
[Sponsors] 
October 29, 2015, 07:35 
BC Natural Convection Boundary Layer

#1 
New Member
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6 
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 heattransfer from the wall (hot) to the surrounding air. At first I tried to use the CavityCase 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 1e12; } top { type zeroGradient; } bottom { type fixedValue; value uniform 0.00015; } side { type fixedValue; value uniform 1e12; } Code:
hot { type fixedValue; value uniform 1e12; 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 1e12; Cmu 0.09; kappa 0.41; E 9.8; beta1 0.075; } Code:
ALL type calculated; value uniform 100000; 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; 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; } 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); } 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; } 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; } Dominik 

November 3, 2015, 04:22 

#2 
New Member
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6 
Can anybody help me?


November 3, 2015, 12:40 

#3 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 594
Rep Power: 17 
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 

November 4, 2015, 03:07 

#4 
New Member
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6 
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! 

November 4, 2015, 03:25 

#5 
Senior Member
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11 
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? 

November 4, 2015, 06:28 

#6 
New Member
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6 
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_rghfile. 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; } 

November 4, 2015, 07:59 

#7 
Senior Member
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11 
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! 

November 4, 2015, 08:12 

#8 
New Member
Dominik
Join Date: Oct 2015
Location: Stuttgart
Posts: 8
Rep Power: 6 
Hey!
I'm using compressible gas within a nonsteady flow. I want to investigate the heat transfer on a vertical/horizontal flat plate with natural/forced convection. Kind Regards 

November 4, 2015, 08:37 

#9  
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 594
Rep Power: 17 
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:


November 6, 2015, 03:17 

#10 
Senior Member
Agustín Villa
Join Date: Apr 2013
Location: Fuenlabrada
Posts: 256
Rep Power: 11 
Hi Dominic! Did you obtain some results?
Are you comparing with any benchmark? 

Tags 
buoyantpimplefoam, convection heat flux, open cavity 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Wind turbine simulation  Saturn  CFX  58  July 3, 2020 01:13 
Radiation in semitransparent media with surfacetosurface model?  mpeppels  CFX  11  August 22, 2019 07:30 
Radiation interface  hinca  CFX  15  January 26, 2014 17:11 
natural convection boundary condition  thomasyangfly  FLOW3D  3  September 11, 2012 10:14 
Questions about Boundary Layer Thickness and Turbulence Models  famerfamer  STARCCM+  3  July 12, 2012 09:47 