PIPE16 Element Description

PIPE16 is a uniaxial element with tension-compression, torsion, and bending capabilities. The element has six degrees of freedom at two nodes: translations in the nodal x, y, and z directions and rotations about the nodal x, y, and z axes. See PIPE16 - Elastic Straight Pipe for more details about this element.

Figure 16.1: PIPE16 Geometry

PIPE16 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 16.1: PIPE16 Geometry. The element input data include two or three nodes, the pipe outer diameter and wall thickness, stress intensification and flexibility factors, internal fluid density, exterior insulation density and thickness, corrosion thickness allowance, insulation surface area, pipe wall mass, axial pipe stiffness, rotordynamic spin, and the isotropic material properties.

The element X-axis is oriented from node I toward node J. For the two-node option, the element Y-axis is automatically calculated to be parallel to the global X-Y plane. Several orientations are shown in Figure 16.1: PIPE16 Geometry. For the case where 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 (as shown). For user control of the element orientation about the element X-axis, use the third node option. The third node (K), if used, defines a plane (with I and J) containing the element X and Z axes (as shown). Input and output locations around the pipe circumference identified as being at 0° are located along the element Y-axis, and similarly 90° is along the element Z-axis.

The stress-intensification factor modifies the bending stress. Stress intensification factors can be input at end I (SIFI) and end J (SIFJ), if KEYOPT(2) = 0, or determined by the program using a tee-joint calculation if KEYOPT(2) = 1, 2, or 3. Stress-intensification factor values less than 1.0 are set equal to 1.0. The flexibility factor (FLEX) is divided into the cross-sectional moment of inertia to produce a modified moment of inertia for the bending stiffness calculation. FLEX defaults to 1.0 but may be input as any positive value.

The element mass is calculated from the pipe wall material, the external insulation, and the internal fluid. The insulation and the fluid contribute only to the element mass matrix. The corrosion thickness allowance contributes only to the stress calculations. A positive wall mass real constant overrides the pipe wall mass calculation. A nonzero insulation area real constant overrides the insulation surface area calculation (from the pipe outer diameter and length). A nonzero stiffness real constant overrides the calculated axial pipe stiffness.

Element loads are described in Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 16.1: PIPE16 Geometry. Internal pressure (PINT) and external pressure (POUT) are input as positive values. The internal and external pressure loads are designed for closed-loop static pressure environments and therefore include pressure loads on fictitious "end caps" so that the pressure loads induce an axial stress and/or reaction in the pipe system. If a dynamic situation needs to be represented, such as a pipe venting to a lower pressure area or the internal flow is past a constriction in the pipe, these end cap loads may need to be modified by applying a nodal force normal to the cross-section of the pipe with the magnitude representing the change in pressure. Alternatively, the precomputed end cap loads can be removed using KEYOPT(8) = 1 and the appropriate end cap loads added by the user. The transverse pressures (PX, PY, and PZ) may represent wind or drag loads (per unit length of the pipe) and are defined in the global Cartesian directions. Positive transverse pressures act in the positive coordinate directions. The normal component or the projected full pressure may be used (KEYOPT(5)). Tapered pressures are not recognized. Only constant pressures are supported for this element. See PIPE16 - Elastic Straight Pipe for more information.

Temperatures may be input as element body loads at the nodes. Temperatures may have wall gradients or diametral gradients (KEYOPT(1)). The average wall temperature at θ = 0° is calculated as 2 * TAVG - T(180) and the average wall temperature at θ = -90° is calculated as 2 * TAVG - T(90). The element temperatures are assumed to be linear along the length. The first temperature at node I (TOUT(I) or TAVG(I)) 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 pattern of input temperatures, unspecified temperatures default to TUNIF.

For piping analyses, the PIPE module of PREP7 may be used to generate the input for this element. KEYOPT(4) is used to identify the element type for output labeling and for postprocessing operations.

KEYOPT(7) is used to compute an unsymmetric gyroscopic damping matrix (often used for rotordynamic analyses). The rotational frequency is input with the SPIN real constant (radians/time, positive in the positive element x direction).

A summary of the element input is given in "PIPE16 Input Summary". A general description of element input is given in Element Input.

PIPE16 Output Data

The solution output associated with the element is in two forms:

Several items are illustrated in Figure 16.2: PIPE16 Stress Output.

The direct stress (SAXL) includes the internal pressure (closed end) effect. The direct stress does not include the axial component of the transverse thermal stress (STH). The principal stresses and the stress intensity include the shear force stress component, and are based on the stresses at the two extreme points on opposite sides of the neutral axis. These quantities are calculated at the outer surface and might not occur at the same location around the pipe circumference. Angles listed in the output are measured as shown (θ) in Figure 16.2: PIPE16 Stress Output. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 16.2: PIPE16 Stress Output

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

The following tables list output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table of this manual for more information. The following notation is used in Table 16.3: PIPE16 Item and Sequence Numbers (Node I) through Table 16.5: PIPE16 Item and Sequence Numbers:

PIPE16 Assumptions and Restrictions

PIPE16 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

Ansys Professional  —