<!-- source-page: 1081 -->

# Film conditions

Surface-based film conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 34.4.4.

<table><tr><td>Load ID(*SFILM)</td><td>Abaqus/CAELoad/Interaction</td><td>Units</td><td>Description</td></tr><tr><td>F</td><td>Surface film condition</td><td> $JL^{-2}T^{-1}\theta^{-1}$ </td><td>Film coefficient and sink temperature (units of  $\theta$ ) provided on the element surface.</td></tr></table>

# Radiation types

Surface-based radiation conditions are available only for EC3D8RT elements. They are specified as described in “Thermal loads,” Section 34.4.4.

<table><tr><td>Load ID(*SRADIATE)</td><td>Abaqus/CAELoad/Interaction</td><td>Units</td><td>Description</td></tr><tr><td>R</td><td>Surface radiation</td><td>Dimensionless</td><td>Emissivity and sink temperature (units of θ) provided on the element surface.</td></tr></table>

# Element output

A set of output variables is written for each Eulerian material instance listed in the Eulerian section definition. The output variable names are automatically appended with the material instance names. For example, if you define material instances named “steel” and “tin” and request stress output, the first stress components will be written to separate output variables named “S11\_steel” and “S11\_tin.”

All output is given in global coordinates.

# Stress and other tensor components

Stress and other tensors (excluding total strain tensors) are available. All tensors have the same components. For example, the stress components are as follows:

<table><tr><td>S11</td><td>XX, direct stress.</td></tr><tr><td>S22</td><td>YY, direct stress.</td></tr><tr><td>S33</td><td>ZZ, direct stress.</td></tr><tr><td>S12</td><td>XY, shear stress.</td></tr><tr><td>S13</td><td>XZ, shear stress.</td></tr><tr><td>S23</td><td>YZ, shear stress.</td></tr></table>

<!-- source-page: 1082 -->

# Element-averaged quantities

Several output variables are also available as element-averaged quantities. These variables are computed as a volume fraction weighted average of all materials present in the element. Use of these variables can substantially decrease the size of the output database for models with many Eulerian materials. For example:

SVAVG

Volume fraction averaged stress.

# Node ordering and face numbering on elements

All elements must have eight nodes. Degenerate elements are not supported.

![](images/page-1082_af58b4ecb0b81445c1bab15b809d4ed8f876ee91fb20496dcd46b51655e326e3.jpg)

Element faces 

<table><tr><td>Face 1</td><td>1 - 2 - 3 - 4 face</td></tr><tr><td>Face 2</td><td>5 - 8 - 7 - 6 face</td></tr><tr><td>Face 3</td><td>1 - 5 - 6 - 2 face</td></tr><tr><td>Face 4</td><td>2 - 6 - 7 - 3 face</td></tr><tr><td>Face 5</td><td>3 - 7 - 8 - 4 face</td></tr><tr><td>Face 6</td><td>4 - 8 - 5 - 1 face</td></tr></table>

<!-- source-page: 1083 -->

# Numbering of integration points for output

The single integration point is located at the centroid of the element. All materials within the element are evaluated at this integration point.

<!-- source-page: 1084 -->

<!-- source-page: 1085 -->

# 32.15 Fluid pipe elements

• “Fluid pipe elements,” Section 32.15.1   
• “User-defined element library,” Section 32.17.2

<!-- source-page: 1086 -->

<!-- source-page: 1087 -->

# 32.15.1 FLUID PIPE ELEMENTS

Product: Abaqus/Standard

# References

• “Fluid pipe element library,” Section 32.15.2   
• \*FLUID PIPE SECTION   
• \*FLUID PIPE FLOW LOSS

# Overview

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.

# 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,” Section 6.8.2, and “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). They can also be used to model one-dimensional wellbores in geomechanics.

# Choosing an appropriate element

Two types of fluid pipe elements are provided. 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 only Newtonian fluids (see “Viscosity,” Section 26.1.4).

Input File Usage: Use all of the following options:

\*FLUID PIPE SECTION, MATERIAL=material name   
\*MATERIAL, NAME=material name   
\*DENSITY, PORE FLUID   
\*VISCOSITY, DEFINITION=NEWTONIAN

<!-- source-page: 1088 -->

# 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 $\begin{array} { r } { \dot { D } _ { h } = \frac { ( 4 A ) } { P } } \end{array}$ . 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

$$
\triangle P - \rho g \triangle Z = (C _ {L} + K _ {i}) \frac {\rho V ^ {2}}{2},
$$

where

• $P _ { 1 } , P _ { 2 }$ are the pressures at the nodes and $\triangle P = ( P _ { 1 } - P _ { 2 } )$ ;   
• $Z _ { 1 } , Z _ { 2 }$ are the elevations at the nodes and $\triangle Z = ( Z _ { 1 } - Z _ { 2 } )$ ;   
• is the fluid velocity in the pipe.   
• $\rho$ is the fluid density;   
• is the acceleration due to gravity;   
• $\begin{array} { r } { C _ { L } = \frac { f L } { D _ { h } } } \end{array}$ D is the loss coefficient;   
• is the friction factor of the pipe;   
• 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 through the pipe can be related to the fluid and pipe parameters as $Q = \rho A V$ .

# 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 . The general form of the loss coefficient is written as

$$
C _ {L} = \frac {f (L (1 + \alpha) + L _ {a})}{D _ {h}}.
$$

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

$$
\triangle P - \rho g \triangle Z = (C _ {L} + K _ {1}) \frac {\rho V ^ {2}}{2};
$$

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

$$
\triangle P - \rho g \triangle Z = (C _ {L} + K _ {2}) \frac {\rho V ^ {2}}{2}.
$$

<!-- source-page: 1089 -->

Abaqus/Standard supports four different methods for defining the friction factor :

• 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 . The friction factor is empirically calculated as

$$
f = \frac {6 4}{R e}: R e <   2 5 0 0
$$

$$
f = \frac {0 . 3 1 6 4}{R e ^ {0} . 2 5}: R e \geq 2 5 0 0.
$$

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 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

$$
\begin{array}{l} f = 8 \left[ \left(\frac {8}{R e}\right) ^ {1 2} + \frac {1}{(A + B) ^ {1 . 5}} \right] ^ {\frac {1}{1 2}}, \\ A = \left[ - 2. 4 5 7 \ln \left(\left(\frac {7}{R e}\right) ^ {0. 9} + 0. 2 7 \left(\frac {K _ {s}}{D _ {h}}\right)\right) \right] ^ {1 6}, \\ B = \left(\frac {3 7 3 5 0}{R e}\right) ^ {1 6}. \\ \end{array}
$$

Input File Usage: \*FLUID PIPE FLOW LOSS, TYPE=CHURCHILL

<!-- source-page: 1090 -->

# Specifying the friction loss behavior as a table of Reynolds number versus friction factor

You can input a table of 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 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 an initial temperature or field distribution over the nodes of the 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

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
