Chapter 31: Using Weldments
Tutorial: Working with Weldments
This tutorial guides you through building a section of a tubular truss support. You can create many
different types of weldments, from simple small gauge frames to large architectural designs such as
this one. This tutorial also helps you to navigate successfully through some 3D sketch functionality
for creating fully defined sketches.Follow these steps to learn about working with weldments:- Open a new part. If you have Toolbox, then activate it by choosing Tools ➪ Add-
Ins ➪ SolidWorks Toolbox. If you do not have Toolbox, then simply draw two concentric
circles on the Front plane of a new part. The circles should have diameters of 10.02
inches and 10.75 inches. Alternatively, you can copy the library feature from the
CD-ROM for Chapter 31 to the location specified at the end of Step 5. - If you have Toolbox, then choose Toolbox ➪ Structural Steel.
- Select ANSI Inch, P Pipe, P10. This profile has an inside diameter of 10.02 inches and
an outside diameter of 10.75 inches. Click the Create button, and then click Done. - Use Custom Properties to add any properties that you would like to have automati-
cally added to the Cut list. - Remembering the technique from Chapter 18 on library features, first close any
open sketches, then select the sketch from the FeatureManager, and then save the
part as a Library Feature Part file to a path such as D:\Library\Weldment
Profiles\Custom\Pipe\P-Pipe10in.sldlfp.
Note
The Custom folder (located in the first level under the Weldment Profiles) will be recognized as the Standard,
similar to ANSI or ISO (International Organization for Standardization). The next folder down, Pipe, will be
recognized as the Type, and the name of the file will be recognized as the Size, in the same way as shown in
Figure 31.6. n
- Choose Tools ➪ Options ➪ File Locations ➪ Weldment Profiles, and add your non-
installation directory location to the list of folders. Alternatively, you can remove the
Program Files location from the list, and copy the files from that location to your own
library location. - Open another new part, and open a new 3D sketch in the part. Double-click the Top
(ZX) plane to activate it, and click the Center Rectangle sketch entity. - Draw a rectangle around the Origin. The sketch should now look like Figure 31.22.
Apply an Equal relation to two adjacent sides of the rectangle, and dimension any of the
lines as 120 inches. - Turn off the rectangle, and double-click in blank space to de-activate sketching on
the Top plane. - Activate the Line sketch tool and press Tab until the cursor indicates the XY plane.