3-D 3-Node Elbow
MP ME ST PR PRN <> <> <> <> <> <> PP <> EME MFS

ELBOW290 Element Description

The ELBOW290 element is suitable for analyzing pipe structures with initially circular cross-sections and thin to moderately thick pipe walls. The element accounts for cross-section distortion, which can be commonly observed in curved pipe structures under loading.

ELBOW290 is a quadratic (three-node) pipe element in 3-D. The element has six degrees of freedom at each node (the translations in the x, y, and z directions and rotations about the x, y, and z directions). The element is well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in pipe thickness is accounted for in geometrically nonlinear analyses. The element accounts for follower (load stiffness) effects of distributed pressures.

ELBOW290 can be used in layered applications for modeling laminated composite pipes. The accuracy in modeling composite pipes is governed by the first-order shear-deformation theory (generally referred to as Mindlin-Reissner shell theory).

ELBOW290 supports the pipe cross-section defined via SECTYPE, SECDATA, and SECOFFSET commands.

For more detailed information about this element, see ELBOW290 - 3-D 3-Node Elbow in the Mechanical APDL Theory Reference.

Figure 290.1  ELBOW290 Geometry

ELBOW290 Geometry

A general description of the element coordinate system is available in Coordinate Systems in this document. Following is information about specific coordinate systems as they apply to ELBOW290.

Beam Coordinate Systems

The beam coordinate systems (x-y-z) are used for defining beam offsets and diametral temperature gradients.

No orientation node (default)

Using orientation node L

The x axis is always the axial direction pointing from node I to node J. The optional orientation node L, if used, defines a plane containing the x and z axes at node K. If this element is used in a large-deflection analysis, the location of the orientation node L is used only to initially orient the element.

When no orientation node is used, z is perpendicular to the curvature plane, uniquely determined by the I, J, and K nodes. If I, J, and K are colinear, the y axis is automatically calculated to be parallel to the global X-Y plane. In cases where the element is parallel to the global Z axis (or within a 0.01 percent slope of the axis), the element y axis is oriented parallel to the global Y axis.

For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the Modeling and Meshing Guide. See Quadratic Elements (Midside Nodes) in the same document for information about midside nodes. For details about generating the optional orientation node L automatically, see the LMESH and LATT command descriptions.

Local Cylindrical Coordinate Systems

The cylindrical coordinate systems (A-R-T) are used for defining internal section motions (that is, axial-A, radial-R, and hoop-T displacements and rotations).

The cylindrical systems are always created from the default beam coordinate systems (beam system without orientation node L), with A being the same as beam axis x, and an angle α (0 < α < 360 degrees) from R to the beam axis y.

Element and Layer Coordinate Systems

The element coordinate systems (e1-e2-e3) are defined at the mid-surfaces of the pipe wall. The e1, e2, and e3 axes are parallel respectively to cylindrical axes A, T, and R in the undeformed configuration. Each element coordinate system is updated independently to account for large material rotation during a geometrically nonlinear analysis. Support is not available for user-defined element coordinate systems.

The layer coordinate systems (L1-L2-L3) are identical to the element coordinate system if no layer orientation angles are specified; otherwise, the layer coordinate system can be generated by rotating the corresponding element coordinate system about the shell normal (axis e3). Material properties are defined in the layer systems; therefore, the layer system is also called the material coordinate system.

ELBOW290 Input Data

The geometry and node locations for ELBOW290 are shown in Figure 290.1. The element is defined by nodes I, J, and K in the global coordinate system.

When using ELBOW290, the subtended angle φ should not exceed 45 degrees:

ELBOW290 Cross Sections

The element is a one-dimensional line element in space. The cross-section details are provided separately (via the SECDATA command). A section is associated with the element by specifying the section ID number (SECNUM). A section number is an independent element attribute.

ELBOW290 can only be associated with the pipe cross section (SECTYPE,,PIPE). For elements with homogenous materials, the material of the pipe is defined as an element attribute (MAT).

The layup of a composite pipe can be defined with a shell section (SECTYPE). Shell section commands provide the input options for specifying the thickness, material, orientation and number of integration points through the thickness of the layers. ANSYS obtains the actual layer thicknesses used for ELBOW290 element calculations (by scaling the input layer thickness) so that they are consistent with the total wall thickness given by the pipe section. A single-layer shell section definition is possible, allowing flexibility with regard to the number of integration points used and other options.

