SOLIDWORKS includes a library of standard structural members, such as tubes, pipes, c-channels, beams, angles and unistrut. By creating a sketch that represents the skeleton of a frame, these structural members can then be inserted onto the sketched lines. From there, various end treatments can be applied to determine how the lines join together.
When inserting a structural member, there is a button in the Property Manager called "Locate Profile". This allows a point or endpoint in the weldment profile to be referenced as the insertion point for the structural member.
Weldment profiles are basically the sketches used to extrude the structural members. They are created by simply saving a sketch as a library feature part (*.sldlfp). By default, Weldment Profiles are located at C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\weldment profiles, but any location can be used if it is specified in the system options for file locations.
SOLIDWORKS provides several Weldment Profiles organized by standard, i.e. Ansi Inch, AS, BSI, CISC, DIN, GB, ISO, GIS and Unistrut. These can be loaded from the Design Library Task Pane > SOLIDWORKS Content > Weldments folder.
Editing Weldment Profiles
If the Weldment Profile does not have the desired insertion points, then they can be added by editing the sketch of the profile. For example, in the image of the pipes above, the design intent calls for the distance between the pipes to be measured from outside to outside rather than on-center. This is a ½” Schedule 40 pipe and is one of the default Weldment Profiles included with SOLIDWORKS. It has one point in the center, and we will add four more around the outer edge.
Since we are customizing a library, it is good practice to copy the folder to a location outside of any SOLIDWORKS directory. This keeps the default files intact should they ever need to be restored. It also avoids the possibility of the customized files being unintentionally deleted during an uninstall of SOLIDWORKS. Make sure to add this new folder in Options > System Options > File Locations > Show folders for: Weldment Profiles.
Using the Segment Command to Add Points
Now, the fun part. As mentioned above, Weldment Profiles are simply 2D sketches saved as library feature part files (*.sldlfp). Open the profiles for the pipe, and edit the sketch to add four points. An easy way to add sketch points is to use the Segment command. Select the outer circle, and go to Tools > Sketch Tools > Segment. In the screen shot below, Segment was added to the shortcut toolbar. Quick tip: Press the S key in a part, assembly, drawing or sketch, and the context sensitive shortcut toolbar will appear.
Add four sketch points to the outer circle. These points will then be selectable when using Locate Profile in the Structural Member Property Manager. Take it further by sketching a square around the circle to have four more points in the corners, if you wish.
If you feel that additional sketch points should be incorporated into the default weldment profiles, we encourage you to submit an enhancement request through the SOLIDWORKS Customer Portal.
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