
[Sponsors] 
November 17, 2005, 10:30 
I am running timedependent ic

#1 
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 9 
I am running timedependent icoFoam on a simple 2D funnellike geometry (80 cells). The simulation converges fast, but the results look very strange in ParaFoam, with velocity arrows going everywhere. The pressure is showing some striping, wh, at least when looking at the cellvalues. Face pressure looks ok. I ran the same case in fluent, with a more expected result for velocity.
I have been looking at it for a while now, and can't figure out where I am going wrong. From what I have read, this seem like a pressurevelocityinterpolation error, but I took the fvSchemes from the elbowtutorial case, and have been testing different schemes to no avail. I have posted pictures of the velocity fields temporary at my homepage. http://www.tfd.chalmers.se/~md8hemra/foamcase.html In case anybody could have a look or/and a tip, it would be very appreciated! For boundary conditions I have (inlet at top): U=(0,0.1,0), grad(p)=0 (outlet at bottom): grad(U)=0, p=0 (front and back walls): type empty (side walls): noslip for u, grad(p)=0; The cells are a bit skew, but this should be taken care of by Foam as far as I can tell! With best regards. Rasmus Hemph (fvSchemes and fvSolution shown below) fvSchemes ddtSchemes { default CrankNicholson; } gradSchemes { default Gauss linear; } divSchemes { default none; div(U) Gauss linear; div(phi,U) Gauss Gamma2V 1; } laplacianSchemes { default none; aplacian(1A(U),p) Gauss linear corrected; laplacian(nu,U) Gauss; } interpolationSchemes { default linear; interpolate(HbyA) Gauss linear corrected; } snGradSchemes { default corrected; } fluxRequired { default no; p; } solvers { p ICCG 1e6 0.0; U BICCG 1e5 0.0; } PISO { nCorrectors 6; nNonOrthogonalCorrectors 2; } 

November 17, 2005, 19:10 
Hello,
actually the case does

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hello,
actually the case doesn't work in OpenFOAM 1.2. I solved it using your BCs and your grid but I don't have the problems you noticed. I replaced Gamma2V with limitedLinearV 1 in div schemes for div(phi,U). I emailed you the case. Results are here:
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 18, 2005, 11:02 
Thanks alot for your help Albe

#3 
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 9 
Thanks alot for your help Alberto! With your assistance, I have traced the problems to the time step size. Going below 1e3 seconds causes unstability and unphysical solutions. I have tried with all time schemes (Euler, CrankNicholson, backward) available in OpenFOAM, but see the same behaviour for all schemes. I post the results for three timesteps after three seconds of simulation time.
I am more accustomed to the opposite problem, that the timestep is to large! However, I wanted to lower the timestep, (to 1e6s) which is the timescale of particle collisions which I want to couple to the fluid flow. Is there a scheme or solver more suitable for smaller time steps? 1e2 seconds Euler 1e3 seconds Euler 1e4 seconds Euler 

November 18, 2005, 11:20 
Thanks alot for your help Albe

#4 
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 9 
Thanks alot for your help Alberto! With your assistance, I have traced the problems to the time step size. Going below 1e3 seconds causes unstability and unphysical solutions. I have tried with all time schemes (Euler, CrankNicholson, backward) available in OpenFOAM, but see the same behaviour for all schemes. I post the results for three timesteps after three seconds of simulation time.
I am more accustomed to the opposite problem, that the timestep is to large! However, I wanted to lower the timestep, (to 1e6s) which is the timescale of particle collisions which I want to couple to the fluid flow. Lowering the tolerances of the linear solvers to below 1e10 has not helped. Is there a scheme or solver more suitable for smaller time steps? 1e2 seconds Euler 1e3 seconds Euler 1e4 seconds Euler 

November 18, 2005, 17:00 
I have the same problem using

#5 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
I have the same problem using a time step of 10^6 s.
Why do you use such a coarse grid? Your domain is 30x50cm, so your rectangular cells are about 6x2.7cm, so the order of magnitude of the cell Peclet number is: Pé = u*DX_max/nu = 0.1 m/s * 0.06 / 1.589e05 = 377 In these conditions, the linear (central difference) scheme is unstable, so you have to switch to something different for convection. If you want to use the linear method you should have Pé < 2 at each cell. What seems strange to me is that I have the same problem using upwind too. Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 22, 2005, 11:17 
You are right, I of course sho

#6 
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 9 
You are right, I of course should have used an upwind biased scheme. The grid is so coarse due to the inclusion of particles. I have played some more with Fluent, and can not reproduce any of the strange flow I see in OpenFOAM: even with all 2nd order schemes and very small timesteps (1e6s) I get the expected result. For now I will decouple the time step of the particles from that of the fluid and solve NavierStokes on a larger time scale. It is not ideal however, and I hope to eventually locate the reason for this behaviour. Anyhow, thanks again for your help!


December 16, 2005, 15:27 
Dear all,
I have the same q

#7 
Senior Member
Guoxiang
Join Date: Mar 2009
Posts: 109
Rep Power: 9 
Dear all,
I have the same question. Another, I want to change the value of X, Y and Z of U to simulate like particle. Could you please give some advice? Thank you very much, Guoxiang 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Density in icoFoam Densidad en icoFoam  manuel  OpenFOAM Running, Solving & CFD  8  September 22, 2010 04:10 
Not getting results from icoFoam  claws  OpenFOAM Installation  7  September 16, 2008 22:06 
Curious???  Will Hero  CDadapco  0  March 21, 2005 06:04 
Just Curious??  Will Hero  CDadapco  0  March 21, 2005 06:01 
A very curious beginner  Sudip Kumar ghosh  Main CFD Forum  7  September 13, 1998 11:28 