3-D 3-Node Pipe
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).
Elasticity, hyperelasticity, plasticity, creep, and other nonlinear material models are supported. Internal fluid and external insulation are supported. Added mass, hydrodynamic added mass and loading, and buoyant loading are available.
For more detailed information about this element, see PIPE289 - 3-D 3-Node Pipe in the .
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:
Area of the cross-section
Length of the member (not the element length)
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|
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].)
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
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 . 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 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.
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.
Element loads are described in Element Loading. 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. For ocean loading, you can define added mass directly via the OCDATA and OCTABLE commands (rather than by issuing the SECCONTROL command as is typical with other load types.)
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.
OFFSETZ arguments of the SECOFFSET command appropriately.
By default, the program uses the centroid as the reference axis for
the pipe elements.
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,
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.
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,
VAL1). This specifies a uniform
temperature over the cross section at the specified node. (BF command input is not accepted at node K.)
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.
I, J, K, and L (the optional, but recommended, orientation node)
|UX, UY, UZ, ROTX, ROTY, ROTZ|
|Accessed via SECTYPE,,PIPE and SECDATA commands.|
|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|
|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.|
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.
|Birth and death|
|Element technology autoselect|
Through wall gradient
Hoop strain treatment
Thin pipe theory
Thick pipe theory
End cap loads
Internal and external pressures cause loads on end caps
Internal and external pressures do not cause loads on end caps
Active only when OUTPR,ESOL is active:
Output control for section forces/moments and strains/curvatures:
Same as KEYOPT(7) = 0 plus current section area
Same as KEYOPT(7) = 1 plus element basis directions (X,Y,Z)
Shear stress output:
Output a combined state of the following two types (default)
Output only torsion-related shear stresses
Output only flexure-related transverse-shear stresses
Output control at integration points:
Maximum and minimum stresses/strains
Same as KEYOPT(9) = 1 plus stresses and strains at each section node
Output control for values extrapolated to the element and section nodes:
Maximum and minimum stresses/strains
Same as KEYOPT(11) = 1 plus stresses and strains along the exterior boundary of the cross-section
Same as KEYOPT(11) = 1 plus stresses and strains at all section nodes
Additional hydrodynamic printout
Results file format:
Store averaged results at each section corner node (default).
Store non-averaged results at each section integration point. (The volume of data may be excessive.)
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 289.1: PIPE289 Element Output Definitions
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).
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.
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
|C.G.:X, Y, Z||Element center of gravity||Y||1|
|Area||Area of cross-section||2||Y|
|S:x, y, z, xy, yz, xz||Section point stresses||3||Y|
|EPEL:x, y, z, xy, yz, xz||Elastic strains||3||Y|
|EPTO:x, y, z, xy, yz, xz||Section point total mechanical strains (EPEL + EPPL + EPCR)||3||Y|
|EPTT:x, y, z, xy, yz, xz||Section point total strains (EPEL + EPPL + EPCR + EPTH)||3||Y|
|EPPL:x, y, z, xy, yz, xz||Section point plastic strains||3||Y|
|EPCR:x, y, z, xy, yz, xz||Section point creep strains||3||Y|
|EPTH:x, y, z, xy, yz, xz||Section point thermal strains||3||Y|
|NL:SEPL||Plastic yield stress||-||4|
|NL:SRAT||Plastic yielding (1 = actively yielding, 0 = not yielding)||-||4|
|NL:EPEQ||Accumulated equivalent plastic strain||-||4|
