Divide Frames
Load Combinations
Springs
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 Beam button 
to access the Beam form. In that form:
Type 1 in the Number of Spans edit box.
Type 20 ft (be sure to type the ft) in the Span Length edit box.
Uncheck the Restraints check box
Click the + (plus) symbol beside the Beams drop-down list to access the Frame Properties form.
Click the Add New Property button to access the Add Frame Section Property form. Choose Concrete in the Frame Section Property Type drop-down list. Click the Rectangular button to access the Rectangular Section form.
Type CONBEAM in the Section Name edit box.
Type 42 in the Depth (t3) edit box.
Type 24 in the Width (t2) edit box.
Click the + (plus) symbol beside the Material drop-down list to access the Define Materials form.
Click the Add New Material Quick button to access the Quick Material Definition form.
Select Concrete in the Material Type drop-down list.
Select f'c 3000Psi in the Specification drop-down list.
Click the OK button to return to the Define Materials form.
Highlight the 3000Psi definition in the Materials display area and click the Modify/Show Material button to access the Material Property Data form.
Set the Units to 
.
Verify that 0.15 is entered in the Weight per Unit Volume edit box.
Change the Units to .
Enter 3120 in the Modulus of Elasticity edit box.
Verify that 0.2 is entered in the Poisson's Ratio edit box.
Click the OK buttons on the Material Property Data and Define Materials forms to return to the Rectangular Section form.
Click the OK buttons on the Rectangular Section, Frame Properties and the Beam form to close those forms and display the template model in the program windows.
Click the drop-down list to set the units to .
Click the “X” in the top right-hand corner of the 3-D View window to close it.
Select the line (frame) object by clicking on it.
Click the Edit menu > Edit Lines > Divide Frames command to access the Divide Selected Frames form.
Fill in the form as shown in the adjacent figure and click the OK button.
Click the Define menu > Load Patterns command to access the Define Load Patterns form. In that form:
Type LIVE in the Load Pattern Name edit box.
Select LIVE from the Type drop-down list.
Click the Add New Load Pattern button.
Click the OK button.
Click the Define menu > Load Combinations command to access the Define Load Combinations form. In that form:
Click the Add New Combo button to access the Load Combination Data form. In that form:
Accept the default Load Combination Name, COMB1.
Accept the default Combination Type, Linear Add.
Verify that DEAD is selected in the Load Case Name drop-down list.
Verify that 1 is entered in the Scale Factor edit box.
Click the Add button.
Select LIVE from the Load Case Name drop-down list.
Click the Add button.
Click the OK buttons on the Load Combination Data and Define Load Combinations forms to exit all forms.
Select all of the line (frame) objects by “windowing.”
Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:
Verify that the Load Pattern Name is DEAD.
In the Load Type and Direction area, verify that the Forces option is selected and that the Gravity direction is selected.
In the Uniform Load area, type 10.6 in the Load edit box..
Click the OK button.
Click the Get Previous Selection button 
(or the Select menu > Get Previous Selection command).
Click the Assign menu > Frame Loads > Distributed command to access the Frame Distributed Loads form. In that form:
Select LIVE from the Load Pattern Name drop-down list.
In the Uniform Load area type 5.4 in the Load edit box..
Click the OK button.
Click the Show Undeformed Shape button 
to remove the display of frame uniform load assignments.
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 16 (6 feet from the right end) by clicking on it.
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Verify that the Load Pattern Name shown is DEAD.
Type -250 in the Force Global Z edit box in the Loads area.
Click the OK button.
Click the Get Previous Selection button (or the Select menu > Get Previous Selection command).
Click the Assign menu > Joint Loads > Forces command to access the Joint Forces form. In that form:
Select LIVE from the Load Pattern Name drop-down list.
Type -150 in the Force Global Z edit box in the Loads area.
Click the OK button.
Click the Show Undeformed Shape button to remove the displayed joint load assignments.
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 drop-down list in the status bar to change the units to .
Select all of the objects by “windowing.”
Click the Assign menu > Joint > Springs command to access the Joint Springs form. In that form:
Type 50 in the Translation 3 edit box.
Click the OK button.
Click the Analyze menu > Set Analysis Options command to access the Analysis Options form. In that form:
Uncheck the UX, UY, RX and RZ check boxes leaving just the UZ and RY boxes checked.
Click the OK button.
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 load case is set to Run in the Action list.
Verify that the LIVE load 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 > Frames/Cables command to access the Member Force Diagram for Frames form. In that form:
Select COMB1 from the Case/Combo Name drop-down list.
Select the Moment 3-3 option in the Component area.
Select the Show Values on Diagram option.
Click the OK button to display the moment diagram.
Note: To change the font size, click the Options menu > Dimensions/ Tolerances command to display the Dimensions/Tolerances Preferences form. Type in a new font size in the Minimum Graphic Font Size edit box (usually about 6 points is sufficient) and click the OK button.
Note: Right click on any of the frame objects to view details of the moment diagram for that member.
Click the Show Deformed Shape button 
(or the Display menu > Show Deformed Shape command) to access the Deformed Shape form. In that form:
Select COMB1 from the Case/Combo Name drop-down list.
Click the OK button.
Right click on the joint at the far right end of the beam to view its deflection.