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

Courant Number become bigger and bigger!!!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 16, 2009, 05:22
Default
  #21
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Hi,

I used sonicFoam for solving the flow through a nozzle. I encountered the same problem of diverging Courant number after a few iterations.

Changing the numerical scheme for the divergence terms did solve the problem. After some time, I found that my specific heat capacity (c_v) was specified incorrectly. When I changed c_v from 1.78571 to 717.51 and started the iteration process, the Courant number did also diverge, however it is stable over many time step before it suddenly diverges.

Can anyone explain this to me?
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0

Last edited by Julian K.; June 16, 2009 at 09:17.
Julian K. is offline   Reply With Quote

Old   June 16, 2009, 16:41
Default
  #22
Member
 
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 8
joern is on a distinguished road
did you just change Cv and nothing else?

if you just set up Cv and don't change R and U, then you get a completely different case.

with Cv the speed of sound is defined as:
c=sqr(R*p/rho*Cv + p/rho)

if you just change Cv, you change c.

check all other variables, possibly there is a problem.
joern is offline   Reply With Quote

Old   June 17, 2009, 08:49
Default
  #23
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
I changed the Cv value, only. Now, I'm sure that I defined R and Cv correctly.

After some investigation of the flow, I encountered another possible source for the diverging Courant-number. The following happens:

I'm simulating a supersonic convergent-divergent nozzle. There is a shock in the divergent part of the nozzle causing the boundary layer to separate, which creates a vortice. This vortice is transported towards the outlet. When it hit the outlet, there is a sudden and dramatic increase in velocity in this region, which is pointing into the nozzle. Thus the Courant-number increases.
I'm quiet sure that this increase in velocity is artificial. I suppose, it occurs because of reversed flow due to the vortice. The BC at the outlet obivously does not let the vortice pass. I already used the 'totalPressure' BC and a 'fixedValue' BC for the outlet, however, the effect occurs for both types.

Can anyone suggest a BC which is more appropriate?
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   June 17, 2009, 09:11
Default
  #24
Member
 
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 8
joern is on a distinguished road
ok, i never used 'totalpressure', but 'fixedValue' is wrong.

for mu=0 the sonicFoam solver solves the Euler-Equations.
These Equations have the eigenvalues v-c, v and v+c.
For a supersonic flow all these eigenvalues are >0 so error shocks run all in your flow-direction.

So have to set 3 fixedValues at inlet and no value at the outlet.
try 'zeroGradient' at the outlet.
joern is offline   Reply With Quote

Old   June 23, 2009, 11:18
Default
  #25
New Member
 
Join Date: Jun 2009
Posts: 8
Rep Power: 8
statesman is on a distinguished road
ok here is my update which i also posted in another thread :

Hey ive been following this discussion

I am trying to model barrell shocks in an axisymmetric model. Inlet air is M=1. The exit is a subsonic outlet.

I am using rhoSonicFoam [modified to read p , rho, T, U fields , so that the solver can accept derived BCs ] , Im using non-reflective BCs at the exit for rho, since for subsonic outlet , the eigenvalue correspding to rho is -ve. However i am not getting the inlet BCs correct .


I ll summarize the Bc i have tried :--

p
Inlet : totalPressure outlet : fixedValue [ static]

rho
inlet: fixedValue outlet : nonReflective.

U
inlet : 350 outlet : zeroGradient

T
Inlet : 250 outlet : zerogradient

U & T are fine..
kindly suggest me a better combination ....
statesman is offline   Reply With Quote

Old   July 7, 2009, 04:34
Default
  #26
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
I used the BC 'waveTransmissive' in order to have a non-reflecting BC. Find more infos here: http://www.openfoamwiki.net/index.ph...dary_condition

and here:

Pressure Inlet Velocity
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   July 7, 2009, 10:04
Default
  #27
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
hey thank you ..

