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:

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 Choice
K-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:

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:

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

Table 2: AISC Library "Section Type"
If the section name differs from the type, it is noted in parentheses ( ).

* When 4 numbers are given, the fourth number is the distance between the legs of the
angle. For example, the 2L8x4x7/8x3/4LLBB are double 8x4 angles, 7/8 inch thick legs
with the long legs back to back and separated by 3/4 inch.

 

Note

  1. 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.

  2. The AISC 2005 database corresponds to the data in the Thirteenth Edition of the AISC Steel Construction Manual.

 

How to Create a New Library:

How to Add a Cross Section to a Library:

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


 

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

 

See Also:

Variable Cross-Section Wizard

AISC Library