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

BC Natural Convection Boundary Layer

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 29, 2015, 07:35
Default BC Natural Convection Boundary Layer
  #1
New Member
 
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6
dodobenq is on a distinguished road
Hey Guys,

I'm trying to simulate the natural convection boundary layer along a vertical flat plate. The aim of this case is to investigate the heat-transfer from the wall (hot) to the surrounding air.
At first I tried to use the Cavity-Case with one heated wall. But then I got some interactions with the surrounding walls, e. g. the ambient temperature raises up. Therefore I'm trying to "open" the bottom and the top of the cavity and thereby in theory the hot air raise up and fresh air moves in. But now I have some problems in finding the right BC. I am thankful for all help and information!!!

Some facts:
- I'm using buoyantPimpleFoam
- I'm using kOmegaSST
- The Cavity has 4 types of patches: hot(wall), top(patch), bottom(patch), side(wall)

Now my BC:
k
Code:
hot
    {
        type            fixedValue;
        value           uniform 1e-12;
    }
top 
    {
        type            zeroGradient;
    }
bottom
    {
        type            fixedValue;
        value           uniform 0.00015;
    }
side
    {
        type            fixedValue;
        value           uniform 1e-12;
    }
omega
Code:
hot
    {
        type            fixedValue;
        value           uniform 1e-12;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        beta1           0.075;
    }
top
    {
        type            zeroGradient;
    }
bottom  
    {
        type            fixedValue;
        value           uniform 0.0045;
    }
side 
    {
        type            fixedValue;
        value           uniform 1e-12;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        beta1           0.075;
    }
p
Code:
ALL
        type            calculated;
        value           uniform 100000;
p_rgh
Code:
hot
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
top              
    {
        type         fixedValue;
    value        uniform 100000;
    }
bottom
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
side        
    {
        type         fixedFluxPressure;
        value         uniform 100000;
T
Code:
hot
    {
        type            fixedValue;
        value           uniform 333.15; // 60°C
    }
top               
    {
        type            zeroGradient;
    }
bottom           
    {
        type            fixedValue;
        value           uniform 289.15; 
    }
side            
    {
        type            fixedValue;
        value           uniform 289.15; 
    }
U
Code:
hot
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
top              
    {
        type            zeroGradient;
    }
bottom   
    {
      type        outletInlet;
    phi        phi;
    outletValue    uniform (0 0 0);
    value        uniform (0 0 0);
    }
side            
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
mut
Code:
hot
    {
        type            mutkWallFunction;
        Cmu             0.09; 
        kappa           0.41; 
        E               9.8;  
        value           uniform 0;
    }
top       
    {
        type            calculated;
    }
bottom            
    {
        type            calculated;
    }
side           
    {
        type            mutkWallFunction;
        Cmu             0.09; 
        kappa           0.41; 
        E               9.8;  
        value           uniform 0;
    }
nut
Code:
hot
    {
        type            nutLowReWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0;
    }
top                // oben
    {
        type            calculated;
    }
bottom            // unten 
    {
        type            calculated;
    }
side            // Seite 
    {
        type            nutLowReWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0;
    }
Kind Regards,
Dominik
dodobenq is offline   Reply With Quote

Old   November 3, 2015, 04:22
Default
  #2
New Member
 
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6
dodobenq is on a distinguished road
Can anybody help me?
dodobenq is offline   Reply With Quote

Old   November 3, 2015, 12:40
Default
  #3
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 594
Rep Power: 17
jherb is on a distinguished road
What is the problem with your settings? Does the simulation run?

For k I would suggest for both, top and bottom turbulentIntensityKineticEnergyInlet and for omega compressible::turbulentMixingLengthFrequencyInlet. Actually, I am not sure at all why there is a compressible version for omega but non for k.
For side use you have to decide if you want to use some wall function approach.

Could you get some outflow at the bottom?

Is a fixed temperature boundary condition at hot correct? The alternative could be the boundary condition compressible::turbulentHeatFluxTemperature
jherb is offline   Reply With Quote

Old   November 4, 2015, 03:07
Default
  #4
New Member
 
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6
dodobenq is on a distinguished road
Thanks jherb for your answer!
The number of Iterations explodes after 2 seconds of simulated time :/

I'll try to put your suggestions in the case.
But now I've some further questions:
1) Is there also a "turbulentIntensityKineticEnergyOUTLET" for the patch "top" or
do I have to set it to "turbulentIntensityKineticEnergyInlet" as well?

