PIPE289

3-D 3-Node Pipe

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

## PIPE289 Element Description

The PIPE289 element is suitable for analyzing slender to moderately stubby/thick pipe structures. The element is based on Timoshenko beam theory. Shear-deformation effects are included.

PIPE289 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.

PIPE289 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).

For more detailed information about this element, see PIPE289 - 3-D 3-Node Pipe in the Mechanical APDL Theory Reference.

## PIPE289 Element Technology and Usage Recommendations

PIPE289 is based on Timoshenko beam theory, 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. (For cases where cross-section distortion must be considered, it is preferable to use ELBOW290.)

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

G

Shear modulus

A

Area of the cross-section

L

Length of the member (not the element length)

EI

Flexural rigidity

For pipes, (GAL2 / EI) can be reduced to: 2L2 / ((1 + ν) (Ro2 + Ri2)), or for thin-walled pipes: L2 / ((1 + ν) R2), where ν = Poisson's ratio, Ro = outer radius, Ri = inner radius, and R = average radius.

The following illustration provides an estimate of transverse-shear deformation in a cantilever pipe subjected to a tip load. Although the results cannot be extrapolated to other applications, the example serves generally. ANSYS, Inc. recommends a slenderness ratio greater than 30.

Slenderness Ratio (GAL2/(EI)) δ Timoshenko / δ Euler-Bernoulli
251.120
501.060
1001.030
10001.003

The element supports an elastic relationship between transverse-shear forces and transverse-shear strains.

Unlike other cubic (Hermitian) polynomial-based elements, PIPE289 is based on quadratic polynomials; therefore, offsets in specification of distributed pressure loads are not allowed. The element has linear bending-moment variation. Refinement of the mesh is recommended in order to accommodate such loading. The element 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.

PIPE289 supports both thin-pipe (KEYOPT(4) = 1) and thick-pipe (KEYOPT(4) = 2) options. The thin-pipe option assumes a plane stress state in the pipe wall and ignore the stress in the wall thickness direction. The thick-pipe option accounts for the full 3-D stress state and generally leads to more accurate results in thick-walled pipes where through-the-thickness stress can be significant. The element allows change in cross-sectional area in large-deflection analysis. While the thick-pipe option can accurately determine the cross-section area change from the actual material constitutive properties, the thin-pipe option calculates the approximate area change based on a simple material incompressibility assumption. The thin pipe option runs slightly faster than the thick pipe option. The thick pipe option should generally be avoided for very thin-walled pipes (for example, Do/Tw > 200.0), and the thin pipe option should generally be avoided for somewhat thick-walled pipes (for example, Do/Tw < 100.0). The thick pipe option is required for a “solid” pipe section (Do/Tw = 2.0). For more information, see the SECDATA command.

For the mass matrix and 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 PIPE289 is a higher-order element. Consistent mass matrix is the default behavior. You can add mass per unit length using the SECCONTROL command's `ADDMAS` values. See "PIPE289 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].)

## PIPE289 Input Data

The geometry, node locations, coordinate system, and pressure directions for this element are shown in Figure 289.1: PIPE289 Geometry. PIPE289 is defined by nodes I, J, and K in the global coordinate system. If ocean loading is present, the global origin is normally at the mean sea level, with the global Z-axis pointing away from the center of the earth; however, the vertical location can be adjusted via `Zmsl` (`Val6`) on the OCDATA command (following the OCTYPE,BASIC command).

Because the section is round, the element orientation is important only for defining offsets and temperatures, and interpreting bending moment directions and stress locations.

Node L is the 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 Mechanical APDL Modeling and Meshing Guide. See the LMESH and LATT command descriptions for details on generating the K node automatically.

You can define PIPE289 without the orientation node. The element x-axis is oriented from node I toward node J. 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. If 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. To control the element orientation about the element x-axis, use the L (orientation) 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 this element is used in a large-deflection analysis, the location of the orientation node only initially orients the element.

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

Internal fluid and external insulation are supported. Added mass, hydrodynamic added mass, and hydrodynamic and buoyant loading, are available via the OCDATA and OCTABLE commands. See the SECCONTROL command for defining added mass.

