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

IcoFoam unstability, courant number gets large!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2010, 13:11
Default IcoFoam unstability, courant number gets large!
  #1
New Member
 
vivien
Join Date: Mar 2009
Posts: 18
Rep Power: 8
vivien is on a distinguished road
Hi, everyone,

I am trying to run a icoFoam with a big mesh. the mesh contains very small elements. I have run the checkMesh and it shows to be ok. I start the simulation with very small time steps(10-7) and it gives a courant number about 0.02. But after a certain interations, the courant number start to increase and the simulation becomes unstable, can somebody give me suggestions?

Many Thanks!

Vivien

FVscheme
ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss upwind;
}

laplacianSchemes
{
default none;
laplacian(nu,U) Gauss linear limited 0.7;
laplacian((1|A(U)),p) Gauss linear limited 1.0;
}

interpolationSchemes
{
default linear;
interpolate(HbyA) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

FVsolution

solvers
{
p ICCG 1e-06 0;
U BICCG 1e-05 0;
}

PISO
{
momentumPredictor yes;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

CheckMesh

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 1412976
faces: 15410430
internal faces: 14837762
cells: 7562048
boundary patches: 4
point zones: 0
face zones: 1
cell zones: 1

Overall number of cells of each type:
hexahedra: 0
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 7562048
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
walls 103946 52781 ok (non-closed singly connected)
inlet 349 198 ok (non-closed singly connected)
outlet 460 256 ok (non-closed singly connected)
walls 467913 234323 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.066982359 -0.047683548 1.6543907) (-0.019686867 0.037543221 1.6653831)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (1.1197576e-17 -1.7322355e-17 1.4746822e-16) OK.
Max cell openness = 2.7923378e-16 OK.
Max aspect ratio = 5.5543271 OK.
Minumum face area = 6.476086e-12. Maximum face area = 9.1024527e-08. Face area magnitudes OK.
Min volume = 1.1082091e-17. Max volume = 6.4997273e-12. Total volume = 1.9463392e-06. Cell volumes OK.
Mesh non-orthogonality Max: 66.920089 average: 14.782049
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.71939697 OK.

Mesh OK.
vivien is offline   Reply With Quote

Old   June 18, 2010, 10:26
Default
  #2
Member
 
toto
Join Date: Jun 2009
Posts: 71
Rep Power: 8
ronaldo is on a distinguished road
you need relaxation factor. Let me know, if it doesnt woork
ronaldo is offline   Reply With Quote

Old   June 18, 2010, 10:31
Default
  #3
New Member
 
vivien
Join Date: Mar 2009
Posts: 18
Rep Power: 8
vivien is on a distinguished road
I thought I can not put a relaxation factor in transient simulation? Correct me if I am wrong...

Thanks!

Vivien
vivien is offline   Reply With Quote

Old   June 18, 2010, 10:53
Default
  #4
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
Quote:
Originally Posted by vivien View Post
I thought I can not put a relaxation factor in transient simulation? Correct me if I am wrong...

Thanks!

Vivien
You are correct. You should not relax using icoFoam, but this doesn't mean you cannot use under-relaxation in unsteady solvers. You can in pimpleFoam.

Since you use a fully tetrahedral mesh, you might want to use limited schemes for the gradients, and perform some non-orthogonal corrector step (your mesh is borderline, with max non-orthogonality ~ 66).

P.S. What version of OpenFOAM are you using?

Best,
__________________
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   June 18, 2010, 11:07
Default
  #5
Member
 
toto
Join Date: Jun 2009
Posts: 71
Rep Power: 8
ronaldo is on a distinguished road
I am using OpenFOAM 1.5
ronaldo is offline   Reply With Quote

Old   June 18, 2010, 11:51
Default
  #6
New Member
 
Christian
Join Date: Feb 2010
Location: Payerne, Switzerland
Posts: 9
Rep Power: 7
cves is on a distinguished road
Hello,

I got approximately the same problem and you can fix it as Alberto propose by using pimpleFoam or transientSimpleFoam with relaxation. However the problem will remain if the time step that you use is too big. Indeed your flow will not be converged at each time step... I am still trying to find something in order to run large time step in unsteady simulation.

