How to Merge Bodies in SOLIDWORKS

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When you work with plastic parts, molded components, or 3D-printable assemblies, you will often end up with more than one solid body in a single part file. At some point, you may want to turn those bodies into a single solid so you can simplify the model, prepare it for manufacturing, or export an STL. In SOLIDWORKS, the main tool for doing this is the Combine feature.

This article explains what “merging bodies” really means in SOLIDWORKS, shows two practical examples, and then walks through best practices, limitations, and troubleshooting tips.

What does “merging bodies” mean in SOLIDWORKS?

In a standard single-body part, every feature contributes to one continuous solid volume. In a multibody part, the part file contains two or more separate solid bodies listed in the Solid Bodies folder of the FeatureManager tree.

Merging bodies is essentially a Boolean operation between those bodies. The Combine command offers three operation types:

Add – merges all selected bodies into one body (union of volumes).
Subtract – removes material from a main body using one or more other bodies as cutting tools.
Common – keeps only the volume shared by all selected bodies; everything else is removed (intersection of volumes).

The key points to remember are:

Combine works on solid bodies only (not surface bodies).
All bodies must exist in the same part file.
You must have at least two solid bodies in the Solid Bodies folder for Combine to be available.

Let’s walk through this using a screw and housing example first, then a drone propeller example.

Example 1 – Merging a screw and housing with Combine (Add operation)

In this example, the part contains two bodies:

A flat head screw.
A plastic body that supports and locks the screw in place.

In the image below, you can see both bodies in the graphics area, and in the top-left of the FeatureManager tree you can see two bodies listed in the Solid Bodies folder (named Redondeo18 and Redondeo22). This tells us we are working with a multibody part.

Image 1: Multibody part and Solid Bodies folder in the FeatureManager tree

Accessing the Combine command

There are several ways to launch the Combine feature. The method shown in this tutorial uses the shortcut menu at the top-left of the SOLIDWORKS window:

Move your mouse to the top-left corner of SOLIDWORKS, where you see the SOLIDWORKS logo and a small arrow next to it.
Hover over the arrow to expand the shortcut menu.
From this menu, click Features to open a dropdown list of feature tools.
Scroll down the list and click Combine.

Once selected, the Combine PropertyManager appears on the left side of the screen.

Image 2: Accessing the Combine command from the SOLIDWORKS menu

Tip: The same command is also available via Insert > Features > Combine or from the Features toolbar, depending on your interface setup.

Using the Combine PropertyManager – Add operation

With the PropertyManager open, you can choose the type of operation and which bodies to include:

Under Operation Type, select Add. This tells SOLIDWORKS that you want to merge the volumes of the selected bodies into a single body.
In the Bodies to Combine box, select the two bodies (the screw and the plastic housing). You can pick them either in the graphics area or directly from the Solid Bodies folder in the tree.
Optionally, click Preview to see the result.
Click the green checkmark to confirm the Combine feature.

Image 3: Combine PropertyManager – Add operation with bodies selected

Once you confirm the operation, SOLIDWORKS creates a new feature in the tree named something like Combine1. The Solid Bodies folder now shows a single body instead of two, indicating that the screw and housing bodies have been merged into one continuous solid.

Image 4: Bodies selected for Combine > Add

Image 5: After Combine – the Solid Bodies folder contains a single merged body (Combine1)

This approach is very useful when you’ve modeled separate features as individual bodies for convenience, but your end goal is a single printed or machined component.

Example 2 – Combining a drone propeller and rod

Let’s look at another scenario: a drone model where a propeller is mounted on a rod. The propeller and the rod are two separate solid bodies in the same part file, and we want to combine them into one continuous body.

We will again use the Combine feature with the Add operation, this time accessed from the main menu.

Step-by-step workflow

In the FeatureManager tree, confirm you have a part with at least two solid bodies (the propeller and the rod).
Go to Insert on the main menu.
Click on Features to expand the list of feature tools.
From the Features dropdown, click on Combine.
As soon as you click Combine, the PropertyManager opens and shows fields for the operation type and body selection.
In the graphics area or the Solid Bodies folder, select the propeller and the rod as the bodies you want to include in the operation.
Under Operation Type, select Add, then click OK to finalize the combine operation.

After you confirm the feature:

A new Combine feature appears in the FeatureManager tree.
The previous two bodies (propeller and rod) are replaced by a single merged solid body.

These are the simple steps that need to be followed to combine components using the Add option. Finally, you can see the combined icon in the feature tree as shown below:

the new Combine feature indicating the merged result.

Other Combine operation types: Subtract and Common

Although this article focuses on merging bodies with the Add option, the other two operation types are extremely useful for design work:

Subtract

Subtract uses one or more bodies as cutting tools to remove material from a main body. Typical uses include:

Creating cavities using a “tool” body (e.g., subtracting a part shape from a mold block).
Cutting complex grooves or pockets where it is easier to model the cutting body than the final cavity.

In the PropertyManager:

Select Subtract.
Choose the Main Body (the body you want to keep).
Then choose one or more Bodies to Subtract (the cutting tools).

The overlapping volume is removed from the main body; the subtracted bodies themselves are removed from the Solid Bodies folder as part of the operation.

Common

Common keeps only the overlapping volume shared by all the selected bodies. Everything that is not common is removed. This is helpful when:

You want the intersection of parts (for example, for a gasket or contact volume).
You need to quickly derive the shared region between two shapes for analysis or reference geometry.

The workflow is similar: you select Common, pick all relevant bodies, and accept the preview. SOLIDWORKS returns a new body that represents only the intersecting volume.