### PIPE289 Cross-Sections

PIPE289 can be associated only with the pipe cross-section (SECTYPE,,PIPE). The material of the pipe is defined as an element attribute (MAT).

PIPE289 is provided with section-relevant quantities (area of integration, position, etc.) automatically at a number of section points using the SECDATA command. Each section is assumed to be an assembly of a predetermined number of cells and is numerically integrated.

Section Flexibility

To apply section flexibility factors, use the SFLEX command. The command is valid only for linear material properties and small strain analyses, and does not support offsets, temperature loading, or initial state loading. Stress output is based on the section forces, including axial force, bending moments, torsional moment, transverse shear forces, and pressures; strain output is based on the nodal displacements.

Forces are applied at nodes I, J, and K. If the centroidal axis is not colinear with the element x-axis because of node-location offsets, applied axial forces will cause bending. 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, the program uses the centroid as the reference axis for the pipe elements.

Pressure Input

Internal and external pressures are input on an average basis over the element. Lateral pressures are input as force per unit length. End "pressures" are input as forces.

To input surface-load information on the element faces, issue the SFE command

On faces 1 and 2, internal and external pressures are input, respectively, on an average basis over the element.

On face 3, the input (`VAL1`) is the global Z coordinate of the free surface of the internal fluid of the pipe. Specify this value with ACEL,0,0,`ACEL_Z`, where `ACEL_Z` is a positive number. The free surface coordinate is used for the internal mass and pressure effects. If `VAL1` on the SFE command is zero, no fluid inside of the pipe is considered. If the internal fluid free surface should be at Z = 0, use a very small number instead. The pressure calculation presumes that the fluid density above an element to the free surface is constant. For cases where the internal fluid consists of more than one type of fluid (such as oil over water), the free surface coordinate of the elements in the fluids below the top fluid need to be adjusted (lowered) to account for the less dense fluid(s) above them. `VAL1` does not update with large deflections (NLGEOM,ON); if changes are necessary, the SFE command can be reissued at later load steps.

The internal fluid mass is assumed to be lumped along the centerline of the pipe, so as the centerline of a horizontal pipe moves across the free surface, the mass changes in step-function fashion. The free surface location is stepped, even if you specify ramped loading (KBC,0).

On face 4 and face 5, lateral pressures are input as force-per-unit-length.

On face 6 and face 7, end "pressures" are input as forces.

Faces 4 through 8 are shown by the circled numbers in Figure 289.1: PIPE289 Geometry.

Temperature Input

When KEYOPT(1) = 0, temperatures can be input as element body loads at the inner and outer surfaces at both ends of the pipe element so that the temperature varies linearly through the wall thickness. If only two temperatures are specified, those two temperatures are used at both ends of the pipe element (that is, there is no gradient along the length). If only the first temperature is specified, all others default to the first. The following graphic illustrates temperature input at a node when KEYOPT(1) = 0:

When KEYOPT(1) = 1, temperatures can be input as element body loads at three locations at both nodes of the pipe element so that the temperature varies linearly in the element y and z directions. At either end of the element, temperatures can be input at these locations:

• At the element x-axis (T(0,0))

• At the outer radius from the x-axis in the element y-direction (T(Ro,0))

• At the outer radius from the x-axis in the element z-direction (T(0,Ro))

The following graphic illustrates temperature input at a node when KEYOPT(1) = 1:

Element locations (T(Y,Z)) are given according to the convention used in Figure 289.1: PIPE289 Geometry.

For pipe elements, element body load commands (BFE) accept an element number and a list of values, 1 through 6 for temperatures TI(0,0), TI(1,0), TI(0,1), TJ(0,0), TJ(1,0), and TJ(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:

• If all temperatures after the first are unspecified, they default to the first. This pattern applies a uniform temperature over the entire element. (The first coordinate temperature, if unspecified, defaults to TUNIF.)

• If all three 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. This pattern applies a temperature gradient that varies linearly over the cross section but remains constant along the length of the element.

