To use the SOLIDWORKS Split tool, open a part, choose Insert > Features > Split, select a plane, planar face, or surface body that crosses the part, and click Cut Part. Then keep the resulting bodies you need; use Save Bodies if you want them as separate part files.
What the Split tool does
Split is a part feature that divides a solid body into two or more separate solid bodies. It uses one or more trimming tools—such as a plane or surface—to define where the cut occurs. The result is a multibody part: the bodies remain in one part document unless you save them out as individual files.
This distinction matters. A split does not automatically create separate part documents or an assembly. It changes the part’s feature history and creates body-level geometry that you can keep, edit, save, or use in later features. The split feature is useful when a design needs to be modeled as one continuous shape initially, then separated into components at a later stage.
The command is different from Split Line. Split Line projects or intersects a sketch or other geometry to divide faces for tasks such as applying appearances, creating surface boundaries, or defining regions. It does not normally separate a solid into multiple solid bodies. Use Split when you need distinct bodies; use Split Line when you need boundaries on faces.
Prepare the part and trimming tool
Before opening Split, decide where the division should be and create geometry that crosses the part at that location. A reference plane is often the simplest trimming tool for a straight, predictable division. You can create one from the Reference Geometry tools, or use an existing plane. A surface body or planar face can also serve as a trimming tool when its shape or position better matches the intended separation.
The trimming tool must intersect the solid in a way that produces the sections you want. A plane that stops short of the model, or a surface that touches the part without cutting through it, may produce no usable split. If the intended cut is angled, create or position the plane at the required angle first. For a more complex boundary, construct a suitable surface and check that it passes through the entire region to be divided.
- Save the part before major changes, especially if it has a long feature history.
- Inspect the model from more than one direction so you can confirm the tool crosses the intended area.
- Choose the tool based on the desired cut: a plane for a flat division, or a surface for a shaped division.
- Check whether the cut will leave each intended result as a valid solid body rather than a zero-thickness or disconnected sliver.
How to split a part step by step
- Open the part document and make sure the feature or reference geometry you intend to use is visible and available for selection.
- Choose Insert > Features > Split. SOLIDWORKS opens the Split PropertyManager.
- In Trim Tools, select the plane, planar face, or surface body that will cut the part. If the model needs multiple cutting boundaries, add the appropriate tools where the interface allows them.
- Click Cut Part to calculate the division. Review the preview and the entries under Resulting Bodies. If the preview is wrong, cancel or adjust the trim tool before accepting the feature.
- Select the bodies you want to retain. The list lets you inspect the outcomes produced by the cut; body names may be generic until you rename them.
- Confirm the feature with the green check mark. The resulting bodies are now part of the multibody model and appear in the Solid Bodies folder when that folder is shown in the FeatureManager design tree.
The exact PropertyManager layout can vary slightly between SOLIDWORKS releases, but the essential sequence is the same: choose trimming geometry, calculate the cut, inspect the resulting bodies, and confirm. Do not accept the feature solely because the preview looks plausible from one angle. Rotate the model and verify that the division follows the intended boundary on every side.
Keep, rename, and save the resulting bodies
Keeping bodies and saving bodies are related but separate decisions. Keeping a body preserves it inside the current part document. Saving bodies creates separate part files from selected bodies, which is helpful when each section needs its own part number, drawing, manufacturing process, or assembly position.
To create separate files, use the Save Bodies option from the Split workflow or the corresponding Save Bodies command available for the multibody part. In the Save Bodies interface, specify file names and locations for the bodies you want to export. SOLIDWORKS can also create an assembly from the saved bodies when that option is available in the dialog. Review the file paths and names before confirming; the output files are separate documents, so they need to be managed alongside the original part.
Clear names make a multibody model easier to maintain. Rename bodies in the Solid Bodies folder to describe their role, such as UpperHousing and LowerHousing, rather than relying on default names like Body1. If you later edit the split position, check the saved files and any assembly references to ensure they still represent the intended design. Saving bodies does not remove the need to manage the original master part and its dependent documents.
Practical examples and workflow choices
Imagine a molded enclosure modeled as a single solid. A plane through its mid-height can divide it into a lid and base. After using Split, keep both bodies and save them as separate part files if they will be produced or documented independently. If the enclosure has a stepped seam, a surface shaped to follow that seam may be a better trimming tool than a flat plane.