For shell section input, you can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. When only one integration point is specified, the point is always located midway between the top and bottom surfaces. If three or more points are specified, one point is located on the top surface, one point is located on the bottom surface, and the remaining points are distributed at equal distances between the top and bottom points. The default number of integration points for each layer is 3. When a single layer is defined and plasticity is present, however, the number of integration points is changed to a minimum of five during solution.

In "Element and Layer Coordinate Systems", the layer coordinate system can be obtained by rotating the corresponding element coordinate system about the shell normal (axis e3) by angle θ (in degrees). The value of θ for each layer is given by the SECDATA command input for the shell section.

For details about associating a shell section with a pipe section, see the SECDATA command documentation.

Cross-Section Deformation

The level of accuracy in elbow cross-sectional deformation is given by the number of Fourier terms around the circumference of the cross section. The accuracy can be adjusted via KEYOPT(2) = n, where n is an integer value from 0 through 8, as follows:

KEYOPT(2) = 0 -- Only uniform radial expansion and transverse shears through the pipe wall are allowed. Suitable for simulating straight pipes without undergoing bending.
KEYOPT(2) = 1 -- Radial expansion and transverse shears are allowed to vary along the circumference to account for bending. Suitable for straight pipes in small-deformation analysis.
KEYOPT(2) = 2 through 8 -- Allow general section deformation, including radial expansion, ovalization, and warping. Suitable for curved pipes or straight pipes in large-deformation analysis. The default is KEYOPT(2) = 2. Higher values for KEYOPT(2) may be necessary for pipes with thinner walls, as they are more susceptible to complex cross-section deformation than are pipes with thicker walls.

Element computation becomes more intensive as the value of KEYOPT(2) increases. Use a KEYOPT(2) value that offers an optimal balance between accuracy and computational cost.

Cross-Section Constraints

The constraints on the elbow cross-section can be applied at the element nodes I, J, and K with the following section degrees of freedom labels:

SE – section radial expansion
SO – section ovalization
SW – section warping
SRA – local shell normal rotation about cylindrical axis A
SRT – local shell normal rotation about cylindrical axis T
SECT – all section deformation

Only fixed cross-section constraints are allowed via the D command. Delete section constraints via the DDELE command. For example, to constrain the warping and ovalization of the cross-section at node n, issue this command:


To allow only the radial expansion of the cross-section, use the following commands:


It is not practical to maintain the continuity of cross-section deformation between two adjacent elements joined at a sharp angle. For such cases, ANSYS recommends coupling the nodal displacements and rotations but leaving the cross-section deformation uncoupled. The ELBOW command can automate the process by uncoupling the cross-section deformation for any adjacent elements with cross-sections intersecting at an angle greater than 20 degrees.

Element loads are described in Nodal Loading. Forces are applied at the nodes. By default, ELBOW290 element nodes are located at the center of the cross-section. Use the SECOFFSET command's OFFSETY and OFFSETZ arguments for the pipe section to define locations other than the centroid for force application.

Pressures may be input as surface loads on the element faces as shown by the circled numbers in the following illustration. Positive pressures act into the pipe wall.

The end-cap pressure effect is included by default. The end-cap effect on one or both ends of the element can be deactivated via KEYOPT(6). When subjected to internal and external pressures, ELBOW290 with end caps (KEYOPT(6) = 0) is always in equilibrium; that is, no net forces are produced. Without end caps (KEYOPT(6) = 1), the element is also in equilibrium except for the case when the element is curved. With end caps only at one end (KEYOPT(6) = 2 or 3), the element is obviously not in equilibrium.

Pressure Load Stiffness

The effects of pressure load stiffness are included by default for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, issue an NROPT,UNSYM command.


When KEYOPT(1) = 0, a layer-wise pattern is used. T1 and T2 are temperatures at inner wall, T3 and T4 and the interface temperatures between layer 1 and layer 2, ending with temperatures at the exterior of the pipe. All undefined temperatures are default to TUNIF. If exactly (NL + 1) temperatures are given (where NL is the number of layers), then one temperature is taken as the uniform temperature at the bottom of each layer, with the last temperature for the exterior of the pipe.

