Creating a welded profile with SOLIDWORKS

Initial situation

We're going to create a rectangular profile compatible with the welded construction module or the structure system on SOLIDWORKS.

Objective

The aim is to create several sizes of the rectangular tube and store it in a library.

How to proceed

• Open a blank Part file

• Select Face plane -> Open sketch and create profile (add corner fillets).

  The origin will be the profile insertion point...

• Use the "Point" sketching tool to add points where the profile might later be hooked in.

Tip Add a maximum number of points (with clearance if necessary) to provide a wide range of profile orientation options during design.

• Rename dimensions as "Widths" and "Lengths".

• In the document properties, enter a description linked to the dimensions (in the "Value/expression" box, type your text, then point with the mouse at the dimensions).

Example here: Type "Rectangular tube" -> select length dimension -> type "x" -> select width dimension -> type "x" -> select thickness dimension

• Then validate the window and validate the sketch. Display the dimensions by right-clicking on the annotation folder in the creation tree, then right-clicking on one of the dimensions to be configured:

• A window opens with a table. Double-click on each dimension to be modified, then enter the different profile sizes:

• Click on apply and close the table, all your configurations are now created.

• Select sketch1 in the design tree, then save in .sldlfp format (save the profile in your profile folder). A small "L" should appear next to the sketch if the action has been successful:

• Specify library folder path in options if not already done