www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS


3-D Linear Finite Strain Beam

MP ME ST PR PRN DS DSS <> <> <> <> PP VT

Product Restrictions

BEAM188 Element Description

BEAM188 is suitable for analyzing slender to moderately stubby/thick beam structures. This element is based on Timoshenko beam theory. Shear deformation effects are included.

BEAM188 is a linear (2-node) or a quadratic beam element in 3-D. BEAM188 has six or seven degrees of freedom at each node, with the number of degrees of freedom depending on the value of KEYOPT(1). When KEYOPT(1) = 0 (the default), six degrees of freedom occur at each node. These include translations in the x, y, and z directions and rotations about the x, y, and z directions. When KEYOPT(1) = 1, a seventh degree of freedom (warping magnitude) is also considered. This element is well-suited for linear, large rotation, and/or large strain nonlinear applications.

BEAM188 includes stress stiffness terms, by default, in any analysis with NLGEOM,ON. The provided stress stiffness terms enable the elements to analyze flexural, lateral, and torsional stability problems (using eigenvalue buckling or collapse studies with arc length methods).

BEAM188 can be used with any beam cross-section defined via SECTYPE, SECDATA, SECOFFSET, SECWRITE, and SECREAD. The cross-section associated with the beam may be linearly tapered.

Elasticity, creep, and plasticity models are supported (irrespective of cross-section subtype). A cross-section associated with this element type can be a built-up section referencing more than one material.

BEAM188 ignores any real constant data beginning with Release 6.0. See the SECCONTROLS command for defining the transverse shear stiffness, and added mass.

For BEAM188, the element coordinate system (/PSYMB,ESYS) is not relevant.

Figure 188.1  BEAM188 Geometry

BEAM188 Input Data

The geometry, node locations, and coordinate system for this element are shown in Figure 188.1: "BEAM188 Geometry". BEAM188 is defined by nodes I and J in the global coordinate system.

Node K is a preferred way to define the orientation of the element. For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the Modeling and Meshing Guide. See the LMESH and LATT command descriptions for details on generating the K node automatically.

BEAM188 may also be defined without the orientation node. In this case, the element x-axis is oriented from node I (end 1) toward node J (end 2). For the two-node option, the default orientation of the element y-axis is automatically calculated to be parallel to the global X-Y plane. 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 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) is used only to initially orient the element.

The beam elements are one-dimensional line elements in space. The cross-section details are provided separately using the SECTYPE and SECDATA commands (see Beam Analysis and Cross Sections in the Structural Analysis Guide for details). A section is associated with the beam elements by specifying the section ID number (SECNUM). A section number is an independent element attribute. In addition to a constant cross-section, you can also define a tapered cross-section by using the TAPER option on the SECTYPE command (see Defining a Tapered Beam).

The beam elements are based on Timoshenko beam theory, which is a first order shear deformation theory: transverse shear strain is constant through the cross-section; that is, cross-sections remain plane and undistorted after deformation. BEAM188 is a first order Timoshenko beam element which uses one point of integration along the length with default KEYOPT(3) setting. Therefore, when SMISC quantities are requested at nodes I and J, the centroidal values are reported for both end nodes. With KEYOPT(3) set to 2, two points of integration are used resulting in linear variation along the length.

BEAM188/BEAM189 elements can be used for slender or stout beams. Due to the limitations of first order shear deformation theory, only moderately "thick" beams may be analyzed. The slenderness ratio of a beam structure (GAL2/(EI)) may be used in judging the applicability of the element, where:


Shear modulus


Area of the cross section


Length of the member


Flexural rigidity

It is important to note that this ratio should be calculated using some global distance measures, and not based on individual element dimensions. The following graphic provides an estimate of transverse shear deformation in a cantilever beam subjected to a tip load. Although the results cannot be extrapolated to any other application, the example serves well as a general guideline. We recommend that the slenderness ratio should be greater than 30.

Figure 188.2  Transverse Shear Deformation Estimation

Slenderness Ratio (GAL2/(EI)) δ Timoshenko / δ Euler-Bernoulli

These elements support an elastic relationship between transverse shear forces and transverse shear strains. You can override default values of transverse shear stiffnesses using the SECCONTROLS command.

