1
2
6
5
4
3

Previous: paraFoam Up: Test case: Backward-Facing-Step Next: Evaluating mass flow at

This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Evaluating pressure coefficient $ C_p$ at the top wall of the channel

    • $ C_p$ pressure coefficient is in general4.1:

     

    $\displaystyle C_{p} = \frac{p - p_{\infty}}{\frac{1}{2}\rho_{\infty} U_{\infty}^{2}}$(4.1)

     

     

    • We are going to evaluate pressure coefficient at the boundary, specifically at the UpperWall patch.
    • It means we need to know value of pressure $ p$ at the boundary.
    • We use OpenFOAM post-processing functionality for sampling value of pressure.
    • The postProcess utility employs function object framework.
    • We use function object surfaceFieldValue.
    • An example of using this function object can be seen in its header file

      # cat $FOAM_SRC/functionObjects/field/fieldValues/surfaceFieldValue/surfaceFieldValue.H

       

    • We create a new file called sampleUpperPatch in system directory.
    • (It can be done for example by command # touch system/sampleUpperPatch . The ‘touch’ command creates an empty text file. Use mcedit, or other text editor, to add following text to the file.)
      type            surfaceFieldValue;
libs            ("libfieldFunctionObjects.so");

writeControl    writeTime;
writeFields     true;

surfaceFormat   raw;
regionType      patch;
name            upperWall;

operation       none;

fields
(
    p
);

       

    • We would like to sample field ‘p’ at the regionType ‘patch’ with name ‘upperWall’. The data will be stored in raw format.
    • The function object can be launched from case directory:

      # cd $FOAM_RUN/pitzDaily

      # postProcess -func sampleUpperPatch

       

    • Output is following:
      /*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  dev                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : dev-e2ccbbbb
Exec   : postProcess -func sampleUpperPatch
Date   : Jun 16 2017
Time   : 12:00:00
Host   : $HOSTNAME
PID    : $$
Case   : $FOAM_RUN/pitzDaily
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

surfaceFieldValue sampleUpperPatch:
    total faces  = 223
    total area   = 0.00031106


Time = 0

Reading fields:
    volScalarFields: p

Executing functionObjects


Time = 100

Reading fields:
    volScalarFields: p

Executing functionObjects


Time = 200

Reading fields:
    volScalarFields: p

Executing functionObjects


Time = 287

Reading fields:
    volScalarFields: p

Executing functionObjects


End

    • In test case directory is directory postProcessing containing new folder sampleUpperPatch, look inside:
      # cd ./postProcessing
      # ls

       

      sampleUpperPatch  sets
      # cd ./sampleUpperPatch
      # ls

       

      surface

      # cd ./surface
      # ls

       

      0  100  200  287

      # cd ./287
      # ls

      patch_upperWall.raw  p_patch_upperWall.raw
    • Look at file data:
      # more ./p_patch_upperWall.raw
      # p  FACE_DATA 223
#  x  y  z  p
-0.0198086 0.0254 0 -1.90829
-0.0182574 0.0254 0 -3.67105
-0.0167681 0.0254 0 -4.67569
-0.0153384 0.0254 0 -4.97477
-0.0139658 0.0254 0 -5.12385
-0.012648 0.0254 0 -5.26736
-0.0113829 0.0254 0 -5.38125
-0.0101683 0.0254 0 -5.46206

    • For plotting $ C_p$ at top wall channel we use e.g. an open-source program gnuplot
    • $ {\textcolor{blue}{\mathsf {In \ Linux: }}}$ Run gnuplot:
      # gnuplot
    • $ {\textcolor{red}{\mathsf {In \ Windows: }}}$ Run gnuplot outside of terminal. Use File > Change Directory and navigate to the location of file p_upperWallData.raw and confirm with OK.
    • In gnuplot environment type command:
      gnuplot> plot './p_patch_upperWall.raw' using 1:($4/(0.5*100)) with lines
    • $ p_{\infty} = 0\ m^2s^{-2},\ U_{\infty} = 10.0\ m\,s^{-1}$
openfoam tutorial backward facing step pitzDaily Cp pressure

Figure: $ C_p$ at the top wall, Backward-Facing-Step OpenFOAM tutorial

1
2
6
5
4
3

Previous: paraFoam Up: Test case: Backward-Facing-Step Next: Evaluating mass flow at

OpenFOAM Training by CFD Support,   CFD SUPPORT,   info@cfdsupport.com    +420 212 243 883      © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

6
2
1
5
4
3

Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation   Contents   Index

Create Computational Mesh

The computational mesh can be either imported, or the computational mesh can be created using snappyHexMesh. See tutorials.

OpenFOAM Training by CFD Support,   CFD SUPPORT,   info@cfdsupport.com    +420 212 243 883      © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

1
2
6
5
4
3

Previous: Incompressible Mathematical Model Up: TCFD Solvers Next: Finite Volume Method
This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Unstructured Grid

The computational mesh data is kept in unstructured OpenFOAM format. See e.g. [12].

OpenFOAM Training by CFD Support,   CFD SUPPORT,   info@cfdsupport.com    +420 212 243 883      © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic