BEAM4


3D Elastic Beam

Valid Products: Pro | Premium | Enterprise | PrepPost | Solver | AS add-on

BEAM4 Element Description

Although this archived element is available for use in your analysis, Ansys, Inc. recommends using a current-technology element such as BEAM188 (KEYOPT(3) = 3).

BEAM4 is a uniaxial element with tension, compression, torsion, and bending capabilities. The element has six degrees of freedom at each node: translations in the nodal x, y, and z directions and rotations about the nodal x, y, and z axes. Stress stiffening and large deflection capabilities are included. A consistent tangent stiffness matrix option is available for use in large deflection (finite rotation) analyses.

Figure 4.1: BEAM4 Geometry

BEAM4 Geometry

BEAM4 Input Data

The geometry, node locations, and coordinate systems for this element are shown in Figure 4.1: BEAM4 Geometry. The element is defined by two or three nodes, the cross-sectional area, two area moments of inertia (IZZ and IYY), two thicknesses (TKY and TKZ), an angle of orientation (θ) about the element x-axis, the torsional moment of inertia (IXX), and the material properties. For stiffness purposes, the torsional moment of inertia, if IXX is equal to 0.0 or not specified, is assumed to be equal to the polar moment of inertia (IYY + IZZ). For inertial purposes, the torsional (rotational) moment of inertia used is the polar moment of inertia, and is therefore not affected by the value entered for IXX. The IXX value should be positive and is usually less than the polar moment of inertia. An added mass per unit length may be input with the ADDMAS value.

The element x-axis is oriented from node I toward node J. For the two-node option, the default (θ = 0°) orientation of the element y-axis is automatically calculated to be parallel to the global X-Y plane. Several orientations are shown in Figure 4.1: BEAM4 Geometry. For the case where the element is parallel to the global Z axis (or within a 0.01 percent slope of it), the element y axis is oriented parallel to the global Y axis (as shown). For user control of the element orientation about the element x-axis, use the θ angle (THETA) or the third node option. If both are defined, the third node option takes precedence. The third node (K), if used, defines a plane (with I and J) containing the element x and z axes (as shown). If this element is used in a large deflection analysis, it should be noted that the location of the third node (K), or the angle (THETA), is used only to initially orient the element. (For information about orientation nodes and beam meshing, see Meshing Your Solid Model in the Modeling and Meshing Guide.)

The initial strain in the element (ISTRN) is given by Δ/L, where Δ is the difference between the element length, L, (as defined by the I and J node locations) and the zero strain length. The shear deflection constants (SHEARZ and SHEARY) are used only if shear deflection is to be included. A zero value of SHEAR_ may be used to neglect shear deflection in a particular direction.

KEYOPT(2) is used to activate the consistent tangent stiffness matrix (that is, a matrix composed of the main tangent stiffness matrix plus the consistent stress stiffness matrix) in large deflection analyses (NLGEOM,ON). You can often obtain more rapid convergence in a geometrically nonlinear analysis, such as a nonlinear buckling or postbuckling analysis, by activating this option. However, you should not use this option if you are using the element to simulate a rigid link or a group of coupled nodes. The resulting abrupt changes in stiffness within the structure make the consistent tangent stiffness matrix unsuitable for such applications.

KEYOPT(7) is used to compute an unsymmetric gyroscopic damping matrix (often used for rotordynamic analyses). The rotational frequency is input with the SPIN real constant (radians/time, positive in the positive element x direction). The element must be symmetric with this option (for example, IYY = IZZ and SHEARY = SHEARZ).

Element loads are described in Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 4.1: BEAM4 Geometry. Positive normal pressures act into the element. Lateral pressures are input as a force per unit length. End "pressures" are input as a force. Temperatures may be input as element body loads at the eight "corner" locations shown in Figure 4.1: BEAM4 Geometry. The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If only T1 and T2 are input, T3 defaults to T2 and T4 defaults to T1. If only T1 and T4 are input, T2 defaults to T1 and T3 defaults to T4. In both cases, T5 through T8 default to T1 through T4. For any other input pattern, unspecified temperatures default to TUNIF.