Best regards

Christian
cves is offline   Reply With Quote

Old   June 18, 2010, 12:38
Default larger time steps
  #7
Senior Member
 
Christian Lucas
Join Date: Aug 2009
Location: Braunschweig, Germany
Posts: 198
Rep Power: 8
Chris Lucas is on a distinguished road
Hi Christian,

one way to run a transient simulation with larger time steps can be achieved by including an additional loop in the solver, e.g. interFoam.

In interFoam, this loop has to be constructed in a way, that it includes the pressure and the velocity equation. Additionally, you must include relaxation within the loop by using the "storePrevIter" function before the calculation of the p and u equation and the "relax" function has to be used afterwards.


However, I am not sure if including this additional loop will result in other problems with the solver.

Regards,
Christian
Chris Lucas is offline   Reply With Quote

Old   June 18, 2010, 14:46
Default
  #8
New Member
 
Christian
Join Date: Feb 2010
Location: Payerne, Switzerland
Posts: 9
Rep Power: 7
cves is on a distinguished road
Hi Chris Lucas,

Thank for the post, I will take a look at the code of interFoam. But in fact, I should give you more informations about my case.

I have modified the pimple solver:
- Time loop: increase time step and apply dynamic mesh motion.
- Pimple loop: Solve the U equations, apply under-relaxation and correct turbulence.
- Piso loop: Store previous pressure, solve pressure equation and apply under-relaxation.

I should also mention that I can reached convergence with bigger time step by increasing the number of pimple loops. However, in this case I have no significant improvement in computational time compare to the small time steps. As my mesh is between 10 and 25 millions of cells, I have to take care about the time of my simulations.

Best regards,

Christian
cves is offline   Reply With Quote

Old   October 7, 2010, 03:25
Default PimpleFoam for TubDyM solver in OF 1.5-dev
  #9
Member
 
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 7
aldo.iannetti is on a distinguished road
Hi,
Is there someone who wants tu debug and correct my pimpleFoam solver applied on turbulence and dynamic meshes solver?

Thanks
Attached Files
File Type: zip simpleTurbDyMFoam.zip (15.5 KB, 20 views)
aldo.iannetti is offline   Reply With Quote

Old   October 15, 2010, 15:09
Default
  #10
Member
 
s.rasoul_varedi
Join Date: Feb 2010
Posts: 82
Rep Power: 6
desert_1250 is an unknown quantity at this point
Send a message via Yahoo to desert_1250
hi all of foamers
i have one question, why when i use icoFoam for cylinder case stady (standard case in OF) for centimeter dimention & velosity mgnitude 1m/s at the left pach,this error " floating point exception (core dumped) " occurs and the simulation becames unstable ?
desert_1250 is offline   Reply With Quote

Old   July 23, 2013, 12:48
Question
  #11
Senior Member
 
Join Date: Nov 2012
Posts: 168
Rep Power: 4
hz283 is on a distinguished road
Hi All,

Now I have the same problems. If the parameter nOuterCorrectors is set to be 1 in transient time marching, then is it still meaningful to use the velocity and pressure under-relaxation factors? Because in this case, there are not outer iteration steps.


Quote:
Originally Posted by cves View Post
Hi Chris Lucas,

Thank for the post, I will take a look at the code of interFoam. But in fact, I should give you more informations about my case.

I have modified the pimple solver:
- Time loop: increase time step and apply dynamic mesh motion.
- Pimple loop: Solve the U equations, apply under-relaxation and correct turbulence.
- Piso loop: Store previous pressure, solve pressure equation and apply under-relaxation.

I should also mention that I can reached convergence with bigger time step by increasing the number of pimple loops. However, in this case I have no significant improvement in computational time compare to the small time steps. As my mesh is between 10 and 25 millions of cells, I have to take care about the time of my simulations.

Best regards,

Christian
hz283 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
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
RMS Courant Number vs MAX Courant Number zoozoozoo Main CFD Forum 3 June 12, 2012 13:44
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
Courant number msrinath80 OpenFOAM Running, Solving & CFD 1 May 29, 2006 17:20


All times are GMT -4. The time now is 10:54.