[Armin.Sh]

Hi dear FOAMers,

I'm going to run a Lagrangian particle tracking after running a transient simulation for the continuous phase, which means the carrier flow velocity changes in each time step.

On the other hand, it seems that the current particle tracking in OpenFOAM has only been considered for the steady carrier flows (with fixed, i.e. "frozen" velocity). In other words, it reads the data from the start time and doesn't consider the changes of the continuous phase flow velocity in the next time steps.

I tried to solve this issue by entering the following part into the solver code:

Info<< "Reading field U\n" << endl;
    volVectorField U
    (
        IOobject
        (
          "U",
          runTime.timeName(),
          mesh,
          IOobject::MUST_READ,
          IOobject::NO_WRITE
        ),
        mesh
    );

It reads now the velocity in each time step, but apparently still doesn't apply it to the solving equations, because the results are as before. In conclusion, it seems that I should now change the code, where the velocity is applied to the particle tracking equations.

I'd like to know if somebody knows, how to overcome this issue or at least where the code containing main equations for the Lagrangian particle tracking is.

Thanks in advance!
Armin

[kuprat]

Hi, it looks like as of 2017 there was no capability of releasing particles into a time-dependent velocity field obtained by interpolation of pre-computed velocity field stored in multiple time directories.
https://bugs.openfoam.org/view.php?id=2681
Now it is 2019, has someone done this? I am working on deposition of particles in human respiratory tract where we can reasonably assume periodic breathing. If we could re-use velocity field over multiple breaths it would be perfect.

[Nomis]

Dear kuprat,



I am also interested in simulating droplet in a transient velocity field.

How did you solve the issue?


Greetings Simon

[kuprat]

Hi Simon,
After getting no response, I assumed no one had injected particles into a precomputed TRANSIENT velocity field. So I ended up using MPPICFoam which meant that I had to redundantly compute the velocity field over several periodic breaths and inject particles into the field. It's possible nobody has actually tried to inject into a precomputed transient velocity field because if the field varies on a fine time scale you would have to store a massive number of timesteps to limit time interpolation error. What I mean is that you may be used to outputting answers every 1.e-2 seconds which is ok for graphics, but if you want the particle tracking to be accurate you might want to interpolate pre-computed velocities every 1.e-3 seconds and it would take too much disk space to store that.
Andrew

[oswald]

Hi all,


I actually did use precomputed velocity fields in multiple time folders for a transient particle simulation. But you have to loop over the existing time folders and you have to read in the new/changed fields for every time step.


oswald

[Nomis]

Hi Andrew, thanks for the quick reply.

[oswald]

Hi Simon,


just in case you missed it as we were writing at almost the same time: Lagrangian particle tracking with a transient carrier flow


oswald

[reidwill]

Hi all,

I was wondering if anyone has successfully done this?

I am currently trying to complete this with a looping transient U field which correlates to a rotational MRF motion in my model.

I currently have the "volVectorField U" being pulled each timestep similar to Armin's initial post but the solver still seems to be ignoring this and continuing to use the initial U field in createFields.H.

Oswald could you possibly go into more detail about how you achieved it?

Cheers,
Reid

[joshwilliams]

Hi Reid,


If I understand correctly, I have had this problem before and solved it as follows. To read a pre-computed velocity field at each timestep, one must modify the solver to read the pre-computed field and load this as a different variable name (say you declare the variable "U" in createFields, you set a variable "newU" at each time step). Then U = newU, should work.

// get header file for pre-computed velocity
IOobject newUHeader
(
 "U",
 runTime.timeName(),
 mesh,
 IOobject::MUST_READ,
 IOobject::NO_WRITE
);


// check field exists
if (newUHeader.typeHeaderOk<volVectorField>(true))
{
    Info << "new U field found" << endl;
    volVectorField newU
    (
         newUHeader,
         mesh
    );
    // set velocity declared in createFields.H to the pre-computed velocity
    U = newU;
}

Hope this helps.
Best,
Josh

[oswald]

Hi Reid,


I think Josh's solution should do the trick? Have you tried it yet?

[joshwilliams]

There was a similar discussion here. The icoUncoupledKinematicParcelFoam solver is a good starting point for modification. If you just add the code given in my previous post, it should work.



Linking a velocity field to particles using icouncoupledKinematicParcelFoam