[maybee]

hi,

few question about the above mentioned solvers:

1. What are the differences between the two solvers? Is the main difference that multiphaseeulerfoam is useable for processes which have dispersed and segregated flow regimes and multiphaseinterfoam is only for dispersed flow regimes?

2. Is there a flow chart available which shows the solution procedure of multiphaseeulerfoam? I had only found one for the interfoam solver.

greetings
maybee

[sharonyue]

Originally Posted by maybee

hi,

few question about the above mentioned solvers:

1. What are the differences between the two solvers? Is the main difference that multiphaseeulerfoam is useable for processes which have dispersed and segregated flow regimes and multiphaseinterfoam is only for dispersed flow regimes?

2. Is there a flow chart available which shows the solution procedure of multiphaseeulerfoam? I had only found one for the interfoam solver.

greetings
maybee

This is a quick review of this eulerFoam ad interFoam. http://www.openfoam.org/version2.1.0/multiphase.php

multiphaseEulerFoam is similar with twoPhaseEulerFoam, about twoPhaseEulerFoam, check this out: http://powerlab.fsb.hr/ped/kturbo/Op...chePhD2002.pdf

Regards,

[kwardle]

Maybee,Henry Weller and I published a paper (open access) on the multiphaseEulerFoam solver which you can find here: http://dx.doi.org/10.1155/2013/128936.


To answer your question, multiphaseInterFoam is simply a n-phase version on interFoam which is used for segregated flows (with a sharp interface). multiphaseEulerFoam is built on a similar basis as twoPhaseEulerFoam using the multi-fluid transport formulation---momentum equation per phase--- as referenced in the previous post, but it is more than just an n-phase version of that solver. It also brings in flexible sharp interface capability for selected phase pairs on top of the multi-fluid framework. This means that it can do both dispersed and segregated flows simultaneously. Have a look at the paper and let me know if you have questions. You can also find other info at my personal website www.mcs.anl.gov\~wardle.


-Kent

[maybee]

Thx a lot for the informations. Very interesting work you have done with the "multiphaseEulerFoam" solver by implementing an algorithm that is able to handle mixed flows in terms of segregated and dispersed.

I still have some quesitons, although they are of more general nature :

When simulating a multiflowprocess are three general options (source: Rusche PhD 2002):

1. DNS: direct numerical solution
2. Euler-Model
3. Euler-Lagrange

In 1. the Navier-Stokes equations are not modified anymore and even small influences like turbulences are solved very accurate by a very fine mesh.
In 2. and 3. there are generally used more simplified versions of the Navier-Stokes-Equations. Models like RANS (Reynold Averaged Navier Stokes), URANS and LES (Large Eddy Simulations) are available here.

First Question:
Is the difference between RANS-Model and LES-Model that in the RANS-model generally the RANS equations are used and the whole turbulence effects are modelled, but in LES you set some kind of limit where all turbulences above this limit are solved completely like in DNS and all tubulences below this limit are modelled like when using RANS?

Second Question:
Is multiphaseEulerFOAM compatible with LES as well as RANS? I have looked up example bubbleColumn and there is used LES for example.

Third Question:
If my assumptions in "First Question" are right are the turbulence modells used in LES for the small turbulences below the set limit are the same as used for RANS like described here:

http://www.cfd-online.com/Wiki/RANS-...bulence_models

?

EDIT:

Fourth Question:
In the paper on the multiphaseEulerFoam solver is used a "compression velocity" u ⃗c which is shortly described starting below equation (8) with

the velocity u ⃗c is applied normally to the interface
to compress the volume fraction field and maintain a sharp interface.

and by the description of equation (9) with

The ∇α/|∇α| term gives the interface unit normal vector for the direction of the applied compression velocity. The magnitude of the velocity |u| ⃗ is used since dispersion of the interface (which is being counteracted by the compression velocity) can only occur as fast as the magnitude of the local velocity in the worst case. The coefficient Cα is the primary means of controlling the interfacial compression.

I don't understand what u ⃗c really is and the physical model how it is gained by equation (9)?
Furthermore I want to know if the value of Cα is only restricted in multiphaseEulerFoam to 1 and 0 ?

greetings
maybee

[kwardle]

Q1 - Sort of. In RANS, the Reynolds averaged Navier Stokes equations are solved. These equations have been manipulated such that the fluctuating velocity component is removed and only the (Reynolds) average velocity field is solved for. Additional transport equations and/or algebraic models are used to capture the turbulence contributions through a turbulent viscosity term. In LES, the filtered NS equations are solved--these look similar to the Reynolds averaged equations but are not the same. In these equations, the full instability and behavior of the NS equations in regards to fluctuating velocity are solved for the domain above a specified 'filter width' which is related to the local mesh size. To account for turbulence contributions below the filter width (the so-called subgrid scale) algebraic or transport models are used. I am not an expert in this particular area, but that is my understanding and there are plenty of resources you could find to get the details as pertaining to single phase flows.