When KEYOPT(1) = 1, temperatures can be input as element body loads at three locations at both end nodes of the element so that the temperature varies linearly in the beam y axis and z axis directions. At both ends, the element temperatures are input at the section centroid (TAVG), at the outer radius from the centroid in the element y direction (Ty), and at the outer radius from the centroid in the element z-direction (Tz). The first coordinate temperature TAVG 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. The following graphic illustrates temperature input when KEYOPT(1) = 1:

Transverse Shear Stiffness

ELBOW290 includes the effects of transverse shear deformation through the pipe wall. The transverse shear stiffness of the element is a 2 x 2 matrix, as shown:

For a single-layer elbow with isotropic material, default transverse shear stiffnesses are as follows:

where k = 5/6, G = shear modulus, and h = pipe wall thickness.

You can override the default transverse shear stiffness values by assigning different values via the SECCONTROLS command for the shell section.

ELBOW290 Input Summary


I, J, K, and L (the optional orientation node)

Degrees of Freedom
Section Information
Accessed via SECTYPE,,PIPE and SECDATA commands.
Material Properties
Specify BETD only once for the element (use MAT command to assign the material property set). REFT may be provided once for the element, or it may assigned on a per-layer basis.
Surface Loads
Pressure -- 
Internal pressure
External pressure
Body Loads
Temperatures -- 
For KEYOPT(1) = 0 -- T1, T2 (at bottom of layer 1), T3, T4 (between layers 1-2); similarly for between next layers, ending with temperatures at top of layer NL (2 * (NL + 1) maximum).
For KEYOPT(1) = 1 -- TAVG(I), Ty(I), Tz(I), TAVG(J), Ty(J), Tz(J)
Special Features
Birth and death
Large deflection
Large strain
Nonlinear stabilization
Stress stiffening
User-defined material
Viscoplasticity / Creep

Temperature input

0 -- 

Layerwise input

1 -- 

Diametral gradient


Number of Fourier terms (used for cross-sectional flexibility)

0 -- 

Uniform radial expansion

1 -- 

Nonuniform radial expansion to account for bending

2 through 8 --

General section deformation (default = 2)


End cap loads

0 -- 

Internal and external pressures cause loads on end caps

1 -- 

Internal and external pressures do not cause loads on end caps

2 -- 

Internal and external pressures cause loads on element node I

3 -- 

Internal and external pressures cause loads on element node J


Specify layer data storage:

0 -- 

Store data for bottom of bottom layer and top of top layer (multilayer elements) (default)

1 -- 

Store data for TOP and BOTTOM, for all layers (multilayer elements)

2 -- 

Store data for TOP, BOTTOM, and MID for all layers; applies to single-layer and multilayer elements. (The volume of data may be considerable.)

ELBOW290 Output Data

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

Integration Stations

Integration stations along the length and within the cross-section of the elbow are shown in Figure 290.2.

Figure 290.2  ELBOW290 Element Integration Stations

ELBOW290 Element Integration Stations

Element solution is available at all integration points through element printout (OUTPR). Solution via the POST1 postprocessor is available at element nodes and selected section integration locations (see KEYOPT(8) settings for more details).

Stress Output

Several items are illustrated in Figure 290.3:

Figure 290.3  ELBOW290 Stress Output

ELBOW290 Stress Output

KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available at the layer interfaces. KEYOPT(8) must be set to either 1 or 2 to output these stresses in the POST1 postprocessor. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to review results.

The element shell stress resultants (N11, M11, Q13, etc.) are parallel to the element coordinate system (e1-e2-e3), as are the shell membrane strains and curvatures (ε11, κ11, γ13, etc.) of the element. Shell stress resultants and generalized shell strains are available via the SMISC option at the element end nodes I and J only.

ELBOW290 also outputs beam-related stress resultants (Fx, My, TQ, etc) and linearized stresses (SDIR, SByT, SByB, etc) at two element end nodes I and J to SMISC records. Beam stress resultants and linearized stresses are parallel to the beam coordinate system (x-y-z).

Linearized Stress

It is customary in pipe design to employ components of axial stress that contribute to axial loads and bending in each direction separately. Therefore, ELBOW290 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 36) and A is the area of the cross section (SMISC quantities 7 and 42).

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 2,37,3,38). 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.

The reported stresses are strictly valid only for elastic behavior of members. ELBOW290 always employs combined stresses in order to support nonlinear material behavior. When the elements are associated with nonlinear materials, the component stresses can at best be regarded as linearized approximations and should be interpreted with caution.

ELBOW290 does not provide extensive element printout. Because the POST1 postprocessor provides more comprehensive output processing tools, ANSYS suggests issuing the OUTRES command to ensure that the required results are stored in the database. To view 3-D deformed shapes for ELBOW290, 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, expand the modes with element results calculation active via the MXPAND command's Elcalc = YES option.

