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

rhoCentralFoam flat plate boundary layer issues

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 9, 2011, 12:21
Default rhoCentralFoam flat plate boundary layer issues
  #1
Member
 
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 5
laurensvd is on a distinguished road
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 k-epsilon wall model (but that wasnt stable if i wanted to keep the same setup as in the previous solvers) and the k-omega 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!
laurensvd is offline   Reply With Quote

Old   November 9, 2011, 14:38
Default
  #2
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
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)

Strange rhoCentralFoam behavior after restart...

Regards

V.

PS-Anyway, could you also post your case settings (BC's, schemes, etc.)?

Last edited by vkrastev; November 9, 2011 at 14:42. Reason: adding ps
vkrastev is offline   Reply With Quote

Old   November 10, 2011, 04:02
Default
  #3
Member
 
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 5
laurensvd is on a distinguished road
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; }
laurensvd is offline   Reply With Quote

Old   November 10, 2011, 09:10
Default
  #4
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by laurensvd View Post
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; }
I see some confusion in your fvSchemes file...Anyway, assuming that you have already fixed the phi update problem, I can give you the following advices:

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.
vkrastev is offline   Reply With Quote

Old   November 10, 2011, 09:33
Default
  #5
Member
 
Laurens Van Dyck
Join Date: Jul 2011
Location: Netherlands/Germany
Posts: 34
Rep Power: 5
laurensvd is on a distinguished road
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.
laurensvd is offline   Reply With Quote

Old   November 13, 2011, 08:52
Default
  #6
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by laurensvd View Post
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!
You are welcome! Happy to see that rhoCentralFoam returns good results in the b. l. as I'm using it quite extensively (though not for b. l. measurements)!

Regards

V.
vkrastev is offline   Reply With Quote

Old   September 13, 2013, 03:10
Default A problem
  #7
Member
 
lfgmarc's Avatar
 
Luis Felipe Gutierrez Marcantoni
Join Date: Oct 2010
Location: Cordoba-Argentina
Posts: 46
Rep Power: 6
lfgmarc is on a distinguished road
Send a message via MSN to lfgmarc
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.
lfgmarc 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
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


All times are GMT -4. The time now is 02:15.