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July 7, 2008 at 9:28am
by Bill The Weldment functionality of SolidWorks can be expanded by developing custom profiles. This will allow users to create cut lists for extruded products, lumber or other designs which require a cut list for manufacturing.
An easy way to create a weldment profile is to modify an existing profile by adding or copy-and-pasting your own sketch geometry.
Set up the folder structure:
1. Locate existing weldment profile directory (System Options > File Locations).
a. Typically C:\Program Files\SolidWorks\SolidWorks\data\weldment profiles\ansi inch
2. Create new top level custom library folder (optional).
a. Separating custom files from standard install files helps ensure the files aren’t overwritten in the event a repair or reinstall is required.
b. The custom library folder structure should adhere to the following convention to function within the Structural Member property manager within SolidWorks.
i. <SolidWorks weldment profiles directory>\Standard Name\Profile Type
ii. Example: C:\Program Files\SolidWorks\SolidWorks\data\weldment profiles\ansi inch\c channel
3. One method of quickly creating Weldment folders is to add the folders into the Design Library and then drag-and-drop sketch profiles into the appropriate folders.
Create a profile by modifying an existing library file:
1. Open any weldment profile library part from the child folders.
a. This example modified the 3 x 5.sldlfp file.
2. Save the file to a new Library File (Save As > change file type to ‘Library File’).
3. Delete the existing sketch geometry if necessary.
4. Draw or copy-and-paste the new profile geometry into place.
a. Create additional sketch points on the profile where the user may want to locate the profile on the weldment sketch. This will increase the usability and flexibility of the profile.
5. Rename the dimensions on the sketch to match existing file properties. This will save time and ensure the syntax is correct for use in the Weldment Cut List on the drawing.