• For any other input pattern, unspecified temperatures default to TUNIF.

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

Other Input

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

The end-cap pressure effect is included by default. The end-cap effect can be deactivated via KEYOPT(6). When subjected to internal and external pressures, PIPE289 with end caps (KEYOPT(6) = 0) is always in equilibrium; that is, no net forces are produced. Because the element curvature is not considered for the end-cap orientations, the element is also in equilibrium without end caps (KEYOPT(6) = 1), even when the element is curved.

### PIPE289 Input Summary

Nodes

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

Degrees of Freedom
 UX, UY, UZ, ROTX, ROTY, ROTZ
Section Information
 Accessed via SECTYPE,,PIPE and SECDATA commands.
Material Properties
 TB command: See Element Support for Material Models for this element. MP command: 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, BETD, DMPR
Pressure --
 face 1- Internal pressure face 2 - External pressure face 3 - Z coordinate of free surface of fluid on inside of pipe face 4 (I-J) (-z normal direction) face 5 (I-J) (-y normal direction) face 6 (I-J) (+x tangential direction) face 7 (I) (+x axial direction) face 8 (J) (-x axial direction) --- I and J denote end nodes. Use a negative value for loading in the opposite direction. Input pressure values for faces 1, 2, and 3 via the SFE command. Input pressure values for faces 4 through 8 via the SFBEAM command Distributed pressure offsets are not available for faces 4, 5, and 6.
Temperatures --

TOUT(I), TIN(I), TOUT(J), TIN(J) if KEYOPT(1) = 0.

TAVG(I), Ty(I), Tz(I), TAVG(J), Ty(J), Tz(J) if KEYOPT(1) = 1.

Special Features
 Birth and death Coriolis effect Element technology autoselect Initial state Large deflection Linear perturbation Nonlinear stabilization Ocean loading Stress stiffening
KEYOPT(1)

Temperature input

0 --

1 --

KEYOPT(4)

Hoop strain treatment

1 --

Thin pipe theory

2 --

Thick pipe theory

KEYOPT(6)

0 --

Internal and external pressures cause loads on end caps

1 --

Internal and external pressures do not cause loads on end caps

KEYOPT(7), KEYOPT(9), KEYOPT(11), and KEYOPT(12)

Active only when OUTPR,ESOL is active:

KEYOPT(7)

Output control for section forces/moments and strains/curvatures:

0 --

Output section forces/moments, strains/curvatures, internal and external pressures, and effective tension(default)

1 --

Same as KEYOPT(7) = 0 plus current section area

2 --

Same as KEYOPT(7) = 1 plus element basis directions (X,Y,Z)

3 --

Output section forces/moments, strains/curvatures, internal and external pressures, and effective tension

KEYOPT(8)

Shear stress output:

0 --

Output a combined state of the following two types (default)

1 --

Output only torsion-related shear stresses

2 --

Output only flexure-related transverse-shear stresses

KEYOPT(9)

Output control at integration points:

0 --

None (default)

1 --

Maximum and minimum stresses/strains

2 --

Same as KEYOPT(9) = 1 plus stresses and strains at each section node

KEYOPT(11)

Output control for values extrapolated to the element and section nodes:

0 --

None (default)

1 --

Maximum and minimum stresses/strains

2 --

Same as KEYOPT(11) = 1 plus stresses and strains along the exterior boundary of the cross-section

3 --

Same as KEYOPT(11) = 1 plus stresses and strains at all section nodes

KEYOPT(12)

Hydrodynamic output (not available in harmonic analyses that include ocean wave effects (HROCEAN)):

0 --

None (default)

1 --

KEYOPT(15)

Results file format:

0 --

Store averaged results at each section corner node (default).

1 --

Store non-averaged results at each section integration point. (The volume of data may be excessive.)

## PIPE289 Output Data

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

For ways to view results, see the Basic Analysis Guide.

To view 3-D deformed shapes for PIPE289, 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).

