Learning Forum

[sachintom1992]

I need to modify the existing CHF wall boiling model in Ansys fluent to solve for annular flow regime. How I can write UDF  for wall boiling model in Fluent and where to hook it?

 

 

[DrAmine]

What kind of flow regime do you have? It should not be an easy task by the way.

[DrAmine]

What kind of flow regime do you have? It should not be an easy task by the way.

[sachintom1992]

Dear sir,

              I am working on liquid sodium flow boiling in an annulus channel similiar to that of single pin fuel sub channel of SFR. The various flow regimes possible for liquid sdoium flow boiling are the subcooled flow boiling regime(bubbly flow) then the transition regime(slug/churn dominant) and the dispersed annular flow regime and the liquid film dryout (CHF condition). I am trying with Eulerian-Eulerain Multiphase flow model with CHF WHFP. I ma able to get reasonable result for bubbly flow and slug/churn dominant but i am not able to solve for dispersed annular and finally most flow. Is it possible with modifying WHFP for high void fraction regimes?

 

[DrAmine]

The modifications which you can do are limited to providing nucleation site density, bubble departure diameter and other sub-models. The blending of the regime can be changed but you cannot provide a new formulation for it.

I assume the fuel channel are vertical ring channel? So actually CHF RPI cam be used but you need to be careful with all submodels.

[sachintom1992]

Dear sir,

             I seen in Fluent theory guide CHF model by Ioilev et al. consider thin film boiling also into consideration. How to activate this model instead of critical vapor fraction based one?

[DrAmine]

It is mentioned under Including the Boiling Model in the User's Guide.

[sachintom1992]

 Dear sir,

              Can we consider same constitutive correlations for interfacial area concentration, drag coefficient , interfacial heat transfer for slug flow regime and annular flow regime as both are like LSI regimes?

[DrAmine]

Lsi: large scale interface model of our competitor? Yes.

[sachintom1992]

Dear sir,

            I have doubts about interfacial  constitutive correlations in two-fluid model. Can we use the empirical correlations  those are used in lumped analysis (porous media approximation, subchannel level analysis of reactor flow channel) as such into CFD code?For ex. interfacial area concentration in lumped analysis codes consider as :  (4*(vapor fraction)^0.5)/Dh   Dh hydraulic diameter. This is  for annular flow regime. But in CFD codes thy give as gradient of vapor fraction as IAC correlation for annular flow regime. What is the difference between both?

[DrAmine]

Ask your professor for assistance here. I would adapt lumped parameter correlations to CFD means using them directly is wrong.

[sachintom1992]

Dear sir,

             Thanks a lot for your replies. Can u help me with drag coefficient correlation for LSI regime? From literature I seen it is expressed in terms of  tangential shear stress acting along the interacting phases (GENTOP model). how to make it as udf?

 

[DrAmine]

It is already implemented in AIAD so no need to implement it on your own.

[sachintom1992]

Dear sir,

          

[sachintom1992]

Dear sir,

            Thanks a lot for your reply.

[sachintom1992]

Dear sir,

              The default CHF model in Ansys fluent consider flow patterns as:  bubbly flow regime(void fraction<0.3) transition (0.30.7). The interfacial constitutive relations use blending functions between each flow regimes. Suppose I want to consider the flow regimes as: bubbly flow regime(void fraction<0.3) transition (0.3

 

[DrAmine]

You can define your closure laws for drag, non-drag forces as you want. The internal code will just start blending at 0.3 and 0.7 so that you provide your UDF's to differentiate in the regime larger than 0.7.

It might work!

[sachintom1992]

Dear sir,

            It means  I need to give closure laws only for void fraction<0.3 and void fraction>0.7. In between does  the code will blend suitably?

[DrAmine]

The code will blend as documented.

[DrAmine]

But you want an additional blend on top  where you want to provide your own exchange laws. So basically the code will blend starting from 0.7 and now you need to provide different laws based on the volume fraction.

[sachintom1992]

Sir,

      Can I give the correlations from bubbly flow regime itself. As in 0.3

[DrAmine]

That does sustain any use changes. The only thing you can do is providing the closure laws based on your volume fraction and here you account to whatever you want , The function used to blend is documented. 

[sachintom1992]

Sir,

 The above is udf code for interfacial area concentration from bubbly regime to annular flow regime. Here the w variable i am using within the if statement is not taking proper values into the fluent code. I am unable to solve the issue. Please help me on this.

 

 

#include "udf.h"
#include "mem.h"

#define GRA 9.81
#define ST 0.12

DEFINE_EXCHANGE_PROPERTY(custom_ia,c,t,i,j)
{
//Thread *ps = THREAD_SUB_THREAD(t,j);
//real Ref1, Wed1, E1, Edv1;
real muL, rho_f, rho_g;
real dh = 0.0085;               // hydraulic diameter in m
real ai1, ai2, ai;
real w = 0;
real vof_j, diam, area_intf;
real fd = 0;
real fb = 0;
real fs = 0;
//real z = 0;

Thread *thread_f, *thread_g;

thread_f = THREAD_SUB_THREAD(t,i);/* continuous */
thread_g = THREAD_SUB_THREAD(t,j);/* discontinuo*/

vof_j = C_VOF(c,thread_g);
diam = C_PHASE_DIAMETER(c,thread_g);

rho_f = C_R(c, thread_f);   // liquid density
rho_g = C_R(c, thread_g);   // vapor density
muL = C_MU_L(c,thread_f);   // liquid viscosity



/* weighting function in transition region*/
if(vof_j<=0.3)
{
    w = 0;                
}
else if(0.3{   
    w = (0.5)*(1-cos(3.14*((vof_j-0.3)/(0.7-0.3))));    
}
else if(vof_j>=0.7)
{
    w = 1;
}

