10.3 Session file configuration

In the following the possible options are shown for the incompressible Navier-Stokes. The Expansion section for an incompressible flow simulation can be set as for other solvers regardless of the projection type. Here an example for a 3D simulation (for 2D simulations the specified fields would be just u,v,p).

1<EXPANSIONS> 
2  <E COMPOSITE="C[0]" NUMMODES="6" FIELDS="u,v,w,p" TYPE="MODIFIED" /> 
3</EXPANSIONS>

In case of a simulation using the Direct Solver we need to set FIELDS=u,v as the pressure expansion order will be automatically set to fulfil the inf-sup condition. Possible choices for the expansion TYPE are:

Basis TYPE
Modal MODIFIED
Nodal GLL_LAGRANGE
Nodal SEM GLL_LAGRANGE_SEM

10.3.1 Solver Info

The following parameters can be specified in the SOLVERINFO section of the session file:

10.3.2 Parameters

The following parameters can be specified in the PARAMETERS section of the session file:

10.3.3 Womersley Boundary Condition

It is possible to define the time-dependent Womersley velocity profile for pulsatile flow in a pipe. The modulation of the velocity profile is based on the desired peak or centerline velocity which can be represented by a Fourier expansion Umax = A(ωn)ent where A are the Fourier modes and ω the frequency. The womersely solution is then defined as:

                     2   ∑N  ˜     J0(i3∕2αnr-∕R-) iωnt
w (r,t) = A0 (1− (r∕R ) )+   An [1−    J0(i3∕2α)   ]e
                         n=1

where the womersley number α is defined:

       ∘ -----
α  = R   2πn-
  n       Tν

and  ˜
An (n = 1 : N)are the Fourier coefficients scaled in the following way:

                  1
A˜n = 2An ∕[1− ----3∕2--]
              J0(i  α )

The Womersley velocity profile is implemented in the following way:

1<REGION REF="0"> 
2                <D VAR="u" USERDEFINEDTYPE="Womersley:WomParams.xml" VALUE="0" /> 
3                <D VAR="v" USERDEFINEDTYPE="Womersley:WomParams.xml" VALUE="0" /> 
4                <D VAR="w" USERDEFINEDTYPE="Womersley:WomParams.xml" VALUE="0" /> 
5                <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> 
6</REGION>

A file containing the Fourier coefficients, , must be in the directory where the solver is called from. The name of the file is defined by the string given in the attribute USERDEFINEDTYPE after the “:” and contains the real and imaginary coefficients. This file has the format

1<NEKTAR> 
2  <WOMERSLEYBC> 
3    <WOMPARAMS> 
4      <W PROPERTY="Radius" VALUE="0.5" /> 
5      <W PROPERTY="Period" VALUE="1.0" /> 
6      <W PROPERTY="axisnormal" VALUE="0.0,0.0,1.0" /> 
7      <W PROPERTY="axispoint" VALUE="0.0,0.0,0.0" /> 
8    </WOMPARAMS> 
9 
10    <FOURIERCOEFFS> 
11      <F ID="0"> 0.600393641193,    0.0               </F> 
12      <F ID="1"> -0.277707172935,   0.0767582715413   </F> 
13      <F ID="2"> -0.0229953131146,  0.0760936232478   </F> 
14      <F ID="3"> 0.00858135174058,  0.017089888642    </F> 
15      <F ID="4"> 0.0140332527651,   0.0171575122496   </F> 
16      <F ID="5"> 0.0156970122129,   -0.00547357750345 </F> 
17      <F ID="6"> 0.00473626554238,  -0.00498786519876 </F> 
18      <F ID="7"> 0.00204434981523,  -0.00614566561937 </F> 
19      <F ID="8"> -0.000274697215201, 0.000153571881197 </F> 
20      <F ID="9"> -0.000148037910774, 2.68919619581e-05 </F> 
21    </FOURIERCOEFFS> 
22  </WOMERSLEYBC> 
23</NEKTAR>

Each value of is provided in the FOURIERCOEFFS section and provided as separate entries containing the real and imaginary components, i.e. the mean component provided above is 0.600393641193,0.0.