### 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, PIPE289 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 * R0 / I SByB = Mz * R0 / I SBzT = My * R0 / I SBzB = -My * R0 / I

where My, Mz are bending moments (SMISC quantities 2,15,3,16), R0 is the outside radius, and I is the moment of inertia of the cross-section. The program uses the maximum and minimum cross-section dimensions.

Corresponding definitions for the component strains are:

 EPELDIR = Ex EPELByT = -Kz * R0 EPELByB = Kz * R0 EPELBzT = Ky * R0 EPELBzB = -Ky * R0

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. PIPE289 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.

When using KEYOPT(9) with the cubic option (KEYOPT(3) = 3), the integration point at the middle of the element is reported last in the integration-point printout.

### PIPE289 Element Output Definitions

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.

For the stress and strain components, X refers to axial, Y refers to hoop, and Z refers to radial.

Table 289.1:  PIPE289 Element Output Definitions

NameDefinitionOR
ELElement numberYY
NODESElement connectivityYY
MATMaterial numberYY
C.G.:X, Y, ZElement center of gravityY1
AreaArea of cross-section2Y
S:x, y, z, xy, yz, xzSection point stresses3Y
EPEL:x, y, z, xy, yz, xzElastic strains3Y
EPTO:x, y, z, xy, yz, xzSection point total mechanical strains (EPEL + EPPL + EPCR)3Y
EPTT:x, y, z, xy, yz, xzSection point total strains (EPEL + EPPL + EPCR + EPTH)3Y
EPPL:x, y, z, xy, yz, xzSection point plastic strains3Y
EPCR:x, y, z, xy, yz, xzSection point creep strains3Y
EPTH:x, y, z, xy, yz, xzSection point thermal strains3Y
NL:SEPLPlastic yield stress-4
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding)-4
NL:HPRESHydrostatic pressure-4
NL:EPEQAccumulated equivalent plastic strain-4
NL:CREQAccumulated equivalent creep strain-4
NL:PLWKPlastic work/volume-4
SEND:ELASTIC, PLASTIC, CREEPStrain energy densities-4
TQTorsional momentYY
TETorsional strainYY
SFy, SFzSection shear forces2Y
SEy, SEzSection shear strains2Y
Ky, KzCurvatureYY
ExAxial strainYY
FxAxial force (excluding insulation)YY
My, MzBending momentsYY
INT PRESSInternal pressure at integration point55
EXT PRESSExternal pressure at integration point55
EFFECTIVE TENSEffective tension at integration point55
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
EPELDIRAxial strain at the end-Y
EPELByTBending strain on the element +Y side of the pipe-Y
EPELByBBending strain on the element -Y side of the pipe-Y
EPELBzTBending strain on the element +Z side of the pipe-Y
EPELBzBBending strain on the element -Z side of the pipe-Y
TEMPTemperatures at all section corner nodes-Y
LOCI:X, Y, ZIntegration point locations-6
SVAR:1, 2, ... , NState variables-7
GLOBAL COORDElement centroid location9Y
VR, VZRadial and vertical fluid particle velocities (VR is always > 0) 9Y
AR, AZRadial and vertical fluid particle accelerations9Y
ETAWave amplitude over center of element9Y
TFLUIDFluid temperature (printed if VISC is nonzero) 9Y
VISCViscosity (output if VISC is nonzero)9Y
REN, RETNormal and tangential Reynolds numbers (if VISC is nonzero) 9Y
CTInput tangential drag coefficients evaluated at Reynolds numbers 9Y
CDY, CDZInput normal drag coefficients evaluated at Reynolds numbers 9Y
CMY, CMZInput inertia coefficients evaluated at Reynolds numbers9Y
URT, URNTangential (parallel to element axis) and normal relative velocities9Y
ABURNVector sum of normal (URN) velocities 9Y
ANAccelerations normal to element9Y
FX, FY, FZHydrodynamic tangential and normal forces per unit length in element coordinates9Y

1. Available only at the centroid as a *GET item, or on the NMISC record for ocean loading.

2. See KEYOPT(7) description.

3. See KEYOPT(9) and KEYOPT(11) descriptions.

4. Available if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.

6. Available only if OUTRES,LOCI is used.

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

8. Values are given as the average of the hydrodynamic integration points, which are distributed along the wetted portion of the element.

