ELBOW290

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*.

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.

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.

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.

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.

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:

D,n,SW,,,,,SO

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.

**Temperatures**

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.

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

**Degrees of Freedom**UX, UY, UZ, ROTX, ROTY, ROTZ **Section Information**Accessed via **SECTYPE**,,PIPE and**SECDATA**commands.**Material Properties**EX, EY, EZ, (PRXY, PRYZ, PRXZ, or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, GXY, GYZ, GXZ, ALPD 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 Elasticity Hyperelasticity Large deflection Large strain Nonlinear stabilization Plasticity Stress stiffening User-defined material Viscoelasticity Viscoplasticity / Creep **KEYOPT(1)**Temperature input

**0 --**Layerwise input

**1 --**Diametral gradient

**KEYOPT(2)**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)

**KEYOPT(6)**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

**KEYOPT(8)**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.)

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

Nodal displacements and reactions included in the overall nodal solution

Additional element output as described in Table 290.1: ELBOW290 Element Output Definitions

**Integration Stations**

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

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:

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 (ε_{11}, κ_{11}, γ_{13}, 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 * y_{max} / Izz |

SByB = -Mz * y_{min} / Izz |

SBzT = My * z_{max} / Iyy |

SBzB = My * z_{min} / Iyy |

where My, Mz are bending moments (SMISC quantities 2,37,3,38).
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.

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**

Name | Definition | O | R |
---|---|---|---|

EL | Element number | Y | Y |

NODES | Element connectivity | - | Y |

MAT | Material number | - | Y |

THICK | Average wall thickness | - | Y |

AREA | Area of cross-section | - | Y |

XC, YC, ZC | Location where results are reported | - | 4 |

LOCI:X, Y, Z | Integration point locations | - | 5 |

TEMP | 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) | - | Y |

LOC | TOP, MID, BOT, or integration point location | - | 1 |

S:X, Y, Z, XY, YZ, XZ | Stresses | 3 | 1 |

S:INT | Stress intensity | - | 1 |

S:EQV | Equivalent stress | - | 1 |

EPEL:X, Y, Z, XY | Elastic strains | 3 | 1 |

EPEL:EQV | Equivalent elastic strains [7] | - | 1 |

EPTH:X, Y, Z, XY | Thermal strains | 3 | 1 |

EPTH:EQV | Equivalent thermal strains [7] | - | 1 |

EPPL:X, Y, Z, XY | Average plastic strains | 3 | 2 |

EPPL:EQV | Equivalent plastic strains [7] | - | 2 |

EPCR:X, Y, Z, XY | Average creep strains | 3 | 2 |

EPCR:EQV | Equivalent creep strains [7] | - | 2 |

EPTO:X, Y, Z, XY | Total mechanical strains (EPEL + EPPL + EPCR) | 3 | - |

EPTO:EQV | Total equivalent mechanical strains (EPEL + EPPL + EPCR) | - | - |

NL:EPEQ | Accumulated equivalent plastic strain | - | 2 |

NL:CREQ | Accumulated equivalent creep strain | - | 2 |

NL:SRAT | Plastic yielding (1 = actively yielding, 0 = not yielding) | - | 2 |

NL:PLWK | Plastic work | - | 2 |

NL:HPRES | Hydrostatic pressure | - | 2 |

SEND:ELASTIC, PLASTIC, CREEP | Strain energy densities | - | 2 |

Fx | Section axial force | - | Y |

My, Mz | Section bending moments | - | Y |

TQ | Section torsional moment | - | Y |

SFy, SFz | Section shear forces | - | Y |

SDIR | Axial direct stress | - | Y |

SByT | Bending stress on the element +y side of the pipe | - | Y |

SByB | Bending stress on the element -y side of the pipe | - | Y |

SBzT | Bending stress on the element +z side of the pipe | - | Y |

SBzB | Bending stress on the element -z side of the pipe | - | Y |

N11, N22, N12 | Wall 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 |

ε_{11}, ε_{22}, ε_{12} | Wall membrane strains | - | Y |

κ_{11}, κ_{22}, κ_{12} | Wall curvatures | - | Y |

γ_{13}, γ_{23} | Wall transverse shear strains | - | Y |

SVAR:1, 2, ... , N | State variables | - | 6 |

The subsequent stress solution repeats for top, middle, and bottom surfaces.

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.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.

Available only at the centroid as a

***GET**item.Available via an

**OUTRES**,LOCI command only.Available only if the UserMat subroutine and

**TB**,STATE command are used.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:

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

**Item**predetermined Item label for

**ETABLE****I,J**sequence number for data at nodes I and J

**Table 290.2 ELBOW290 Item and Sequence Numbers**

Output Quantity Name | ETABLE and ESOL Command Input | ||
---|---|---|---|

Item | I | J | |

Fx | SMISC | 1 | 36 |

My | SMISC | 2 | 37 |

Mz | SMISC | 3 | 38 |

TQ | SMISC | 4 | 39 |

SFz | SMISC | 5 | 40 |

SFy | SMISC | 6 | 41 |

Area | SMISC | 7 | 42 |

SDIR | SMISC | 8 | 43 |

SByT | SMISC | 9 | 44 |

SByB | SMISC | 10 | 45 |

SBzT | SMISC | 11 | 46 |

SBzB | SMISC | 12 | 47 |

N11 | SMISC | 14 | 49 |

N22 | SMISC | 15 | 50 |

N12 | SMISC | 16 | 51 |

M11 | SMISC | 17 | 52 |

M22 | SMISC | 18 | 53 |

M12 | SMISC | 19 | 54 |

Q13 | SMISC | 20 | 55 |

Q23 | SMISC | 21 | 56 |

ε_{11} | SMISC | 22 | 57 |

ε_{22} | SMISC | 23 | 58 |

ε_{12} | SMISC | 24 | 59 |

κ_{11} | SMISC | 25 | 60 |

κ_{22} | SMISC | 26 | 61 |

κ_{12} | SMISC | 27 | 62 |

γ_{13} | SMISC | 28 | 63 |

γ_{23} | SMISC | 29 | 64 |

THICK | SMISC | 30 | 65 |

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.

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.