the body. If you rename the body, that name will be retained. The advantage of renaming the bodies is to capture the purpose (or the design intent) of the body. The advantage of using the default name is to see the feature name related to that body.

A Final Note
While multi-body modeling is a powerful feature, at the end of the day, manufacturing and suppliers typically want a part that is a single-body part file. If a part is made up of more than one body, it should be an assembly made up of multiple parts. Don't use multi-body modeling to represent an assembly. When the design is complete, there should be only one body shown within the Solid Bodies folder. The Combine function can be used to merge the bodies.