PIPE288 Element Description

The PIPE288 element is suitable for analyzing slender to moderately stubby pipe structures. The element is based on Timoshenko beam theory. Shear-deformation effects are included.

PIPE288 is a linear, quadratic, or cubic two-node pipe element in 3D. 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.

PIPE288 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.

Figure 288.1: PIPE288 Geometry

PIPE288 Element Technology and Usage Recommendations

PIPE288 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.

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:

For pipes, (GAL² / EI) can be reduced to: 2L² / ((1 + ν) (R_o² + R_i²)), or for thin-walled pipes: L² / ((1 + ν) R²), where ν = Poisson's ratio, R_o = outer radius, R_i = 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.

Figure 288.2: Transverse-Shear-Deformation Estimation

The PIPE288 element supports an elastic relationship between transverse-shear forces and transverse-shear strains.

When KEYOPT(3) = 0 (linear, default), PIPE288 is based on linear shape functions. It uses one point of integration along the length; therefore, all element solution quantities are constant along the length. For example, when SMISC quantities are requested at nodes I and J, the centroidal values are reported for both end nodes. This option is recommended if the element is used as stiffener and it is necessary to maintain compatibility with a first-order shell element (such as SHELL181). Only constant bending moments can be represented exactly with this option. Mesh refinement is generally required in typical applications.

When KEYOPT(3) = 2 (quadratic), PIPE288 has an internal node in the interpolation scheme, effectively making this a beam element based on quadratic shape functions. Two points of integration are used, resulting in linear variation of element solution quantities along the length. Linearly varying bending moments are represented exactly.

When KEYOPT(3) = 3 (cubic), PIPE288 has two internal nodes and adopts cubic shape functions. Quadratically varying bending moments are represented exactly. Three points of integration along the length are used, resulting in quadratic variation of element solution quantities along the length. Unlike typical cubic (Hermitian) formulations, cubic interpolation is used for all displacements and rotations.

In general, the more complex the element, the fewer elements are needed. Quadratic and cubic options are recommended when higher-order element interpolations are desired in situations where:

PIPE288 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 3D 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 SECDATA.

Two limitations are associated with the quadratic and cubic options in PIPE288:

As a result of the limitations associated with the quadratic and cubic options, you will notice discrepancies in the results between PIPE289 and the quadratic option of PIPE288 if the midside nodes of the PIPE289 model have specified boundary/loading/initial conditions and/or the midside nodes are not located exactly at the element midpoint. Similarly, the cubic option of PIPE288 may not be identical to a traditional cubic (Hermitian) beam element.

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. LUMPM,ON activates lumped mass matrix. Consistent mass matrix is the default behavior. You can add mass per unit length via the SECCONTROL ADDMAS values. See "PIPE288 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).)

When KEYOPT(5) = 1, PIPE288 deforms in the XY plane only. It has three degrees of freedom at each node (translations in the x and y directions, and rotation about the z direction).

PIPE288 Input Data

The geometry, node locations, coordinate system, and pressure directions for this element are shown in Figure 288.1: PIPE288 Geometry. PIPE288 is defined by nodes I and J 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 OCDATA (following OCTYPE,BASIC). Ocean loading is not supported for PIPE288 in the XY plane (KEYOPT(5) = 1).

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 K is the preferred method for defining the orientation of PIPE288 in 3D space (KEYOPT(5) = 0). For information about orientation nodes and beam meshing, see Generating a Beam Mesh With Orientation Nodes in the Modeling and Meshing Guide. See LMESH and LATT descriptions for information about generating the K node automatically.

PIPE288 in 3D space can also be defined 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 orientation-node option. If both are defined, the orientation-node option takes precedence. The orientation node K, 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 K only initially orients the element.

The orientation of PIPE288 in the XY plane is determined by the location of nodes I and J. The element x axis is oriented from node I (end 1) toward node J (end 2). The element y axis is along the negative global Z axis. Orientation node K is not needed.

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

PIPE288 Cross-Sections

PIPE288 can be associated only with the pipe cross-section (SECTYPE,,PIPE). The material of the pipe is defined as an element attribute (MAT).

PIPE288 is provided with section-relevant quantities (area of integration, position, etc.) automatically at a number of section points (SECDATA). Each section is assumed to be an assembly of a predetermined number of cells and is numerically integrated.

Figure 288.3: Typical Cross-Section Cell

Section Flexibility

You can apply section-flexibility factors (SFLEX), valid only for linear material properties and small strain analyses. Offsets, temperature loading, and initial-state loading are not supported. 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.

PIPE288 Loads

Element loads are described in Element Loading. Internal fluid and external insulation are supported. Added mass (including for ocean loading), hydrodynamic added mass, and hydrodynamic and buoyant loading, are available (OCDATA and OCTABLE). Ocean loading is not supported for PIPE289 in the XY plane (KEYOPT(5) = 1).

Forces are applied at the nodes I and J. If the centroidal axis is not colinear with the element x axis because of 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 (SECOFFSET) 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 SFE

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 SFE 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, you can reissue SFE 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 288.1: PIPE288 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(R_o,0)) (not supported for (KEYOPT(5) = 1)

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

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 288.1: PIPE288 Geometry.

For pipe elements, element body-load commands (BFE) accept an element number and a list of values, 1 through 6 for temperatures T_I(0,0), T_I(1,0), T_I(0,1), T_J(0,0), T_J(1,0), and T_J(0,1). This input can be used to specify temperature gradients that vary linearly both over the cross section and along the length of the element. Values of T_I(1,0) and T_J(1,0) are ignored for PIPE288 in the XY plane (KEYOPT(5) = 1).

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.

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 NROPT,UNSYM.

PIPE288 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 3D deformed shapes for PIPE288, issue OUTRES,MISC or OUTRES,ALL for static or transient analyses. To view 3D mode shapes for a modal or eigenvalue buckling analysis, expand the modes with element results calculation active (via Elcalc = YES on MXPAND).

PIPE288 Assumptions and Restrictions

PIPE288 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  —