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SOLIDWORKS 2014- Configuration Based Weldment Profiles

Monday February 10, 2014 at 11:42am
The weldments feature set in SOLIDWORKS is a powerful way of generating geometry off the back of standard profiles- whether this be tube, box section or channels. We have always had to rely on creating each profile variant as a separate profile sketch which is then saved to be used for the Structural Member feature. 
Looking back at the 2013 downloadable profiles, the ANSI standard has 233 files to download, manage and customise! Now in 2014 SOLIDWORKS has streamlined this process, harnessing the power of configurations. The logical step has now allowed users to create profiles on a configuration basis, but still maintain and use the older profiles and methodology. The benefit here is that you can have one file representing the profile shape, which then has all of the size variants built in through configurations. The obvious advantage is far fewer documents on the machine to manage, but also if custom properties need adding, you now only have to add the property to the single source file. The final, and arguably most useful advantage of this method is when changing profiles. It may be typical that you wish to go from a 100mm to a 150mm square tube for example- in the past because you were changing the profile document, it may have meant that downstream features linked to the original profile generated errors- this is because the ID of the edge was no longer found. With configurations, the size variants are all built off the same sketch, and therefore lines would have the same ID reference making swapping them over error free.
So here is a snap shot of the listed configurations, generated by an excel based design table (note this isn't a requirement but the fatest way of generating configurations.
The excel spreadsheet can have the column heading representing key dimensions that may alter between each profile:
When using these profiles within the Structural Member feature, the familar pull down menus are still used, but the profile is tagged with the suffix "Configured" to show that it uses the new 2014 style.
For older versions the second pull down menu in the list would have related to a folder where the profiles lived, but with configuration based profiles, this pull down now refers to the file- this affects the folder structure that needs to be adpoted for these new versions- further info below.
As mentioned the folder structure has to be a little different for these- basically they need to be located one less folder deep. In the SOLIDWORKS Options File Locations - Weldment Profiles, the linked folder in the past needed to have two subfolders nested beneath (in 2013)- the Standard and the Type, in this Type folder would be all of the separate documents for each profile. For these configuration based profiles, you only need one sub folder for the Standard- the file residing in that folder represents the Type and then the configuration represents the size. All a little confusing, so hopefully this image captures it all!!
So in summary- with this new function you can create any new profiles with the configuration method but the old style profiles are very much relevant and can still be used in the normal manner.
Configure Away!!
By Jon Crookes
Applications Engineer

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