
[Sponsors] 
January 19, 2013, 18:42 
Convergence problem with flow facing a backstep (case files now attached)

#1 
Member
David
Join Date: Aug 2012
Posts: 48
Rep Power: 5 
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. Last edited by GM_XIII; January 20, 2013 at 16:17. Reason: Attach case files 

January 22, 2013, 00:23 

#2 
Member
Eric R
Join Date: Jul 2012
Posts: 83
Rep Power: 5 
Can we see your output file?


January 22, 2013, 06:10 

#3 
New Member
Max Meinicke
Join Date: Jul 2012
Posts: 6
Rep Power: 5 
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; } 

January 22, 2013, 09:02 

#4 
Member
David
Join Date: Aug 2012
Posts: 48
Rep Power: 5 
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?


January 22, 2013, 10:29 

#5 
New Member
Max Meinicke
Join Date: Jul 2012
Posts: 6
Rep Power: 5 
Use simpleFoam. It has the following properties:
 steady state


January 22, 2013, 11:24 

#6 
Member
Aathavan
Join Date: Nov 2012
Posts: 70
Rep Power: 5 
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 

January 22, 2013, 11:45 

#7 
Member
David
Join Date: Aug 2012
Posts: 48
Rep Power: 5 
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.


January 22, 2013, 14:22 

#8 
New Member
Max Meinicke
Join Date: Jul 2012
Posts: 6
Rep Power: 5 
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? Last edited by maxmeinicke; January 23, 2013 at 05:07. Reason: corrections 

January 23, 2013, 03:47 

#9 
Member
Aathavan
Join Date: Nov 2012
Posts: 70
Rep Power: 5 
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 

January 23, 2013, 06:52 

#10 
New Member
Max Meinicke
Join Date: Jul 2012
Posts: 6
Rep Power: 5 
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... 

January 28, 2013, 22:54 

#11 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 420
Rep Power: 15 
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Postdoctoral Fellow Research Center for Computational Mechanics (CIMEC)  CONICET/FICHUNL T.E.: 543424511594 Ext. 1005 Güemes 3450  (3000) Santa Fe Santa Fe  Argentina http://www.cimec.org.ar 

January 29, 2013, 02:43 

#12 
Member
Aathavan
Join Date: Nov 2012
Posts: 70
Rep Power: 5 
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 

January 29, 2013, 04:16 

#13 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,018
Rep Power: 18 
I opened Santiago's link and got an English PDF.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

March 26, 2014, 03:55 

#14  
Member
CFDUser
Join Date: Mar 2014
Posts: 55
Rep Power: 4 
Quote:
I also would like to see your result, may be velocity contort is quiet enough. can you post here? 

March 27, 2014, 04:56 

#15  
Member
David
Join Date: Aug 2012
Posts: 48
Rep Power: 5 
Quote:
Regards 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Modeling unsteady multiphase flow in porous media  convergence problem  Vaibhav Kumar  Main CFD Forum  1  July 22, 2012 04:32 
transient, impregnating flow problem  fgommer  FLUENT  0  February 29, 2012 17:10 
simpleFoam convergence problems for pipe flow problem  Mike Graham  OpenFOAM Running, Solving & CFD  0  January 30, 2012 15:40 
Problem with Convergence at high flow rates  Syed  CDadapco  1  April 10, 2007 15:18 
Periodic flow boundary condition problem  sudha  FLUENT  3  April 28, 2004 08:40 