The St. Venant warping functions for torsional behavior are determined in the undeformed state, and are used to define shear strain even after yielding. ANSYS does not provide options to recalculate in deformed configuration the torsional shear distribution on cross-sections during the analysis and possible partial plastic yielding of cross-sections. As such, large inelastic deformation due to torsional loading should be treated and verified with caution. Under such circumstances, alternative modeling using solid or shell elements is recommended.

BEAM188/BEAM189 elements support "restrained warping" analysis by making available a seventh degree of freedom at each beam node. By default, BEAM188 elements assume that the warping of a cross-section is small enough that it may be neglected (KEYOPT(1) = 0). You can activate the warping degree of freedom by using KEYOPT(1) = 1. With the warping degree of freedom activated, each node has seven degrees of freedom: UX, UY, UZ, ROTX, ROTY, ROTZ, and WARP. With KEYOPT(1) = 1, bimoment and bicurvature are output.

In practice, when two elements with "restrained warping" come together at a sharp angle, you need to couple the displacements and rotations, but leave the out-of-plane warping decoupled. This is normally accomplished by having two nodes at a physical location and using appropriate constraints. This process is made easier (or automated) by the ENDRELEASE command, which decouples the out-of plane warping for any adjacent elements with cross-sections intersecting at an angle greater than 20 degrees.

BEAM188 allows change in cross-sectional inertia properties as a function of axial elongation. By default, the cross-sectional area changes such that the volume of the element is preserved after deformation. The default is suitable for elastoplastic applications. By using KEYOPT(2), you can choose to keep the cross-section constant or rigid. Scaling is not an option for nonlinear general beam sections (SECTYPE,,GENB).

Element output is available at element integration stations and at section integration points.

Integration stations (Gauss points) along the length of the beam are shown in Figure 188.3: "BEAM188 Element Integration Stations".

Figure 188.3  BEAM188 Element Integration Stations

The section strains and forces (including bending moments) may be obtained at these integration stations. The element supports output options to extrapolate such quantities to the nodes of the element.

BEAM188/BEAM189 can be associated with either of these cross section types:

  • Generalized beam cross sections (SECTYPE,,GENB), where the relationships of generalized stresses to generalized strains are input directly.

  • Standard library section types or user meshes which define the geometry of the beam cross section (SECTYPE,,BEAM). The material of the beam is defined either as an element attribute (MAT), or as part of section buildup (for multi-material cross sections).

Generalized Beam Cross Sections

When using nonlinear general beam sections, neither the geometric properties nor the material is explicitly specified. Generalized stress implies the axial force, bending moments, torque, and transverse shear forces. Similarly, generalized strain implies the axial strain, bending curvatures, twisting curvature, and transverse shear strains. (For more information, see Using Nonlinear General Beam Sections.) This is an abstract method for representing cross section behavior; therefore, input often consists of experimental data or the results of other analyses.

The BEAM188/BEAM189 elements, in general, support an elastic relationship between transverse shear forces and transverse shear strains. You can override default values of transverse shear stiffnesses via the SECCONTROLS command.

When the beam element is associated with a generalized beam (SECTYPE,,GENB) cross section type, the relationship of transverse shear force to the transverse shear strain can be nonlinear elastic or plastic, an especially useful capability when flexible spot welds are modeled. In such a case, the SECCONTROLS command does not apply.

Standard Library Sections

BEAM188/BEAM189 are provided with section-relevant quantities (area of integration, position, Poisson function, function derivatives, etc.) automatically at a number of section points using SECTYPE and SECDATA. Each section is assumed to be an assembly of a predetermined number of 9-node cells. The following graphic illustrates models using the rectangular section subtype and the channel section subtype. Each cross-section cell has 4 integration points and each may be associated with an independent material type.

Figure 188.4  Cross-Section Cells

BEAM188/BEAM189 provide options for output at the section integration points and/or section nodes. You can request output only on the exterior boundary of the cross-section. (PRSSOL prints the section nodal and section integration point results. Stresses and strains are printed at section nodes, and plastic strains, plastic work, and creep strains are printed at section integration points.)

When the material associated with the elements has inelastic behavior or when the temperature varies across the section, constitutive calculations are performed at the section integration points. For more common elastic applications, the element uses precalculated properties of the section at the element integration points. However, the stresses and strains are calculated in the output pass at the section integration points.