KEYOPT(9) is used to request output at intermediate locations. It is based on equilibrium (free body of a portion of the element) considerations and is not valid if:

  • stress stiffening is turned on (SSTIF,ON)

  • more than one component of angular velocity is applied (OMEGA)

  • any angular velocities or accelerations are applied with the CGOMGA, DOMEGA, or DCGOMG commands.

A summary of the element input is given in "BEAM4 Input Summary". A general description of element input is given in Element Input.

BEAM4 Input Summary

Nodes

I, J, K (K orientation node is optional)

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants
AREA, IZZ, IYY, TKZ, TKY, THETA
ISTRN, IXX, SHEARZ, SHEARY, SPIN, ADDMAS
See Table 4.1: BEAM4 Real Constants for a description of the real constants.
Material Properties

EX, ALPX (or CTEX or THSX), DENS, GXY, BETD, ALPD, DMPR

Surface Loads
Pressures -- 
face 1 (I-J) (-Z normal direction)
face 2 (I-J) (-Y normal direction)
face 3 (I-J) (+X tangential direction)
face 4 (I) (+X axial direction)
face 5 (J) (-X axial direction)
(use negative value for opposite loading)
Body Loads
Temperatures -- 

T1, T2, T3, T4, T5, T6, T7, T8

Special Features
Stress stiffening
Large deflection
Birth and death
KEYOPT(2)

Stress stiffening option:

0 -- 

Use only the main tangent stiffness matrix when NLGEOM is ON. (Stress stiffening effects used in linear buckling or other linear prestressed analyses must be activated separately with PSTRES,ON.)

1 -- 

Use the consistent tangent stiffness matrix (that is, a matrix composed of the main tangent stiffness matrix plus the consistent stress stiffness matrix) when NLGEOM is ON. (SSTIF,ON will be ignored for this element when KEYOPT(2) = 1 is activated.)

KEYOPT(6)

Member force and moment output:

0 -- 

No printout of member forces or moments

1 -- 

Print out member forces and moments in the element coordinate system

KEYOPT(7)

Gyroscopic damping matrix:

0 -- 

No gyroscopic damping matrix

1 -- 

Compute gyroscopic damping matrix. Real constant SPIN must be greater than zero. IYY must equal IZZ.

KEYOPT(9)

Output at intermediate points between ends I and J:

N -- 

Output at N intermediate locations (N = 0, 1, 3, 5, 7, 9)

Table 4.1: BEAM4 Real Constants

No.NameDescription
1AREACross-sectional area
2IZZArea moment of inertia
3IYYArea moment of inertia
4TKZThickness along Z axis
5TKYThickness along Y axis
6THETAOrientation about X axis
7ISTRNInitial strain
8IXXTorsional moment of inertia
9SHEARZShear deflection constant Z [1]
10SHEARYShear deflection constant Y [2]
11SPINRotational frequency (required if KEYOPT(7) = 1)
12ADDMASAdded mass/unit length

  1. SHEARZ goes with IZZ; if SHEARZ = 0, there is no shear deflection in the element Y direction.

  2. SHEARY goes with IYY; if SHEARY = 0, there is no shear deflection in the element Z direction.

BEAM4 Output Data

The solution output associated with the element is in two forms:

Several items are illustrated in Figure 4.2: BEAM4 Stress Output.

