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

Curious results in icoFoam differ from fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 17, 2005, 10:30
Default I am running time-dependent ic
  #1
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
I am running time-dependent icoFoam on a simple 2D funnel-like 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 cell-values. 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 pressure-velocity-interpolation error, but I took the fvSchemes from the elbow-tutorial 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(1|A(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 1e-6 0.0;
U BICCG 1e-5 0.0;
}

PISO
{
nCorrectors 6;
nNonOrthogonalCorrectors 2;
}
hemph is offline   Reply With Quote

Old   November 17, 2005, 19:10
Default Hello, actually the case does
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 18, 2005, 11:02
Default Thanks alot for your help Albe
  #3
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
Thanks alot for your help Alberto! With your assistance, I have traced the problems to the time step size. Going below 1e-3 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 1e-6s) 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?

1e-2 seconds Euler
1e-3 seconds Euler
1e-4 seconds Euler
hemph is offline   Reply With Quote

Old   November 18, 2005, 11:20
Default Thanks alot for your help Albe
  #4
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
Thanks alot for your help Alberto! With your assistance, I have traced the problems to the time step size. Going below 1e-3 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 1e-6s) 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 1e-10 has not helped.

Is there a scheme or solver more suitable for smaller time steps?

1e-2 seconds Euler
1e-3 seconds Euler
1e-4 seconds Euler
hemph is offline   Reply With Quote

Old   November 18, 2005, 17:00
Default I have the same problem using
  #5
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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 / 1.589e-05 = 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 live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 22, 2005, 11:17
Default You are right, I of course sho
  #6
Senior Member
 
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 8
hemph is on a distinguished road
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 (1e-6s) I get the expected result. For now I will decouple the time step of the particles from that of the fluid and solve Navier-Stokes 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!
hemph is offline   Reply With Quote

Old   December 16, 2005, 15:27
Default Dear all, I have the same q
  #7
Senior Member
 
Guoxiang
Join Date: Mar 2009
Posts: 109
Rep Power: 8
liugx212 is on a distinguished road
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
liugx212 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
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 CD-adapco 0 March 21, 2005 06:04
Just Curious?? Will Hero CD-adapco 0 March 21, 2005 06:01
A very curious beginner Sudip Kumar ghosh Main CFD Forum 7 September 13, 1998 11:28


All times are GMT -4. The time now is 16:32.