If the section is assigned the subtype ASEC, only the generalized stresses and strains (axial force, bending moments, transverse shears, curvatures, and shear strains) are available for output. 3-D contour plots and deformed shapes are not available. The ASEC subtype can be displayed only as a thin rectangle to verify beam orientation.

BEAM188/BEAM189 allow for the analysis of built-up beams, (i.e., those fabricated of two or more pieces of material joined together to form a single, solid beam). The pieces are assumed to be perfectly bonded together. Therefore, the beam behaves as a single member.

The multi-material cross-section capability is applicable only where the assumptions of a beam behavior (Timoshenko or Bernoulli-Euler beam theory) holds.

In other words, what is supported is a simple extension of a conventional Timoshenko beam theory. It may be used in applications such as:

  • bimetallic strips

  • beams with metallic reinforcement

  • sensors where layers of a different material has been deposited

BEAM188/BEAM189 do not account for coupling of bending and twisting at the section stiffness level. The transverse shears are also treated in an uncoupled manner. This may have a significant effect on layered composite and sandwich beams if the layup is unbalanced.

BEAM188/BEAM189 do not use higher order theories to account for variation in distribution of shear stresses. Use ANSYS solid elements if such effects must be considered.

Always validate the application of BEAM188/BEAM189 for particular applications, either with experiments or other numerical analysis. Use the restrained warping option with built-up sections after due verification.

For the mass matrix and evaluation of consistent load vectors, a higher order integration rule than that used for stiffness matrix is employed. The elements support both consistent and lumped mass matrices. Use LUMPM,ON to activate lumped mass matrix. Consistent mass matrix is used by default. An added mass per unit length may be input with the ADDMAS section controls. See "BEAM188 Input Summary".

Forces are applied at the nodes (which also define the element x-axis). If the centroidal axis is not colinear with the element x-axis, applied axial forces will cause bending. Applied shear forces will cause torsional strains and moment if the centroid and shear center of the cross-section are different. The nodes should therefore be located at the desired points where you want to apply the forces. Use the OFFSETY and OFFSETZ arguments of the SECOFFSET command appropriately. By default, ANSYS uses the centroid as the reference axis for the beam elements.

Element loads are described in Node and Element Loads. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 188.1: "BEAM188 Geometry". Positive normal pressures act into the element. Lateral pressures are input as force per unit length. End "pressures" are input as forces.

When KEYOPT(3) = 0 (default), BEAM188 is based on linear polynomials, unlike other Hermitian polynomial-based elements (for example, BEAM4). Refinement of the mesh is recommended in general.

When KEYOPT(3) = 2, ANSYS adds an internal node in the interpolation scheme, effectively making this a Timoshenko beam element based on quadratic shape functions. This option is highly recommended unless this element is used as a stiffener and you must maintain compatibility with a first order shell element. Linearly varying bending moments are represented exactly. The quadratic option is similar to BEAM189, with the following differences:

  • The initial geometry is always a straight line with BEAM188 with or without the quadratic option.

  • Because you cannot access the internal nodes, you cannot define boundary/loading/initial conditions on those nodes; therefore, you will notice discrepancies between BEAM188 and BEAM189 results if both midside and end nodes have specified boundary/loading/initial conditions in a BEAM189 model.

Offsets in specification of distributed loads are not allowed. Non-nodal concentrated forces are not supported. Use the quadratic option (KEYOPT(3) = 2) when the element is associated with tapered cross-sections.

Temperatures may be input as element body loads at three locations at each end node of the beam. At each end, the element temperatures are input at the element x-axis (T(0,0)), at one unit from the x-axis in the element y-direction (T(1,0)), and at one unit from the x-axis in the element z-direction (T(0,1)). The first coordinate temperature T(0,0) defaults to TUNIF. If all temperatures after the first are unspecified, they default to the first. If all temperatures at node I are input, and all temperatures at node J are unspecified, the node J temperatures default to the corresponding node I temperatures. For any other input pattern, unspecified temperatures default to TUNIF.

You can apply an initial stress state to this element via the INISTATE command. For more information, see the INISTATE command, and also Initial Stress Loading in the Basic Analysis Guide. Alternately, you can set KEYOPT(10) = 1 to read initial stresses from the user subroutine USTRESS. For details on user subroutines, see the Guide to ANSYS User Programmable Features.