ok , they have said that the "waveTransmissive" BC is more general , but just for confirmation . can it be used for U & p [subsonic outlet ] both ???
mihir1310 is offline   Reply With Quote

Old   July 7, 2009, 10:42
Default
  #28
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Quote:
can it be used for U & p [subsonic outlet ] both ???
You can use is for U, as well as for p. You have to set the 'field' variable in the definition of the outlet, accordingly:

Code:
outflow
{
type waveTransmissive;
[...]
field U; //the name of the field that we are working on; here you put p or U for pressure or velocity, respectively [...]
}
I don't know how adequate this BC is for subsonic outlets. All I know is that it simulates a farfield. This way, waves should be transmitted and not reflected.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   July 7, 2009, 10:47
Default
  #29
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
hey thanx..
Quote:
U
inlet
{
type fixedValue;
value uniform (350 0 0);
}
outlet
{
type waveTransmissive;
field U;
phi phiv;
rho rho;
psi psi;
gamma 1.4;
lInf 0.05;
fieldInf (10 0 0 );
value uniform (10 0 0 );
}
Quote:
p
inlet
{
type fixedValue;
value uniform 52800;
}
outlet
{
type waveTransmissive;
field p;
phi phi;
rho rho;
psi psi;
gamma 1.4;
lInf 0.05;
fieldInf 2400;
value uniform 2400;
}
t
inlet fixed
outlet zeroGradient

these r my BC .are they correct ? . ill proceed with my new simulation & see where it leads me
mihir1310 is offline   Reply With Quote

Old   July 13, 2009, 04:41
Default
  #30
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Well, I think your BCs are correctly defined. Let me know if your results are okay.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   July 28, 2009, 17:00
Default CFL criterion
  #31
New Member
 
Barath Ezhilan
Join Date: Jun 2009
Posts: 20
Rep Power: 8
barath.ezhilan is on a distinguished road
I am currently simulating vortex breakdown in a conical diffuser and am doing unsteady simulations using transientSimpleFoam and LAunderGibsonRSTM model.

I have a doubt. The generally suggested criteria that CFL<1, is it the Courant Number mean value or the max courant number value???

I have a mean Courant Number of close to 0.13 and Maximum Courant Number of close to 7.

(Courant Number mean: 0.130184 max: 7.10512 velocity magnitude: 3.59437)

And I am able to capture the vortex. (URANS using conventional k-e and k-w models dont work!!!!)

Is it the correct solution that I have got or is the solution unphysical as the CFL condition states??

Quote:
Originally Posted by joern View Post
if the coNum gets bigger and bigger it has nothing to do with variable timestepping.

if the solver isnt stable with very low deltaT then it wouldn't be stable for variable timestepping, either. CoNum is just a nessesary condition for stability.
the icoFoam solver is just a simple solver for incompressible N-S-Equations with a PISO correction.
For most FV solvers it is enough if you use a CoNum of <0.5 . The CoNum is U*deltaT/deltaX. I dont know the maximum of U in the N-S Equations but for the Euler Equations (rhoSonic) this is U+c, cause this is an eigenvalue of this system and so its a speed of error waves for this equations.
if you know the maximum speed of error waves, you can set your CoNum small enough and you have the nessesary condition for stability.

if the solver is still not stable, then its not a problem of the CoNum. then its a problem of your BC or of your schemes.

For example: if you use a linear scheme for the div term in rhoSonic then your solver will diverge no matter what you do. Even for deltaT=1e-100 it will crash cause it is an unbounded scheme what isnt stable for these kind of equations.
so try some more stable schemes like upwind or minmod.
barath.ezhilan is offline   Reply With Quote

Old   August 6, 2009, 12:40
Default
  #32
New Member
 
Join Date: Jun 2009
Posts: 8
Rep Power: 8
statesman is on a distinguished road
Quote:
Originally Posted by Julian K. View Post
Well, I think your BCs are correctly defined. Let me know if your results are okay.

