Sooner or later, an error shows up while you are editing a model in SOLIDWORKS. It usually looks like one of these:
- "A feature failed."
- "The sketch turned red."
- "The shape of the model looks off, and I am not sure why."
In that moment, you may wonder, "Where do I even start fixing this?"
If you leave the error alone, or patch it up on the spot, it tends to come back later as a lot of rework.
SOLIDWORKS has tools that help you find the cause of an error and fix it safely.
This article explains three of them for beginners: Force Rebuild, SketchXpert, and the Rollback Bar.
Once you know these three, errors become much less scary. If error messages make you nervous, I recommend reading on.
A Quick Fix to Try Early: Force Rebuild (Ctrl + Q)
When an error appears, a Force Rebuild is one of the first things worth trying.
You run it with Ctrl + Q.
- You changed a dimension or a mate, but the shape or position of the model did not change.
- A file that opened fine before suddenly shows an error.
- You did nothing unusual, and an error appears anyway.
To keep things fast, SOLIDWORKS normally recalculates only the parts of the model that changed.
Because of that, the model’s internal calculation results can, in rare cases, become inconsistent, and a normal rebuild does not always clear it up.
A Force Rebuild recalculates every feature from the top of the FeatureManager design tree (the list of features on the left side of the screen), which gives the model a fresh start.

When a model is complicated, a Force Rebuild alone can make the error disappear more often than you might expect.
| Item | Rebuild (traffic-light icon, Ctrl + B) | Force Rebuild (Ctrl + Q) |
|---|---|---|
| What is recalculated | Only what changed | Every feature, from the top |
| Effect | Reflects small changes | Resets the calculation and recalculates it from scratch |
| How to run it | Click the traffic-light icon, or press Ctrl + B | Hold Ctrl and press Q |
A Force Rebuild recalculates the whole model, so on a complex model it can take a while. On a small model it is quick to try. On a large one, you may prefer to try a normal rebuild first and use Force Rebuild when that does not help.
If a document has several configurations (variations of the same model), there is also Force Rebuild All Configurations (Ctrl + Shift + Q).
For Sketch Errors: SketchXpert
When a sketch has an error, there is a feature that helps a great deal. It is called SketchXpert.
Red or yellow lines in a sketch usually mean that it is over defined: it has too many dimensions or relations (geometric constraints such as Horizontal or Coincident), and some of them contradict each other.
It is not always easy to tell which one is causing the problem just by looking at it.
How to Use SketchXpert
- In the sketch with the error, look at the status bar at the bottom of the window. You should see Over Defined in red. Click it.
- SketchXpert opens. Click the Diagnose button.
- SketchXpert proposes several possible solutions. Use the arrow buttons to step through them, and pick the one that gives the shape you intended. The graphics area updates to show each solution.
- Click Accept to apply the solution.
The relations or dimensions that conflict with the shape you chose are removed, and the error should be resolved. Because SketchXpert removes constraints, check that the result still matches your design intent.
Seeing Every Relation: Display/Delete Relations
Another command worth knowing is Display/Delete Relations.
Open the sketch in edit mode and choose Display/Delete Relations from the Sketch tab of the CommandManager.
It lists the relations used in the sketch, and its Filter lets you narrow the list.
This way you can see at a glance which relation is the problem, and delete it right there.
- The sketch is shown in red or yellow.
- You cannot tell at a glance which relation is causing the error.
- You want to move a sketch line, but it is fully defined and will not move. (Display/Delete Relations lets you find and remove the relation that is holding it.)

Keeping every sketch Fully Defined (black) is the basic habit behind stable, error-free models.
Use these tools to keep your sketches clean.
For Feature Errors: The Rollback Bar
A SOLIDWORKS model is built from a history: features stacked one on top of another.
When one feature fails, the features after it often fail in a chain.
At the very bottom of the FeatureManager design tree is the Rollback Bar, a blue bar. If you drag it up, you can temporarily take the model back to an earlier point in its history.
The features below the bar are rolled back (they appear grayed out), so the model shows only what was built up to that point.
To go back to the present, drag the bar to the bottom again, or right-click a feature and choose Roll To End.
- A feature shows a yellow or red warning, but you cannot tell which change caused it.
- You want to edit a feature in the middle of the tree, but you are afraid of breaking the features after it.
- You want to check how the model was built.
Debugging with the Rollback Bar has two benefits:
- Isolating the error: Move the bar back to just before the feature that fails. The model then shows only what was built before the error, so you can check the earlier features one by one and find the cause.
- Editing safely: To edit a feature in the middle of the tree, move the bar to just after that feature. After you edit it, you can check right away whether the features that follow still work.

Think of the Rollback Bar as a time machine for your model.
When an error appears, go back in time, find the cause, fix it, and then return to the present.
Summary
This article introduced three commands to try when an error appears.
Together, they can make debugging and editing a model easier.
| Command | What it helps with |
|---|---|
| Force Rebuild (Ctrl + Q) | Inconsistent calculation results in the model |
| SketchXpert | Over defined sketches (conflicting relations and dimensions) |
| Rollback Bar | Failed features, and edits in the middle of the tree |
If you get comfortable with these commands, you can work through errors and keep your models stable and clean.
The next time you hit trouble, give these three a try!

Once you can deal with errors on your own, you are no longer held back by them, and you can edit with confidence.
Thank you for reading to the end.











