|
[Sponsors] |
August 23, 2021, 10:46 |
Water-Air simulations
|
#1 |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
Correct me if I'm wrong: in Flow 3d, for open channel simulations, generally simulations consider only one fluid, water. I've rarely seen simulations with two fluids.
Is there a solver in openFoam able to do the same thing, or the only solution, for open channel simulations, is to use interFoam and therefore simulations with two fluids? |
|
August 25, 2021, 12:13 |
|
#2 |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
In other words, for open channel simulations, which openFoam solvers can be used? Is there only interFoam?
|
|
August 30, 2021, 09:21 |
|
#3 |
Senior Member
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 369
Rep Power: 8 |
interFoam is a solver for a two-fluid system with interface resolution.
so you need fluid properties (densities, kinematic viscosities, and interfacial tension) for both fluids. |
|
August 31, 2021, 11:01 |
|
#4 | |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
Quote:
From my experience, I know that many free-flow simulations in Flow3D(the area for which Flow3D is famous) are based on simulations with only one fluid. I'm asking to the more experienced forum's users if this capability is due to the use of TruVOF or something else. Also, is there a solver in openFoam that can do the same thing? Thank you. |
||
September 1, 2021, 01:36 |
|
#5 |
Senior Member
|
There is an interface-tracking dynamic mesh. I'm not sure this fits your needs or not. I have an interest in this function but I have never used...
https://www.openfoam.com/news/main-n...rface-tracking |
|
September 1, 2021, 03:25 |
|
#6 | |
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
Quote:
|
||
September 1, 2021, 04:17 |
|
#7 | |
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,290
Rep Power: 34 |
Quote:
Flow 3D indeed could solve for one phase. For this to happen there has to be a boundary condition to be applied on the free surface. The advantage of this approach is that the velocities from air could be neglected and thus allowing higher time steps. However this is not the only way to do this, for example the implicit VOF in Wildkatze could have much higher courant numbers without smearing the interface. We do all the time. For openfoam it is hard to tell. |
||
September 1, 2021, 05:12 |
|
#8 | ||
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
Quote:
Quote:
You can easily implement an implicit VoF In OpenFOAM, a là flow3d, but still the aforementioned problem will exist. |
|||
September 1, 2021, 05:23 |
|
#9 | ||
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,290
Rep Power: 34 |
Quote:
Flow 3D people obviously disagree with you here. They have multiple examples of using this. The method is limited but not as much as you are declaring here. Quote:
Ever heard of validations and benchamarking. We have done that a lot with this implicit appraoch. As far as mass conversation goes, we have developed methods to keep that in check. We have infact done calculations (on unstructured polyhedral meshes) such a fluel capturing air due to sloshing and match the experimental values. A calculation where mass conservation and numerical errors are of utmost importance because air captured by fuel is quite low. It all depends on what the method is and how it is implemented. |
|||
September 1, 2021, 05:33 |
|
#10 |
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,290
Rep Power: 34 |
Here you go one famous benchmark with courant number well above 5. Done on unstrcutured mesh.
|
|
September 1, 2021, 06:06 |
|
#11 | |||
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
Quote:
I will go a step further: being able to resolve "shocks" accurately in ALE implies that you need to re-mesh (using MESQUITE, or other) which defeats the purpose of having a "faster" solver. Then there is the problem of remeshing and boundary layer inflation (you'll have to dispense of the latter), which begs the question: What's more important, resolving wall-bounded turbulence or the jump? A hard choice if you are studying an USBR dissipation bucket... Unless you implement ALE under DG, this method is only physically relevant, and computationally cheap, for flows that do not undergo shocks, or hydraulic jumps, or breaking waves. Quote:
Quote:
We may start arguing about it's importance for "real-life RANS/DES-CFD", and then I'd mention it's a problem of intellectual cleanliness and not of accuracy nor approximation. |
||||
September 1, 2021, 06:24 |
|
#12 | |
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
Quote:
On a structured mesh things may go better, and with a smaller Co EVEN BETTER. |
||
September 2, 2021, 04:11 |
|
#14 |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
I am looking for an openFoam solver that allows simulation of open channels with a single fluid, similar to what Flow3d allows...
