|
[Sponsors] |
Lagrangian particle tracking with a transient carrier flow |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 21, 2017, 13:38 |
Lagrangian particle tracking with a transient carrier flow
|
#1 |
New Member
Join Date: Dec 2016
Posts: 9
Rep Power: 9 |
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: Code:
Info<< "Reading field U\n" << endl; volVectorField U ( IOobject ( "U", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::NO_WRITE ), mesh ); 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 |
|
April 16, 2019, 01:05 |
Interpolation of carrier phase velocity time points
|
#2 |
New Member
Andrew Kuprat
Join Date: Jan 2016
Posts: 3
Rep Power: 10 |
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. |
|
October 21, 2020, 11:44 |
|
#3 |
New Member
Simon
Join Date: Jan 2014
Location: Freiburg, Germany
Posts: 15
Rep Power: 12 |
Dear kuprat,
I am also interested in simulating droplet in a transient velocity field. How did you solve the issue? Greetings Simon |
|
October 21, 2020, 18:24 |
Re: particles in precomputed velocity field
|
#4 |
New Member
Andrew Kuprat
Join Date: Jan 2016
Posts: 3
Rep Power: 10 |
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 |
|
October 22, 2020, 04:10 |
|
#5 |
Member
Join Date: Sep 2010
Location: Leipzig, Germany
Posts: 96
Rep Power: 16 |
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 |
|
October 22, 2020, 04:11 |
|
#6 |
New Member
Simon
Join Date: Jan 2014
Location: Freiburg, Germany
Posts: 15
Rep Power: 12 |
Hi Andrew, thanks for the quick reply.
|
|
October 23, 2020, 07:23 |
|
#7 |
Member
Join Date: Sep 2010
Location: Leipzig, Germany
Posts: 96
Rep Power: 16 |
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 |
|
January 9, 2022, 01:28 |
|
#8 |
New Member
Reid
Join Date: Jun 2021
Location: New Zealand
Posts: 3
Rep Power: 5 |
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 Last edited by reidwill; January 9, 2022 at 07:44. |
|
January 10, 2022, 13:54 |
|
#9 |
Senior Member
Josh Williams
Join Date: Feb 2021
Location: Scotland
Posts: 113
Rep Power: 5 |
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. Code:
// 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 |
|
January 17, 2022, 04:22 |
|
#10 |
Member
Join Date: Sep 2010
Location: Leipzig, Germany
Posts: 96
Rep Power: 16 |
Hi Reid,
I think Josh's solution should do the trick? Have you tried it yet? |
|
January 17, 2022, 05:55 |
|
#11 |
Senior Member
Josh Williams
Join Date: Feb 2021
Location: Scotland
Posts: 113
Rep Power: 5 |
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 |
|
Tags |
lagrangian, particle tracking, transient flow |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
dispersion model with lagragian particle tracking model for incompressible flows | eelcovv | OpenFOAM Running, Solving & CFD | 54 | April 10, 2018 10:36 |
Multiphase flow - incorrect velocity on inlet | Mike_Tom | CFX | 6 | September 29, 2016 02:27 |
Lagrangian Particle Tracking Initial step | Bruce Hartley | OpenFOAM Programming & Development | 4 | September 2, 2015 06:32 |
particle tracking in unsteady flow | peterchen | FLUENT | 1 | July 22, 2010 23:18 |
Particle Tracking in Multiphase Flow | Paul | CFX | 0 | December 15, 2003 12:32 |