Combine vs. “Merge result” and other tools

Combine is not the only way bodies can be merged in SOLIDWORKS. It helps to understand how it fits with other tools:

Merge result (Boss/Base features) – Features like Extruded Boss/Base, Revolve, and Loft have a Merge result checkbox. When this box is checked, any new material that touches an existing body is merged into that body. When it is unchecked, the feature creates a new solid body. Many users deliberately uncheck Merge result while modeling and only use Combine toward the end, when they are ready to finalize the shape.
Intersect – The Intersect feature (Insert > Features > Intersect) can do everything Combine does and more: it works with solids, surfaces, and planes, and lets you keep or remove multiple regions at once. It is very powerful, but also a bit more complex to set up.
Indent – For cases where you want to imprint or offset the shape of one body into another (for example, generating a clearance pocket), the Indent feature can be more direct than using Combine > Subtract plus extra steps.
Split and Save Bodies – If you have a multibody part and later decide you want individual part files, you can use Split or Save Bodies to create separate part documents from each body.

In short, Merge result controls whether a given feature creates a new body or merges into an existing one as it is built. Combine is a dedicated Boolean operation that works on bodies that already exist.

Best practices when merging bodies in SOLIDWORKS

Here are some practical tips that can save time and make your feature tree easier to manage:

Model flexibly, combine late. For complex shapes, it is often easier to keep bodies separate while you design, then add a Combine feature near the end of the tree to create the final merged body.
Name important bodies. Before combining, give key bodies descriptive names in the Solid Bodies folder (for example, “Housing”, “Screw”, “Insert”). This makes it easier to pick them in the PropertyManager.
Use configurations if needed. If you need both merged and unmerged versions of a model, create a configuration where the Combine feature is suppressed and another where it is unsuppressed.
For 3D printing, aim for one watertight body per printed piece. Many slicers expect a single continuous volume for each physical part. Use Combine > Add to ensure there are no internal overlaps or gaps in the model before exporting to STL.
Be careful with weldments. Weldment cut lists rely on separate bodies to calculate lengths and profiles correctly. Avoid using Combine on weldment bodies unless you are certain you do not need accurate cut-list data.

Limitations and potential drawbacks of merging bodies

Merging bodies with Combine is straightforward, but there are some important limitations and trade-offs to keep in mind:

Combine only works within one part file.
You cannot directly combine bodies from different part files. If you need that, insert one part into another (Insert > Part) or create a multibody part from an assembly, then use Combine on the resulting bodies.
Only solid bodies are supported.
Combine ignores surface bodies. If you have a mix of solids and surfaces (for example, because of how an assembly was saved as a part), you may have to thicken or knit surfaces into solids before Combine can be used.
Intersecting volume is required for Subtract/Common.
For the Subtract and Common operations, there must be an overlapping volume between the selected bodies. If they do not intersect, SOLIDWORKS will return an empty or failed result.
Feature tree becomes less granular.
Once bodies are merged, you lose the ability to select them as separate bodies for later operations like Body-Move/Copy, Delete/Keep Body, or body-level appearances. You can still edit upstream features, but some workflows become less flexible.
Weldment cut lists can be affected.
For weldments, combining structural members into one body can prevent SOLIDWORKS from calculating individual cut-list properties correctly. In many cases it is better to leave weldment bodies uncombined and use configurations or display states to control appearance.
Large, highly-detailed single bodies can impact performance.
Combine itself is usually very fast, but if you merge many patterned and filleted bodies into a single, extremely complex solid, rebuilds and downstream operations (like shelling or simulation meshing) can become heavier. Consider keeping logical sub-bodies separate if you do not strictly need a single merged solid.

Overall, Combine is “cheap” computationally, but the resulting model can still become heavy if you merge a lot of complicated geometry. Think about whether you truly need one body, or whether multiple bodies plus a clean feature structure would serve you better.

Troubleshooting – When Combine will not work

If the Combine feature is greyed out or fails to produce a result, check the following:

Is there a Solid Bodies folder?
If you do not see a Solid Bodies folder, you probably have a standard single-body part. Use features with Merge result unchecked or import additional parts to create multiple bodies first.
Do you really have multiple solid bodies?
Sometimes imported geometry or “assembly saved as part” workflows produce surface bodies instead of solid bodies. In that case, Combine will not be available. Try knitting or thickening surfaces into solids or re-importing with different options.
Are the bodies overlapping correctly?
For Subtract or Common operations, non-intersecting or barely-touching bodies can cause failures or an empty result. Adjust the geometry or check for zero-thickness conditions at the interface.
Is the geometry clean?
Small gaps, sliver faces, and self-intersections in imported models can cause Boolean operations to fail. Use tools like Import Diagnostics, Check, or clean up sketches and edges before trying Combine again.
Are you working in an assembly instead of a part?
The Combine feature works in part documents, not directly in assemblies. If you want to “merge” an assembly into a single body, consider saving the assembly as a part, using Tools > Make Multibody Part (in newer versions), or inserting assembly components into a part and then using Combine.

Summary

The Combine feature is the primary tool for merging solid bodies in a SOLIDWORKS part. It lets you:

Merge multiple bodies into one with the Add option.
Create cavities and tool bodies with Subtract.
Extract shared volumes with Common.

As long as you keep in mind the requirements (solid bodies, same part file) and the trade-offs (losing body-level flexibility, possible impact on weldment cut lists), Combine is a reliable way to clean up multibody parts and prepare them for manufacturing, analysis, or 3D printing.

Use the workflows shown in the screw-and-housing and drone examples as templates, and then adapt them to your own parts wherever you need a clean, single solid body as the final result.