|NL:CREQ||Accumulated equivalent creep strain||-||4|
|SEND:ELASTIC, PLASTIC, CREEP||Strain energy densities||-||4|
|SFy, SFz||Section shear forces||2||Y|
|SEy, SEz||Section shear strains||2||Y|
|Fx||Axial force (excluding insulation)||Y||Y|
|My, Mz||Bending moments||Y||Y|
|INT PRESS||Internal pressure at integration point||5||5|
|EXT PRESS||External pressure at integration point||5||5|
|EFFECTIVE TENS||Effective tension at integration point||5||5|
|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|
|EPELDIR||Axial strain at the end||-||Y|
|EPELByT||Bending strain on the element +Y side of the pipe||-||Y|
|EPELByB||Bending strain on the element -Y side of the pipe||-||Y|
|EPELBzT||Bending strain on the element +Z side of the pipe||-||Y|
|EPELBzB||Bending strain on the element -Z side of the pipe||-||Y|
|TEMP||Temperatures at all section corner nodes||-||Y|
|LOCI:X, Y, Z||Integration point locations||-||6|
|SVAR:1, 2, ... , N||State variables||-||7|
|The following values apply to ocean loading only: |
|GLOBAL COORD||Element centroid location||9||Y|
|VR, VZ||Radial and vertical fluid particle velocities (VR is always > 0)||9||Y|
|AR, AZ||Radial and vertical fluid particle accelerations||9||Y|
|PHDYN||Dynamic fluid pressure head||9||Y|
|ETA||Wave amplitude over center of element||9||Y|
|TFLUID||Fluid temperature (printed if VISC is nonzero)||9||Y|
|VISC||Viscosity (output if VISC is nonzero)||9||Y|
|REN, RET||Normal and tangential Reynolds numbers (if VISC is nonzero)||9||Y|
|CT||Input tangential drag coefficients evaluated at Reynolds numbers||9||Y|
|CDY, CDZ||Input normal drag coefficients evaluated at Reynolds numbers||9||Y|
|CMY, CMZ||Input inertia coefficients evaluated at Reynolds numbers||9||Y|
|URT, URN||Tangential (parallel to element axis) and normal relative velocities||9||Y|
|ABURN||Vector sum of normal (URN) velocities||9||Y|
|AN||Accelerations normal to element||9||Y|
|FX, FY, FZ||Hydrodynamic tangential and normal forces per unit length in element coordinates||9||Y|
|ARGU||Effective position of wave (radians)||9||Y|
Available if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.
Available only if ocean loading is present.
Available only if OUTRES,LOCI is used.
Applies to ocean loading only.
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:
Table 289.2: PIPE289 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|INT PRESS ||SMISC||--||61||65|
|EXT PRESS ||SMISC||--||62||66|
|EFFECTIVE TENS ||SMISC||--||63||67|
|S:x, y, z, xy, yz, xz||LS||--||CI, DI||CJ, DJ|
|EPEL:x, y, z, xy, yz, xz||LEPEL||--||CI, DI||CJ, DJ|
|EPTH:x, y, z, xy, yz, xz||LEPTH||--||CI, DI||CJ, DJ|
|EPPL:x, y, z, xy, yz, xz||LEPPL||--||CI, DI||CJ, DJ|
|EPCR:x, y, z, xy, yz, xz||LEPCR||--||CI, DI||CJ, DJ|
|EPTO:x, y, z, xy, yz, xz||LEPTO||--||CI, DI||CJ, DJ|
|EPTT:x, y, z, xy, yz, xz||LEPTT||--||CI, DI||CJ, DJ|
|NL: SEPL, SRAT, HPRES, EPEQ, CREQ, PLWK||NLIN||--||EI, FI||EJ, FJ|
|The following output quantities are valid for ocean loading only and are averaged values for the element: |
|GLOBAL COORD||NMISC||1, 2, 3||--||--|
|VR, VZ||NMISC||4, 5||--||--|
|AR, AZ||NMISC||6, 7 ||--||--|
|REN, RET||NMISC||12, 13 ||--||--|
|CDY, CDZ||NMISC||15, 16||--||--|
|CMY, CMZ||NMISC||17, 18 ||--||--|
|URT, URN||NMISC||19, 20, 21||--||--|
|AN||NMISC||23, 24 ||--||--|
|FX, FY, FZ||NMISC||25, 26, 27||--||--|
Internal pressure (INT PRESS), external pressure (EXT PRESS), and effective tension (EFFECTIVE TENS) occur at integration points, and not at end nodes.
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 = (
nn- 1) * 6 + COMP
nnMaxis 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.
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 = (
nc- 1) * 24 + (i - 1) * 6 + COMP
ncMaxis 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.
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- 1) * 10 + COMP
nnMax 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.
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- 1) * 10 + COMP
ncMax 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.
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.
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.
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.
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.
Ocean loading is not available.
ANSYS Mechanical Premium
Birth and death is not available.