CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

two mixing compresible fluids solver

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 23, 2015, 07:11
Default
  #21
New Member
 
Jignesh Chokshi
Join Date: Aug 2011
Posts: 7
Rep Power: 13
Jimmy Chokshi is on a distinguished road
Quote:
Originally Posted by ziemowitzima View Post
Hi,
Give me your email, I will send you the working case with few words of explanations.
I would attached it here, but size of the file seems to be too large (1.4MB), and I could not attached it to my reply.

best
Hi,

Can you please send this working case to chokshirl@gmail.com ?

Many thanks !!
Jimmy Chokshi is offline   Reply With Quote

Old   April 23, 2015, 07:14
Default
  #22
New Member
 
Jignesh Chokshi
Join Date: Aug 2011
Posts: 7
Rep Power: 13
Jimmy Chokshi is on a distinguished road
Hi,

Can you please send this working case to chokshirl@gmail.com ?

Many thanks !!
Jimmy Chokshi is offline   Reply With Quote

Old   May 20, 2020, 07:14
Default
  #23
New Member
 
Hendrik von Schöning
Join Date: May 2020
Posts: 6
Rep Power: 4
HVonSch is on a distinguished road
Hello everyone,


I had the same problem (multi-fluid-mixing flow, single phase, compressible, stationary).

I combined rhoSimpleFoam and reactingFoam to a new solver, which integrates in rhoSimpleFoam.
I called it rhoMixingSimpleFoam. It is attached to this post.


EDIT: Please keep in mind, that this solver is not well tested or validated in any way!
Also: In this solver the turbulent species transport is modelled via alphat and is thus equal to the turbulent heat fluxes. This is not always the case!



Installation:
Just copy the dir "rhoMixingSimpleFoam" to the rhoSimpleFoam-directory (/path_to_Openfoam/applications/solvers/compressible/rhoSimpleFoam/), enter it and run wmake.


Also attached is the following thermophysicalProperties which is used by this solver:
Code:
thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

inertSpecie air;

species (air CO2);

air
{
    specie
    {
        nMoles          1;
        molWeight       28.965; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           6000;
        Tcommon         1000;
        highCpCoeffs    ( 3.08792717E+00 1.24597184E-03 -4.23718945E-07 6.74774789E-11 -3.97076972E-15 -9.95262755E+02 5.95960930E+00 );
        lowCpCoeffs     ( 3.56839620E+00 -6.78729429E-04 1.55371476E-06 -3.29937060E-12 -4.66395387E-13 -1.06234659E+03 3.71582965E+00 );
        // no source, sorry
    }
    transport
    {
        As          1.460846342e-06; // (White - Viscous Fluid Flow)
        Ts          111;
    }
}

CO2
{
    specie
    {
        nMoles          1;
        molWeight       44.01; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           3500;
        Tcommon         1000;
        highCpCoeffs    ( 3.85746029E+00 4.41437026E-03 -2.21481404E-06 5.23490188E-10 -4.72084164E-14 -4.87591660E+04 2.27163806E+00 );
        lowCpCoeffs     ( 2.35677352E+00 8.98459677E-03 -7.12356269E-06 2.45919022E-09 -1.43699548E-13 -4.83719697E+04 9.90105222E+00 );
         //http://combustion.berkeley.edu/gri-mech/data/nasa_plnm.html
    }
    transport
    {
        As              1.503425096e-06; // (White - Viscous Fluid Flow)
        Ts              222;
    }
}
Attached Files
File Type: gz rhoMixingSimipleFoam.tar.gz (3.6 KB, 4 views)
petr.f. likes this.

Last edited by HVonSch; June 2, 2020 at 08:30. Reason: Added information about validity and assumptions
HVonSch is offline   Reply With Quote

Old   May 31, 2020, 16:15
Default
  #24
New Member
 
Kamal Khemani
Join Date: Feb 2019
Location: India
Posts: 2
Rep Power: 0
KAMAL KHEMANI is on a distinguished road
Quote:
Originally Posted by HVonSch View Post
Hello everyone,


I had the same problem (multi-fluid-mixing flow, single phase, compressible, stationary).


I combined rhoSimpleFoam and reactingFoam to a new solver, which integrates in rhoSimpleFoam.
I called it rhoMixingSimpleFoam. It is attached to this post.


Just copy the dir "rhoMixingSimpleFoam" to the rhoSimpleFoam-directory (/path_to_Openfoam/applications/solvers/compressible/rhoSimpleFoam/), enter it and run wmake.