/*blending function*/


fd = 1/(1+exp(70*((1-vof_j)-0.3)));
fb = 1/(1+exp(70*(vof_j-0.3)));
fs = 1-fd-fb;

    ai1 = 6.*vof_j/diam;               /*bubbly regime IAC equation*/
 

    ai2 =  (4*pow(vof_j,0.5))/dh ;
 
    ai = fb*ai1 + fd*ai2 + fs*((1-w)*(ai1)+w*(ai2)) ;       /*blending equation*/
 
    area_intf = MAX(0.0,ai);
 


 C_UDMI(c,t,1) = area_intf;
 C_UDMI(c,t,2) = w;
 C_UDMI(c,t,3) = fb;
 C_UDMI(c,t,4) = fs;
 C_UDMI(c,t,5) = fd;

return area_intf;
}

 

[sachintom1992]

Sir,

     I have a small doubt about how  transition regime  (i.e. between bubbly regime and annular flow regime) interfacial correlations to be considered.

                           Suppose an interfacial parameter say Interfacial area concentration is considered in transition regime as:

                                                              Ai (transition) = (1-w)*Ai(bubbly) + w*Ai(annular)   where w weighting function

Here Ai(bubbly) has to be evaluated at alpha=0.3 or at corresponding alpha (say 0.5) in the transition regime. Also Ai(annular) to be evaluated at 0.7 or at corresponding alpha (say 0.5) in the transition regime.

Please help me on this doubt.

[DrAmine]

yes the weighting function should do that biasing for you. The manual contains some examples of possible functions.

[sachintom1992]

Sir,

     My doubt is how Ai bubbly and Ai annular to be evaluated? Is it at say alpha = 0.3 and alpha =0.7 and weight it or at each alpha values say at 0.4, 0.5,0.6 etc.and weight it?

[sachintom1992]

Sir,

    One doubt regarding multi phase turbulence model. Suppose I wants to capture violently pulsating flow regime i.e. area averaged vapor fraction  at any cross-section fluctuates b/w say 0.8 to 0.5 and I need to capture the behaviour without loosing the interface. Is the mixture based treatment or per-phase based turbulence treatment will be better for it?

 

 

[DrAmine]

I would rather decide on stability as per phase is prone to stiffness issues as contains more physics but not all closure laws are available. I have done runs with both apporaches.

[sachintom1992]

Sir,

    While doing the simulation I am getting error as "Turbulent viscosity limited to 10^5 in certain cells" and case is diverging. Is it happening because of not choosing proper turbulence treatment? Mine flow pattern itself is getting disturbed with this error. What about turbulence damping? Can it preserve such a large scale interface without any trouble?

The attached is area averaged vapor fraction at end of heated section I got in my simulation. When violent pulsation happens it is diverging. 

[DrAmine]

Might be for a lot of reason: bad mesh, wrong BC, very fine mesh (RPI does not like fine wall mesh yplus>30) etc. Hard to say at this stage why!

[sachintom1992]

Sir,

    Is the surface tension force is added in two-fluid model or we need to consider add it as source term udf?

[DrAmine]

You need to add it if required. I won't add it in a boiling simulation.

[sachintom1992]

Sir,

    I need to consider large scale interface (slug/annular) in my flow boiling simulations. In literature I have seen they are considering surface tension force also in Momentum equation(Thomas Hohne et al. 2012)for LSI regime capture. If I given it as source term UDF whether same mesh will be sufficient for simulation? Usually for flow boiling mesh is coarse type?

Regards,

Sachin

[DrAmine]

If you are doing all stuff via UDF you can try to distribute mass source Nd heat source. Aiad model is also included in Fluent.

I recommend though to implement everything via UDF.

[sachintom1992]

Sir,

     What is happening with my simulation is high vapor fraction regime(say area averaged vapor fraction 0.5-0.8 region) the model is not properly capturing the interface. It is unable to maintain the Large interface.

So first I added turbulence damping term in epsilon equation as source term sill it was not going proper. So now I feel like surface tension is playing a role here.Can surface tension force maintain the interface properly?

Also as per you have told with default two-fluid model for flow boiling simulation surface tension force is not included I need to add it as source term udf. Is the Continuum Surface Force model or Height function based will be better?

[DrAmine]

Yea it can but require resolution.
If you enable multifluid VOF you can account for surface tension force. I would focus on that and neglect first subgrid boiling effect.

[sachintom1992]

Sir,

     Where this surface tension force UDF has to be attached. Is it axial momentum or radial momentum equation for either of the phases?

[DrAmine]

If you are using Multi Fluid VOF you do not need to add any surface tension UDF. 

[sachintom1992]

Sir,

    Using Multifluid VOF is like solving two phase flow problem. I need to consider wall boiling also. Mine is flow boiling problem. 

[DrAmine]

I recommended to mode your boiling via UDF or neglect the subgrid boiling effect.

 

Anyway I will just answer here: surface tension force to be added as source term in momentum equation. 

I recommend that you create another new thread with clear description as this thread get confusing and long..

[srikashi]

Dear sir

I am simulating subcooled flow boiling and also CHF in rectangular microchannel using Fluent wall boiling model....my doubt is

1) can we use CHF model for simulating subcooled flow boiling

2) upto what heat flux we can use RPI wall boiling.....can we go upto critical heat flux and still use RPI model....??

3) while using CHF model I am experiencing convergence issues ......I have used Psuedotransient approach ....what should be the ideal time scale facator....

pls someone clarify

thanks i advance

[Rob]

Please create a new topic for attention.