When you start SAP2000 Version 24, you should see the following interface window:

---

Step 1: New Model - To start a new problem, select New Model under the File menu.

The New Model window gives many different templates for general structures. On this menu, you can select the units for the problem; the default is Kip, ft, F. You can change the unit when necessary, and SAP2000 converts the values. In this example, the units are Kip and in. Click on the Beam icon on the first row of templates.

The Beam template menu should appear.

 

 

In this example, the beam has three spans of 12 ft. or 144 in. Enter the values and click OK.

 

The SAP2000 interface displays the geometry of the beam. By default, the left support is a pin, and the remaining supports are rollers.

Since we do not need a 3-D view of the beam, click on the window label and delete the left-hand side window so that you have an xz view of the beam.

---

Step 2: Define Structural Supports - To define the location and type of structural support, select the support location by clicking on the joint with the pointer. A blue "X" should appear at the joint to indicate it is currently selected. Next, click on the Assign tab at the top of the SAP2000 interface, then click on Joint, and then the Restraints ... button on the bottom toolbar.

The Assign Joint Restraints menu appears as shown. Usually, the directions 1, 2, and 3 listed on the menu correspond to the x, y, and z directions. The Fast Restraints buttons may be used for most problems when working on two-dimensional structures. If the support conditions for your problem are not listed in the Fast Restraints section of the menu, you should select the appropriate combination of restraints.

In this beam example, the support at A is fixed, B and C are rollers, and D is a pin.

Select the far left node with the pointer (an X should appear at the joint), then click the Fixed button  and then OK. Since B and C are rollers, they are set. Next, click on node D with the pointer, select the Pin button   and then OK.

After the supports have been defined, the beam should appear in the SAP2000 interface window as follows:

This example's grid lines are unimportant, so they are turned off. Click on the View menu at the top of the SAP2000 interface and then Show Grid.

---

Step 3: Apply Forces – Two loads are applied to the beam in this example.

The first beam element has two equally spaced point loads, and the last element has a distributed load.

To apply the point loads on the first element, select the beam element with the pointer, click on Assign, then Frame Loads, and then Point. The following menu appears. Click on Absolute Distance from End-I and enter the position and value of the two point loads. This example shows two 6 Kip loads at 4 ft. intervals (48 in. intervals).

 

Click OK, and the loads are displayed on the beam:

< <

Next, click on the far right element and select Assign, Frame Loads, and Distributed. The following menu should be displayed. The distributed load is 3k/ft or 0.25 k/in in this example. Enter these values into the menu and click OK.

 

The distributed loading is displayed on the beam.

The point loads are not deleted; they are currently not displayed. Select Display, Show Object Load Assigns, Frame, and then OK to see all frame loads.

---

Step 4: Set Analysis Options -This example models the beam in the x-z plane. Click on the Analyze menu at the top of the SAP2000 interface window and then click Set Analysis Options to limit analysis to variables in the x-z plane. The Analysis Options menu appears as follows:

 

To restrict SAP2000 to variables in the x-z plane, select the Plane Frame button and click OK. 

---

Step 5: Define Material Properties

SAP2000 assumes the loads acting on a structure, including the weight of each element. In our beam analysis, we assume that each element is weightless. To define the properties of a material, select the Define menu at the top of the SAP2000 interface window and then click on Materials. The Define Materials window appears as shown below:

On this menu, you can change the properties of materials. Select the A992Fy50 (steel with a yield stress of 50 ksi) material in this example and click the Modify/Show Material... button. Material Property Data window is displayed.

 

Change the value in the Weight per unit Volume input field to zero. Click OK to return to the Define Materials window, then click OK again. Now, we have a material named A992Fy50 that has no weight per volume. For this example problem, the default values for the Mass per unit Volume, Modulus of elasticity, Poisson's ratio, and the Coefficient of Thermal Expansion can be used. For most linear elastic statically loaded structures, only values for Weight per unit Volume and Modulus of Elasticity are required.

---

Step 6: Define Frame Sections - To define the cross-section properties of a structural element, click on the Define menu located at the top of the SAP2000 interface window, then click on Section Properties, then Frame Sections..., and then the Frame Properties window is displayed.

The default Frame Section label is FSEC1. To change the properties of the frame section, click on the Modify/Show Property... button. The I/Wide Flange Section window is displayed.