Code:
p

boundaryField
{
    inlet           
    {
         type totalPressure; 
      p0 uniform 1.0135e5; 
         U U; 
      phi phi; 
      rho none; 
      psi none; 
      gamma 1.4; 
     // value uniform 12780.45;     
    }

    outlet          
    {
        type            waveTransmissive;
        value           uniform 1000;
     field           U;
        gamma           1.4;
     phi             phi;
        rho             rho;
        psi             psi;
        lInf            0.5;
        fieldInf        1000;
        
        
    }

U

internalField   uniform (260.39 0 0);

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform (700 0 0);
    }

    outlet          
    {
        //type            zeroGradient;
    type            waveTransmissive;
        value           uniform (10 0 0 );
     field           U;
        gamma           1.4;
     phi             phi;
        rho             rho;
        psi             psi;
        lInf            0.5;
        fieldInf        (10 0 0 );
        
        

    }
So you know im trying to simulate barrel shock & mach disc in a free underexpanded jet . These BCs are a much better improvement over the previous results . However , the reflections arent completely eliminated , just damped. So for initial runtimes the results are very satisfactory , with very sharp shockfronts, & satisfactory comparison with literature data. However, as time progresses , the reflections still prevail. If you want i can post some results, [just tell me how to ] . FOr now im pasting the fluxes across the each boundary field which may give a clue as to whats going on :--
Code:
Mass flux at axis = 0
Mass flux at back = -0.000445458
Mass flux at front = 0.000445456
Mass flux at frontAndBackPlanes = 0
Mass flux at inlet = -0.000497143
Mass flux at outlet = 0.000572761
Mass flux at wall = 0
Time = 0.019552 Net mass flux = 7.56164e-05

Time = 0.0195521
P.S. I ve been playing around with the lInf value ... varying it by an order of a decimal
statesman is offline   Reply With Quote

Old   August 18, 2009, 05:36
Default
  #33
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Dear Statesman,

for my simulations (critical CD-nozzle) I'm using the 'rhoCentralFoam' solver. I read, that it should be more precise than the other incompressible solvers http://openfoamwiki.net/index.php/TestLucaG

Maybe, this will help.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   September 10, 2009, 06:09
Default
  #34
New Member
 
Join Date: Sep 2009
Posts: 4
Rep Power: 7
sandrak is on a distinguished road
I'm currently using the rhoSonicFoam solver (OpenFoam 1.6) and my Courant number is exploding as well, although I'm sure my bc are correct, since my case is very similar to the forewardStep tutorial.
Therefore I went back to the forewardStep tutorial and changed the mesh. I just moved the vertice of the obstacle corner a little right (from (0.6 0.2 z) to (1 0.2 z)). But even with this small change the courant number explodes after a while. Since the changing of the mesh causes some cells to be deformed and some getting a bit smaller I decreased the time step to 0.001 (from 0.002). But it didn't help.

For me rhoSonicFoam only worked for the turorial cases. What can I do?
sandrak is offline   Reply With Quote

Old   September 10, 2009, 08:24
Default
  #35
Member
 
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 8
joern is on a distinguished road
sandrak, plese give some more info.

what are your BCs?
what is your U?
how is your start CoNum?
what are your initial values?
what schemes do you use?

1. rhoSonic is just stable for Ma>2. If you use a lower Ma, you need a far smaller timestep.

2. you have to use bounded schemes for div. rhoSonic solves the Euler Equations, they are convection dominated and if the convection is not bounded, the solver is unstable.
joern is offline   Reply With Quote

Old   September 10, 2009, 08:30
Default
  #36
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Hi Sandrak,

maybe you should try to use 'rhoCentralFoam'. According to the literature I gave in my last post, this solvers is more accurate than 'rhoSonicFoam'. Furthermore, from my point of view it seems to be even more stable, as well, at least in my case.