The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

A summary of the element input is given in "BEAM188 Input Summary".

BEAM188 Input Summary


I, J, K (K, the orientation node, is optional but recommended)

Degrees of Freedom
Section Controls
(TXZ and TXY default to A*GXZ and A*GXY, respectively, where A = cross-sectional area)
Material Properties


Surface Loads
Pressure -- 
face 1 (I-J) (-z normal direction),
face 2 (I-J) (-y normal direction),
face 3 (I-J) (+x tangential direction),
face 4 (J) (+x axial direction),
face 5 (I) (-x direction).
(use a negative value for loading in the opposite direction)
I and J denote the end nodes.
Body Loads
Temperatures -- 

T(0,0), T(1,0), T(0,1) at each end node

Special Features
Viscoelasticity (PRONY, SHIFT)
Viscoplasticity/Creep (CREEP, RATE)
Other material (USER)
Stress stiffening
Large deflection
Large strain
Initial stress import
Nonlinear stabilization
Birth and death (requires KEYOPT(11) = 1)
Automatic selection of element technology
Generalized cross section (nonlinear elastic, elasto-plastic, temperature-dependent)


Items in parentheses refer to data tables associated with the TB command. See the Theory Reference for ANSYS and ANSYS Workbench for details of the material models.


See Automatic Selection of Element Technologies and ETCONTROL for more information on selection of element technologies.


Warping degree of freedom:

0 -- 

Default; six degrees of freedom per node, unrestrained warping

1 -- 

Seven degrees of freedom per node (including warping). Bimoment and bicurvature are output.


Cross-section scaling, applies only if NLGEOM,ON has been invoked:

0 -- 

Default; cross-section is scaled as a function of axial stretch

1 -- 

Section is assumed to be rigid (classical beam theory)


Interpolation scheme:

0 -- 

Default; linear polynomial. Mesh refinement is recommended.

2 -- 

Quadratic shape functions (effectively a Timoshenko beam element); uses an internal node (inaccessible to users) to enhance element accuracy, allowing exact representation of linearly varying bending moments


Shear stress output:

0 -- 

Default; output only torsion-related shear stresses

1 -- 

Output only flexure-related transverse shear stresses

2 -- 

Output a combined state of the previous two types

KEYOPT(6) through KEYOPT(9) are active only when OUTPR,ESOL is active. When KEYOPT(6), (7), (8), and (9) are active, the strains reported in the element output are total strains. "Total" implies the inclusion of thermal strains. When the material associated with the element has plasticity, plastic strain and plastic work are also provided. Alternatively, use PRSSOL in /POST1.


Output control at element integration point:

0 -- 

Default; output section forces, strains, and bending moments

1 -- 

Same as KEYOPT(6) = 0 plus current section area

2 -- 

Same as KEYOPT(6) = 1 plus element basis directions (X,Y,Z)

3 -- 

Output section forces/moments and strains/curvatures extrapolated to element nodes


Output control at section integration point (not available when section subtype = ASEC):

0 -- 

Default; none

1 -- 

Maximum and minimum stresses/strains

2 -- 

Same as KEYOPT(7) = 1 plus stresses and strains at each section point


Output control at section nodes (not available when section subtype = ASEC):

0 -- 

Default; none

1 -- 

Maximum and minimum stresses/strains

2 -- 

Same as KEYOPT(8) = 1 plus stresses and strains along the exterior boundary of the cross-section

3 -- 

Same as KEYOPT(8) = 1 plus stresses and strains at each section node


Output control for extrapolated values at element nodes and section nodes (not available when section subtype = ASEC):

0 -- 

Default; none

1 -- 

Maximum and minimum stresses/strains

2 -- 

Same as KEYOPT(9) = 1 plus stresses and strains along the exterior boundary of the cross-section

3 -- 

Same as KEYOPT(9) = 1 plus stresses and strains at all section nodes


User-defined initial stresses:

0 -- 

No user subroutine to provide initial stresses (default)

1 -- 

Read initial stress data from user subroutine USTRESS


See the Guide to ANSYS User Programmable Features for user written subroutines.


