Mesh Area Objects
Trick Problem
Click the File menu > New Model command to access the New Model form.
Click the drop-down list to set the units to 
.
Click on the Grid Only button 
to access the Quick Grid Lines form. In that form:
Select the Cartesian Tab.
In the Number of Grid Lines area:
Type 3 in the X direction edit box.
Type 3 in the Y direction edit box.
Type 1 in the Z direction edit box.
In the Grid Spacing area:
Type 4 the X direction edit box.
Type 6 the Y direction edit box.
Click the OK button.
Click the X in the top right-hand corner of the 3-D View window to close it.
Click the Define menu> Section Properties > Area Sections command to access the Area Sections form. In that form:
Select Shell in the Select Section Type to Add drop-down list.
Click the Add New Section button to access the Shell Section Data form. In that form:
Verify that the Shell - Thin option is selected in the Type area.
Click the + (plus) symbol beside the Material drop-down list to access the Define Materials form.
Highlight the 4000Psi definition in the Material display list and click the Modify/Show Material button to access the Material Property Data form. In that form:
Change the Units to 
.
Change the Modulus of Elasticity to 3600.
Verify that the Poissons Ratio is 0.2.
Click the OK button to close the Material Property Data and the Define Materials forms and return to the Shell Section Data form.
Verify that both the Membrane and the Bending thicknesses are 1.
Click the OK buttons on the Shell Section Data and Area Sections forms to close all forms.
Verify that the Snap to Points and Grid Intersections button 
on the side toolbar is depressed.
Click the Draw Rectangular Area Element button 
or the Draw menu > Draw Rectangular Area command to access the Properties of Object form. In that form:
Verify that the selected Section is ASEC1.
Click on upper left-hand corner grid intersection (Point B in the problem statement) and then click on the lower right-hand grid intersection (Point A) to draw an area object over the entire structure.
Click the Set Select Mode button 
to exit the Draw mode and enter Select mode.
Click on the area object to select it.
Click the Edit menu > Edit Areas > Divide Areas command to access the Divide Selected Areas form.
Fill in this form as shown in the figure, including setting the Units to , and click the OK button.
Select the joints that are labeled A, B and C in the problem statement.
Click the Assign menu > Joint > Restraints command to access the Joint Restraints form. In that form:
Uncheck the Translation 1 and Translation 2 check boxes.
Verify that the Translation 3 check box is checked.
Verify that the Rotation about 1, 2 and 3 check boxes are not checked.
Click the OK button.
Click the Show Undeformed Shape button 
to remove the display of joint restraints and reset the window display (and title).
Click the Set Display Options button 
(or the View menu > Set Display Options command) to access the Display Options for Active Window form. In that form:
Check the Labels box in the Joints area.
Click the OK button.
Select joint 106 (coordinates 7, 12, 0) by clicking on it. Note that the Options menu > Preferences > Dimensions and Tolerances command can be used to access the Dimensions and Tolerances form; on that form change the Minimum Font Size to increase the size of the joint labels and make them easier to read.
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Type -814 in the Force Global Z edit box in the Loads area.
Click the OK button.
Select joint 16 (coordinates 1, 6, 0) by clicking on it.
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Type -698 in the Force Global Z edit box in the Loads area.
Click the OK button.
Select joint 32 (coordinates 2, 3, 0) by clicking on it.
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Type -901 in the Force Global Z edit box in the Loads area.
Click the OK button.
Click the Show Undeformed Shape button to reset the window display.
Click the Set Display Options button (or the View menu > Set Display Options command) to access the Display Options for Active Window form. In that form:
Uncheck the Labels box in the Joints area.
Click the OK button.
Click the Analyze menu > Set Analysis Options command to access the Analysis Options form. In that form:
Click the Plane Grid XY Plane button 
to set the available degrees of freedom.
Click the OK button.
Click the Set Default 3D View button 
to switch to a 3-D View.
Click the Run Analysis button 
to access the Set Load Cases to Run form. In that form:
Highlight (select) MODAL in the Case Name list and click the Run/Do Not Run Case button.
Verify that the DEAD analysis case is set to Run in the Action list.
Click the Run Now button to run the analysis.
When the analysis is complete, check the messages in the SAP Analysis Monitor window (there should be no warnings or errors) and then click the OK button to close the window.
Click the Display menu > Show Forces/Stresses > Joints command to access the Joint Reaction Forces form and click the OK button to view the support reactions.
Note: The reaction at the joint labeled C in the problem statement is virtually zero (0). The reason for this apparently odd result is that the resultant of all the applied loads lies on a line connecting the support points labeled A and B, and thus by simple statics, the reaction at support point C must be zero. Note that you could move the support point labeled C anywhere on the structure (except on the line connecting support points A and B because this would result in an unstable structure) and the resulting reactions would not change.