The maximum stress is computed as the direct stress plus the absolute values of both bending stresses. The minimum stress is the direct stress minus the absolute value of both bending stresses. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 4.2: BEAM4 Stress Output

BEAM4 Stress Output

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file jobname.out. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 4.2: BEAM4 Element Output Definitions

NameDefinitionOR
ELElement numberYY
NODESElement node number (I and J)YY
MATMaterial number for the elementYY
VOLU:Element volume-Y
XC, YC, ZCLocation where results are reportedY3
TEMPTemperatures at integration points T1, T2, T3, T4, T5, T6, T7, T8YY
PRESPressure P1 at nodes I, J; OFFST1 at I, J; P2 at I, J; OFFST2 at I, J; P3 at I, J; OFFST3 at I, J; P4 at I; P5 at JYY
SDIRAxial direct stress11
SBYTBending stress on the element +Y side of the beam11
SBYBBending stress on the element -Y side of the beam 11
SBZTBending stress on the element +Z side of the beam 11
SBZBBending stress on the element -Z side of the beam 11
SMAXMaximum stress (direct stress + bending stress)11
SMINMinimum stress (direct stress - bending stress)11
EPELDIRAxial elastic strain at the end11
EPELBYTBending elastic strain on the element +Y side of the beam 11
EPELBYBBending elastic strain on the element -Y side of the beam 11
EPELBZTBending elastic strain on the element +Z side of the beam 11
EPELBZBBending elastic strain on the element -Z side of the beam 11
EPTHDIRAxial thermal strain at the end11
EPTHBYTBending thermal strain on the element +Y side of the beam11
EPTHBYBBending thermal strain on the element -Y side of the beam11
EPTHBZTBending thermal strain on the element +Z side of the beam11
EPTHBZBBending thermal strain on the element -Z side of the beam11
EPINAXLInitial axial strain in the element1 1
MFOR(X, Y, Z)Member forces in the element coordinate system X, Y, Z directions2Y
MMOM(X, Y, Z)Member moments in the element coordinate system X, Y, Z directions 2Y

  1. The item repeats for end I, intermediate locations (see KEYOPT(9)), and end J.

  2. If KEYOPT(6) = 1.

  3. Available only at centroid as a *GET item.

The following tables list output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) of the Basic Analysis Guide and The Item and Sequence Number Table of this manual for more information. The following notation is used in Table 4.3: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 0) through Table 4.8: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 9):

Name

output quantity as defined in the Table 4.2: BEAM4 Element Output Definitions

Item

predetermined Item label for ETABLE command

E

sequence number for single-valued or constant element data

I,J

sequence number for data at nodes I and J

ILN

sequence number for data at Intermediate Location N

Table 4.3: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 0)

Output Quantity NameETABLE and ESOL Command Input
ItemEIJ
SDIRLS-16
SBYTLS-27
SBYBLS-38
SBZTLS-49
SBZBLS-510
EPELDIRLEPEL-16
EPELBYTLEPEL-27
EPELBYBLEPEL-38
EPELBZTLEPEL-49
EPELBZBLEPEL-510
SMAXNMISC-13
SMINNMISC-24
EPTHDIRLEPTH-16
EPTHBYTLEPTH-27
EPTHBYBLEPTH-38
EPTHBZTLEPTH-49
EPTHBZBLEPTH-510
EPINAXLLEPTH11--
MFORXSMISC-17
MFORYSMISC-28
MFORZSMISC-39
MMOMXSMISC-410
MMOMYSMISC-511
MMOMZSMISC-612
P1SMISC-1314
OFFST1SMISC-1516
P2SMISC-1718
OFFST2SMISC-1920
P3SMISC-2122
OFFST3SMISC-2324
P4SMISC-25-
P5SMISC--26

 Pseudo Node
 12345678
TEMPLBFE12345678

Table 4.4: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 1)

Output Quantity NameETABLE and ESOL Command Input
ItemEIIL1J
SDIRLS-1611
SBYTLS-2712
SBYBLS-3813
SBZTLS-4914
SBZBLS-51015
EPELDIRLEPEL-1611
EPELBYTLEPEL-2712
EPELBYBLEPEL-3813
EPELBZTLEPEL-4914
EPELBZBLEPEL-51015
SMAXNMISC-135
SMINNMISC-246
EPTHDIRLEPTH-1611
EPTHBYTLEPTH-2712
EPTHBYBLEPTH-3813
EPTHBZTLEPTH-4914
EPTHBZBLEPTH-51015
EPINAXLLEPTH16---
MFORXSMISC-1713
MFORYSMISC-2814
MFORZSMISC-3915
MMOMXSMISC-41016
MMOMYSMISC-51117
MMOMZSMISC-61218
P1SMISC-19-20
OFFST1SMISC-21-22
P2SMISC-23-24
OFFST2SMISC-25-26
P3SMISC-27-28
OFFST3SMISC-29-30
P4SMISC-31--
P5SMISC---32

