# Beam Elements

What is a Beam Element?

A beam element is a slender structural member that offers resistance to forces and bending under applied loads. A beam element differs from a truss element in that a beam resists moments (twisting and bending) at the connections.

These three node elements are formulated in three-dimensional space. The first two nodes (I-node and J-node) are specified by the element geometry.  The third node (K-node) is used to orient each beam element in 3-D space (see Figure 1). A maximum of three translational degrees-of-freedom and three rotational degrees-of-freedom are defined for beam elements (see Figure 2). Three orthogonal forces (one axial and two shear) and three orthogonal moments (one torsion and two bending) are calculated at each end of each element. Optionally, the maximum normal stresses produced by combined axial and bending loads are calculated. Uniform inertia loads in three directions, fixed-end forces, and intermediate loads are the basic element based loadings.

Figure 1: Beam Elements

Figure 2: Beam Element Degrees-of-Freedom

 Caution The mass moment of inertia about the longitudinal axis, I1 is not calculated for beam elements. Only the m×R2 effect is considered, where R is the distance from the reference point to the element. The mass moment of inertia about the other axes, I2 and I3, are calculated based on the slender rod formula (I2 = I3 = M×L2/12). This would affect any analysis type that includes angular acceleration loads or effects.

When to Use Beam Elements

The basic guidelines for when to use a beam element are:

• The length of the element is much greater than the width or depth.

• The element has constant cross-sectional properties.

• The element must be able to transfer moments.

• The element must be able to handle a load distributed across its length.

Part, Layer and Surface Properties for Beam Elements

The following chart describes what is controlled by the part, layer and surface properties for beams.

 Part Number Material properties and stress-free reference temperature Layer Number Cross-sectional properties Surface Number Orientation

Beam Element Orientation

Most beams have a strong axis of bending and a weak axis of bending. Since beam members are represented as a line and a line is an object with no inherent orientation of the cross section, there needs to be a method of specifying the orientation of the strong or weak axis in three-dimensional space. This orientation is controlled by the surface number of the line.

More specifically, the surface number of the line creates a point in space, called the K-node. The two ends of the beam element (the I- and J-nodes) and the K-node form a plane (see Figure 3). Beam elements are defined by the local axes 1, 2 and 3, where axis 1 is from the I-node to the J-node, axis 2 lies in the plane formed by the I-, J- and K-nodes, and axis 3 is formed by the right-hand rule. With the element axes set, the cross-sectional properties A, Sa2, Sa3, J1, I2, I3, Z2 and Z3 can be entered appropriately in the "Element Definition" dialog.

Figure 3: Axis 2 Lies in the Plane of the I-, J- and K-nodes

For example, Figure 4 shows part of two models, each containing a W10x45 I-beam. Note that both members have the same physical orientation; that is, the webs are parallel. However, the analyst chose to set the K-node above the beam element in model A and to the side of the beam element in model B. Even though the cross-sectional properties are the same, the moment of inertia about axis 2 (I2) and the moment of inertia about axis 3 (I3) need to be entered differently.

Figure 4: Entering the Cross-Sectional Properties Appropriate for the Beam Orientation

Table 1 shows where the K-node occurs for various surface numbers. The first choice location is where the K-node is created provided the I-, J- and K-nodes form a plane. If the beam element is colinear with the K-node, then a unique plane cannot be formed. In this case, the second choice location is used for that element.

Table 1: Correlation of Surface Number and K-Node (Axis 2 Orientation)

 Surface Number First Choice K-node Location Second ChoiceK-node Location 1 1E14 in +Y 1E14 in -X 2 1E14 in +Z 1E14 in +Y 3 1E14 in +X 1E14 in +Z 4 1E14 in -Y 1E14 in +X 5 1E14 in -Z 1E14 in -Y 6 1E14 in -X 1E14 in -Z

The surface number, hence the default orientation, can be changed by selecting the beam elements using the "Selection: Select: Lines" command and right clicking in the display area. Select the "Modify Attributes.." command and change the value in the "Surface:" field.

In some situations, a global K-node location may not be suitable. In this case, select the beam elements in the FEA Editor environment using the "Selection: Select: Lines" command and right click in the display area. Select the "Beam Orientations: New.." command. Type in the X, Y and Z coordinates of the K-node for these beams. If you want to select a specific node in the model, click on the vertex, or enter the vertex ID in the "ID" field. A blue circle will appear at the specified coordinate. Figure 5 shows an example of a beam orientation where you would wantto define the origin as the k-node.