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 number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 290.1  ELBOW290 Element Output Definitions

ELElement numberYY
NODESElement connectivity-Y
MATMaterial number-Y
THICKAverage wall thickness-Y
AREAArea of cross-section-Y
XC, YC, ZCLocation where results are reported-4
LOCI:X, Y, ZIntegration point locations-5
TEMPT1, T2 at bottom of layer 1, T3, T4 between layers 1-2, similarly for between next layers, ending with temperatures at top of layer NL (2 * (NL + 1) maximum)-Y
LOCTOP, MID, BOT, or integration point location-1
S:X, Y, Z, XY, YZ, XZStresses31
S:INTStress intensity-1
S:EQVEquivalent stress-1
EPEL:X, Y, Z, XYElastic strains31
EPEL:EQVEquivalent elastic strains [7]-1
EPTH:X, Y, Z, XYThermal strains31
EPTH:EQVEquivalent thermal strains [7]-1
EPPL:X, Y, Z, XYAverage plastic strains32
EPPL:EQVEquivalent plastic strains [7]-2
EPCR:X, Y, Z, XYAverage creep strains32
EPCR:EQVEquivalent creep strains [7]-2
EPTO:X, Y, Z, XYTotal mechanical strains (EPEL + EPPL + EPCR)3-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)--
NL:EPEQAccumulated equivalent plastic strain-2
NL:CREQAccumulated equivalent creep strain-2
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding)-2
NL:PLWKPlastic work-2
NL:HPRESHydrostatic pressure-2
SEND:ELASTIC, PLASTIC, CREEPStrain energy densities-2
FxSection axial force-Y
My, MzSection bending moments-Y
TQSection torsional moment-Y
SFy, SFzSection shear forces -Y
SDIRAxial direct stress -Y
SByTBending stress on the element +y side of the pipe -Y
SByBBending stress on the element -y side of the pipe -Y
SBzTBending stress on the element +z side of the pipe -Y
SBzBBending stress on the element -z side of the pipe -Y
N11, N22, N12Wall in-plane forces (per unit length)-Y
M11, M22, M12 Wall out-of-plane moments (per unit length) -Y
Q13, Q23 Wall transverse shear forces (per unit length) -Y
 ε11, ε22, ε12 Wall membrane strains -Y
 κ11, κ22, κ12 Wall curvatures -Y
 γ13, γ23 Wall transverse shear strains -Y
SVAR:1, 2, ... , NState variables -6
  1. The subsequent stress solution repeats for top, middle, and bottom surfaces.

  2. Nonlinear solution output for top, middle, and bottom surfaces, if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.

  3. Stresses, total strains, plastic strains, elastic strains, creep strains, and thermal strains in the element coordinate system are available for output (at all section points through thickness). If layers are in use, the results are in the layer coordinate system.

  4. Available only at the centroid as a *GET item.

  5. Available via an OUTRES,LOCI command only.

  6. Available only if the UserMat subroutine and TB,STATE command are used.

  7. The equivalent strains use an effective Poisson's ratio. For elastic and thermal, you set the value (MP,PRXY). For plastic and creep, ANSYS sets the value at 0.5.

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

Table 290.2: ELBOW290 Item and Sequence Numbers lists output available for the ETABLE command using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The output tables use the following notation:


output quantity as defined in Table 290.1: ELBOW290 Element Output Definitions


predetermined Item label for ETABLE


sequence number for data at nodes I and J

Table 290.2  ELBOW290 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input

ELBOW290 Assumptions and Restrictions

  • The element cannot have zero length.

  • Zero wall thickness is not allowed. (Zero thickness layers are allowed.)

  • In a nonlinear analysis, the solution is terminated if the thickness at any integration point vanishes (within a small numerical tolerance).

  • This element works best with the full Newton-Raphson solution scheme (the default behavior in solution control).

  • No slippage is assumed between the element layers. Shear deflections are included in the element; however, normals to the center wall surface before deformation are assumed to remain straight after deformation.

  • If multiple load steps are used, the number of layers must remain unchanged between load steps.

  • If the layer material is hyperelastic, the layer orientation angle has no effect .

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Apply prestress effects via a PSTRES command.

  • The through-thickness stress SZ is always zero.

  • The effects of fluid motion inside the pipe are ignored.

ELBOW290 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.

Release 14.0 - © 2011 SAS IP, Inc. All rights reserved.