[wididid]

Hello,

I have been simulating a rocket thrusting into oncoming flow using rhoCentralFoam. I have been trying to use the max courant number setting in controlDict to cap the time steps. This has previously been working fine by having the simulation run at the largest time step for the courant number. However, after some time, the simulation drops to a very small courant number and time step causing the simulation to make almost no progress. For now I have simply fixed the deltaT to allow the simulation to continue, but what is the reason for this drop in courant number after a while of simulation?

Thank you

[alexvaleije]

Hi there,

Since the Courant number depends on:

1º velocity
2º cell size
3º time step

it is very likely that u have some cells with a very high velocity value. Due to that, the code lowers the time step to adjust it to the maximum Courant number that you have previuosly set.

I hope that info could help u,

Alex

[wididid]

Thank you for the reply.

The maximum courant number that I have specified is .5. After running at this courant number for a while, the courant number drops to a very low number, something like 1e-17(Order may be wrong, but it is still a small number). If this is because the simulation is detecting that velocity and the cell size require a very small courant number to proceed, is there a fix I can apply to my problem?

[nandhakumar]

Hello

1. Try to change your mesh sizes that is alter your mesh size as per velocity. At high velocity region dont use very fine mesh. Actually reduction in time step indicates solution blow up(apparently i think). So try running in pimpleFoam with high value of nOuterCorrectors like 50-100.


2. Try to initialize proper boundary condition, like k and epsilon value if it is a turbulent model.


3. Try to use lower order schemes for divergence (i.e bounded gauss upwind).


update the results




Thank you

[alexvaleije]

Originally Posted by nandhakumar

Hello

1. Try to change your mesh sizes that is alter your mesh size as per velocity. At high velocity region dont use very fine mesh. Actually reduction in time step indicates solution blow up(apparently i think). So try running in pimpleFoam with high value of nOuterCorrectors like 50-100.


2. Try to initialize proper boundary condition, like k and epsilon value if it is a turbulent model.


3. Try to use lower order schemes for divergence (i.e bounded gauss upwind).


update the results




Thank you

In addition to this, another thing you can do is checking where your high Courant number values are very high. This can be done with "postProcess -func CourantNo -time XXXX".

With this you can check with paraview where this is happening, and if it is only a small zone or if it is a general thing. In case it is only a small, non important zone, you could try to fix the time step value instead of setting it according to the maximum Courant value.


Alex

[wididid]

I tried running "postProcess -func CourantNo" (I wasn't sure what to put in "XXXX". Is this for specifying a single time step?) and it failed to execute because "CourantNO cannot find required object phi of type surfaceScalarField". What is the issue here?

Thanks

[alexvaleije]

Originally Posted by wididid

I tried running "postProcess -func CourantNo" (I wasn't sure what to put in "XXXX". Is this for specifying a single time step?) and it failed to execute because "CourantNO cannot find required object phi of type surfaceScalarField". What is the issue here?

Thanks

I've just checked your problem and u are completely right. This is because the solver "rhoCentralFoam" doesn't write the field "phi", although, of course, it is needed to calculate the solution.

If you still want to do this, the easiest way to go is modyfing the solver, making a small change in the createFields.H to make phi writable. In OF 4.1 the line which defines phi is this:

surfaceScalarField phi("phi", fvc::flux(rhoU));

You'd have to comment it and put something like this instead

volScalarField phi
(
IOobject
(
"phi",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
fvc::flux(rhoU)
);

Also, you would havce to compile it under a new name and all that, I don't know if you know how to do that. There's a lot of info of how to do that, but if u are not quite sure, come over here again.

Once the field phi is calculated and written in the temporal folders, you should be able of postprocessig the Courant.


PS: the XXX refers to the name of the folder you want to postpro. If you don't specify a value, the function will calculate it for all of them

Example:

postProcess -func CourantNo -time 25.1 (this will calculate for time 25.1)

postProcess -func CourantNo (this will calculate for all of them)


Alex

[atelcikti1]

Originally Posted by wididid

Hello,

I have been simulating a rocket thrusting into oncoming flow using rhoCentralFoam. I have been trying to use the max courant number setting in controlDict to cap the time steps. This has previously been working fine by having the simulation run at the largest time step for the courant number. However, after some time, the simulation drops to a very small courant number and time step causing the simulation to make almost no progress. For now I have simply fixed the deltaT to allow the simulation to continue, but what is the reason for this drop in courant number after a while of simulation?

Thank you

Hi wididid,

Could you solve this problem? I have similar issue. I checked the replies into this post, but they didnt help my problem. I am expecting large values of velocity in domain and i cant do anything about it. My time steps, courant number also decreases to 1e-13s which solution does not progress.

[peterhess]

Is it possible, that something else limits Co Number?

Which Di Number do you have?

Post one step of your log file.

Or try something like:

// Maximum diffusion number
maxDi 1000;

in your controlDict.

Or simply turn off the adjustTimeStep using:

adjustTimeStep no;

Regards

Peter

[atelcikti1]

Hi Peter,

I have tried constant time steps at 1e-8, but they didn't work at past. Now, i am trying your maxDi trick on control dict. It seems going well now, but i am not sure, solution needs some time.

What does that diffusion number mean? It seems obviously not physical mass/thermal diff number. I couldn't find any explanation on internet. Can you share some document or link?

[peterhess]

If it works, please confirm, so that others can use the suggestion.

You may use a finer mesh by the way, that could also help.

If not working, run checkMesh please and post the output, to see if your mesh is fine or not.

https://www.researchgate.net/post/Wh...rical-solution

Regards

Peter

[atelcikti1]

Originally Posted by peterhess

If it works, please confirm, so that others can use the suggestion.

You may use a finer mesh by the way, that could also help.

If not working, run checkMesh please and post the output, to see if your mesh is fine or not.

https://www.researchgate.net/post/Wh...rical-solution

Regards

Peter

Hi Peter,

I have tried and get the correct solution. I can confirm maxDi (limiting diffusion number) didn't help. Indeed, solution is very sensitive to initial conditions. So I patch the domain with inlet properties (total press, temperature, very low velocity, inlet species mol fractions etc.), then i get the solution and my timesteps didn't drop below 4e-8. However, obviously this method is not time accurate in terms of initial conditions.