1
2
6
5
4
3

Previous: Evaluating pressure coefficient at Up: Test case: Backward-Facing-Step Next: Monitoring the convergence

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

Evaluating mass flow at the domain boundaries

  • The aim of this section is calculation of flow through a specified patch.
  • We use postProcess utility and functionObject flowRatePatch for summing the flux on patch faces.
  • For solvers where the flux is volumetric (i.e. for incompressible solvers)), the flow rate is volumetric; where flux is mass flux (i.e. for compressible solvers), the flow rate is mass flow rate.

  • Print help for this utility:
    # postProcess -help
    Usage: postProcess [OPTIONS]
options:
  -case
    specify alternate case directory, default is the cwd -constant include the ‘constant/’ dir in the times list -dict read control dictionary from specified location -field Specify the name of the field to be processed, e.g. U -fields Specify a list of fields to be processed, e.g. ‘(U T p)’ – regular expressions not currently supported -func Specify the name of the functionObject to execute, e.g. Q -funcs Specify the names of the functionObjects to execute, e.g. ‘(Q div(U))’ -latestTime select the latest time -list List the available configured functionObjects -newTimes select the new times -noFunctionObjects do not execute functionObjects -noZero exclude the ‘0/’ dir from the times list -parallel run in parallel -region specify alternative mesh region -roots <(dir1 .. dirN)> slave root directories for distributed running -time comma-separated time ranges – eg, ‘:10,20,40:70,1000:’ -srcDoc display source code in browser -doc display application documentation in browser -help print the usage
  • The available functionObjects by utility postProcess can be listed by typing # postProcess -list
  • In case of steady-state solution we evaluate last time layer only
  • Use switch -latestTime

  • patchName are inlet and outlet
  • Run utility for inlet:
    # postProcess -func 'flowRatePatch(name=inlet)' -latestTime
  • Screen output:
    /*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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 flowRatePatch(name=inlet) -latestTime
Date   : Jun 16 2017
Time   : 12:01:00
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 = 287

surfaceFieldValue flowRatePatch(name=inlet):
    total faces  = 30
    total area   = 2.54e-05


Time = 287

Reading fields:
    surfaceScalarFields: phi

Executing functionObjects
surfaceFieldValue flowRatePatch(name=inlet) write:
    sum(inlet) of phi = -0.000254


End
  • Same for outlet:
    # postProcess -func 'flowRatePatch(name=outlet)' -latestTime
  • Screen output:
    /*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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 flowRatePatch(name=outlet) -latestTime
Date   : Jun 16 2017
Time   : 12:01:00
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 = 287

surfaceFieldValue flowRatePatch(name=outlet):
    total faces  = 57
    total area   = 3.32e-05


Time = 287

Reading fields:
    surfaceScalarFields: phi

Executing functionObjects
surfaceFieldValue flowRatePatch(name=outlet) write:
    sum(outlet) of phi = 0.00025399


End
  • Resulting flux at the inlet $ \phi_{inlet} = -0.0002539999$
  • Resulting flux at the outlet $ \phi_{outlet} = 0.0002539904$
  • $ \vert\phi_{inlet} + \phi_{outlet}\vert \leq 1\cdot 10^{-8} $
1
2
6
5
4
3

Previous: Evaluating pressure coefficient at Up: Test case: Backward-Facing-Step Next: Monitoring the convergence

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: Unstructured Grid Up: TCFD Solvers Next: Three Dimensional
This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Finite Volume Method

Solver is based on Finite Volume Method more information can be found e.g. in [2], [10] or [9].

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