In CATIA, Split is a feature that divides geometry using a selected cutting element and lets you keep the side you want. In Part Design it can remove one side of a solid; in Generative Shape Design it can trim a surface or curve, so the exact result depends on the workbench and the element selected.
What the Split option does
Split is a geometry operation, not simply a command to make a visible line across an object. It uses one element as a boundary to cut another. The result is typically a portion of the original element, with the unwanted side discarded. For a solid, this changes the shape of the part; for a surface or curve, it changes the extent of that geometry.
A useful mental model is a sheet of paper passing through a block. The sheet is the splitting element, and the block is the geometry being cut. CATIA calculates which regions lie on either side of the sheet. You then choose the side to retain. A plane is a common cutting element, but a suitable surface or face can also be used, depending on the command and the geometry.
The command is especially useful when a part needs a clean, controlled cut that follows a designed boundary. It is not the same as hiding half of a model, making a section view, or dividing a body into two separately managed solids. Those actions have different purposes and may require other tools.
Two common contexts: Part Design and Generative Shape Design
CATIA has Split operations in more than one workbench. The word is the same, but the object being edited and the result differ. In CATIA V5, the Part Design version is used for solid modeling, while Generative Shape Design (GSD) provides operations for wireframe and surface geometry. Menus and toolbar placement can vary with release, workbench configuration, and customization.
- Part Design: Split a solid body with a plane, surface, or usable face and retain one side. The result is a modified solid feature in the part’s history.
- Generative Shape Design: Split a surface or curve with another geometric element. This is often part of surface trimming, boundary creation, or preparing geometry for later operations.
Before choosing the command, check what is selected in the specification tree and which workbench is active. If the target is a solid body, use the solid-modeling workflow. If the target is a surface or curve, use the relevant GSD operation. A tutorial for one workbench may show a dialog or icon that does not match the other.
How to split a solid in Part Design
In CATIA V5 Part Design, the Split command is generally found among the surface-based features, commonly through Insert > Surface-Based Features > Split. The exact interface can differ in other CATIA versions. The basic sequence is to choose the solid to modify, select a cutting element, preview the result, and retain the required side.
- Prepare the cutting element. Create or identify a plane, surface, or face that crosses the solid where the cut is required. A plane is often easiest to position and adjust.
- Start Split. Invoke the Part Design Split command while working with the intended body. If CATIA prompts for a target or cutting element, select the correct geometry in the viewport or specification tree.
- Check the preview. CATIA displays the proposed result when the selected element intersects the solid. Inspect the cut location and the portion that will remain.
- Reverse the retained side if needed. Use the direction or side-reversal control in the dialog if the preview keeps the wrong portion. The control may be presented as an arrow, an opposite-side option, or a related selection control depending on the release.
- Confirm and update. Accept the operation, then check the resulting solid and the specification tree. If the feature does not update, examine the cutting element and any upstream dependencies.
For example, imagine a housing that must be shortened along an angled face. Create a plane at the required angle and position it through the housing, then split the solid and retain the side containing the mounting features. If the preview removes the mounting side instead, reverse the retained side rather than rebuilding the plane. The plane controls where the cut lies; the side choice controls which portion survives.
Preparing a reliable cutting element
A split depends on a valid intersection. A plane that sits entirely outside the solid cannot divide it, and a surface that only touches the solid at a tangent may not produce the clean two-sided result you expect. Position the cutter so it passes through the intended region with enough extent to cross the target geometry. When using a bounded surface, confirm that its boundaries reach across the whole area to be cut.
Before running the feature, consider these checks:
- Intersection: Does the cutter actually cross the target, rather than merely approach or touch it?
- Orientation: Is the plane or surface positioned at the intended angle and offset?
- Extent: Does a finite surface cover the complete cut region? Extend or enlarge it if the cut stops short.
- Selection: Have you selected the intended body, face, or surface rather than a nearby reference element?
- Model stability: Is the cutter based on references that will remain valid if upstream geometry changes?
When an existing face is used as the cutter, remember that it moves or disappears if the feature that created it changes. A dedicated reference plane or purpose-built surface can be more robust for a design that is likely to be revised. This is not a rule that every model must follow; it is a way to reduce fragile references in a complicated feature tree.
What happens to the model and feature tree
Part Design is parametric: a Split feature records its inputs in the model history rather than replacing the part with an uneditable picture. The feature typically appears in the specification tree, where you can reopen its definition, change its references, or reverse the retained side. Later features depend on the resulting shape, so changing the plane or surface can also affect downstream operations.