Similarly in the WOMPARAMS section the key parameters of the boundary condition are also provided as:

10.3.4 Forcing

10.3.4.1 MovingBody

Note: This force type is only supported for the Quasi-3D incompressible Navier-Stokes solver.

This force type allows the user to solve the interaction system of an incompressible fluid flowing past a flexible moving bodies  [27]. By this forcing function, one can eliminate the difficulty of moving mesh by using body-fitted coordinates, so that an additional acceleration term(i.e., forcing term) is introduced to the momentum equations by the non-inertial transform from the deformed and moving coordinate system to non-deformed and stationary one.

1<FORCE TYPE="MovingBody"> 
2</FORCE>

Available options of the motion type for the moving body include free, constrained and forced vibrations, which can be specified in the SOLVERINFO section. The free type of motion allows the body to move in both streamwise and crossflow directions, while the constrained type limits the motion only in the crossflow direction. For the forced type, the vibration profiles of the body should be specified as a given function or read from input file in MovingBody section. here an example,

1<SOLVERINFO> 
2    <I PROPERTY="EQTYPE"    VALUE="UnsteadyNavierStokes" /> 
3    <I PROPERTY="SolverType"    VALUE="VelocityCorrectionScheme" /> 
4    <I PROPERTY="EvolutionOperator"    VALUE="SkewSymmetric" /> 
5    <I PROPERTY="Projection"    VALUE="Galerkin" /> 
6    <I PROPERTY="GlobalSysSoln"    VALUE="DirectStaticCond"/> 
7    <I PROPERTY="TimeIntegrationMethod"    VALUE="IMEXOrder2" /> 
8    <I PROPERTY="HOMOGENEOUS"    VALUE="1D"/> 
9    <I PROPERTY="USEFFT"    VALUE="FFTW"/> 
10    <I PROPERTY="VibrationType"    VALUE="FREE"/> 
11</SOLVERINFO>

A moving body type boundary condition should be specified in BOUNDARYCONDITIONS for the velocities on the moving body,

1<BOUNDARYCONDITIONS> 
2    <REGION REF="0"> 
3        <D VAR="u" USERDEFINEDTYPE="MovingBody" VALUE="0" /> 
4        <D VAR="v" USERDEFINEDTYPE="MovingBody" VALUE="0" /> 
5        <D VAR="w" VALUE="0" /> 
6        <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> 
7     </REGION> 
8</BOUNDARYCONDITIONS>

For the simulation of low mass ratio, there is an option to activate fictitious mass method for stabilizing explicit coupling between the fluid solver and structural dynamic solver. Here we need to specify the values of fictitious mass and damping in PARAMETERS, for example,

1<SOLVERINFO> 
2    <I PROPERTY="FictitiousMassMethod"    VALUE="True"/> 
3</SOLVERINFO> 
4<PARAMETERS> 
5    <P> FictDamp      = 1000    </P> 
6    <P> FictMass       = 1.5       </P> 
7</PARAMETERS>

A filter calles as MovingBody is encapsulated in this module to evaluate the aerodynamic forces along the moving body surface. The forces for each computational plane are projected along the Cartesian axes and the pressure and viscous contributions are computed in each direction.

The following parameters are supported:

Option name Required Default

Description

OutputFile session

Prefix of the output filename to which the forces are written.

Frequency 1

Number of timesteps after which output is written.

Boundary -

Boundary surfaces on which the forces are to be evaluated.

To enable the filter, add the following to the FORCE tag::

1  <FORCE TYPE="MovingBody"> 
2      <PARAM NAME="OutputFile">DragLift.frc</PARAM> 
3      <PARAM NAME="OutputFrequency">10</PARAM> 
4      <PARAM NAME="Boundary"> B[0] </PARAM> 
5  </FORCE>

During the execution a file named DragLift.frc will be created and the value of the aerodynamic forces on boundary 0, defined in the GEOMETRY section, will be output every 10 time steps.evaluates the aerodynamic forces along the moving body surface. The forces for each computational plane are projected along the Cartesian axes and the pressure and viscous contributions are computed in each direction.

Also, to use this module a MAPPING needs to be specified, as described in section 10.6. In the case of free and constrained motion presented here, the functions defined by the mapping act as initial conditions. Also, when using the MovingBody forcing, it is not necessary to set the TIMEDEPENDENT property of the mapping.