Figure 5: Skewed Beam Orientation

The direction of axis 1 can be reversed in the FEA Editor by selecting the elements to change ("Selection: Select: Lines"), right-clicking, and choosing "Beam Orientations: Invert I and J Nodes". This ability is useful for loads that depend on the I and J nodes and for controlling the direction of axis 3. (Recall that axis 3 is formed from the right-hand rule of axes 1 and 2.) If any of the selected elements have a load that depends on the I/J orientation, the user is prompted whether the loads should be reversed or not. Since the I and J nodes are being swapped, choosing "Yes" to reverse the input for the load will maintain the current graphical display; that is, the I and J nodes are inverted, and the I/J end with the load is also inverted. Choosing "No" will keep the original input, so an end release for node I will switch to the opposite end of the element since the position of the I node is changed.

The orientation of the elements can be displayed in the FEA Editor environment using the "View: Options: Element Orientations" command. The orientation can also be checked in the Results environment using the "Display Options: Show Orientation Marks: Element Orientations" command. Choose to show the "Axis 1", "Axis 2", and/or "Axis 3" using red, green, and blue arrows, respectively. See Figure 6.

Figure 6: Beam Orientation Symbol.

Different arrows are used for each axis.

Specifying the Cross-Sectional Properties of Beam Elements

The "Sectional Properties" table in the "Cross-Section" tab of the "Element Definition" dialog is used to define the cross-sectional properties for each layer in the beam element part. A separate row will appear in the table for each layer in the part.  The sectional property columns are:

• A: Specify the cross-sectional area in this column. This is the area of the beam resisting the axial force (d=FxL/(AxE)). This area must be greater than 0.0.

• J1: Specify the torsional resistance in this column. The torsional resistance is the area moment of inertia resisting the torsional moment M1. The angle of twist within an element is calculated by q=M1xL/(J1xG) where L is the length and G is the shear modulus. For most cross-sections, the torsional resistance is much less than the polar moment of inertia. (For a circular section, J1 equals the polar moment of inertia.) The torsional resistance must be greater than 0.0.

• I2: Specify the area moment of inertia about the local 2 axis in this column. (This is also referred to as I2-2.) The local 2 axis passes through the neutral axis of the cross section and is in the plane formed by the element and the k-node (see paragraph above). The moment of inertia must be greater than 0.0.

• I3: Specify the area moment of inertia about the local 3 axis in this column. (This is also referred to as I3-3.) The local 3 axis passes through the neutral axis of the cross section and forms the right-hand rule with the element (axis 1) and axis 2. The moment of inertia must be greater than 0.0.

• S2: Specify the section modulus about the local 2 axis in this column. The section modulus is calculated from S2=I2/C3max, where C3max is measured parallel to the 3 axis from the neutral axis to the furthermost point on the cross section. This value is not required but is necessary for the bending stress calculation about axis 2 (=M2/S2). If this value is 0.0, the bending stress about the local 2 axis will be set to 0.

• S3: Specify the section modulus about the local 3 axis in this column. The section modulus is calculated from S3=I3/C2max, where C2max is measured parallel to the 2 axis from the neutral axis to the furthermost point on the cross section. This value is not required but is necessary for the bending stress calculation about axis 3 (=M3/S3). If this value is 0.0, the bending stress about the local 3 axis will be set to 0.

• Sa2: Specify the shear area parallel to the local 2 axis. The shear area is the effective beam cross-sectional area resisting the shear force R2 (shear force parallel to axis 2). If the shear area is 0.0, the shear deflection in the local 2 direction is ignored (usually a safe assumption). The shear area correction is only needed if the beam width is comparable to the beam length.

• Sa3: Specify the shear area parallel to the local 3 axis. The shear area is the effective beam cross-sectional area resisting the shear force R3 (shear force parallel to axis 3). If the shear area is 0.0, the shear deflection in the local 3 direction is ignored (usually a safe assumption). The shear area correction is only needed if the beam width is comparable to the beam length.

 Note Hand calculations for the deflection of beams rarely include the effects due to shear within a beam. For example, the well-known equations for the maximum deflection for a cantilever beam and simply supported beam due to a point load (FL3/(3EI) and FL3/(48EI), respectively) only consider the bending effects. If shear effects are included in the finite element analysis by entering values for Sa2 and Sa3, the calculated displacements can be higher than the hand calculations.

If you know the dimensions of the cross-section instead of the properties, you can use the cross-section libraries to determine the necessary values.