Set section properties:

0 -- 

Automatically determine if pre-integrated section properties can be used (default)

1 -- 

Use numerical integration of section (required for birth/death functionality)


Tapered section treatment:

0 -- 

Linear tapered section analysis; cross section properties are evaluated at each Gauss point (default). This is more accurate, but computationally intense.

1 -- 

Average cross section analysis; for elements with tapered sections, cross section properties are evaluated at the centroid only. This is an approximation of the order of the mesh size; however, it is faster.

BEAM188 Output Data

The solution output associated with these elements is in two forms:

Where necessary, ANSYS recommends KEYOPT(8) = 2 and KEYOPT(9) = 2. See the Basic Analysis Guide for ways to view results.

To view 3-D deformed shapes for BEAM188, issue an OUTRES,MISC or OUTRES,ALL command for static or transient analyses. To view 3-D mode shapes for a modal or eigenvalue buckling analysis, you must expand the modes with element results calculation active (via the MXPAND command's Elcalc = YES option).

Linearized Stress

It is customary in beam design to employ components of axial stress that contribute to axial loads and bending in each direction separately. Therefore, BEAM188 provides a linearized stress output as part of its SMISC output record, as indicated in the following definitions:

SDIR is the stress component due to axial load.

SDIR = FX/A, where FX is the axial load (SMISC quantities 1 and 14) and A is the area of the cross section.

SBYT and SBYB are bending stress components.

SBYT = -MZ * ymax / Izz
SBYB = -MZ * ymin / Izz
SBZT = MY * zmax / Iyy
SBZB = MY * zmin / Iyy

where MY, MZ are bending moments (SMISC quantities 2,15,3,16). Coordinates ymax, ymin, zmax, and zmin are the maximum and minimum y, z coordinates in the cross section measured from the centroid. Values Iyy and Izz are moments of inertia of the cross section. Except for the ASEC type of beam cross section, ANSYS uses the maximum and minimum cross section dimensions. For the ASEC type of cross section, the maximum and minimum in each of Y and Z direction is assumed to be +0.5 to -0.5, respectively.

Corresponding definitions for the component strains are:

EPELBYT = -KZ * ymax
EPELBYB = -KZ * ymin
EPELBZT = KY * zmax
EPELBZB = KY * zmin

where EX, KY, and KZ are generalized strains and curvatures (SMISC quantities 7,8,9, 20,21 and 22).

The reported stresses are strictly valid only for elastic behavior of members. BEAM188 always employs combined stresses in order to support nonlinear material behavior. When the elements are associated with nonlinear materials, the component stresses may at best be regarded as linearized approximations and should be interpreted with caution.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates 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 number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available.

Table 188.1  BEAM188 Element Output Definitions

ELElement numberYY
NODESElement connectivityYY
MATMaterial numberYY
C.G.:X, Y, ZCenter of gravityYY
AREAArea of cross-section1Y
SF:Y, ZSection shear forces1Y
SE:Y, ZSection shear strains1Y
S:XX, XZ, XYSection point stresses2Y
EPTO:XX, XZ, XYSection point total strains (EPEL + EPPL + EPTH)2Y
EPPL:XX, XZ, XYSection point plastic strains2Y
EPCR:XX, XZ, XYSection point creep strains2Y
EPTH:XX, XZ, XYSection point thermal strains2Y
MXTorsional momentYY
KXTorsional strainYY
KY, KZCurvatureYY
EXAxial strainYY
FXAxial forceYY
MY, MZBending momentsYY
SDIRAxial direct stress-1
SBYTBending stress on the element +Y side of the beam-1
SBYBBending stress on the element -Y side of the beam-1
SBZTBending stress on the element +Z side of the beam-1
SBZBBending stress on the element -Z side of the beam-1
EPELDIRAxial strain at the end-1
EPELBYTBending strain on the element +Y side of the beam.-1
EPELBYBBending strain on the element -Y side of the beam.-1
EPELBZTBending strain on the element +Z side of the beam.-1
EPELBZBBending strain on the element -Zside of the beam.-1
TEMPTemperatures T0, T1(1,0), T2(0,1)-1


More output is described via the PRSSOL command in /POST1.

