
[Sponsors] 
Circular Cylinder at low Reynold number mesh and non orthogonal corrections 

LinkBack  Thread Tools  Display Modes 
May 13, 2008, 04:10 
Hello everybody,
I try to s

#1 
New Member
Christophe Kassiotis
Join Date: Mar 2009
Location: Paris
Posts: 17
Rep Power: 10 
Sponsored Links
I try to solve the benchmark proposed ans studied by Schäfer and Turek in this paper. I have found some linked topic here and here, but they don't really answer my questions. For the moment, I consider the first case proposed in the benchmark (steady simulation, parabolic input velocity with max 0,3m/s leading to a Reynold number around 20). You will find here some pictures of typical meshes I use: And the "annoying" results: As one can see, the velocity field is not really physical as the flow don't want to enter the fine mesh surrounding the cylinder. I use icoFoam with steadyState time integration scheme. The initial condition are zero velocity and pressure fields (according to the description of the benchmark). I'm doing one time step (Is the steady solution independant of the size of the time step ?). For PISO algorithm I tried many solution with high number of orthogonal and nonOrthogonal correctors (let's say respectively 300 and 20)...leading to more time expensive computation but not really better results. I also checked the mesh with the checkMesh utility: Mesh nonorthogonality Max: 44.01408683 average: 11.32517179 Nonorthogonality check OK. My question are the following: 1  is it absolutely necessary to compute first a solution with potential foam (as proposed in one of the thread)?...I think it will not really respect the benchmark proposed I my case. 2  Do you see any mistake in my procedure? 3  Is they a way to link the nonorthogonality results obtained by checkMesh to the number of orthogonal and nonOrthogonal correctors. 4  Other question : in the paper by Schäfer and Turek they speak about a recirculation area that as to be measured. What is this? Is they an easy way to automatically measure this in OpenFoam (not seeing the results in paraFoam)? Thank you for any help or comments. 

Sponsored Links 
May 13, 2008, 05:19 
1) No, it is no need to comput

#2 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
1) No, it is no need to compute potential solution  this may only improve solution convergence
2) YOU SHOULD NOT USE icoFoam with steadystate time integration scheme, because icoFoam uses TRANSIENT precvel coupling algo, PISO 3) Your mesh thikness in Ydirection is too small, mesh thikness should be about 50100 diamterers of cylinder (character length). what is your BC's on upper and lower walls? opt. number of non orthogonal correctors is 13 4) I can't donload papers by your references
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

May 13, 2008, 05:47 
the solver icoFoam isn't stati

#3 
New Member
Mark Michael
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 5
Rep Power: 10 
the solver icoFoam isn't stationary ! this solver needs an time integration scheme, because it solves the isothermal incompressible NavierStokesequation ! so it also need timesteps !
Get some Books about "Fluidmechanics" and "wake flow around a circular cylinder" there you find many specifications about "recirculation area" ! Can you send me the paper per email ? I can't open the link ! astadfm@gmx.de 

May 13, 2008, 06:00 
Thank you for the hints.
1

#4 
New Member
Christophe Kassiotis
Join Date: Mar 2009
Location: Paris
Posts: 17
Rep Power: 10 
Thank you for the hints.
1  Ok, It was what I was thinking about potential solution. 2  Not use icoFoam means use something like simpleFoam ? 3  The mesh thikness, is, I admit, really not enough to avoid influence of boundary conditions on the flow around the cylinder, especially with the noslip boundary condition I impose...but this is how the problem is defined in the paper (hope the link will work now). 

May 14, 2008, 07:03 
2  yes, use simpleFoam with t

#5 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 12 
2  yes, use simpleFoam with turbulence "off" and
turbulenceModel "laminar" (file constant/turbulenceProperties) 3  for freestream boundary i'm using pressureInletOutletVelocity for U and outletInlet for p. And, of course, if you want to compare your results with those in paper, you must use BC's from paper 4  the link work
__________________
Winter OpenFOAM days in Moscow  http://www.isprasopen.ru/en/conf/cfd.html 

May 14, 2008, 11:09 
Hello again,
I try for the

#6 
New Member
Christophe Kassiotis
Join Date: Mar 2009
Location: Paris
Posts: 17
Rep Power: 10 
Hello again,
I try for the moment two strategies in parallel, with, for both, initial state computed by potential foam solver. with simpleFoam (steadyState for time integration, output specified through the use of inletOutlet, laminar flow without any turbulence as a model): The results are the following They are not so bad. Unfortunately in notice two problems :
with icoFoam: I run the computation with an Euler time integration scheme. This seems to behave as awaited. Unfortunately, the Drag coefficient exhibits the following shape when drawing respect to time (the value at the end is not so bad, as one awaited around 5.5). I think this is linked to the computation of pressure, no ? When one plot the pressure respect to time, one see a kind of "slow" diffusion. So my question are the following :
Thank you again for your help and advices ! 

May 15, 2008, 06:07 
Hello everybody,
In fact, i

#7 
New Member
Christophe Kassiotis
Join Date: Mar 2009
Location: Paris
Posts: 17
Rep Power: 10 
Hello everybody,
In fact, it seems that, according to results from F. Bos computing the drag coefficient for a circular cylinder that the big overestimate at the beginning with icoFoam is a normal behavior before convergence In the following, you will find different numerical experiments:
So, I think that I will use icoFoam, let it run a certain time and take the final value  which is close to the one expected at first glance  for the drag coefficient. I remain interested by any comments and/or remarks. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
reynold number on inlet  Fayyaz Hussain  FLUENT  2  June 18, 2007 12:24 
LOW REYNOLD NUMBER  Limonghi  Main CFD Forum  1  March 13, 2007 12:37 
urgent:low reynold number Kepsilon model  prasanna  FLUENT  3  January 1, 2007 14:20 
low turbulent reynold number  CCARE  CFX  4  March 12, 2004 07:36 
Reynold number???  Jame D.J.  CFX  5  July 30, 2002 08:27 
Sponsored Links 