How to Fix Rebuild Errors in SOLIDWORKS?

Rebuild errors in SOLIDWORKS can feel dramatic: you change one sketch dimension, hit rebuild, and suddenly a clean FeatureManager Design Tree turns into a stack of red and yellow icons. The good news is that rebuild errors are usually logical—and fixable—once you troubleshoot them in the right order.

This guide explains what “rebuild” means, how to use the different rebuild commands, how to interpret rebuild errors vs warnings, and a practical workflow to repair a broken model (without creating new problems downstream).

What Is Rebuild in SOLIDWORKS?

SOLIDWORKS is a parametric, history-based modeler. That means your part or assembly is built from an ordered list of features (extrudes, cuts, fillets, patterns, mates, etc.). When you edit something—especially a sketch, a reference plane, or a feature definition—SOLIDWORKS may need to recalculate (“rebuild”) the model so the geometry reflects your changes.

When a change requires recalculation, SOLIDWORKS flags the model and specific items in the FeatureManager Design Tree with a rebuild symbol. Many users describe it as a “traffic light” icon because it resembles a small stoplight overlay.

If you see this rebuild icon beside the document name or a feature, it means the model is out of date relative to the latest edits. Rebuilding forces SOLIDWORKS to regenerate the geometry in the correct order (top-to-bottom in the tree) so the model matches the design intent.

How Do You Rebuild Your Model?

Most of the time, SOLIDWORKS rebuilds automatically as you work. When it doesn’t—or when you want to control the process—you can rebuild manually in several ways:

• Click the Rebuild icon on the Standard toolbar
• Use the menu: Edit > Rebuild
• Keyboard shortcut: Ctrl + B (standard rebuild)

Standard rebuild is designed to be fast: it typically rebuilds only what SOLIDWORKS believes needs updating since the last rebuild.

Rebuild vs Force Rebuild (and why both matter)

When you’re troubleshooting, knowing the rebuild “levels” helps you choose the right tool:

• Rebuild (Ctrl + B): Fast rebuild—typically recalculates only items that changed or are marked as needing rebuild.
• Force Rebuild (Ctrl + Q): Full rebuild—rebuilds the whole model feature-by-feature in sequence.
• Rebuild All Configurations (Ctrl + Shift + B): Rebuilds across configurations (useful when different configs suppress/unsuppress different features).
• Force Rebuild All Configurations (Ctrl + Shift + Q): The most thorough option when configuration-related issues are suspected.

Optional but powerful: “Verification on Rebuild”

If you’re dealing with stubborn geometry failures (especially surfaces, complex fillets, shells, or imported bodies), consider temporarily enabling Verification on Rebuild (sometimes described as advanced body/geometry checking). It increases the rigor of geometric validation during rebuilds—at the cost of performance. A common best practice is to enable it during troubleshooting or as part of a final “release check,” then disable it for day-to-day modeling if rebuilds become slow.

What Are Rebuild Errors?

Rebuild errors and warnings are problems SOLIDWORKS finds while regenerating the model. You’ll see icons on the document name (top of the FeatureManager tree) and on the specific features/sketches that caused the issue.

These are the two most important categories:

1. Rebuild Error: An icon with a down arrow in a red circle indicates an error exists in the model. Errors mean one or more features failed—so the resulting geometry is missing, incomplete, or invalid. Typically, the part/assembly name appears in red, and the failing feature often shows a red circle with an X. The feature text is also shown in red.

2. Rebuild Warning: A down arrow in a yellow triangle indicates a warning under the node. Warnings often mean missing references, dangling sketch relations, or something that may change behavior but does not completely prevent geometry creation. The part/assembly name may show in yellow. The specific feature can show a yellow triangle with an exclamation mark, and its text may appear in yellow.

Note: Warnings are commonly issued by sketches absorbed under a feature. You may need to expand the feature to find which sketch is warning. When you expand a feature, you may see the symbol change (because the warning is coming from an item underneath that feature node).

If a document or feature has both an error and a warning, the error icon is displayed.

How to Fix Rebuild Errors in SOLIDWORKS (Practical Workflow)

Most rebuild failures come from the parametric “parent/child” relationship: you edited, deleted, or replaced geometry used by later features, and downstream features no longer have valid references or conditions.

1) Decide what SOLIDWORKS should do when an error occurs

When a rebuild error occurs, SOLIDWORKS can either continue rebuilding (ignoring the error) or stop so you can repair immediately. If you’re diagnosing a broken model, stopping is usually the fastest path to a clean tree because it prevents one upstream failure from cascading into dozens of children.

When prompted, choose Stop and Repair if you want to fix issues as they occur, or Continue (Ignore Error) if you only want to see the full list of affected items.

You can also set this behavior in SOLIDWORKS options. Click the Settings icon on the Standard toolbar, then go to System Options > Messages/Errors/Warnings to control what happens when rebuild errors and warnings are encountered.

Tip: In general, keep this setting on Stop while troubleshooting. Because features rebuild in the order they were created, one failing parent feature can cause multiple child failures. Fixing the first “real” error near the top of the tree often clears many downstream warnings/errors automatically.

2) Fix from the top of the FeatureManager tree downward

Start with the first error you see (closest to the top). If you jump to a later fillet or pattern and “band-aid” it, you can waste time—because the real issue might be a missing sketch plane or changed profile near the beginning of the model.

3) Use the Rollback Bar to isolate the problem

The Rollback Bar lets you roll the model back to an earlier point in the FeatureManager history so features below the bar are temporarily removed from the model. This is extremely useful for debugging because it narrows the rebuild scope to the area you’re currently repairing.

Rollback Bar is present at the very end of the Feature Tree. Click and drag the bar to the feature that is below the one giving the error/warning, or right-click the feature just below the error and choose Rollback.