  1. See KEYOPT(6) description.

  2. See KEYOPT(7), KEYOPT(8), KEYOPT(9) descriptions.

  3. See KEYOPT(1) description.

Table 188.2: "BEAM188 Item and Sequence Numbers" lists output available through ETABLE using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this manual for more information. Table 188.2: "BEAM188 Item and Sequence Numbers" uses the following notation:


output quantity as defined in the Table 188.1: "BEAM188 Element Output Definitions"


predetermined Item label for ETABLE


sequence number for data at nodes I and J

Table 188.2  BEAM188 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
S:XX, XZ, XYLSi3 * nNode + i
EPTO:XX, XZ, XYLEPELi3 * nNode + i
EPTH:XX, XZ, XYLEPTHi3 * nNode + i
EPPL:XX, XZ, XYLEPPLi3 * nIntg + i
EPCR:XX, XZ, XYLEPCRi3 * nIntg + i


The value i in Table 188.2: "BEAM188 Item and Sequence Numbers" refers to the order of the node or integration point of the beam where 1 i (3 * nNode) (number of nodes), or 1 i (3 * nIntg) (number of integration points).

For more usage details, see Plot and Review the Section Results and Sample Problem with Cantilever Beams, Command Method.

Transverse Shear Stress Output

BEAM188/BEAM189 formulation is based on three stress components:

  • one axial

  • two shear stress components

The shear stresses are caused by torsional and transverse loads. BEAM188/BEAM189 are based on first order shear deformation theory, also popularly known as Timoshenko Beam theory. The transverse shear strain is constant for the cross section, and hence the shear energy is based on a transverse shear force. This shear force is redistributed by predetermined shear stress distribution coefficients across the beam cross-section, and made available for output purposes. By default, ANSYS will only output the shear stresses caused by torsional loading. KEYOPT(4) of BEAM188/BEAM189 may be used to activate output of shear stresses caused by flexure or transverse loading.

The accuracy of transverse shear distribution is directly proportional to the mesh density of cross-section modeling (for determination of warping, shear center and other section geometric properties). The traction free state at the edges of cross-section, is met only in a well-refined model of the cross-section.

By default, ANSYS uses a mesh density (for cross-section model) that provides accurate results for torsional rigidity, warping rigidity, inertia properties, and shear center determination. The default mesh employed is also appropriate for nonlinear material calculations. However, more refined cross-section models may be necessary if the shear stress distribution due to transverse loads must be captured very accurately. Note that increasing cross-section mesh size, does not imply larger computational cost if the associated material is linear. SECTYPE and SECDATA command descriptions allow specification of cross-section mesh density.

The transverse shear distribution calculation neglects the effects of Poisson's ratio. The Poisson's ratio affects the shear correction factor and shear stress distribution slightly.

BEAM188 Assumptions and Restrictions

  • The beam must not have zero length.

  • By default (KEYOPT(1) = 0), the effect of warping restraint is assumed to be negligible.

  • Cross-section failure or folding is not accounted for.

  • Rotational degrees of freedom are not included in the lumped mass matrix if offsets are present.

  • It is a common practice in civil engineering to model the frame members of a typical multi-storied structure using a single element for each member. Because of cubic interpolation of lateral displacement, BEAM4 and BEAM44 are well-suited for such an approach. However, if BEAM188 is used in that type of application, be sure to use several elements for each frame member. BEAM188 includes the effects of transverse shear.

  • This element works best with the full Newton-Raphson solution scheme (that is, the default choice in solution control). For nonlinear problems that are dominated by large rotations, we recommend that you do not use PRED,ON.

  • Note that only moderately "thick" beams may be analyzed. See "BEAM188 Input Data" for more information.

  • When a cross-section has multiple materials and you issue the /ESHAPE command (which displays elements with shapes determined from the real constants or section definition) to produce contour plots of stresses (and other quantities), the element averages the stresses across material boundaries. To limit this behavior, use small cross-section cells around the material boundaries. There are no input options to bypass this behavior.

  • For this element, the /ESHAPE command supports visualization of stresses, but not of plastic strains.

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). It is ignored in geometrically linear analyses (NLGEOM,OFF) when specified by SSTIF,ON. Prestress effects can be activated by the PSTRES command.

  • When the element is associated with nonlinear general beam sections (SECTYPE,,GENB), additional restrictions apply. For more information, see Considerations for Employing Nonlinear General Beam Sections.

BEAM188 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 only special features allowed are stress stiffening and large deflections.