 Pseudo Node
 12345678
TEMPLBFE12345678

Table 4.5: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 3)

Output Quantity NameETABLE and ESOL Command Input
ItemEIIL1IL2IL3J
SDIRLS-16111621
SBYTLS-27121722
SBYBLS-38131823
SBZTLS-49141924
SBZBLS-510152025
EPELDIRLEPEL-16111621
EPELBYTLEPEL-27121722
EPELBYBLEPEL-38131823
EPELBZTLEPEL-49141924
EPELBZBLEPEL-510152025
SMAXNMISC-13579
SMINNMISC-246810
EPTHDIRLEPTH-16111621
EPTHBYTLEPTH-27121722
EPTHBYBLEPTH-38131823
EPTHBZTLEPTH-49141924
EPTHBZBLEPTH-510152025
EPINAXLLEPTH26-----
MFORXSMISC-17131925
MFORYSMISC-28142026
MFORZSMISC-39152127
MMOMXSMISC-410162228
MMOMYSMISC-511172329
MMOMZSMISC-612182430
P1SMISC-31---32
OFFST1SMISC-33---34
P2SMISC-35---36
OFFST2SMISC-37---38
P3SMISC-39---40
OFFST3SMISC-41---42
P4SMISC-43--- 
P5SMISC-----44

 Pseudo Node
 12345678
TEMPLBFE12345678

Table 4.6: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 5)

Output Quantity NameETABLE and ESOL Command Input
ItemEIIL1IL2IL3IL4IL5J
SDIRLS-161116212631
SBYTLS-271217222732
SBYBLS-381318232833
SBZTLS-491419242934
SBZBLS-5101520253035
EPELDIRLEPEL-161116212631
EPELBYTLEPEL-271217222732
EPELBYBLEPEL-381318232833
EPELBZTLEPEL-491419242934
EPELBZBLEPEL-5101520253035
SMAXNMISC-135791113
SMINNMISC-2468101214
EPTHDIRLEPTH-161116212631
EPTHBYTLEPTH-271217222732
EPTHBYBLEPTH-381318232833
EPTHBZTLEPTH-491419242934
EPTHBZBLEPTH-5101520253035
EPINAXLLEPTH36-------
MFORXSMISC-171319253137
MFORYSMISC-281420263238
MFORZSMISC-391521273339
MMOMXSMISC-4101622283440
MMOMYSMISC-5111723293541
MMOMZSMISC-6121824303642
P1SMISC-43-----44
OFFST1SMISC-45-----46
P2SMISC-47-----48
OFFST2SMISC-49-----50
P3SMISC-51-----52
OFFST3SMISC-53-----54
P4SMISC-55------
P5SMISC-------56

 Pseudo Node
 12345678
TEMPLBFE12345678

Table 4.7: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 7)

Output Quantity NameETABLE and ESOL Command Input
ItemEIIL1IL2IL3IL4IL5IL6IL7J
SDIRLS-1611162126313641
SBYTLS-2712172227323742
SBYBLS-3813182328333843
SBZTLS-4914192429343944
SBZBLS-51015202530354045
EPELDIRLEPEL-1611162126313641
EPELBYTLEPEL-2712172227323742
EPELBYBLEPEL-3813182328333843
EPELBZTLEPEL-4914192429343944
EPELBZBLEPEL-51015202530354045
SMAXNMISC-1357911131517
SMINNMISC-24681012141618
EPTHDIRLEPTH-1611162126313641
EPTHBYTLEPTH-2712172227323742
EPTHBYBLEPTH-3813182328333843
EPTHBZTLEPTH-4914192429343944
EPTHBZBLEPTH-51015202530354045
EPINAXLLEPTH46---------
MFORXSMISC-1713192531374349
MFORYSMISC-2814202632384450
MFORZSMISC-3915212733394551
MMOMXSMISC-41016222834404652
MMOMYSMISC-51117232935414753
MMOMZSMISC-61218243036424854
P1SMISC-55-------56
OFFST1SMISC-57-------58
P2SMISC-59-------60
OFFST2SMISC-61-------62
P3SMISC-63-------64
OFFST3SMISC-65-------66
P4SMISC-67--------
P5SMISC---------68

