BEAM189 Element Description

The BEAM189 element is suitable for analyzing slender to moderately stubby/thick beam structures. The element is based on Timoshenko beam theory which includes shear-deformation effects. The element provides options for unrestrained warping and restrained warping of cross-sections.

The element is a quadratic three-node beam element in 3-D. With default settings, 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. An optional seventh degree of freedom (warping magnitude) is available. The element is well-suited for linear, large rotation, and/or large-strain nonlinear applications.

The element 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 or nonlinear stabilization).

Elasticity, plasticity, creep and other nonlinear material models are supported. A cross-section associated with this element type can be a built-up section referencing more than one material. Added mass, hydrodynamic added mass and loading, and buoyant loading are available.

For more detailed information about this element, see BEAM189 - 3-D 3-Node Beam in the Mechanical APDL Theory Reference.

Figure 189.1:  BEAM189 Geometry

BEAM189 Element Technology and Usage Recommendations

BEAM189 is 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).

The element can be used for slender or stout beams. Due to the limitations of first-order shear-deformation theory, slender to moderately thick beams can be analyzed. Use the slenderness ratio of a beam structure (GAL²/(EI)) to judge the applicability of the element, where:

Calculate the ratio using some global distance measures, rather than basing it upon individual element dimensions. The following illustration shows 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. A slenderness ratio greater than 30 is recommended.

Figure 189.2:  Transverse-Shear Deformation Estimation

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 SECCONTROL command.

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

BEAM189 supports “restrained warping” analysis by making available a seventh degree of freedom at each beam node. By default, BEAM189 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, ROTZ, ROTY, and WARP. With KEYOPT(1) = 1, bimoment and bicurvature are output.

Unlike other cubic (Hermitian) polynomial-based elements, BEAM189 is based on quadratic polynomials; therefore, offsets in specification of distributed pressure loads are not allowed.BEAM189 has linear bending-moment variation. Refinement of the mesh is recommended in order to accommodate such loading. BEAM189 is computationally efficient and has super-convergence properties with respect to mesh refinement. For example, the quadratic beam with a two point Gaussian integration is known to be of same accuracy as a Hermitian element.

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.

BEAM189 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).

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. Avoid using LUMPM,ON as BEAM189 is a higher-order element. Consistent mass matrix is used by default. You can add mass per unit length via the SECCONTROL command's ADDMAS values. See "BEAM189 Input Summary".

When ocean loading is applied, the loading is nonlinear (that is, based on the square of the relative velocity between the structure and the water). Accordingly, the full Newton-Raphson option (NROPT,FULL) may be necessary to achieve optimal results. (Full Newton-Raphson is applied automatically in an analysis involving large-deflection effects [NLGEOM,ON].)

The St. Venant warping functions for torsional behavior are determined in the undeformed state, and are used to define shear strain even after yielding. No options are available for recalculating 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.

BEAM189 Input Data

The geometry, node locations, coordinate system, and pressure directions for this element are shown in Figure 189.1: BEAM189 Geometry. BEAM189 is defined by nodes I, J, and K in the global coordinate system.

Node L 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. Also, see Quadratic Elements (Midside Nodes) in the same manual for the use of midside nodes. See the LMESH and LATT command descriptions for details on generating the L node automatically. For a description of the low-order beam, see BEAM188.

The element can also be defined without the orientation node L. In this case, the element x-axis is oriented from node I (end 1) toward node J (end 2). When no orientation node is used, 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 L node option. If both are defined, the orientation node option takes precedence. The orientation node L, if used, defines a plane (with I and J) containing the element x and z-axes (as shown). If using this element in a large-deflection analysis, be aware that the location of the orientation node L is used only to initially orient the element.

The number of degrees of freedom depends 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.

The element is a one-dimensional line element in space. The cross-section details are provided separately via 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 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. (For more information, see Defining a Tapered Beam or Pipe.)

BEAM189 ignores any real constant data beginning with Release 6.0. See SECCONTROL command for defining the transverse-shear stiffness, and added mass.

A summary of the element input follows in "BEAM189 Input Summary".

BEAM189 Cross-Sections

BEAM189 can be associated with these cross-section types (SECTYPE,,Type):

Standard Library Sections

BEAM189 is provided with section-relevant quantities (area of integration, position, 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 nine-node cells. Each cross-section cell has four integration points and each can be associated with an independent material type.

Figure 189.3:  Cross-Section Cells

The number of cells in the cross-sections influences the accuracy of section properties and ability to model nonlinear stress-strain relationship through the cross-section. The element has a nested structure of integration (along the length and in the cross-section).

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 nodes.

