Convergence problem with flow facing a backstep (case files now attached)
1 Attachment(s)
I am starting with OpenFoam so this can be a silly question. I have experience with other CFD programs but i decide to start learning OpenFoam.
Problem data: Incompressible airfoil facing a backstep, Steady, I am using the icoFoam solver. I have convergence problems as the Courant goes up as the residuals. Feel free to ask for further information and thanks in advance. 
Can we see your output file?

Hi,
icoFoam is a transient solver. You can identify that under: <OPENFOAM_DIR>/applications/solvers/incompressible/icoFoam/icoFoam.C line 58 (OF2.1.x) fvm::ddt(U) > transient So you must not set steadyState ddtSchemes in system/fvSchemes. For example: use full implicit Euler scheme. Search the following folder for all available ddtSchemes: <OPENFOAM_DIR>/src/finiteVolume/finiteVolume/ddtSchemes To identify their name for fvSchemes, have a look into their header files (*.H). Search for the string in TypeName. That's what you can put into fvSchemes. Example: EulerDdtScheme.H > line 71 (OF2.1.x): TypeName("Euler"); > ddtSchemes { default Euler; } 
Thank you, I thought that a transient solver could manage steady cases with that fvShemes, my fault of couse. I would like to do it Steady becouse if i do it transient i need to set a very low time step in order to keep the coutant number low. So, what's the best solver to solve this case as Steady?

Use simpleFoam. It has the following properties:
 steady state

Hi Maxmeinicke,
I have a small silly question, [ pressure p is not the real pressure in [N/m2], but it is p / rho [m2/s2] ] according your post, to get the real pressure in [N/m2], what should we do? how to convert the simpleFoam simulation pressure in to real pressure???? I am bit confused by the unit of (p/rho > m2/s2), can you please explain about it? Thanks, Aadhavan 
Thank you mate, I finally did it :) I haven't realised that you could use a turbulent solver and then specify that the case is laminar. Now it is done, I will upload the case files in case someone could be interested.

Congratulations to you :)
unit calculation: compressible: p = F / A = N / m2 = kg * m / s2 / m2 = kg / m / s2 OpenFOAM notation: 'dimensions [1 1 2 0 0 0 0];' incompressible: p / rho = F / A / rho = N / m2 / (kg / m3) = kg * m / s2 / m2 / (kg / m3) = m2 / s2 OpenFOAM notation: 'dimensions [0 2 2 0 0 0 0];' Have a look into the pressure boundary files in time folder 0 for incompressible and compressible tutorial cases. unit explanation: In OpenFOAM basic solvers, 'incompressible' means constant density and 'compressible' means the density varies. So in compressible solvers a density transport equation is solved (rhoEqn). If the density is constant, you can divide all terms in the transport equations by the density. You will find out that the density is removed from all terms except the pressure term and the viscosity term. That is why with compressible and incompressible solvers one must be careful with units. compressible uses:
p_compr = p_incompr * rho mu_compr = nu_incompr * rho As you can see, the units scale with rho. So if you calculate water, mu is 1000 times larger than nu. To calculate the real pressure for an incompressible solver, multiply with the density. If I would like to write the real pressure to the timefolders, I would derive a new solver and add a new volScalarField p_real. If someone knows, how to manage writing the real pressure for incompressible solvers to time folders using functions and without creating a new solver, please let us know. If you have more questions, please ask. which OF version do you use? 
Hi,
Thanks for your long reply, I am using OF2.0.1. small correction your explanation, pressure p which is actually p / rho [m2 / m2], this should be (m2/s2). Thanks, Aadhavan 
1 Attachment(s)
I've created a new solver simpleFoam2.
It is derived from simpleFoam and outputs the real pressure pReal. just extract the file and read the README... 

Hi Santiag,
Can you please say something about it. I tried to look at it but I am not able. It seems it is in French or some other language. is there any English version. Thanks, Aadhavan 
I opened Santiago's link and got an English PDF.

Quote:
I also would like to see your result, may be velocity contort is quiet enough. can you post here? 
Quote:
Regards 
All times are GMT 4. The time now is 07:40. 