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

cyclone-case with lower outlet using simpleReactingFoam (steady-state)

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 10, 2018, 17:12
Default cyclone-case with lower outlet using simpleReactingFoam (steady-state)
  #1
Member
 
Jan Goebel
Join Date: Mar 2009
Location: Mannheim, Baden Wuerttemberg, Germany
Posts: 35
Rep Power: 15
jango is on a distinguished road
Dear community,

I'm currently trying to solve the cyclone case with a lower outlet using simpleReactingParcelFoam for a steady-state case with lagrangian particle tracking. As for a first step I modified the verticalChannel tutorial case to the cyclone boundaries with it's standard thermophysical model and ajusted it to my flow rate, but unfortunately it's diverging after 20 iterations throwing out the following error message:
Code:
Maximum number of iterations exceeded: 100
Checking the results, the particles get injected, and according to the log file, there's a mass flow through both outlets. I guess, that there's some error on my boundary conditions regarding the outlets, as in the verticalChannel case the particle/gas concentration is known and set to a sum of 1 at a single outlet.

In my case I have two outlets and want the solver to calculate the concentration accordingly. Does anybody know the correct settings for the outlet for this case ?

Attached to this post I'll send you my boundary settings for the initial fields, maybe that helps.

Thank you in advance,

Jan
Attached Files
File Type: zip 0.orig_and_solverout.zip (11.2 KB, 6 views)
jango is offline   Reply With Quote

Old   April 11, 2018, 07:23
Default complete case file
  #2
Member
 
Jan Goebel
Join Date: Mar 2009
Location: Mannheim, Baden Wuerttemberg, Germany
Posts: 35
Rep Power: 15
jango is on a distinguished road
Unfortunately I still couldn' t spot out the error. If I run the case with the default thermophysical properties from the verticalChannel tutorial case it's still diverging. Checking out the output for pmin/pmax it can be observed, that the pressure field diverges.

When I change the material properties to my own created thermophysical properties, I get the error message, that specie- keyword is not defined (even though it is)
Attached Files
File Type: zip thermo_own_data.zip (1.2 KB, 13 views)
jango is offline   Reply With Quote

Old   April 16, 2018, 23:59
Default
  #3
Member
 
Kirk Jarvis
Join Date: Mar 2009
Posts: 31
Rep Power: 15
kcjarvis56 is on a distinguished road
The phaseChangeModel in the reactingCloudProperties is set to liquid evaporation. Look at the air flows at the inlet along mass rates of reacting cloud are ratio'ed correctly or it will blow up quickly. You can use none for the phaseChangeModel which may help you get to a running model quick then add the evaporation model if you need it. As far as using your properties it doesn't appear you are using the right thermoType mixture for the solver. I didn't have any luck using multiComponetMixture, it needed to be reactingMixture. Also the error message regarding specie (with your own properties), since you are not using the reactingMixture (as mentioned above) it doesn't read the foamChemistryFiles files you need to put all the information in the thermophysicalProperites file.

For example:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture; // couldn't get to work with simpleReactingParcelFoam
    transport       const;
    thermo          hConst;
    equationOfState incompressiblePerfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

//chemistryReader foamChemistryReader;

//foamChemistryFile "$FOAM_CASE/constant/reactions";

//foamChemistryThermoFile "$FOAM_CASE/constant/thermo.incompressiblePoly";

inertSpecie     air;

liquids
{
    H2O;
}

solids
{}

species
(
    air
    H2O
);

H2O
{
    specie
    {
        nMoles          1;
        molWeight       18.0153;
        pRef            100000;
    }
    equationOfState
    {
        pRef            100000;
    }
    
    thermodynamics
    {
        Cp              4310;
        Hf              6.3225e+05;
    }
    transport
    {

        mu              1.825e-04;
        Pr              1.15;
    }
}

air
{
    specie
    {
        nMoles          1;
        molWeight   18.0153;
        pRef            100000;
    }
    equationOfState
    {
        pRef            100000;
    }

    thermodynamics
    {
//        Cp              1007;
        Cp          2396;
//        Hf              2.257e+06;
        Hf          2.7459e+06;
    }
    transport
    {
//        mu              1.41e-05;
        mu          1.399e-05;
//        Pr              1;
        Pr          1.089;
    }
}




// ************************************************************************* //
Hope this helps.
kcjarvis56 is offline   Reply With Quote

Old   April 17, 2018, 05:06
Default reactingCloud1Properties
  #4
Member
 
Jan Goebel
Join Date: Mar 2009
Location: Mannheim, Baden Wuerttemberg, Germany
Posts: 35
Rep Power: 15
jango is on a distinguished road
Hello Kirk,

thank you for your reply. I finally managed to run my own case by adjusting it to the proper material properties using the standard-steam tables. I also switched off the phase change modell to "none" as the only thing which is needed is the information about the particle behaviour at the wall. Unfortuntely by running different models varying the coefficients of e and mu for the wall behaviour there are no changes regarding the particle masses leaving and remaining into the vessel. It seems that this coefficients doesn't have any effect... Is there a good documentation available for the reactingCloud1Properties dict anywhre available- I've searched the web but couldn't find anything suitable.

Have a nice day,

Jan

Last edited by jango; April 17, 2018 at 07:37. Reason: additional information added
jango is offline   Reply With Quote

Reply

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
Case comparison of steady state and time-averaged transient solutions k.vafiadis CFX 2 October 20, 2012 05:37
Mass Diffusion: Transient and Steady State BC rval CFX 3 November 19, 2008 00:52
steady state, laminar vof_model Garima Chaudhary FLUENT 0 May 24, 2007 03:11
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
About the difference between steady and unsteady problems Lisa Main CFD Forum 11 July 5, 2000 14:37


All times are GMT -4. The time now is 20:08.