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 is displayed only as a thin rectangle to verify beam orientation. BEAM189 treats ASEC as a section type with just one cross-section integration point.

BEAM189 is helpful for analyzing built-up beams, (that is, 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 assumption of beam behavior (Timoshenko or Bernoulli-Euler beam theory) holds.

Therefore, the element models a simple extension of a conventional Timoshenko beam and can be used in applications such as:

BEAM189 does 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 lay-up is unbalanced.

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

KEYOPT(15) specifies the format of the .rst results file. For KEYOPT(15) = 0, the format gives only one averaged result at each section corner node; therefore, this option typically applies to homogeneous sections. For KEYOPT(15) = 1, the format gives one result for each section integration point; therefore, this option typically applies to built-up sections with multiple materials (and generates a larger results file).

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 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.

Generally, BEAM189 supports an elastic relationship between transverse-shear forces and transverse-shear strains. You can override default values of transverse-shear stiffnesses via the SECCONTROL 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 SECCONTROL command does not apply.

Tapered Beam Cross-Sections

A linearly tapered beam is defined by specifying a standard library section or user mesh at each end of the beam. The section geometries are specified at global coordinates, then linear interpolated and evaluated at the element. The sections at the end points must be topologically identical. (For more information, see Defining a Tapered Beam or Pipe.)

BEAM189 Loads

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 points where you want to apply the forces. Use the OFFSETY and OFFSETZ arguments of the SECOFFSET command appropriately.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 189.1: BEAM189 Geometry. Positive normal pressures act into the element. Lateral pressures are input as force per unit length. End "pressures" are input as forces.

At both ends of the element, temperatures can be input at these locations:

Element locations (T(y,z)) are given according to the convention used in Figure 189.1: BEAM189 Geometry.

For beam elements, element body load commands (BFE) accept an element number and a list of values, 1 through 6 for temperatures T_I(0,0), T_I(1,0), T_I(0,1), T_J(0,0), T_J(1,0), and T_J(0,1). This input can be used to specify temperature gradients that vary linearly both over the cross section and along the length of the element.

The following defaults apply to element temperature input:

Alternatively, temperatures at nodes I and J can be defined using nodal body loads (BF,NODE,TEMP,VAL1). When using a nodal body load to define a temperature, a uniform temperature is applied over the cross section at the specified node. (BF command input is not accepted at node K.)

Temperature gradients across the cross-section are not allowed when the beam section has an arbitrary (ASEC) subtype, where the integrated cross-section inertia properties are user-defined (SECTYPE,,BEAM,ASEC).

You can apply an initial stress state to this element via the INISTATE command. For more information, see Initial State in the Basic Analysis Guide.

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.

BEAM189 Output Data

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

To view 3-D deformed shapes for BEAM189, 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, BEAM189 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.

where My, Mz are bending moments (SMISC quantities 2,15,3,16). Coordinates y_max, y_min, z_max, and z_min 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, the program 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:

where Ex, Ky, and Kz are generalized strains and curvatures (SMISC quantities 7,8,9, 20,21 and 22).

The reported linearized stresses are strictly valid only for elastic behavior of members. BEAM189 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:

In the table below, 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 “-” indicates that the item is not available.

More output is described via the PRESOL and *GET,,SECR commands in POST1.

Table 189.2: BEAM 189 Item and Sequence Numbers lists output available via the ETABLE and ESOL commands using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The table uses the following notation:

For more usage details, see Plot and Review the Section Results and Example: Problem with Cantilever Beams.

Transverse-Shear Stress Output

The BEAM189 formulation is based on three stress components:

The shear stresses are caused by torsional and transverse loads. BEAM189 is based on first-order shear-deformation theory, also popularly known as Timoshenko beam theory. The transverse-shear strain is constant for the cross-section; therefore, the shear energy is based on a transverse-shear force. The shear force is redistributed by predetermined shear-stress distribution coefficients across the beam cross-section, and made available for output purposes. By default, the program outputs only the shear stresses caused by torsional loading. Use KEYOPT(4) 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 a cross-section is met only in a well-refined model of the cross-section.

By default, the program uses a mesh density (for cross-section modeling) 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. Increasing cross-section mesh size does not imply larger computational cost if the cross-section is homogeneous and the associated material is linear. Use the SECTYPE and SECDATA commands to adjust cross-section mesh density.

The transverse-shear distribution calculation ignores the effects of Poisson's ratio. The Poisson's ratio affects the shear-correction factor and shear-stress distribution slightly, and this effect is ignored.

BEAM189 Assumptions and Restrictions

BEAM189 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 Mechanical Pro 

ANSYS Mechanical Premium