Thermal Fluid Pipe Elements

Thermal fluid pipe elements in Abaqus/Standard allow you to simulate the pressure loss due to viscous and gravity effects in a fluid pipe network, including the temperature field in the fluid flowing in the pipe, heat exchange between the fluid and the pipe, and heat transfer through the walls of the pipe.

The thermal fluid pipe elements model the flow field using a pure pressure formulation, based on Bernoulli's equation for steady-state flow of a single-phase, incompressible fluid through a fully filled pipe with a constant cross-sectional area. The thermal model includes convection and diffusion of heat in the fluid, as well as conduction of heat along the length and radial (thickness) directions in the pipe.

This page discusses:

Typical Applications
Choosing an Appropriate Element
Assigning a Material Definition to a Set of Fluid Pipe Elements
Multiple Fluid Flow
Using Thermal Fluid Pipe Elements in Symmetric Models
Thermal Fluid Pipe Equations
Specifying the Wall Diameters for Thermal Fluid Pipe Elements
Specifying the Type of Convection between the Fluid and the Pipe Wall
Specifying Initial and Prescribed Conditions
Specifying Loads and Boundary Conditions

Typical Applications

Thermal fluid pipe elements are used to simulate:

the flow of a liquid through a pipe or network of pipes to determine pressure drops and flow rates, and
the temperature field in the flowing fluid and the pipe walls.

These elements can be used in a geostatic or coupled pore fluid diffusion/stress analysis (see Geostatic Stress State and Coupled Pore Fluid Diffusion and Stress Analysis). They can also be used to model one-dimensional wellbores in certain geotechnical applications.

Choosing an Appropriate Element

Several thermal fluid pipe elements are available. They can be broadly classified as follows:

Regular thermal fluid pipe elements (FP2D2T and FP3D2T)
Annular thermal fluid pipe elements (FP2D2AT and FP3D2AT)

For two-dimensional analyses, use element type FP2D2T or FP2D2AT. For three-dimensional analyses, use element type FP3D2T or FP3D2AT. A detailed discussion of the differences between the two classes (regular versus annular) follows.

Figure 1 shows a regular thermal fluid pipe element. It consists of a total of six nodes, three at each end of the element. Although each end has three distinct nodes, they actually share the same geometric location. The first node at each end (shown here in blue) is used to model the fluid flow and has both fluid pressure and temperature degrees of freedom. These nodes are referred to as the "flow nodes." The second and third nodes at each end (shown here in red) define the temperature variation through the wall of the pipe and have only the temperature degree of freedom. These nodes are referred to as the "wall nodes." Figure 2 shows the element connectivity for the regular thermal fluid pipe elements.

Figure 3 shows an annular pipe, which consists of a center region that is the same as a regular pipe (and should be modeled with a regular thermal fluid pipe element) and an annular region that surrounds the center region. The annular region (which must be modeled using an annular thermal fluid pipe element) has a total of eight nodes, four at each end of the pipe sharing the same geometric location. The nodes at the middle of the annulus (shown here in blue) have both fluid pressure and temperature degrees of freedom; they are referred to as the "flow nodes." The "wall nodes" (shown here in red) have only temperature degrees of freedom and model the temperature variation in the inner and outer walls of the annulus. Figure 4 shows the element connectivity for the annular thermal fluid pipe element.

A typical application of the annular pipe element involves modeling the return flow in a piping system. As shown in Figure 3, the fluid flow directions in the center and the annular regions might be opposite to each other. The incoming fluid at the center region and the outgoing fluid in the annular region can be at different temperatures. The temperature degree of freedom at the outermost wall nodes of the regular pipe region (nodes 5 and 6 in Figure 2) and that at the corresponding innermost wall nodes of the annular region (nodes 7 and 8 in Figure 4) must be tied to ensure continuity of the temperature field between the center and the annular regions. In addition, if return flow is modeled, the fluid pressure and temperature degrees of freedom of the bottom "flow node" of the regular thermal fluid pipe element (node 2 in Figure 2) must be tied to the corresponding degrees of freedom of the bottom "flow node" of the annular thermal fluid pipe element (node 2 in Figure 4).

You can use an offset to create the pipe wall nodes of the regular thermal fluid pipe and annular thermal fluid pipe elements.

You can render thermal pipe elements and annular thermal pipe elements using the Visualization module of Abaqus/CAE. For more information, see Controlling the display of thermal fluid pipe elements.

Input File Usage

Use the following option to define an offset used to create the pipe wall nodes:

ELEMENT, OFFSET=number

Assigning a Material Definition to a Set of Fluid Pipe Elements

You must associate a material definition with each pipe element section property.

The material that is defined for the thermal fluid pipe section refers to the fluid that is flowing through the pipe. You must define the following properties for the fluid to describe its flow behavior: fluid density and viscosity. For the viscosity definition, thermal fluid pipe elements support both Newtonian and non-Newtonian fluids. The following non-Newtonian fluid models are supported: power law, Bingham Plastic, and Herschel-Bulkley models (see Viscosity).

