
[Sponsors] 
November 9, 2011, 12:21 
rhoCentralFoam flat plate boundary layer issues

#1 
Member
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 8 
At the moment I am validating some solvers with the flat plate problem. I got good results for the laminar incompressible case (simplefoam) and the turbulent compressible transient (rhoPimpleFoam) case. Now I want to test rhoCentralFoam since this seems to be the solver that is best suited for the more advanced problem I want to set up. However, using the same mesh and boundary conditions and a very similar fvSchemes and fvSolution dict file (ofcourse with some differences since the terms to be calculated are different) I get a bad result on the last case. My wall shear stress is significantly underpredicted (more than 50%). I tried the kepsilon wall model (but that wasnt stable if i wanted to keep the same setup as in the previous solvers) and the komega SST model. When using rhoCentralFoam in an incompressible domain without turbulence my wall shear stress is relatively close to what is expected.
Does anyone have a clue what is going on here and how I could fix it? It would help me tremendously. Thanks in advance! 

November 9, 2011, 14:38 

#2 
Senior Member
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 368
Rep Power: 12 
Hi,
I don't know if this will make some difference in your case, but I suggest you to take a look at this tread (especially post #11) http://www.cfdonline.com/Forums/ope...rrestart.html Regards V. PSAnyway, could you also post your case settings (BC's, schemes, etc.)? Last edited by vkrastev; November 9, 2011 at 14:42. Reason: adding ps 

November 10, 2011, 04:02 

#3 
Member
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 8 
I fixed the error in rhoCentralFoam as described on that page but the problem still persists. Basically I just have a square domain where the lower region is a wall with compressible k and omega wallfunctions, zero velocity zeroGradient for pressure and temperature. The flow is driven by a prescribed velocity at the inlet and a (wavetransmissive) pressure bc at the outlet. I really fail to see why my wall shear stress is so far away from empirical relations whilst with rhoPimpleFoam it was practically identical. The problem is that I cant use rhoPimpleFoam but have to use rhoCentralFoam. This in order to capture some shocks in a more advanced problem which failed to give good results with rhoPimpleFoam.
My fvSolution is the same as in the rhoCentralFoam tutorials (altough i did try lower tolerances and also some other solvers, but to no avail), and fvSchemes can be summarised as this (altough again i tried a 101 different setups for this as well) : fluxScheme Kurganov; //Tadmor ddtSchemes { default Euler; } gradSchemes { default Gauss linear; //faceLimited Gauss linear 1; //leastSquares 1; Gauss linear limited 0.5; } divSchemes { default Gauss linear; //Gauss limitedLinear 1; div(tauMC) Gauss linear; //Gauss linear limited 0.5; div((muEff*dev2(T(grad(U))))) Gauss linear; //Gauss linear limited 0.5; } laplacianSchemes { default Gauss linear corrected; //Gauss linear limited 0.5; } interpolationSchemes { default linear; reconstruct(rho) vanLeer; reconstruct(U) vanLeerV; reconstruct(T) vanLeer;} snGradSchemes { default corrected; } 

November 10, 2011, 09:10 

#4  
Senior Member
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 368
Rep Power: 12 
Quote:
1) try this fvSchemes setting (for me it works fine, though my measurements were not about wall shear stress): // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // fluxScheme Tadmor; ddtSchemes { default Euler; } gradSchemes { default cellLimted leastSquares 1; } divSchemes { default none; div(tauMC) Gauss linear; div(phi,k) Gauss Gamma 1; div(phi,omega) Gauss Gamma 1; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; reconstruct(rho) Gamma 1; reconstruct(U) GammaV 1; reconstruct(T) Gamma 1; } snGradSchemes { default corrected; } // ************************************************** *********************** // 2) be sure that the solution has reached a steady state condition: rhoCentralFoam is a purely unsteady solver, which uses a very small time step in order to satisfy the wave speed based Courant condition, so you'll have to run it for quite a long before obtaining a stable solution (if your case actually admits a steady state condition). Good luck V. 

November 10, 2011, 09:33 

#5 
Member
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 8 
Thanks, Ill try this. Will be a while before I can confirm if it worked though, slow solver indeed
I already tried the cell limited gradschemes (since in my more complex problem it gets rid of some unwanted oscillations) but this gave me a very bad boundary layer profile. Maybe in combination with the other settings it works and otherwise Ill try part of your fvschemes. Edit: Even though it has only been running for 45 minutes it is already obvious that you were right. The wall shear stress is approaching gradually the expected value (and is already really close) and the boundary layer profile only slightly underpredicts the log law. Thank you so much for your help! Last edited by laurensvd; November 10, 2011 at 10:17. 

November 13, 2011, 08:52 

#6  
Senior Member
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 368
Rep Power: 12 
Quote:
Regards V. 

September 13, 2013, 03:10 
A problem

#7 
Member

Hi to all, I'm trying to validate rhoCentralFoam by solving the flat plate problem, but when I try to contrast my results with Blasius' solution (for Minf=0.3, Pinf=100000 and Tinf=288.15) .
I see that although my profile are approaching to the Blasius' profile, as the solution progresses over time the profile shows a tendency to overestimate the boundary layer thickness. Any advice are welcome. Thanks in advance Felipe. Here are the profiles: https://copy.com/i4wct7vmG0Ry
__________________
Felipe G Last edited by lfgmarc; September 13, 2013 at 05:36. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
A question on "Specifying Boundary Layer Deformation Smoothing"  didiean  FLUENT  2  January 16, 2012 22:39 
boundary condition for flat plate  Ardalan  Main CFD Forum  0  June 18, 2010 17:49 
Turbulent boundary layer on a flat plate  seb62  OpenFOAM Running, Solving & CFD  0  January 16, 2009 10:33 
Flat plate boundary layer problem  student  Main CFD Forum  3  May 21, 2007 13:10 
errors  Fahad  Main CFD Forum  0  March 23, 2004 14:20 