2) "turbulentIntensityKineticEnergyInlet" - This functions says, that the inlet is turbulent, right? But I want to simulate a natural convection without any turbulence at the inlet

In the meantime I changed the patch "side" from "wall" to "patch".

THANKS!
dodobenq is offline   Reply With Quote

Old   November 4, 2015, 03:25
Default
  #5
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11
agustinvo is on a distinguished road
Hello

I am dealing as well with this case. I am checking my BC's on each boundary you say.

What I don't understand at all is the fixed p and p_rgh. The solver only solves one of them, then it get the other.

What is the error you get?
agustinvo is offline   Reply With Quote

Old   November 4, 2015, 06:28
Default
  #6
New Member
 
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6
dodobenq is on a distinguished road
Hey Augustin!

I've found another solution for this case on this german website: http://ww3.cad.de/foren/ubb/Forum527...9.shtml#000020

The main problem for this case is the p_rgh-file.
On the website they suggest:
Code:
U
    hot
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    top                // oben
    {        
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    bottom            // unten 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    side            // Seite 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    front            // vorne 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }
---------------------------------
T 
    hot
    {
        type            fixedValue;
        value           uniform 333.15; 
    }

    top                // oben
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15;
    }

    bottom            // unten 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15; 
    }

    side            // Seite 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15;  
    }

    front            // vorne 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15; 
    }
------------
p_rgh
    hot
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
   
    top                // oben
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }

    bottom            // unten 
    {
        type         totalPressure;
        value         uniform 100000;
    U        U;
    gamma        1;
    p0        uniform    100000;
    phi        phi;
    psi        none;
    rho        rho;
    }

    side            // Seite 
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }

    front            // vorne 
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }
I'm trying to run this case now and will report my solutions.
dodobenq is offline   Reply With Quote

Old   November 4, 2015, 07:59
Default
  #7
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11
agustinvo is on a distinguished road
Hi Dominik

Which kind of fluid are you trying to simulate?

I am interested in incompressible ones, but buoyantBoussinesqPimpleFoam is not appropriate for my case. I have to use the incompressible options in buoyantPimpleFoam (the simulation takes a long time) or create a new incompressible solver with buoyancy forces, but this last one does not want to work!
agustinvo is offline   Reply With Quote

Old   November 4, 2015, 08:12
Default
  #8
New Member
 
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6
dodobenq is on a distinguished road
Hey!

I'm using compressible gas within a non-steady flow. I want to investigate the heat transfer on a vertical/horizontal flat plate with natural/forced convection.

Kind Regards
dodobenq is offline   Reply With Quote

Old   November 4, 2015, 08:37
Default
  #9
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 594
Rep Power: 17
jherb is on a distinguished road
Here is the source code of turbulentIntensityKineticEnergyOUTLET:
https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

You could use it for both inlet and outlet, as for the outlet case it automatically is switched to zeroGradient.

You might also set the turbulence at the open boundaries to an outletInlet with an inletvalue of 0 (or perhaps a very small number).


Quote:
Originally Posted by dodobenq View Post
Thanks jherb for your answer!
The number of Iterations explodes after 2 seconds of simulated time :/

I'll try to put your suggestions in the case.
But now I've some further questions:
1) Is there also a "turbulentIntensityKineticEnergyOUTLET" for the patch "top" or
do I have to set it to "turbulentIntensityKineticEnergyInlet" as well?

2) "turbulentIntensityKineticEnergyInlet" - This functions says, that the inlet is turbulent, right? But I want to simulate a natural convection without any turbulence at the inlet

In the meantime I changed the patch "side" from "wall" to "patch".

THANKS!
jherb is offline   Reply With Quote

Old   November 6, 2015, 03:17
Default
  #10
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11
agustinvo is on a distinguished road
Hi Dominic! Did you obtain some results?

Are you comparing with any benchmark?
agustinvo is offline   Reply With Quote

Reply

Tags
buoyantpimplefoam, convection heat flux, open cavity

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
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
Radiation in semi-transparent media with surface-to-surface model? mpeppels CFX 11 August 22, 2019 07:30
Radiation interface hinca CFX 15 January 26, 2014 17:11
natural convection boundary condition thomasyangfly FLOW-3D 3 September 11, 2012 10:14
Questions about Boundary Layer Thickness and Turbulence Models famerfamer STAR-CCM+ 3 July 12, 2012 09:47


All times are GMT -4. The time now is 13:26.