CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

some questions about the setting of a compressible case

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 16, 2011, 17:03
Default some questions about the setting of a compressible case
  #1
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
hi everyone,

I want to use rhoSimpleFoam to simulate a laval nozzel and I have some problems of OpenFoam setting.

1. in the 0 folder, there is a variable alphat. What mena this variable and how to calculate it?

2. Are the pressure and temeprature showed in ParaView totalpressure(temperature) or staticpressure(temperature)?

3. In the file thermophysicalProperties in constant folder, I have set the following for the air:

thermoType hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;
mixture air 1 28.9 1007 0 1.84e-05 0.7;

But what means the value 0 1.84e-05 0.7 here?

4. For pressure I have set a totalpressure boundary condition for the inlet of the nozzel.

type totalPressure;
p0 uniform 203250;
U U;
phi phiv;
rho none;
psi psi;
gamma 1..4;
value uniform 203250;

What is the difference between p0 and value. I think p0 should be the total pressure but what means value uniform 203250, is it the static pressure?

Thanks a lot.
xck1986 is offline   Reply With Quote

Old   January 17, 2011, 04:57
Default
  #2
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,

1 Variable 'alphat' is turbulent thermal diffusivity. You need not worry about it. It is calculated during the run. So even if you delete it from 0 folder there wouldn't be any problem.

2. They are static values if at the point of interest fluid is in motion.

3. 1.85e-6 is value of viscosity coefficient needed because of "constTransport" and 0.7 is Prandtl No. (Refer the User Guide for details)

4. That "value" is where you specify the value of your Po. Just search this BC in this forum and you would find the necessary details.
nakul is offline   Reply With Quote

Old   January 17, 2011, 09:53
Default
  #3
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
Quote:
Originally Posted by nakul View Post
Hi,

1 Variable 'alphat' is turbulent thermal diffusivity. You need not worry about it. It is calculated during the run. So even if you delete it from 0 folder there wouldn't be any problem.

2. They are static values if at the point of interest fluid is in motion.

3. 1.85e-6 is value of viscosity coefficient needed because of "constTransport" and 0.7 is Prandtl No. (Refer the User Guide for details)

4. That "value" is where you specify the value of your Po. Just search this BC in this forum and you would find the necessary details.
Hi Nakul,
thanks a lot for your reply.

And still two questions are not clear for me:

1.In the file thermophysicalProperties,
thermoType hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>;
mixture air 1 28.9 1007 0 1.84e-05 0.7;

What means the value 0here?

2. Is it possible to visualise the Mach Number in ParaView? Do I need to also define the boundary and initial condition for Mach number in the 0 folder?

Thanks again!!!
xck1986 is offline   Reply With Quote

Old   January 20, 2011, 05:27
Default
  #4
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,

As I have told you earlier, if you go through user guide you will find that

1) "1007" is value of Cp and "0" is for heat of formation as required by the "hConstThermo" model.

2) Yes after the simulation ends just execute the command Mach and in each time directory a field called Mach would be created. After that you would be able to visualise Mach No. in paraView.
nakul is offline   Reply With Quote

Old   September 26, 2011, 05:18
Default
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
HI,

I am trying to set up a compressible case with SST turbulence model. For that I am trying to understand the rhoPimpleFoam/ras/cavity tutorial. I´d like to join in with some questions:

1) What is the variable 'R' ? And how to calculate it? (Edit: maybe Reynolds stress? Would match dimensions.)

2) Why do I have to set for an compressible case epsilon and mut (instead of nut)? Do I calculate mut this way: mut = nut * rho ? And do I calculate epsilon just like in an incompressible case?

thanks a lot

Camoesas

Last edited by camoesas; September 26, 2011 at 06:11.
camoesas is offline   Reply With Quote

Old   September 26, 2011, 13:10
Default
  #6
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,

1) Can you post the code snippet in which R is used? The code for the solver is located in applications folders of your OF directory!!