Generally, my problem is that pressure waves are not transmitted across the output. They are reflected, even tough, I use the 'waveTransmissive' BC for p at the outlet (I am currently testing different values for lInf, so maybe I will get better results in some time). With 'rhoSonicFoam' my simulations always crashed after the pressure wave has been reflected. With 'rhoCentralFoam' the pressure wave is reflected as well, however, the simulation does not crash. It's just that the pressure wave will travel towards the inlet of my nozzle. Thus, I suppose that 'rhoCentralFoam' is more stable. Furthermore, the shock is resolved more distinct with 'rhoCentralFoam' than with 'rhoSonicFoam'.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0
Julian K. is offline   Reply With Quote

Old   September 10, 2009, 10:49
Default
  #37
Member
 
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 8
mihir1310 is on a distinguished road
Sandrack

So you are where each of us [ me , Julian , Joern] was a few months ago..

Please post your BCs that you are applying so that we can know better what you are actually doing.
  • So yes the problem you are facing is more than just of timesteps. As Julian said , study the Eigenstructure of the Euler equations for inviscid flow & you shall understand what he means by ""pressure waves are not transmitted across the output""about & how that affects the BCs . You may need nonReflective boundary conditions & rhoSonic isnt the best code for application of these. Try sonicFoam which applies waveTransmissive [which is a non-reflective BC] .
  • & Yes you need bounded schemes , for divSchemes. try the TVD family of schemes to know which one is best suited for your case . You may wanna read how TVD schemes behave w.r.t. shock-resolution.

Just read CFD texts to understand the above mentioned items


Julian
I ve been using sonicFoam with Minmod schemes for divSchemes. & backward for ddtSchemes. SO far I'm very happy in terms of both stability & results.
However would you mind sharing with me the boundary conditions of rhoCentralFoam ? I used the same as i posted earlier , but my code wouldn't run.
mihir1310 is offline   Reply With Quote

Old   September 11, 2009, 05:29
Default
  #38
Member
 
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 8
Julian K. is on a distinguished road
Thanks for the last post Mihir, you have stated the problem quite well.
Here are my boundary conditions I use for my simulation and a brief explanation of what I am doing:

My domain is 2D, axi-Symmetric and consists of a CD noozle,only. That means, I do not have a far field before or after the nozzle. That's probably why I get problems with the outlet BC, because, if I had a far field, the pressure waves could leave the outlet and due to increasing cell size, the waves would be damped, so that at the farfield outlet, there would be a weak BC interaction, only. Anyway, I induce the flow with a pressure difference at dp=300mbar. At the inlet I have atmospheric pressure and thus at the outlet the low pressure.
I am using rhoCentralFoam.
I have uploaded a little video of the pressure contours:http://www.youtube.com/watch?v=-hhriqus2-8

The BCs are:

p
Code:
dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 101325;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 101325;
    }
    outlet
    {
        type            waveTransmissive;
        phi             phi;
        rho             rho;
        psi             psi;
        gamma           1.4;
        fieldInf        71325;
        lInf            0.05;// I have increased this value from 0.05 to 500 now, without noticing any difference.
        value           uniform 71325;
    }
    wall
    {
        type            zeroGradient;
    }
    symmetry
    {
        type            empty;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
    frontAndBackPlanes_pos
    {
        type            wedge;
    }
    frontAndBackPlanes_neg
    {
        type            wedge;
    }
}
U
Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
    }
    wall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    symmetry
    {
        type            empty;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
    frontAndBackPlanes_pos
    {
        type            wedge;
    }
    frontAndBackPlanes_neg
    {
        type            wedge;
    }
}
T
Code:
dimensions      [0 0 0 1 0 0 0];

internalField   uniform 293.14;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 293.14;
    }
    outlet
    {
        type            zeroGradient;
    }
    wall
    {
        type            zeroGradient;
    }
    symmetry
    {
        type            empty;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
    frontAndBackPlanes_pos
    {
        type            wedge;
    }
    frontAndBackPlanes_neg
    {
        type            wedge;
    }
}
fvSchemes
Code:
//fluxScheme Tadmor; // KT
fluxScheme Kurganov; // KNP