Use Roll to Previous to return the bar to its previous position and Roll To End to restore the full model.

Important: Don’t confuse the rollback bar with the Freeze Bar. Rollback is mainly a troubleshooting/history tool; freezing is specifically designed to exclude older features from rebuilds and speed up performance on large parts.

4) Use “What’s Wrong?” for clear error messaging

To see why a feature or sketch failed, right-click the problematic feature/sketch and select What’s Wrong? This is often the fastest way to find the missing reference, invalid condition, or sketch issue that caused the rebuild failure.

5) Use the top node to review all errors/warnings at once

To view a list of all errors and warnings, click the top node (the part/assembly name) in the FeatureManager Design Tree. Hover over items in the list to see tooltips explaining what is wrong, and click an item to jump to it in the tree.

Common SOLIDWORKS Rebuild Errors (and How to Fix Them)

Below are several rebuild errors and warnings you’ll see frequently, along with reliable ways to repair them.

1) Rebuild Warning: Dangling sketch entities (relations/dimensions)

This warning usually means one or more sketch relations or dimensions refer to geometry that no longer exists (for example: an edge was removed, a face changed ID, or a referenced sketch was deleted). In other words, the sketch is trying to stay constrained to something that’s gone.

• While editing the sketch, open Display/Delete Relations from the Sketch toolbar.

• You will notice dangling entities highlighted (often in yellow).
• Change the filter dropdown from All in this sketch to Dangling to list only problematic relations.
• Use Delete All to remove dangling relations, or repair them by replacing the missing references when possible.
• Exit the sketch and rebuild. If you deleted relations, re-add the necessary constraints and dimensions to restore design intent.

Watch out: deleting dangling relations can leave a sketch under-defined and may allow geometry to shift. When possible, repairing or replacing the reference is usually safer than deleting constraints blindly.

2) Rebuild Warning: The face or plane used for a sketch is missing

This occurs when the sketch plane reference (a plane, face, or surface) is no longer valid—commonly because the referenced face disappeared or changed due to upstream edits.

• Right-click the sketch and click Edit Sketch Plane.
• Select a new face/plane to host the sketch (the original if it still exists, or a replacement that matches your intent).

Prevention tip: When practical, sketch on stable reference geometry (default planes, named reference planes, axes) rather than “fragile” model faces that are likely to change later.

3) Rebuild Error: Missing feature conditions

This means the feature can’t solve because one or more required references or end conditions are missing (for example: an “Up to Surface” target no longer exists, a direction reference is missing, or a selected contour is no longer valid).

• Select the feature with the error and click Edit Feature.
• Re-define the missing inputs (end condition, direction, selected contours, reference surface/edge, etc.).

After redefining the feature, rebuild (Ctrl + B). If multiple children depend on it, consider forcing a rebuild (Ctrl + Q) once the parent feature is healthy.

4) Rebuild Error: Cut feature failed to cut the model

Common causes include:

• The sketch changed (profile no longer suitable to cut).
• The wrong Selected Contours were chosen.
• The cut no longer intersects the body (especially after upstream edits).
• In multibody parts, the wrong body is selected under Feature Scope.
• The cut direction is reversed or the end condition misses the solid.

Notice in the above image that under feature scope, the wrong body is selected (the selected body is highlighted in green), hence the rebuild error.

5) Rebuild Warning/Error: Missing edges/faces for fillet or chamfer

Fillets and chamfers are common “victims” of upstream edits. If an earlier feature changes topology, the original edge IDs that the fillet/chamfer referenced may no longer exist.

• Edit the fillet/chamfer feature and reselect the correct edges or faces.
• If some edges truly no longer exist, remove them from the selection set so the feature can solve.

6) Assembly rebuild errors: mate issues

In assemblies, rebuild errors often come from mates. If one component geometry changes, a mate selecting a face/edge may lose reference or become unsolvable.

• Start at the top of the mate list and fix the first mate showing an error.
• Edit the mate and reselect missing entities. If available, use SOLIDWORKS diagnostic tools such as MateXpert to guide mate repair.
• Prefer mating to stable references (planes, axes, mate reference geometry) when possible to reduce mate breakage during design iteration.

How to Prevent Rebuild Errors (So You Don’t Fight Them Later)

You can’t eliminate rebuild problems entirely in a parametric CAD workflow, but you can dramatically reduce them with a few habits:

Model with stable references

• Use default planes or named reference planes for sketches whenever you can.
• Be cautious with face/edge selections that are likely to change when upstream features are edited.

Avoid (or carefully manage) circular references

If your rebuild symbol “won’t go away” even after rebuilding, circular references can be one possible cause in certain workflows (especially with in-context assembly modeling or interdependent relations). If you suspect this, isolate and suppress suspected parent-child loops and rebuild to see what clears the rebuild indicator.

Use Feature Freeze for performance and stability on mature models

For complex parts, the Freeze Bar can reduce rebuild time by excluding older (frozen) features from rebuilds and protecting them from edits. This is especially useful when the “base” of a design is stable and you’re iterating only on later features.

Do a “release rebuild” check

Before sending a model to manufacturing, reuse, or PDM release, it’s a good practice to:

• Temporarily enable Verification on Rebuild if you suspect geometry quality issues.
• Run Ctrl + Q to force a complete rebuild and catch hidden failures.

Final Thoughts

There are many rebuild errors you may encounter in SOLIDWORKS, and listing every possible one would fill a textbook. But the underlying fix pattern is consistent: identify the first failure, understand the missing reference/condition, repair it at the source, and let the downstream features rebuild successfully.

In short: fix top-to-bottom, use “What’s Wrong?”, repair references instead of deleting blindly, and force rebuild (Ctrl + Q) when you need a full integrity check.