
[Sponsors] 
April 23, 2014, 09:12 
multiphaseinterfoam and multiphaseeulerfoam

#1 
Senior Member
Join Date: Jan 2012
Posts: 166
Rep Power: 14 
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 

April 23, 2014, 22:16 

#2  
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Beijing, China
Posts: 844
Rep Power: 18 
Quote:
multiphaseEulerFoam is similar with twoPhaseEulerFoam, about twoPhaseEulerFoam, check this out: http://powerlab.fsb.hr/ped/kturbo/Op...chePhD2002.pdf Regards, 

April 29, 2014, 10:00 

#3 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
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 nphase version on interFoam which is used for segregated flows (with a sharp interface). multiphaseEulerFoam is built on a similar basis as twoPhaseEulerFoam using the multifluid transport formulationmomentum equation per phase as referenced in the previous post, but it is more than just an nphase version of that solver. It also brings in flexible sharp interface capability for selected phase pairs on top of the multifluid 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 Last edited by kwardle; April 29, 2014 at 10:02. Reason: fix links 

April 30, 2014, 07:06 

#4  
Senior Member
Join Date: Jan 2012
Posts: 166
Rep Power: 14 
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. EulerModel 3. EulerLagrange In 1. the NavierStokes 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 NavierStokesEquations. Models like RANS (Reynold Averaged Navier Stokes), URANS and LES (Large Eddy Simulations) are available here. First Question: Is the difference between RANSModel and LESModel that in the RANSmodel 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.cfdonline.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 Quote:
Quote:
Furthermore I want to know if the value of Cα is only restricted in multiphaseEulerFoam to 1 and 0 ? greetings maybee Last edited by maybee; May 1, 2014 at 09:29. 

May 1, 2014, 10:39 

#5 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
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 solvedthese 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 socalled 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 EulerEuler formulation (multifluid with per phase momentum eq) it is more rigorous from a RANS perspective to have a turbulence model per phase and interphase turbulence exchange terms. Have a look at twoPhaseEulerFoam for example. By using LES, we are assuming that the turbulence on the subgrid scale can be considered isotropic and valid for the multiphase mixturethis 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 nearwall regionRANS models are applied in the nearwall 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 artifactnamely 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 

May 1, 2014, 15:42 

#6 
Senior Member
Join Date: Jan 2012
Posts: 166
Rep Power: 14 
Thx a lot for this extensive explanation that gives a great overview.


August 15, 2015, 14:05 

#7  
Senior Member
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 158
Rep Power: 17 
Quote:
thank you in advanced 

August 15, 2015, 15:28 

#8 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
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 fluidfluid interface Courant number 'a la interFoam' it is not any additional burden to use LES and usage of unsteadyRANS would not be any improvement in terms of solution time or accuracy in my opinion. 

August 15, 2015, 16:34 

#9  
Senior Member
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 158
Rep Power: 17 
Quote:
I have two question please: first you mean there is no difference in running time between LES and kepsilon RNG forinstance? 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 

August 15, 2015, 16:46 

#10 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
1) *For a given mesh* I would say there is negligible additional runtime.
2) In the asreleased version, there is no builtin 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 MultifluidVOF Multiphase CFD Solver,” Int. J. Chem. Eng. 2015, 925639, (2015). Last edited by kwardle; August 15, 2015 at 16:48. Reason: full article citation added 

September 3, 2015, 00:25 
compressiblity in multiphaseEulerFoam

#11 
Senior Member
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 158
Rep Power: 17 
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 Last edited by zandi; September 12, 2015 at 02:58. 

September 12, 2015, 14:39 

#12  
Senior Member
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 158
Rep Power: 17 
Quote:
could you help me in changing UEqns.H more please? thank you 

October 27, 2015, 17:45 

#13 
Member
Join Date: Oct 2015
Posts: 48
Rep Power: 10 
Hello cfd
I want to modeling bubbly flow I like to know which one of twophaseEulerFoam or multiphaseEulerFoam is better? thank you 

November 19, 2015, 02:36 

#14 
Senior Member
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 158
Rep Power: 17 

December 8, 2016, 15:24 

#15 
New Member
Alex Machado
Join Date: Feb 2014
Location: Brazil
Posts: 8
Rep Power: 12 
how can I change the cutoff value to turn on/off interface compression?


December 15, 2016, 22:31 

#16  
New Member
Li Linmin
Join Date: Nov 2015
Location: China
Posts: 27
Rep Power: 10 
Quote:
I am using version 1606+, I just modify the setFields file with dambreak4phase tutorial. Anyone can help me ? 

April 15, 2017, 07:25 
Setting up multiphaseEulerFoam

#17 
Member

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. 

September 17, 2017, 02:06 

#18  
Senior Member
Elham
Join Date: Oct 2009
Posts: 184
Rep Power: 16 
Quote:
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 

April 17, 2018, 08:54 
multiphaseEulerFoam  variable interface sharpening

#19  
New Member
Roberto T
Join Date: Mar 2018
Posts: 3
Rep Power: 8 
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. Quote:
Tanks a lot! Roberto 

September 1, 2018, 00:41 

#20  
New Member
Ainal Hoque Gazi
Join Date: May 2018
Location: India
Posts: 27
Rep Power: 8 
Quote:
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. 

Thread Tools  Search this Thread 
Display Modes  

