Rebuild Types and How They Work
SOLIDWORKS Rebuild Types and How They Work
After changes are made to a model, a rebuild is required to update features and check for errors. There are various rebuild tools available for parts, assemblies, drawings, and sketches.
List of Rebuild Commands:
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Icon
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Name
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Description
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|---|---|---|
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Rebuild
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Rebuilds changed features.
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Rebuild All Configurations
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Rebuilds changed features in all configurations.
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Force Rebuild
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Rebuilds all features.
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Force Rebuild All Configurations
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Rebuilds all features in all configurations.
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Force Rebuild Top Level Assembly
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Rebuilds all features in the top-level assembly.
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Note, forced rebuilds can take significantly more time, depending on model complexity.
Rebuild Keyboard Shortcuts:
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Icon
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Name
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Part
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Assembly
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Drawing
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Sketch
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|---|---|---|---|---|---|
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Rebuild
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Ctrl + B
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Ctrl + B
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Ctrl + B
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Ctrl + B
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Rebuild All Configurations
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Ctrl + Shift + B
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Ctrl + Shift + B
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Ctrl + Shift + B
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|
|
Force Rebuild
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Ctrl + Q
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Ctrl + Q
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Ctrl + Q
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Force Rebuild All Configurations
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Ctrl + Shift + Q
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Ctrl + Shift + Q
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Ctrl + Shift + Q
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|
|
Force Rebuild Top Level Assembly
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Ctrl + Q
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|
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Note, the standard Rebuild (Ctrl + B) command can be found on the standard toolbar or the Edit menu. Rebuild All Configurations will also be available in the Edit menu if there are configurations in the model.
Force Rebuild Command
Since the standard Rebuild commands only rebuild the features which have changed since the last save, the system may not recognize a warning or error in other features which may be affected by the changes. A Force Rebuild command (Ctrl + Q or Ctrl + Shift + Q) rebuilds every single feature in the FeatureManager Design Tree and as a result refreshes the entire database of geometry.
Force Rebuilds do not have an icon or menu item choice to execute the command. The only method to run a Force Rebuild is by using the keyboard shortcut combinations.
Configuration Rebuilds
For part and assembly files with more than one configuration, the rebuild status is displayed as a checkmark in front of the configurations. A green check indicates the configuration has been rebuilt successfully and a red X indicates the configuration has rebuild errors. You can switch to the FeatureManager Design Tree to diagnose the errors.
- The image on the LEFT shows configuration named 100C has been rebuilt successfully as indicated by the green check. All other configurations display a dash to indicate the configuration has not been rebuilt since the last changes.
- The image on the RIGHT shows that all configurations have been rebuilt successfully (all display a check icon).
You can also add a ‘Rebuild on Save Mark’ to all or only specific configurations. The system will then rebuild the specified configurations each time the file is saved. A disk icon displays in front of the configurations with the option Rebuild on Save Mark included. Note this will increase the save time as each configuration is rebuild individually. With multiple configurations all being rebuilt with all required information, it may also increase file size. Appropriate testing should be performed to determine how this affects your specific design. You may consider adding the Rebuild on Save Mark to specific configurations you know may be affected by changes while designing.
Verification on Rebuild
Generally, a standard Rebuild or Force Rebuild will update the model and check for errors with any changes made. If you’re working with complex surface or sheet metal models, there is one additional option which may uncover additional rebuild issues.
By default, rebuilds check every new or changed feature against only adjacent faces and edges. This allows for faster rebuild times and will find issues in most models. When working with complex models and surfaces, it’s a good idea to perform a thorough error check to ensure all features rebuild without errors.
Tools > Options> System Options > Performance, enabling ‘Verification on Rebuild (enable advanced body checking)’ will force the model to check new or changed features against all faces and edges of the model. This will decrease performance, so this option should be disabled after the rebuild is complete. If this check is not performed, it is possible that any problems with geometry may not show up until the model is exported to another format for use by another CAD or CAM application.
Technical Support
If you have any questions regarding the SOLIDWORKS search routine or missing file references when opening files, feel free to reach out to MLC CAD Systems technical support. MLC CAD Systems can also provide services to assist with reviewing and possibly repairing/recovering larger data sets if file references are incorrect or missing.