To define the material of this frame section, click on the Material pull-down menu and select our weightless material A992Fy50. Click OK to return to the Frame Properties window, then click OK again.

In this example, the bean has a moment of inertia value of 1,000 in⁴. Click Add New Property on the Frame Properties menu to specify this value. The Add New Property menu is displayed. For this example, click the Frame Section Property Type dropdown menu, select Other, and then click on General.

 

The Property Data menu is displayed. In this example, the Moment of inertia about the 3 axis (the strong axis) is 1,000 in⁴. The value of the Cross-sectional area and the Moment of inertia about the 2 should be a small value of 0.001 to minimize their effect on the results.

Enter the value and click OK. Then click OK on the General Shapes menu, and the Frames Properties menu is displayed. Note that FSEC2 has been added to the list of sections. Click OK.

---

Step 7: Assign Frame Sections - To assign the frame properties of a structural element, select all beam elements with the pointer and click on the Assign menu at the top of the SAP2000 interface window, then click Frame, and then Frame Sections. You can assign the same section properties to multiple elements by selecting all the elements that share the same properties. Choose the FSEC2 frame element from the Assign Frame Sections window and click OK.

The frame section name is displayed next to each element selected. After the frame sections have been assigned, the SAP2000 interface window is displayed.

---

Step 8: Run Analysis - To analyze the model, press the Run Analysis button  The Set Load Cases to Run menu is displayed.

By default, there are two load cases: DEAD and MODAL. More load cases can be added, but only the DEAD load case is required for this example. Click on the Run Now button. If the analysis is successful, the Analysis Complete window is displayed and reports that the analysis is complete. Click OK, and the Save Model File As window is displayed.

<

When you run a model, SAP2000 creates about 40 temporary files, so choosing a particular folder to store the SAP2000 files is beneficial. The Windows Desktop is not a good location. When a folder is selected, name the SAP2000 model file.

In this example, the file name is Beam_tutorial. SAP2000 saves the model information in the file named Beam_tutorial.sdb in the folder selected. The SAP2000 interface window displays an exaggerated deflected shape of the modeled structure.

---

Step 9: Print Beam Forces - To get a quick feel for the relative magnitude of the forces in the beam, click on the Show Forces/Stresses pull-down menu   at the top of the SAP2000 interface, select Frames/Cables/Tendons..., and the Display Frame Forces/Stresses menu is displayed.

Select the Moment 3-3 (the strong axis) and then OK; the moment along the beam is displayed.

The default view is the Fill Diagram, where the relative magnitude of the moments are displayed. Negative bending moments are in red and the positive in blue.

Another way to display force information is to unclick Fill Diagram and click on Show Values on Diagram. In this case, the value of each axial force is displayed next to the elements.

To view more detail about the forces along an element, click on the element in the SAP2000 interface and right-click. The Diagram for Frame Object # (FSEC2) window is displayed. Below are the results for each of the three elements in this example.

 

 

Drag the vertical slider along the element to see values on the loads, shear, moment, and deflection.

To print the results to a file, click on the File menu, select Print Tables..., and the following menu is displayed.

In this example, all we require is the mon the beam, so click on expand the Element Output item under the ANALYSIS RESULTS section, expand the Frame Output item, and then click on Tables: Element Forces - Frames. Also, click on the box Print to File and the TXT file button to define the file format. Click OK and define the name and location of the TXT file.

There is an option for Spreadsheet Format if desired. The default location for the file is the same directory as the problem files. A different location can be specified by clicking File Name and choosing the desired file location and name.

Turn on the frame labels to correlate the results printed in the output file to frame elements in the structure. Click the Show Undeformed Shape button / on the main interface to display the frame element labels. Next, click on the Display Options button   and under the Frame section of the menu, click on Labels.

The frame element numbers or any other information displayed in the main SAP2000 interface can be printed by clicking on the File menu and selecting Print Graphics (the image is sent to the default printer).

The results of the beam analysis presented in the output file are listed by frame element number.

Note that SAP2000 lists the variation of the internal forces and moments along the element. For beam analysis, there are bending moments and shear forces. The values in the "M3" column are the moments about the strong axis.

 

 

---

This website was originally developed by Charles Camp for CIVL 4122. This site is maintained by the Department of Civil Engineering at the University of Memphis. Your comments and questions are welcomed.