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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:

1. 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 DVD to the location specified at the end of Step 5.

2. If you have Toolbox, then choose Toolbox⇒Structural Steel.

3. 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.

4. Use Custom Properties to add any properties that you would like to have automatically added to the cut list.

5. Remembering the techniques on library features, first close any open sketches, 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) is recognized as the Standard, similar to ANSI or ISO (International Organization for Standardization). The next folder down, Pipe, is recognized as the Type, and the name of the file is recognized as the Size, in the same way as shown in Figure 20.6.

6. 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.

7. 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.

8. Draw a rectangle around the Origin. The sketch should now look like Figure 20.26. Apply an Equal relation to two adjacent sides of the rectangle, and dimension any of the lines as 120 inches.

FIGURE 20.26

A centered rectangle in a 3D sketch

9. Turn off the rectangle, and double-click in a blank space to deactivate sketching on the Top plane.

10. Activate the Line sketch tool and press Tab until the cursor indicates the XY plane.

11. Draw a line from one corner of the square down, trying to avoid any automatic relations such as coincident relations to other points and any AlongX, -Y, or -Z relations. Connect the other three corners of the square with the free endpoint of the new line, as shown in Figure 20.27.

FIGURE 20.27

Adding lines

12. Rotate the view slightly. Notice that the first line that you drew in Step 10 and one other line are on a plane. Drag a right-to-left selection box around the point where the four lines converge, and assign an Equal relation to all the lines. This makes the shape into an upside-down pyramid.

13. Drag the point. Notice that it moves up and down, although it seems a little erratic. Place a dimension between the point and the part Origin. Notice that the sketch becomes over-defined and turns red and yellow. Theoretically, this combination should work. SolidWorks does not accept it.

14. Using the Display/Delete Relations tool, delete all the Equal relations that you just added to the part (it may be faster to select Undo from the File menu or to press Ctrl+Z).

15. Draw a vertical construction line from the part Origin to the point where the four lines meet, and assign this line an AlongY relation. Notice that the point drags much more smoothly. This is a good reason for using simpler relation schemes when possible. The four equal relations in this case that had to be solved simultaneously are now replaced