 Pseudo Node
 12345678
TEMPLBFE12345678

Table 4.8: BEAM4 Item and Sequence Numbers (KEYOPT(9) = 9)

Output Quantity NameETABLE and ESOL Command Input
ItemEIIL1IL2IL3IL4IL5IL6IL7IL8IL9J
SDIRLS-16111621263136414651
SBYTLS-27121722273237424752
SBYBLS-38131823283338434853
SBZTLS-49141924293439444954
SBZBLS-510152025303540455055
EPELDIRLEPEL-16111621263136414651
EPELBYTLEPEL-27121722273237424752
EPELBYBLEPEL-38131823283338434853
EPELBZTLEPEL-49141924293439444954
EPELBZBLEPEL-510152025303540455055
SMAXNMISC-13579111315171921
SMINNMISC-246810121416182022
EPTHDIRLEPTH-16111621263136414651
EPTHBYTLEPTH-27121722273237424752
EPTHBYBLEPTH-38131823283338434853
EPTHBZTLEPTH-49141924293439444954
EPTHBZBLEPTH-510152025303540455055
EPINAXLLEPTH56-----------
MFORXSMISC-17131925313743495561
MFORYSMISC-28142026323844505662
MFORZSMISC-39152127333945515763
MMOMXSMISC-410162228344046525864
MMOMYSMISC-511172329354147535965
MMOMZSMISC-612182430364248546066
P1SMISC-67---------68
OFFST1SMISC-69---------70
P2SMISC-71---------72
OFFST2SMISC-73---------74
P3SMISC-75---------76
OFFST3SMISC-77---------78
P4SMISC-79----------
P5SMISC-----------80

 Pseudo Node
 12345678
TEMPLBFE12345678

BEAM4 Assumptions and Restrictions

  • The beam must not have a zero length or area. The moments of inertia, however, may be zero if large deflections are not used.

  • The beam can have any cross-sectional shape for which the moments of inertia can be computed. The stresses, however, will be determined as if the distance between the neutral axis and the extreme fiber is one-half of the corresponding thickness.

  • The element thicknesses are used only in the bending and thermal stress calculations.

  • The applied thermal gradients are assumed to be linear across the thickness in both directions and along the length of the element.

  • If you use the consistent tangent stiffness matrix (KEYOPT(2) = 1), take care to use realistic (that is, "to scale") element real constants. This precaution is necessary because the consistent stress-stiffening matrix is based on the calculated stresses in the element. If you use artificially large or small cross-sectional properties, the calculated stresses will become inaccurate, and the stress-stiffening matrix will suffer corresponding inaccuracies. (Certain components of the stress-stiffening matrix could even overshoot to infinity.) Similar difficulties could arise if unrealistic real constants are used in a linear prestressed or linear buckling analysis (PSTRES,ON).

  • Eigenvalues calculated in a gyroscopic modal analysis can be very sensitive to changes in the initial shift value, leading to potential error in either the real or imaginary (or both) parts of the eigenvalues.

BEAM4 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

Ansys Professional  —  

  • The SPIN real constant (R11) is not available. Input R11 as a blank.

  • KEYOPT(2) can only be set to 0 (default).

  • KEYOPT(7) can only be set to 0 (default).

  • The only special features allowed are stress stiffening and large deflections.