|
|
September 2, 2021, 05:09 |
|
#15 |
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
||
September 2, 2021, 07:20 |
|
#16 | |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
Quote:
I have little experience with openFoam, but from the few projects I've done, I've noticed that interFoam (2 fluids) tends to be more easily unstable than what you get with Flow3D, as well as being much slower computationally. I thought this was due to the fact that interFoam needs to solve the equations for two fluids, hence my question about the existence of an openFoam solver that allow the simulation of open channel considering only one fluid, as Flow3D allows to do. |
||
September 2, 2021, 07:42 |
|
#17 |
Senior Member
|
There is a tutorial case with a liquid filled cavity with free surface. pimpleFoam solver is used. Only one fluid is considered. Free surface moves using an interface-tracking dynamic mesh.
https://develop.openfoam.com/Develop...actAngleCavity |
|
September 2, 2021, 09:22 |
|
#18 | |
Member
Miguel Hernandez
Join Date: Feb 2021
Location: En mi casa
Posts: 56
Rep Power: 5 |
Quote:
|
||
September 2, 2021, 11:04 |
|
#19 | |
Senior Member
Santiago Lopez Castano
Join Date: Nov 2012
Posts: 354
Rep Power: 16 |
Quote:
This distinction IS IMPORTANT because, as you can see, a great deal of confusion can arise if you are not clear on what you want. A single-phase simulation IS NOT THE SAME as a VoF where the air phase IS CLIPPED, or a VoF where the air phase IS NOT CLIPPED. Different algorithms, and somewhat different math, hence the different naming conventions. The thing you are looking for is **interFoam**, a VoF solver for two-immisible fluids, where you can use turbulence models. This solver is not though to be used for particular set of scenarios, as Flow3D does. Since OpenFOAM is not as foolproof as Flow3D, and IT IS NOT A SUITE OF SOLVERS but A LIBRARY FOR FVM which is full of **example solvers**, such as interFoam, you must be willing to go the extra mile (quite literally) in order to make things work. That sometimes imply you need to program things or, at the very least, dive into the code itself, or get scolded in forums like this one . If what you want is a SINGLE-PHASE solver with an upper moving boundary representing a free-surface, then you need to use **interTrackFoam** (PISO + ALE). Last time I checked there is no turbulence modelling implemented within. Setting one is not difficult though. NOTE: interFoam is not that much slower compared to other solvers, when set up correctly. Have in mind that some solvers use pseudo-time integration by default, hence the impression that it "goes" faster. You can use local time stepping also in OpenFOAM. |
||
September 3, 2021, 01:53 |
|
#20 | |
Senior Member
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 1,290
Rep Power: 34 |
Quote:
You mean like better descretization ie better reconstruction and solving continuity equation is a trick?? No we are not adding or substracting any fluid to maintain the mass conservation if this is what you mean by trick. If solving equations by descretisation is a problem to you, then there is nothing that could be done because without it there is no solution to the problem. The scheme that we use is none of what you mentioned. The scheme that i use is something i have designed and the whole thinking about it is very different than the interface tracking that you think of. The method is at its base implicit in nature. This is why it can run on large courants and keep interface sharp. Edited to add: It occured to me that it is openfoam that actually uses the 'trick'. They have extra term added to VOF equation to keep the interface sharp. Wildkatze does not do even that and there is no such option for user to chose from too. |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Water diffusion into air | MGabr | CFX | 19 | September 3, 2023 20:06 |
multiphaseEulerFoam convergence problems | Stefanie.S.W. | OpenFOAM Running, Solving & CFD | 6 | August 28, 2019 05:15 |
Mass Transfer Between AIR and WATER | Math13570 | CFX | 12 | June 29, 2016 09:14 |
3D multiphase micro model: mixing effect of air and water at the T junction | ehsanfareed | FLUENT | 2 | March 22, 2015 23:29 |
I am NOT getting right pressure at the air inlet in water column | kcfd | FLUENT | 2 | November 27, 2012 22:36 |