SolidWorks 2011 Assemblies Bible - Matt Lombard [176]
16. Draw a new line from the point where the four lines come together AlongX in the positive X direction. Dimension this new line as 120 inches. The sketch should now look like Figure 20.28.
FIGURE 20.28
The sketch after Step 16
17. Exit the sketch. Click the Structural Member toolbar button on the Weldments toolbar. In the Standard drop-down list in the Structural Member PropertyManager, select Custom. In the Type drop-down list, select Pipe. In the Size drop-down list, select P-Pipe10in. This is the name that corresponds to the way you saved the library feature part in Step 5.
18. In the Path Segments selection box, select the original four sides of the rectangle. In the Settings panel, make sure that the Apply corner treatment option is selected and that the End Miter icon is selected. This is shown in Figure 20.29. Accept the command when you are done.
19. Expand the Structural Member feature. Notice that the four bodies are listed under it. Click the Cut List folder to expand it. The bodies should also be listed there.
20. Open the 10-inch pipe library feature that you created at the beginning of this tutorial. Edit the two dimensions to subtract 2 inches from each dimension, and add a custom property description called Support Leg. Choose File⇒Save As to save the library feature to the same location as the original, but with the filename P-Pipe8in.sldlfp.
21. Initiate another Structural Member feature, this time selecting the 8-inch size of pipe from the Custom folder. In the Path Segments selection box, select two of the angled lines that go to opposite corners. Keep the feature open for the next step.
Note
Remember that you cannot create three intersecting Structural Members with a single group. To create material on all four lines, you need two separate groups within the Structural Member feature.
FIGURE 20.29
The Structural Member PropertyManager and the sketch after Step 18
22. Make a second group with the other pair of angled lines. Accept the feature when you are satisfied. The model should now look like Figure 20.30.
FIGURE 20.30
The model showing the features accepted in Step 22
23. Apply another Structural Member feature to the 10-foot (120-inch) section, again using the 10-inch-diameter pipe. Notice that this member is not long enough to cut through the peak of the pyramid.
24. Edit the 3D sketch and draw a 12-inch extension to the original line past the peak of the pyramid. Use an additional line rather than extending the existing one. Exit the sketch.
25. Edit the Structural Member feature to add the new line.
Note
You have to deselect the Apply corner treatment option to get this technique to work. If this option is selected, SolidWorks tries to miter or otherwise create a corner treatment between the bodies, which fails when the parts are parallel.
26. The four angled members need to be trimmed on both ends because they extend to the ends of the sketch entities rather than stopping at intersecting members. Initiate the Trim/Extend feature. Select the four angled members in the Bodies to be Trimmed selection box. Select the four members created by the original rectangle as the Trimming Boundary, and make sure that the Bodies option is selected (as opposed to Face/Planar), as shown in Figure 20.31. Accept the feature when you are done.
FIGURE 20.31
The model after Step 26
27. Create another Trim/Extend feature. This time, trim off the point end of the four angled members using the 10-inch horizontal pipe and the small segment as the trimming boundary. Half of the support structure has been modeled to this point.
28. Create the rest of the support structure by mirroring the existing bodies. Create a Mirror feature using the free end of the 10-foot-long member as the mirror plane, and selecting all the bodies in the Bodies to Mirror selection box. Do not select the Merge solids option because you will