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

### PIPE289 Item and Sequence Numbers

Table 289.2: PIPE289 Item and Sequence Numbers lists output available for the ETABLE and ESOL commands using the Sequence Number method. See Creating an Element Table and The Item and Sequence Number Table in this reference for more information. The table uses the following notation:

Name

output quantity as defined in Table 289.1: PIPE289 Element Output Definitions.

Item

predetermined Item label for ETABLE

E,I,J

sequence number for data at nodes I and J

Table 289.2:  PIPE289 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJ
FxSMISC--114
MySMISC--215
MzSMISC--316
TQSMISC--417
SFzSMISC--518
SFySMISC--619
ExSMISC--720
KySMISC--821
KzSMISC--922
TESMISC--1023
SEzSMISC--1124
SEySMISC--1225
AreaSMISC--1326
BMSMISC--2729
BKSMISC--2830
SDIRSMISC--3136
SByTSMISC--3237
SByBSMISC--3338
SBzTSMISC--3439
SBzBSMISC--3540
EPELDIRSMISC--4146
EPELByTSMISC--4247
EPELByBSMISC--4348
EPELBzTSMISC--4449
EPELBzBSMISC--4550
TEMPSMISC--51-5354-56
INT PRESS [1]SMISC--6165
EXT PRESS [1]SMISC--6266
EFFECTIVE TENS [1]SMISC--6367
S:x, y, z, xy, yz, xzLS--CI[2], DI[3]CJ[2], DJ[3]
EPEL:x, y, z, xy, yz, xzLEPEL--CI[2], DI[3]CJ[2], DJ[3]
EPTH:x, y, z, xy, yz, xzLEPTH--CI[2], DI[3]CJ[2], DJ[3]
EPPL:x, y, z, xy, yz, xzLEPPL--CI[2], DI[3]CJ[2], DJ[3]
EPCR:x, y, z, xy, yz, xzLEPCR--CI[2], DI[3]CJ[2], DJ[3]
EPTO:x, y, z, xy, yz, xzLEPTO--CI[2], DI[3]CJ[2], DJ[3]
EPTT:x, y, z, xy, yz, xzLEPTT--CI[2], DI[3]CJ[2], DJ[3]
NL: SEPL, SRAT, HPRES, EPEQ, CREQ, PLWKNLIN--EI[5], FI[7]EJ[5], FJ[7]
The following output quantities are valid for ocean loading only and are averaged values for the element: [8]
GLOBAL COORDNMISC1, 2, 3-- --
VR, VZNMISC4, 5-- --
AR, AZNMISC6, 7 [6]-- --
PHDYNNMISC8 [6]-- --
ETANMISC9 [6]-- --
TFLUIDNMISC10-- --
VISCNMISC11-- --
REN, RETNMISC12, 13 [4]-- --
CTNMISC14-- --
CDY, CDZ NMISC15, 16-- --
CMY, CMZNMISC17, 18 [6]-- --
URT, URNNMISC19, 20, 21-- --
ABURNNMISC22 [6]-- --
ANNMISC23, 24 [6]-- --
FX, FY, FZNMISC25, 26, 27-- --
ARGUNMISC28 [6]-- --

1. Internal pressure (INT PRESS), external pressure (EXT PRESS), and effective tension (EFFECTIVE TENS) occur at integration points, and not at end nodes.

2. CI and CJ are the sequence numbers for accessing the averaged line element solution quantities (LS, LEPEL, LEPTH, LEPPL, LEPCR, LEPTO, and LEPTT) at RST section nodes (section corner nodes where results are available), at element Node I and J respectively. CI and CJ are applicable only when KEYOPT(15) = 0. For a given section corner node `nn`, CI and CJ are given as follows:

CI = (`nn` - 1) * 6 + COMP

CJ = (`nnMax` + `nn` - 1) * 6 + COMP

Where `nnMax` is the total number of RST section nodes, and COMP is the stress or strain component (1 - x, 2 - y, 3 - z, 4 - xy, 5 - yz, 6 - xz). Locations of RST section nodes can be visualized with SECPLOT,,6.

