How does SOLIDWORKS store configuration data? Does a part with ten configurations store ten “copies” of the model?
As we know from File Management class, SOLIDWORKS files are made up of generally three sections: header, instruction set, and database. The instruction set is often described as “the FeatureManager in binary format.” The results of the instruction set create the output, or database, which would include face/edge/vertex definitions, mapping, solid/surface body definitions, and so on: what we think of as “the model” that we see on screen.
When SOLIDWORKS saves a part that has more than one configuration, the database that is written to the file is the active one. It is possible that other databases representing other configurations are also written.
When switching between configurations, SOLIDWORKS keeps configuration data/databases for inactive configurations around. The idea is that switching back to a configuration is faster if the database is around in the background and “ready to go.” Any configurations that have a check in front of them indicate cached data for that configuration. Configurations that have a minus sign do not have cached data.
When you save a file, the cached data for any inactive configurations is written to that file. While this makes switching to these cached configurations as fast as possible, the file itself will be larger because of the “extra” (cached) data.
To ensure that only the current active configuration is written, go to Options, Systems Options, Performance, and activate “Purge cached configuration data.” When this is active, each time you save a document, data for inactive configurations is purged from the file and then the file is written. This would be the option you want if you are interested in keeping your files as trim as possible.
What about “disk icons” in the ConfigurationManager? A user can tell SOLIDWORKS to add a “save marker” to a configuration, which is then indicated by a disk icon in front of the configuration name. These configurations are always cached, whether they are active or not, and therefore also always written to the file when a save operation is performed, regardless of the “Purge active configuration data” switch.
Take the following model’s ConfigurationManager:
In the example above, Machined, Short is the active configuration. It’s “in color.”
Machined, Long is a currently cached configuration. It is not active, but it has a checkmark.
Forged, Short and Forged, Long are not active and are not cached. They have a minus sign.
Default is not active, but is has a save marker which means it is always cached. It has a disk icon and had to be put into that state by a user deliberately.
So, if the file above was saved, in the default scenario (“Purged cached configuration data” turned off), data for three configuration bodies would be saved: Machined Long (active), Machined, Short (currently cached) and Default (save marker/always cached)
If we turn on “Purge cached configuration data” and then perform a save, data for two configuration bodies would be saved: Machined, Long (active) and Default (save marker/always cached). The cached data for Machined, Short would be purged from the file and it would change from cached (check mark) to not cached (minus sign).
In the end, the choice is ours. Do we want to maximize performance when switching between configurations? If so, keep more cached data. Do we want to keep file sizes down? If so, purge cached data. Whatever we choose, it’s great that SOLIDWORKS gives us choices!
By: John Setzer, Training Coordinator