If you haven’t used the SOLIDWORKS freeze bar before, here’s how you can become a little “cooler”. This functionality was added in SOLIDWORKS 2012 and it’s a great way to reduce the rebuild times of your complex part files when working on them and avoid editing the wrong features.
You may not have noticed this tool as it’s not enabled by default. Browsing to Tools > Options > System Options tab > General allows you to ‘Enable Freeze Bar’.
This will add an orange bar just below the file name in the FeatureManager Design Tree. It works in a similar to the Rollback bar at the bottom of the tree. The freeze bar can be dragged anywhere up and down the Design Tree. Any features above the bar will be “frozen”.
SOLIDWORKS Freeze Bar Example
In this example, opening the Feature Statistics from the Evaluate tab of the CommandManager shows there are 83 features taking a total of 2.70 seconds to rebuild the part file.
You can right-click on any feature in the tree and choose to “Freeze” which will move the Freeze Bar after this feature. All features above will also be frozen. Any frozen features cannot be edited or deleted.
With many of the features in the frozen state (greyed out with a lock symbol), the rebuild time is reduced to only 0.86 seconds. You can see how this will save time on models with rebuild-intensive features.
And to thaw out those frozen features, simply drag the Freeze Bar up, or right-click on the bar itself and choose to ‘Roll to Top (Unfreeze All)’.
NOTE: Frozen features that have become out-of-date (due to being in an assembly with references) will have a rebuild indicator. You can right-click on the Freeze Bar and choose ‘Update Frozen Features’. This will update the out-of-date features and return them to the frozen state.