3. DI and DJ are the sequence numbers for accessing the non-averaged line element solution quantities (LS, LEPEL, LEPTH, LEPPL, LEPCR, LEPTO, and LEPTT) at RST section integration points (section integration points where results are available), respectively at element Node I and J. DI and DJ are applicable only when KEYOPT(15) = 1. For the ith integration point (i = 1, 2, 3, or 4) in section cell `nc`, DI and DJ are given as follows:

DI = (`nc` - 1) * 24 + (i - 1) * 6 + COMP

DJ = (`ncMax` + `nc` - 1) * 24 + (i - 1) * 6 + COMP

Where `ncMax` is the total number of RST section cells, and COMP is the stress or strain component (1 - x, 2 - x, 3 - z, 4 - xy, 5 - yz, 6 - xz). Locations of RST section cells can be visualized with SECPLOT,,7.

4. These quantities are output only if a Reynold's number dependency is used.

5. EI and EJ are the sequence numbers for accessing the averaged line element nonlinear solution quantities (NLIN) at RST section nodes (section corner nodes where results are available), at element Node I and J, respectively. EI and EJ are applicable only when KEYOPT(15) = 0. For a given section corner node `nn`, EI and EJ are given as follows:

EI = (`nn` - 1) * 10 + COMP

EJ = (`nn`Max + `nn` - 1) * 10 + COMP

where `nn`Max is the total number of RST section nodes, and COMP is the nonlinear element solution component (1 - SEPL, 2 - SRAT, 3 - HPRES, 4 -EPEQ, 5 - CREQ, 6 - PLWK). Locations of RST section nodes can be visualized via SECPLOT,,6.

7. FI and FJ are the sequence numbers for accessing the nonaveraged line element non-linear solution quantities (NLIN) at RST section integration points (section integration points where results are available), at element Node I and J, respectively. FI and FJ are applicable only when KEYOPT(15) = 1. For a given section integration point `nc`, FI and FJ are given as follows:

FI = (`nc` - 1) * 10 + COMP

FJ = (`nc`Max + `nc` - 1) * 10 + COMP

where `nc`Max is the total number of RST section cells and COMP is the non-linear element solution component (1 - SEPL, 2 - SRAT, 3 - HPRES, 4 - EPEQ, 5 - CREQ, 6 - PLWK). Locations of RST section cells can be visualized via SECPLOT,,7.

8. Values are given as the average of the hydrodynamic integration points, which are distributed along the wetted portion of the element.

### Transverse-Shear Stress Output

The shear stresses are caused by torsional and transverse loads. PIPE289 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. This shear force is redistributed by predetermined shear stress distribution coefficients across the pipe cross-section, and made available for output purposes. Use KEYOPT(8) to output shear stresses caused by flexure or transverse loading.

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. Use the SECDATA command to adjust cross-section mesh density.

The traction-free state at the edges of the cross-section is met only in a well-refined model of the cross-section.

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.

## PIPE289 Assumptions and Restrictions

• The pipe cannot have zero length.

• Cross-section distortion or collapse is not considered; therefore, section ovalization associated with a curved pipe undergoing bending cannot be modeled. Curved pipes are best modeled using ELBOW290.

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

• The element works best with the full Newton-Raphson solution scheme (that is, the default choice in solution control).

• Only moderately "thick" pipes can be analyzed. See "PIPE289 Element Technology and Usage Recommendations" for more information.

• Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Prestress effects can be activated via the PSTRES command.

• Hydrodynamic output via KEYOPT(12) is not available in harmonic analyses that include ocean wave effects (HROCEAN).

• For a random vibration (PSD) analysis, equivalent stress is not calculated.

• Temperature-dependent density of the internal fluid is evaluated at an average temperature of the element. Temperature-dependent density of the insulation is evaluated at an average temperature at each integration point along the length.

## PIPE289 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

• Birth and death is not available.

• Initial state is not available.

• Linear perturbation is not available.