Q2 - multiphaseEulerFoam is configured to work with LES though with some small changes it could be made to work with RANS. However, you will notice that for Euler-Euler formulation (multi-fluid with per phase momentum eq) it is more rigorous from a RANS perspective to have a turbulence model per phase and inter-phase turbulence exchange terms. Have a look at twoPhaseEulerFoam for example. By using LES, we are assuming that the turbulence on the sub-grid scale can be considered isotropic and valid for the multiphase mixture--this is an approximation, but you will see from the literature that there aren't really any multiphase LES models and there is some debate on what is even valid in the multiphase case.

Q3 - Generally, no. There are different models used for the SGS turbulence component in LES the most common being the Smagorinsky model which is a relatively simple algebraic model. There are other LES variants (relatives?) such as Detached Eddy Simulation (DES), of which OF has a few flavors, which do more like what you mention although for the near-wall region---RANS models are applied in the near-wall region and LES in the bulk.

Q4 - The compression velocity u_c is not a physical term. It is a numerical construct to counteract a numerical artifact--namely numerical dispersion of the interface away from sharpness. The worst case for numerical dispersion of the interface would be the magnitude of the local velocity, which is why you see this term there in EQ9. If you have a look at the source, EQ9 is the way u_c is calculated in interFoam which allows for c_alpha to be any positive value with larger values enforcing more aggressive sharpening. In practice, values of c_alpha larger than 1 are unnecessary and increase the problems with interfacial 'spurious currents' (have a look at ref 15 from the paper) in these methods. In addition, since I wanted to also use c_alpha directly as a switching variable to turn interface sharpening on/off, it is restricted to values of 0 or 1 in which case EQ9 reduces to EQ10.

-Kent

[maybee]

Thx a lot for this extensive explanation that gives a great overview.

[zandi]

Originally Posted by kwardle

Q2 - multiphaseEulerFoam is configured to work with LES though with some small changes it could be made to work with RANS.

-Kent

Hey Kwardle. would you please say how we can set RANS in multiphaseEulerFoam please or guide me to a link or tutorial?

thank you in advanced

[kwardle]

As I noted above in the release version of the solver, RANS is not an option. You would have to make some changes to createFields.H & UEqns.H to make the turbulence implementation more generic. For example, in UEqns.H you can see that the turbulent viscosity is pulled from the sgsModel function rather than a generic version:

volScalarField nuEff(sgsModel->nut() + iter().nu());

This could be changed without too much trouble by having a look at one of the other solvers. However, I would question the value of using RANS in this case. Given that the solution will be transient anyway and with a time step governed by the fluid-fluid interface Courant number 'a la interFoam' it is not any additional burden to use LES and usage of unsteady-RANS would not be any improvement in terms of solution time or accuracy in my opinion.

[zandi]

Originally Posted by kwardle

However, I would question the value of using RANS in this case. Given that the solution will be transient anyway and with a time step governed by the fluid-fluid interface Courant number 'a la interFoam' it is not any additional burden to use LES and usage of unsteady-RANS would not be any improvement in terms of solution time or accuracy in my opinion.

Thank you very much.
I have two question please:

first
you mean there is no difference in running time between LES and k-epsilon RNG for-instance?
I want to get a large data out put for example for dynamic pressure.

second
can multiphaseEulerFoam model entrainment of gas from interface between of two phase due to turbulence? for example in an inclined bed when turbulent boundary layer in a flow reaches to the surface we expect the entrance of air above.

really thanks for kind guide

[kwardle]

1) *For a given mesh* I would say there is negligible additional run-time.
2) In the as-released version, there is no built-in mechanism to transfer between resolved and dispersed scales in the way you are talking. However, this can be done. I have recently published a paper discussing the very thing you are asking about. It is in the open International Journal of Chemical Engineering and can be found here.

O. Shonibare and K. E. Wardle, “Numerical Investigation of Vertical Plunging Jet Using a Hybrid Multi-fluid-VOF Multiphase CFD Solver,” Int. J. Chem. Eng. 2015, 925639, (2015).

[zandi]

Hey again friends,
a question about multiphaseEulerFoam
in the file : multiphaseEulerFoam.C
it said it is for compressible fluids (get from twoPhaseEulerFoam)
and
in the file: multiphaseSystems.H
is said it is for incompressible fluids (got from multiphaseInterFoam)

which one is correct for the solver? thank you in advanced
----------------------------------------------
I found the answer incompressible but can be changed

[zandi]

Originally Posted by kwardle

As I noted above in the release version of the solver, RANS is not an option. You would have to make some changes to createFields.H & UEqns.H to make the turbulence implementation more generic. For example, in UEqns.H you can see that the turbulent viscosity is pulled from the sgsModel function rather than a generic version:

volScalarField nuEff(sgsModel->nut() + iter().nu());