This dependency is useful, but it has consequences. Moving a cutting plane may cause a later hole, fillet, or pocket to lose its reference if that feature depended on an edge that the split removed or reshaped. After editing a split, update the part and inspect later features for errors. If a downstream feature fails, the split may still be valid; the failure can arise because the later feature’s reference no longer exists in the same form.
A split normally leaves one selected portion as the result of that feature. If the design requires two separately editable solid bodies, do not assume that Split automatically creates two independent parts. Consider the intended body structure and use the appropriate body-management or Boolean workflow for the design. The distinction matters for downstream features, manufacturing handoff, and how the model is organized.
Split compared with Trim, Pocket, and section tools
These commands can look similar because each can make geometry appear cut, but their roles differ. Choose based on the operation you want, not just the visual outcome.
- Split: Uses an existing geometric element as the boundary and keeps a chosen side of the target. It is a natural choice when the cut should follow a plane or surface.
- Pocket: Removes material from a solid using a sketch-based profile and specified limits. It suits a designed recess or cutout, rather than a cut defined by an arbitrary surface.
- Trim in GSD: Commonly trims or intersects wireframe and surface elements, retaining selected regions. It is aimed at surface construction, not the same solid-body operation as Part Design Split.
- Section view: Displays a cut through a model for inspection or drawing communication without changing the modeled solid. Use a section when you need to see inside, not permanently remove material.
A common misconception is that Split always creates two final pieces. In many standard workflows, the feature keeps one side and discards the other from the resulting element. If both sides are needed as separate geometry, check the options available in the specific command and release, or plan a workflow that explicitly creates and manages both results.
Common problems and how to diagnose them
If Split fails or produces an unexpected result, begin with the geometry rather than repeatedly clicking the command. The most frequent causes are an incorrect target selection, a cutter that does not intersect the target, an unsuitable or incomplete surface, or choosing the wrong side in the preview.
- No valid result: Verify that the cutting element crosses the solid or surface. Move the plane or extend the surface, then update.
- The wrong portion remains: Reverse the side in the Split definition and inspect the preview before confirming.
- Only part of the object is cut: Check whether the cutter is bounded and whether its limits cover the entire target region.
- Update error after a design change: Review the cutter’s references and features downstream of Split. A moved face or deleted edge may have invalidated a dependency.
- It seems to cut nothing: Confirm that the selected element is the target, not the cutter, and that you are using the Split command for the active workbench.
CATIA’s preview and error messages are useful, but they do not replace checking the specification tree. Select the feature and inspect its inputs, then isolate or hide nearby geometry if selection is ambiguous. In a complex part, rename important planes and surfaces with descriptive labels so the intended cutter is easier to identify later.
Choosing the right workflow for an example
Suppose you are shaping a molded cover and need to remove everything above a sloping parting boundary. If the cover is a solid and the boundary is represented by a plane or surface, Part Design Split is a direct approach: define the cutter, preview the retained side, and confirm. If you are instead trimming two overlapping exterior surfaces to create a clean junction before building a solid, the GSD surface workflow is more appropriate.
For a rectangular opening through a bracket, a Pocket based on a sketch may communicate design intent more clearly than splitting the whole solid with a surface. For a drawing that merely needs to show the bracket’s interior, use a section view. These examples illustrate the key question: are you changing a solid, trimming surface geometry, removing material according to a sketch, or only displaying a cut? Answering that first usually identifies the right tool.
Frequently Asked Questions
Where is the Split command in CATIA?
In CATIA V5 Part Design, it is commonly available under Insert > Surface-Based Features > Split. GSD has its own Split operation for surface or wireframe geometry. Toolbar placement and menu names can vary by version and setup.
Can I use a plane to split a CATIA solid?
Yes. A plane is a common splitting element for a Part Design solid, provided it intersects the solid. Use the preview and side-reversal control to keep the intended portion.
Why does Split keep the wrong side?
The feature is retaining the opposite region from the one you intended. Reverse the side in the Split dialog or use its direction control, then confirm that the preview shows the desired result.
Does Split create two separate bodies?
Do not assume so. The usual result is the selected side of the target as a feature in the current modeling context. If both resulting portions are required as separate solids, use a workflow and body structure that explicitly preserves both.
What is the difference between Split and Trim in CATIA?
Part Design Split modifies a solid using a cutting element. GSD Trim is generally used to combine or trim surface geometry by selecting the regions to keep. The appropriate command depends on whether the target is a solid or a surface construction.
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