For the thermal fluid pipe elements, you must also specify the following thermal properties:

Conductivity and specific heat for the fluid
Density, conductivity, and specific heat for the pipe wall

Input File Usage

Use the following options to specify the flow and thermal behaviors of the fluid:

FLUID PIPE SECTION, MATERIAL=material name
MATERIAL, NAME=material name
VISCOSITY, DEFINITION=NEWTONIAN or POWER LAW or HERSCHEL-BULKLEY or BINGHAM PLASTIC
DENSITY, PORE FLUID
CONDUCTIVITY, PORE FLUID
SPECIFIC HEAT, PORE FLUID

In addition, use the following options to specify the thermal properties for the pipe wall:

DENSITY
CONDUCTIVITY
SPECIFIC HEAT

Multiple Fluid Flow

Abaqus allows the use of multiple fluids in an analysis, up to a maximum of four fluid types. This capability is useful in situations where the spatial distribution of the different fluid types is known (precomputed) at all times during the analysis. In other words, the type of fluid at each node in the domain is known at all times during the analysis.

The definition of multiple fluids in an analysis involves assigning a unique integer value that acts as an identifier for each fluid type, and associating each fluid identifier with a specific predefined field variable used to specify the spatial distribution of the fluid as function of time. You can utilize the fluid identifier to specify the viscosity of each fluid. Only the fluid viscosity can be different for different fluids. All other properties (for example, density, thermal) are assumed to be same for all the fluids. The field variable associated with a fluid type allows you to predefine the fluid type at a node as a function of time using amplitude definitions or as functions of both time and space utilizing user subroutine UFIELD or USDFLD.

You specify a value for each field variable, associated with a fluid identifier, at each node. It is recommended that you specify a value for the field variable ( $F V$ ) such that, $0.0 \leq F V \leq 1.0$ . Abaqus assigns the fluid type at an integration point to be the one for which the field variable has the maximum value at that point. If all field variables have the same numerical value at an integration point, the first fluid (fluid identifier 1) is assumed to be active.

Input File Usage

VISCOSITY, FLUID ID=Fluid Id number,DEFINITION=NEWTONIAN or POWER LAW or HERSCHEL-BULKLEY or BINGHAM PLASTIC
FIELD, VARIABLE=Field variable number
FLUID ID FIELD
Fluid Id number,Field variable number

Using Thermal Fluid Pipe Elements in Symmetric Models

You can use thermal fluid pipe elements in models that use symmetry to reduce the model size. The thermal fluid pipe elements model circular geometry. You specify a symmetry value that is greater than 0 and less than or equal to 1. This value is interpreted as scaling of the circular pipe geometry in radians. A value of 1 corresponds to $2 π$ radians, and a value of 0.5 corresponds to $π$ radians. When you specify symmetry, you must scale the full model flow magnitude by the symmetry value. You do not need to apply any symmetric constraints or boundary conditions.

Input File Usage

FLUID PIPE SECTION, SYMMETRY=value

Thermal Fluid Pipe Equations

The governing equations for the fluid flow and pressure drop computation in pipes are described in Fluid Pipe Equations. The different choices of specifying the frictional loss characteristics for the flowing fluid in the thermal pipe are described in Specifying the Friction Loss Behavior. You can model additional fluid pressure losses in thermal fluid pipe elements as described in Additional Loss Terms in Fluid Pipe Elements.

In the thermal fluid pipe elements, the fluid temperature evolution is given by the 1-D transient advection-diffusion equation:

\frac{d θ}{d t} - D \frac{d^{2} θ}{d x^{2}} + V \frac{d θ}{d x} = 0,

where:

$θ$ is the temperature.
$D$ is the fluid thermal diffusivity computed as the ratio of thermal conductivity to thermal capacity, $D = \frac{K_{f}}{ρ_{f} C_{p}^{f}}$ . Here, $ρ_{f}$ is the fluid density, $K_{f}$ is the fluid thermal conductivity, and $C_{p}^{f}$ is the specific heat of the fluid.
$V$ is the velocity of fluid flow.

Specifying the Wall Diameters for Thermal Fluid Pipe Elements

You must define the geometry of the pipe wall as a circular cross-section by specifying the inner and outer wall radii.

Input File Usage

FLUID PIPE WALL

Specifying the Type of Convection between the Fluid and the Pipe Wall

You can define the type of convection to determine the temperature at the interface of the pipe wall and flowing fluid (nodes 3 and 4 for the regular pipe and nodes 3, 4, 7, and 8 for the annular pipe). Newton's law of cooling is used to determine this interface temperature. The convection type determines whether a constant temperature or a constant flux method is used in this computation.

Input File Usage

Use the following option to specify a constant temperature method:

FLUID PIPE THERMAL, TYPE=TEMPERATURE

Use the following option to specify a constant flux method:

FLUID PIPE THERMAL, TYPE=FLUX

Specifying Initial and Prescribed Conditions

You can define an initial temperature or field distribution over the nodes of the thermal fluid pipe elements.

Input File Usage

Use one or both of the following options:

INITIAL CONDITIONS, TYPE=TEMPERATURE
INITIAL CONDITIONS, TYPE=FIELD

Specifying Loads and Boundary Conditions

Thermal fluid pipe elements allow for the specification of pressure boundary conditions and volumetric flow rates at the nodes. At a particular node, you can specify either a pressure or flow rate but not both. You can also specify a gravity load on the thermal fluid pipe element to determine the hydrostatic head at the nodes. You can specify the fluid temperature at the inlet or outlet and at the pipe wall.

Input File Usage

Use the following option to specify the pressure at the inlet or outlet:

BOUNDARY
node or node set, 8, 8, magnitude

Use the following option to specify the flow rate at the inlet or outlet:

CFLOW
node or node set, , magnitude

Use the following option to specify the temperature at the inlet, outlet, or pipe wall:

BOUNDARY
node or node set, 11, 11, magnitude

Use the following option to specify a gravity load on the fluid pipe element:

DLOAD
element or element set, , GRAV, gravity constant, comp1, comp2, comp3