Another common use is dividing a large model into manageable sections. For example, a long cover might be split into two pieces at a planned joint so that each section can be manufactured, handled, or assembled separately. In this situation, place the split where the design can accommodate a real joint. A geometric split alone does not add fasteners, clearance, locating features, or a manufacturing allowance; those details need to be designed separately.
For a simple straight cut, a plane is usually easier to edit and understand than a complex surface. For a curved or irregular interface, a surface tool can describe a non-planar boundary, but it may take more work to build and maintain. Choose the least complicated tool that accurately represents the design intent. A clear, stable reference makes later edits less likely to break the split feature.
Split compared with other SOLIDWORKS methods
Split versus Cut-Extrude: Cut-Extrude removes material according to a sketch and feature direction or end condition. It is a natural choice when the goal is to remove a portion of a part and leave one remaining body. Split is more appropriate when the goal is to create multiple bodies from the material on both sides of a division and then manage those bodies individually.
Split versus Split Line: Split creates separate bodies from a solid when the trimming geometry divides it. Split Line creates edges that partition faces; it is not a substitute for separating the solid into components. A visible line on a face does not by itself mean the part contains multiple bodies.
Split versus Save Bodies: Split defines the geometric division. Save Bodies writes selected resulting bodies to separate part files and may support creating an assembly. If the model already contains multiple bodies, you may be able to save them without adding a new Split feature.
Common problems and how to fix them
- No resulting body appears: Confirm the trimming tool actually intersects the solid. Extend or reposition a surface, or move the plane so it passes through the full region you intend to divide.
- The preview shows the wrong number of sections: Review the tool’s position and shape. One cutting tool does not always create only two bodies; a part’s geometry and the number of intersections determine the resulting regions.
- A thin sliver or invalid result appears: The tool may pass very close to an edge, vertex, or existing face. Adjust its position slightly or revise the surrounding geometry to avoid tiny or zero-thickness regions.
- The feature fails after an upstream edit: A plane or surface may have moved, disappeared, or stopped intersecting the solid. Edit Split, reselect a valid trimming tool if necessary, and inspect the preview before accepting the change.
- A saved part does not update as expected: Check the relationship between the master part, saved body files, and any assembly. Keep the source part and generated files organized, and verify that the saved results reflect the current model revision.
When troubleshooting, suppressing or editing nearby features can help identify whether the problem is the trimming tool or the solid’s existing geometry. If the cut is intended to separate a very complex model, consider splitting the feature tree into simpler stages rather than trying to create every division at once.
Modeling considerations after the split
A split changes the body structure, not the practical requirements of the finished design. If the bodies will become separate physical parts, check for clearance, mating faces, fastening, alignment, and manufacturability. A mathematically exact split can leave coincident faces that are unsuitable for an assembly fit if the design requires a gap or allowance. Add those details deliberately instead of assuming Split creates them.
Feature order also affects editability. Placing a split late in the feature tree can make it a clear final division of a completed shape, while placing it earlier may let later features act on the separate bodies. The right order depends on whether subsequent operations should affect every body or only selected ones. After changing the order, inspect the feature tree and rebuild the model to confirm downstream features still reference the intended geometry.
Frequently Asked Questions
Can the SOLIDWORKS Split tool create more than two bodies?
Yes. The number of resulting bodies depends on the solid’s shape and how the trimming geometry intersects it. Inspect the Resulting Bodies list and preview rather than assuming each trim produces exactly two pieces.
Does Split automatically make separate part files?
No. Split creates bodies within the part document. Use Save Bodies to create separate part files from the bodies you choose, and create or manage an assembly if the components need to be assembled.
Can I split a part with a curved boundary?
Yes, when you create a suitable surface body that intersects the part along the desired boundary. A plane is simpler for a flat cut; a surface is useful when the division needs a more complex shape.
Why is Split Line not separating my part?
Split Line divides faces by creating edges; it does not generally create separate solid bodies. Use Insert > Features > Split when you need to divide the solid into bodies.
Can I change the split after creating it?
Yes. Edit the Split feature in the FeatureManager design tree and adjust its trimming tool or body selections. If the edit changes the saved geometry, also review any separately saved body files and assemblies that depend on it.
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