This could be changed without too much trouble by having a look at one of the other solvers. However, I would question the value of using RANS in this case. Given that the solution will be transient anyway and with a time step governed by the fluid-fluid interface Courant number 'a la interFoam' it is not any additional burden to use LES and usage of unsteady-RANS would not be any improvement in terms of solution time or accuracy in my opinion.

dear Wardle
could you help me in changing UEqns.H more please?
thank you

[masoudsh]

Hello cfd

I want to modeling bubbly flow

I like to know which one of twophaseEulerFoam or multiphaseEulerFoam is better?

thank you

[zandi]

Originally Posted by masoudsh

Hello cfd

I want to modeling bubbly flow

I like to know which one of twophaseEulerFoam or multiphaseEulerFoam is better?

thank you

hi
both are ok.

[amachado]

how can I change the cutoff value to turn on/off interface compression?

[lilinmin]

Originally Posted by paleoCFD

how can I change the cutoff value to turn on/off interface compression?

I am using multiphaseEulerFoam too, but I found that if I set an initial state that liquid with high density in the lower part which is a stable state, the result shows that the fields are always vibrating.
I am using version 1606+, I just modify the setFields file with dambreak4phase tutorial. Anyone can help me ?

[rahulksoni]

I have a case already build upon multiphaseInterFoam with the following details:
1. No. of phase 4: ambient air, water, modified dense water, modified light water; the situation is almost similar to damBreak case with additional inlet and outlet regions.
2. At the inlet phase is introduced which travels through an spiral wall geometry open to atmosphere and then exits at the outlet
An illustrative image of the screenshots (3D and sliced views) of the case is shown in attached image.

Now, I want to convert this case to multiphaseEulerFoam because in reality two of the phases i.e. modified dense water and modified light water were supposed to be heavy/big and lighter/small particles at the inlet. They were assumed as resolved fluid of varying density as defining particle in multiphaseInterFoam is not possible.

Anyone, please help me to tell how do I define dispersed and resolved cases in multiphaseEulerFoam. What files need to be modified. Can I have a sample file with fluid and particle definitions.

[Elham]

Originally Posted by rahulksoni

I have a case already build upon multiphaseInterFoam with the following details:
1. No. of phase 4: ambient air, water, modified dense water, modified light water; the situation is almost similar to damBreak case with additional inlet and outlet regions.
2. At the inlet phase is introduced which travels through an spiral wall geometry open to atmosphere and then exits at the outlet
An illustrative image of the screenshots (3D and sliced views) of the case is shown in attached image.

Now, I want to convert this case to multiphaseEulerFoam because in reality two of the phases i.e. modified dense water and modified light water were supposed to be heavy/big and lighter/small particles at the inlet. They were assumed as resolved fluid of varying density as defining particle in multiphaseInterFoam is not possible.

Anyone, please help me to tell how do I define dispersed and resolved cases in multiphaseEulerFoam. What files need to be modified. Can I have a sample file with fluid and particle definitions.

Dear rahulksoni,

Why did you say that defining particle in multiphaseInterFoam is not possible? You mean setFlieds doesn't work?
I am trying to put some different types of droplets in air flow. Which of the solvers is working: multiphaseInterFoam or multiphaseEulerFoam?

Thanks,

Elham

[tom_rob]

Hi!

I am working with multiphaseEulerFoam and I would like to improve it in order to obtain variable interface sharpening. I would like to obtain something similar to Wardle's solver (link to his work: https://sites.google.com/site/kwardl...putational/cfd).

I am triying to study multiphaseEulerFoam source code, but I can't find source code related to u_c and interface compression equations.

Originally Posted by kwardle

Q4 - If you have a look at the source, EQ9 is the way u_c is calculated in interFoam which allows for c_alpha to be any positive value with larger values enforcing more aggressive sharpening. In practice, values of c_alpha larger than 1 are unnecessary and increase the problems with interfacial 'spurious currents' (have a look at ref 15 from the paper) in these methods. In addition, since I wanted to also use c_alpha directly as a switching variable to turn interface sharpening on/off, it is restricted to values of 0 or 1 in which case EQ9 reduces to EQ10.

-Kent

Could someone give me any suggestion to proceed with my work?

Tanks a lot!

Roberto

[A H Gazi]

Originally Posted by tom_rob

Hi!

I am working with multiphaseEulerFoam and I would like to improve it in order to obtain variable interface sharpening. I would like to obtain something similar to Wardle's solver (link to his work: https://sites.google.com/site/kwardl...putational/cfd).

I am triying to study multiphaseEulerFoam source code, but I can't find source code related to u_c and interface compression equations.



Could someone give me any suggestion to proceed with my work?

Tanks a lot!

Roberto

Hi
I want to model a river flow, in which there will be three layers air,water and sediment from top to bottom.Would you please suggest me which solver should i used in openfoam and where to define the layers thickness.
Thanks.