Chapter 31: Using Weldments
FIGURE 31.26
The model showing the features accepted in Step 22.- 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. - 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. - Edit the Structural Member feature to add the new line.
Note
You will 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. n
- 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 31.27. Accept the feature when you are done. - 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 trim-
ming boundary. - Half of the support structure has been modeled to this point. You can create the rest
of it 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 need to
merge solids manually. Click OK to accept the feature when it is set up properly. The
PropertyManager for the Mirror feature is shown in Figure 31.28.