Fluid Pipe Elements

Fluid pipe elements in Abaqus/Standard allow you to simulate the viscous and gravity pressure loss terms in a fluid pipe network. The pipe elements use a pure pressure formulation and are based on Bernoulli's equation for the case of steady-state flow of a single-phase, incompressible fluid through a fully filled pipe with a constant cross-sectional area.

This page discusses:

Typical Applications
Choosing an Appropriate Element
Assigning a Material Definition to a Set of Fluid Pipe Elements
Multiple Fluid Flow
Using Fluid Pipe Elements in Symmetric Models
Fluid Pipe Equations
Specifying the Friction Loss Behavior
Specifying Initial and Prescribed Conditions
Specifying Loads and Boundary Conditions

Typical Applications

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 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 geomechanics.

Choosing an Appropriate Element

Several fluid pipe element types are available. For two-dimensional and axisymmetric analyses, use element type FP2D2. For three-dimensional analyses, use element type FP3D2.

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 fluid pipe section refers to the fluid that is flowing through the pipe. The properties that must be defined for the fluid are the pore fluid density and viscosity. For the viscosity definition fluid pipe elements support both Newtonian and non-Newtonian fluids. The supported non-Newtonian fluids are power law, Bingham Plastic, and Herschel-Bulkley models (see Viscosity).

Input File Usage

Use the following options to specify the pore fluid density and viscosity:

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

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 (that is, 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 equal to 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 Fluid Pipe Elements in Symmetric Models

You can use fluid pipe elements in models that use symmetry to reduce the model size. The 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

Fluid Pipe Equations

The geometry of a pipe element is expressed in terms of hydraulic area and hydraulic diameter. The hydraulic diameter is expressed in terms of the cross-sectional area (A) of the tube or channel and the wetted perimeter (P) as $D_{h} = \frac{(4 A)}{P}$ . A pipe element is defined by two noncoincident nodes. Using a Darcy-Weisbach approach, Bernoulli's equation (including viscous loss) between two points in space can be written as

△ P - ρ g △ Z = (C_{L} + K_{i}) \frac{ρ V^{2}}{2},

where

$P_{1}, P_{2}$ are the pressures at the nodes and $△ P = (P_{1} - P_{2})$ ;
$Z_{1}, Z_{2}$ are the elevations at the nodes and $△ Z = (Z_{2} - Z_{1})$ ;
$V$ is the fluid velocity in the pipe;
$ρ$ is the fluid density;
$g$ is the acceleration due to gravity;
$C_{L} = \frac{f L}{D_{h}}$ is the loss coefficient;
$f$ is the friction factor of the pipe;
$L$ is the length of the pipe; and
$K_{i}$ is a directional loss term.

The assumption of constant cross-sectional area in a single element results in constant fluid velocity in a pipe element. The mass flow rate $Q$ through the pipe can be related to the fluid and pipe parameters as $Q = ρ A V$ .

Additional Loss Terms in Fluid Pipe Elements

The loss coefficient $C_{L}$ can also include an added pipe length $L_{a}$ as well as a pipe length scaling factor $α$ . The general form of the loss coefficient is written as

C_{L} = \frac{f (L (1 + α) + L_{a})}{D_{h}} .

In addition, you can also specify directional connection loss terms $K_{1}$ and $K_{2}$ . If the flow is from local node 1 to node 2, the total pressure loss is

△ P - ρ g △ Z = (C_{L} + K_{1}) \frac{ρ V^{2}}{2};

and if the flow is from local node 2 to node 1, the dynamic pressure loss is

△ P - ρ g △ Z = (C_{L} + K_{2}) \frac{ρ V^{2}}{2} .

Specifying the Friction Loss Behavior

Abaqus/Standard supports four different methods for defining the friction factor $(f)$ :

Blasius friction loss;
Churchill friction loss;
A tabular option; and
A user subroutine.

Specifying Blasius Friction Loss Behavior for the Fluid Pipe Element

The Blasius friction loss method uses an empirical relation based on the Reynold's number (Re) to determine the friction factor. The method has two different regimes that depend on whether the flow is laminar or turbulent. There is a discontinuous jump in the friction factor when the flow transitions from laminar to turbulent at $R e = 2500$ . The friction factor is empirically calculated as

f = \frac{64}{R e} : R e < 2500

f = \frac{0.3164}{R e^{0.25}} : R e \geq 2500.

Input File Usage

FLUID PIPE FLOW LOSS, TYPE=BLASIUS

Specifying Churchill Friction Loss Behavior for the Fluid Pipe Element

A more comprehensive formula that takes into account the pipe roughness $K_{s}$ and captures the Moody's data accurately is the Churchill's formula. This formula transitions smoothly from laminar to turbulent flow. The friction factor is determined as

f = 8 {[{(\frac{8}{R e})}^{12} + \frac{1}{{(A + B)}^{1.5}}]}^{\frac{1}{12}},

A = {[- 2.457 \ln ({(\frac{7}{R e})}^{0.9} + 0.27 (\frac{K_{s}}{D_{h}}))]}^{16},

B = {(\frac{37350}{R e})}^{16} .

Input File Usage

FLUID PIPE FLOW LOSS, TYPE=CHURCHILL

Specifying the Friction Loss Behavior as a Table of Reynolds Number Versus Friction Factor

You can input a table of $R e$ versus friction. Abaqus interpolates linearly between the values specified in the table. If one of the independent variables is outside the range of specified values, Abaqus uses the value that is closest in the table.

Input File Usage

FLUID PIPE FLOW LOSS, TYPE=TABULAR

Specifying the Friction Factor with a User Subroutine

You can specify the friction factor for the element with user subroutine UFLUIDPIPEFRICTION. The user subroutine is called by every fluid pipe element to determine the friction factor based on the fluid flow rates.

Input File Usage

FLUID PIPE FLOW LOSS, TYPE=USER

Specifying the Laminar Flow Transition for Low Reynolds Number Flows

You can specify the laminar flow transition parameter that is used to switch flow computations from a purely laminar, linear formulation to a nonlinear iterative formulation. The purely laminar formulation uses the Blasius friction factor when the computed Reynold's number is at or below the specified laminar flow transition number. This ensures better convergence when the flow in the pipe is zero or close to zero in magnitude. The default laminar transition flow Reynold's number is 1.0. User subroutine UFLUIDPIPEFRICTION is not called when the computed $R e$ is less than the default or specified value.

Input File Usage

FLUID PIPE FLOW LOSS, 
LAMINAR FLOW TRANSITION=Reynold's number value

Specifying Initial and Prescribed Conditions

You can define a field distribution over the nodes of the fluid pipe elements.

Input File Usage

Use one or both of the following options:

INITIAL CONDITIONS, TYPE=FIELD

Specifying Loads and Boundary Conditions

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

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 a gravity load on the fluid pipe element:

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