ddtSchemes
{
    default            CrankNicholson 1; //Euler;
}

gradSchemes
{
    default           Gauss linear;
}

divSchemes
{
    default        none;
    div(tauMC)        Gauss linear;
}

laplacianSchemes
{
    default            Gauss linear corrected;
}

interpolationSchemes
{
    default              linear;
    reconstruct(rho)     vanLeer; 
    reconstruct(U)       vanLeerV;
    reconstruct(T)       vanLeer;
//    reconstruct(rho)     upwind; 
//    reconstruct(U)       upwind;
//    reconstruct(T)       upwind;
}

snGradSchemes
{
    default             corrected;
}
fvSolution
Code:
solvers
{
    rho  diagonal {};
    rhoU diagonal {};
    rhoE diagonal {};

    U smoothSolver
    {
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-09;
        relTol           0.01;
    };

    h smoothSolver
    {
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-10
        relTol           0;
    };
}
Do you have any suggestions? Especially, for the settings in the fvSchemes and fvSolutions.
If you need more information, let me know.

Mihir, could you also post your fvSchemes? I'd be very interested. Maybe also you rBC setup for P U and T. Thanks.
__________________
grid generation: ICEM CFD 13.0
solver: CFX 13.0

Last edited by Julian K.; September 11, 2009 at 05:47.
Julian K. is offline   Reply With Quote

Old   September 11, 2009, 05:54
Default
  #39
New Member
 
Join Date: Sep 2009
Posts: 4
Rep Power: 7
sandrak is on a distinguished road
Thanks for your replies, they helped. As I said, my case is very similar to the forewardStep case, just a slightly different mesh.
U: inlet fixedValue: (2 0 0), outlet: zeroGradient, wall/obstacle: fixedValue (0 0 0), top: symmetryPlane
p: inlet fixedValue: 1, outlet: zeroGradient, wall/obstacle: zeroGradient, top: symmetryPlane

The shock waves were a really good hint. In my case a pressure wave was reflected at the obstacle and travelled back to my inlet, where I had stated a constant pressure of 1. It happend that a region of very high pressure and very low pressure were at a small distance and thus I got very high velocity behind my inlet and that was, what caused the crash.
After I changed the p bc at the inlet to zeroGradient as well, the program runs stable, even when I change the velocity at the inlet to Mach smaller than 2.

So thanks. I understand the problem much more now.
sandrak is offline   Reply With Quote

Old   September 11, 2009, 06:20
Default
  #40
Member
 
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 8
joern is on a distinguished road
sandrak,

what you discribe is a problem of rhosonicfoam. the solver is a "direct" solver for the decoupled euler-equations. if you use Ma 2 as speed the shockwaves all point into your domain, thats ok.
but the speed is not fast enough to transport reflected shockwaves. if you use Ma 3 it should work.

the real problem is, that the decoupled equations produce an error in U. If the speed is fast enough the solve of the mass equation (for rho) corrects this error.
if the speed is slower this error is not corrected. An solution for that gives the sonicFoam solver. This solver does an pressure-correction (PISO) to correct U and p. there you should be able to use all Ma speeds correct with a possible CoNum of ~1. (The BCs have to be set right)
For sonicFoam make shure that you do outer an inner corrections (fvSolution-PISOControls). If one of them is 0 you never solve the pressure equation and do no correction.
joern 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
CFL number Daniele CFX 5 July 19, 2012 19:11
Number of interation? Tu Phoenics 1 September 28, 2008 14:12
How to get the Global Node Number by UDF : Fluent Yusuke FLUENT 0 October 8, 2007 17:37
SOS! HELP! max number of cells :( Jas Phoenics 4 February 14, 2004 11:12
Boundary region number limitation Pablo Barreiro CD-adapco 1 May 2, 2001 11:13


All times are GMT -4. The time now is 11:27.