Also attached is the following thermophysicalProperties which is used by this solver:
Code:
thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

inertSpecie air;

species (air CO2);

air
{
    specie
    {
        nMoles          1;
        molWeight       28.965; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           6000;
        Tcommon         1000;
        highCpCoeffs    ( 3.08792717E+00 1.24597184E-03 -4.23718945E-07 6.74774789E-11 -3.97076972E-15 -9.95262755E+02 5.95960930E+00 );
        lowCpCoeffs     ( 3.56839620E+00 -6.78729429E-04 1.55371476E-06 -3.29937060E-12 -4.66395387E-13 -1.06234659E+03 3.71582965E+00 );
        // no source, sorry
    }
    transport
    {
        As          1.460846342e-06; // (White - Viscous Fluid Flow)
        Ts          111;
    }
}

CO2
{
    specie
    {
        nMoles          1;
        molWeight       44.01; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           3500;
        Tcommon         1000;
        highCpCoeffs    ( 3.85746029E+00 4.41437026E-03 -2.21481404E-06 5.23490188E-10 -4.72084164E-14 -4.87591660E+04 2.27163806E+00 );
        lowCpCoeffs     ( 2.35677352E+00 8.98459677E-03 -7.12356269E-06 2.45919022E-09 -1.43699548E-13 -4.83719697E+04 9.90105222E+00 );
         //http://combustion.berkeley.edu/gri-mech/data/nasa_plnm.html
    }
    transport
    {
        As              1.503425096e-06; // (White - Viscous Fluid Flow)
        Ts              222;
    }
}
Hi HVonSch, with laminar conditions the temperature shoots up at very high value any reason for that ?
KAMAL KHEMANI is offline   Reply With Quote

Old   June 2, 2020, 08:33
Default
  #25
New Member
 
Hendrik von Schöning
Join Date: May 2020
Posts: 6
Rep Power: 4
HVonSch is on a distinguished road
Hello Kamal,

Is the simulation fully converged?
Please provide more information about your case and the way you are using the species mixing (species, phases) to track down if the error is caused by the solver modification.


Best regards,
Hendrik
HVonSch is offline   Reply With Quote

Old   June 15, 2020, 16:59
Default
  #26
Member
 
Petr Furmanek
Join Date: Jan 2012
Location: Faenza, Italy
Posts: 66
Rep Power: 12
petr.f. is on a distinguished road
Hi Hendrik, I'm checking out your solver (nice work btw.). How do you prescribe boundary conditions for the individual species? Is it in the same way as in case of reactingFoam i.e. by individual files in constant/ dir as e.g. "air" and "CO2"?
petr.f. is offline   Reply With Quote

Old   June 16, 2020, 03:04
Default
  #27
New Member
 
Hendrik von Schöning
Join Date: May 2020
Posts: 6
Rep Power: 4
HVonSch is on a distinguished road
Hello Petr,


thank you!


Yes, BCs are prescribed as in reactingFoam.


For example for CO2:


Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      CO2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            fixedValue;
        value           uniform 0;
    }
    OUTLET
    {
        type            inletOutlet;
        value           uniform 0;
        inletValue      uniform 0;
    }
    PLENUM_INLET
    {
        type            fixedValue;
        value           uniform 1;
    }
    PLENUM_OUTLET
    {
        type            inletOutlet;
        value           uniform 1;
        inletValue      uniform 1;
    }
    WALL
    {
        type            zeroGradient;
    }
}


// ************************************************************************* //
You don't need a BC-file for the "inert species" as its fraction is just 1-sum(other species fractions).


Best,
Hendrik
HVonSch is offline   Reply With Quote

Old   August 13, 2020, 13:40
Default
  #28
Member
 
nikhil108's Avatar
 
Nikhil
Join Date: May 2020
Location: Freiburg
Posts: 43
Rep Power: 4
nikhil108 is on a distinguished road
Hallo Foamers,

can you suggest me a solver for, propane jet leak in to air. Right now, i am using reactingbuoyantfoam, but i want to add dynamic mesh, which is not supported by reactingFoam. any suggestions?.

cheers,
nm.
nikhil108 is offline   Reply With Quote

Reply

Tags
compressible flow, mixing gases

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
smoothSolver diverges - solution in using PBiCG solver? makaveli_lcf OpenFOAM Running, Solving & CFD 3 September 11, 2013 13:44
Getting too many iterations by velocity solving (aborting). Changing U - Solver? suitup OpenFOAM Running, Solving & CFD 0 January 20, 2010 08:45
mixing 4 kind of fluids ranap CFX 2 September 19, 2008 12:55
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 15:08
Error during Solver cfd guy CFX 4 May 8, 2001 07:04


All times are GMT -4. The time now is 18:36.