2) You have to provide BCs for turbulence parameters also. The parameters for which you provide value depend upon the turbulence model that you chose. You may read about OF's SST model on OF wiki (Turbulence Modelling Section). It would clear all your doubts regarding this model.

-Nakul
nakul is offline   Reply With Quote

Old   September 27, 2011, 11:40
Default
  #7
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
Hey Nakul,

1) R is used in tutorials/compressible/rhoPimpleFoam/ras/cavity/0

2) I know I have to provide boundary conditions for turbulence parameters. But in a compressible case you just have to give k and omega for SST Model...

regards
camoesas is offline   Reply With Quote

Old   September 27, 2011, 14:24
Default
  #8
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi

1) Could you just post that file about 'R' here? I won't be having access to OF for few days so I can only reply by having a look at the details of this variable here?

2) If you have confirmed that only k and omega need to be specified, just specify these values in '0' folder. Other files (nut and mut) would be created automatically. You need not create them.

-Nakul
nakul is offline   Reply With Quote

Old   October 4, 2011, 06:22
Default
  #9
Senior Member
 
Join Date: Mar 2009
Posts: 138
Rep Power: 8
camoesas is on a distinguished road
HI Nakul,

Thanks for you´r reply!

Here's the 'R' file:


Code:
/*--------------------------------*- C++ -*----------------------------------*\                                                                                                     
| =========                 |                                                 |                                                                                                     
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |                                                                                                     
|  \\    /   O peration     | Version:  2.0.0                                 |                                                                                                     
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |                                                                                                     
|    \\/     M anipulation  |                                                 |                                                                                                     
\*---------------------------------------------------------------------------*/                                                                                                     
FoamFile                                                                                                                                                                            
{                                                                                                                                                                                   
    version     2.0;                                                                                                                                                                
    format      ascii;                                                                                                                                                              
    class       volSymmTensorField;                                                                                                                                                 
    location    "0";                                                                                                                                                                
    object      R;                                                                                                                                                                  
}                                                                                                                                                                                   
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //                                                                                                     
                                                                                                                                                                                    
dimensions      [ 0 2 -2 0 0 0 0 ];                                                                                                                                                 
                                                                                                                                                                                    
internalField   uniform ( 0 0 0 0 0 0 );                                                                                                                                            
                                                                                                                                                                                    
boundaryField                                                                                                                                                                       
{                                                                                                                                                                                   
    movingWall                                                                                                                                                                      
    {                                                                                                                                                                               
        type            kqRWallFunction;                                                                                                                                            
        value           uniform ( 0 0 0 0 0 0 );                                                                                                                                    
    }                                                                                                                                                                               
                                                                                                                                                                                    
    fixedWalls                                                                                                                                                                      
    {                                                                                                                                                                               
        type            kqRWallFunction;
        value           uniform ( 0 0 0 0 0 0 );
    }

    frontAndBack
    {
        type            empty;
    }
}


// ************************************************************************* //
camoesas is offline   Reply With Quote

Old   October 7, 2011, 17:56
Default
  #10
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Hi,

1) The 'R' is effectively the Reynolds stresses. It's there so if you choose a turbulent model transporting the reynolds stresses the case will run also. But if you the SST model, the solver won't even read 'R' because it isn't needed.
2) Concerning mut, nut (or in LES muSgs or nuSgs), the interest at the zero time folder is to determine which law of the wall, you want to apply. I actually don't know which one is chosen by default when mut/nut is not specified by the user.

Bye

Fred
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Regarding Setting a Case FILE USING Population Balance Module for Crystallisation vicky FLUENT 1 August 8, 2014 21:42
Setting up a turbine nozzle case cfdengineer CFX 2 August 2, 2010 05:49
Question about inlet setting Mahe Phoenics 0 June 12, 2009 23:31
compressible flow question paratap FLUENT 1 May 17, 2004 13:34
Body force - Does it work? Jan Rusås CFX 5 August 27, 2002 09:50


All times are GMT -4. The time now is 20:12.