 Tip See the page "Variable Cross-Section Wizard" to generate a series of cross-sections along the length of a beam to approximate a tapered beam.

Using the Cross-Section Libraries

In order to use the cross-section libraries, you must first select the layer for which you want to define the cross-sectional properties.  After the layer is selected, press the "Cross-Section Libraries..." button.

How to Select a Cross Section from an Existing Library:

• Select the desired library in the "Section database:" drop-down box. Multiple versions of the AISC Library are provided with the software.  (Note: The AISC library is set so that the IYY from the AISC manual corresponds to I2 in the software.)

• Select the desired cross section type using the "Section type" pull down. The types available for each database are given in Table 2 below.

• Select the desired cross section name in the "Section name:" section. You can search for a name by typing a string in the field above the list.

• Review the values in the "Cross-sectional properties" section. If these are acceptable, press the "OK" button. Note that the AISC library may not have all of the values needed to perform an analysis.

 AISC 2005 & 2001 AISC Rev 9 AISC Rev 8 & 7 Shape W W Type W Type W shapes M M Type M Type M shapes S S Type S Type S shapes HP HP Type HP Type HP shapes C C Type C Type Channels - American Standard MC M Type (MC) M Type (MC) Channels - Miscellaneous L L Type L Type Angles - equal legs L L Type UL Type Angles - unequal legs WT WT Type WT Type Structural tees cut from W shapes MT M Type (MT) M Type (MT) Structural tees cut from M shapes ST S Type (ST) S Type (ST) Structural tees cut from S shapes 2L 2L Type DL Type Double angles - equal legs* 2L (LLBB on end of name) 2L Type (first dimension is back-to-back dimension) UD Type (UDL) Double angles - unequal legs* (long legs back to back) 2L (SLBB on end of name) 2L Type (first dimension is back-to-back dimension) UD Type Double angles - unequal legs* (short legs back to back) Pipe (schedule on end of name) P Type S Type (SP, schedule on end of name) Pipe - STD standard weight Pipe (schedule on end of name) P Type (PX) S Type (SP, schedule on end of name) Pipe - XS extra strong Pipe (schedule on end of name) P Type (PXX) S Type (SP, schedule on end of name) Pipe - XXS double extra strong HSS TS Type RTU Structural tubing - rectangular HSS TS Type S Type (STU) Structural tubing - square

 Note In order to visualize the beam cross section in the Results environment, the cross section must be chosen from the AISC 2001 or AISC 2005 database. The AISC 2005 database corresponds to the data in the Thirteenth Edition of the AISC Steel Construction Manual.

How to Create a New Library:

• Press the "Add..." button below the "Section database:" drop-down box..

• Enter a name for the library and press the "OK" button.

• Enter a name for the database file and press the "Save" button. The new library will now appear in the "Section database:" drop-down box.

How to Add a Cross Section to a Library:

• Select the desired library in the "Section database:" drop-down box. You can only add a cross section to a library created by a user.

• Press the "Add..." button below the "Section name:" section and press the "OK" button. The section name should appear in the list in the "Section name:" section.

• Select the new section and enter the desired values in the "Cross-sectional properties" section.

• Press the "Save" button.

How to Define the Dimensions of a Common Cross-Section:

• With a cross section created by a user selected, change the pull-down menu in the upper-right corner from the "User-Defined" option to the desired geometry type.

• Enter the appropriate dimensions shown at the right side of the dialog.

• Press the "Save" button.

Other Beam Element Parameters

In addition to the cross-sectional properties, the only other parameter for beam elements is the stress free reference temperature. This is specified in "Stress Free Reference Temperature" field in the "Thermal" tab of the "Element Definition" dialog. This value is used as the reference temperature to calculate element-based loads associated with constraint of thermal growth using the average of the nodal temperatures. The value you enter in the "Default nodal temperature" field in the "Analysis Parameters" dialog determines the global temperatures on nodes that have no specified temperature.

Basic Steps for Using Beam Elements

• Be sure that a unit system is defined.

• Be sure that the model is using a structural analysis type.

• Right click on the "Element Type" heading for the part that you want to be beam elements..

• Select the "Beam" command.

• Right click on the "Element Definition" heading.

• Select the "Modify Element Definition..." command.

• In the "Cross Section" tab, enter in the proper cross sectional properties for each layer of beams. If you want to use saved properties, press the "Cross-Section Libraries..." button.

• Once all of your sectional properties are entered, press the "OK" button.