[abhinayiyer2408]

Hi Everyone,

I'm working on a Multiphase Evaporation Modeling and I use Fluent 6.3.26 which doesn't have any inbuilt Evaporation Models. I've wrote a couple of programs to model species transport as a User Defined Scalar since I need some freedom on using the gradient of this UDS in my Mass Transfer UDF.

I have two questions regarding this.

1] My Species Transport equation contains only a Diffusivity Term in terms of the temperature. When I write the code for a single-phase flow, the diffusivity term gets complied and runs successfully. But the code that I've written for Multiphase, I get an ACCESS_VIOLATION error during Initialization. The Code is shown below;

DEFINE_DIFFUSIVITY(Species_Diff,c,t,i)
{
Domain *mix_d=Get_Domain(1); /* To obtain domain pointer of the mixture phase*/
real Diff, xc[ND_ND];
real pi=3.14, k=1.38e-23, dia=4e-10;
int zone=3; /* Liquid Zone */
Thread *mix_t=Lookup_Thread(mix_d,zone); /* Liquid thread lookup */

if (C_VOF(c,mix_t) == 1) /* If the Volume fraction is = 1 */
{
C_CENTROID(xc,c,mix_t);
Diff = C_R(c,mix_t)*k*C_T(c,mix_t)/(3.0*pi*C_MU_EFF(c,mix_t)*dia); /* Diffusivity Term */
}
return Diff;
}

I've added the header file. So, the problem is not that. I feel my problem is in the "if statement" that I've provided. Is there any other way to provide the "if statement" ?

2] Do I have to provide 2 different diffusivity term to access both the phases or can it be included in one?

Apart from this, I have a question regarding MASS_TRANSFER() syntax.

Do we have to provide an "if statement" and "loop" for this to access only the interface or does the argument "Thread" in the MASS_TRANSFER() access only the interface?

[`e`]

You've used the Lookup_Thread function instead of the phase-level thread pointer (THREAD_SUB_THREAD). Have a read of the multiphase macros in the UDF manual and you should be able to restrict your diffusion equations according to the phase using conditional if statements.

[abhinayiyer2408]

Hi 'e'. Thanks for the early reply.

I've solved the problem. Thanks a lot for your help. Now I face another problem. I'm using the gradient of this UDS to call into the Interaction Phase. I get an error saying that Fluent is unable to locate the UDS file that I have specified. I don't know why. Can you please help me out with it?

[`e`]

The user-defined scalar (UDS) transport equations shouldn't require a separate file, what exactly is the error message?

[abhinayiyer2408]

Hi e,

The exact error I'm getting is "Mass_Transfer_Trial.obj : error LNK2019: unresolved external symbol _C_UDS0_G referenced in function _mass_transfer
libudf.dll : fatal error LNK1120: 1 unresolved externals".

I have compiled 2 UDFs. One which has the Diffusivity Term for the UDS and the other which is my interface boundary condition. When I compile both together or separately, I get this error. My Code is written below.

FILE 1 :

#include "udf.h"

DEFINE_DIFFUSIVITY(Liq_Species_Transfer,c,t,i)
{
real Diff, pi=3.14, dia=4.0e-10, k=1.38e-23;

Diff = C_R(c,t)*k*C_T(c,t)/(3.0*pi*C_MU_EFF(c,t)*dia);

return Diff;
}

FILE 2:

#include "udf.h"

DEFINE_EXCHANGE_PROPERTY(mass_transfer,c,t,i,j)
{
real m_dot_grad=0.0;
real T_c = 647.0, T_sa = 298.18, H_sa = 2257.0, mw = 18.0152, ma = 28.996;
real V_s,C_s,h_fg,p_ratio,conc,temp_interface,term1_1,t erm1_2,term_1,term2_1,term_2,term3_1,term_3;

temp_interface = C_T(c,t);
term1_1 = (H_sa/UNIVERSAL_GAS_CONSTANT);
term1_2 = ((temp_interface-T_sa)/(temp_interface*T_sa));
term_1 = term1_1*term1_2;
term2_1 = log(temp_interface/T_sa);
term_2 = 0.38*term2_1/T_c;
term3_1 = temp_interface-T_sa;
term_3 = 0.118*term3_1/(T_c*T_c);
p_ratio = (exp(term_1-term_2-term_3));
C_s = 1.0/(1.0+((ma/mw)*(1.0/p_ratio)-1.0));
conc = C_UDS0_G(c,t,i);
V_s = 2.88e-5*conc/(1.0-C_s);
m_dot_grad += V_s*C_R(c,t);

return m_dot_grad;
}

When I debug the code, I found out the problem is in the line where I define my conc term. Without that term, my program simulates. Please help me out with this.

[`e`]

The syntax for the UDS gradient is C_UDSI_G(c,t,i) where i is an index of the scalar; not "C_UDS0_G(c,t,i)". You've also used the same variable as an argument for the "second_column_phase_index". Have a read of these sections in the UDF manual for details.

[abhinayiyer2408]

Hi 'e',

Thanks a lot for your reply and suggestions. I've done the changes that you advised. I tried running the program, but during compilation I get an error like
"..\..\src\Mass_Transfer_Trial.c(20) : error C2440: '=' : cannot convert from 'real *' to 'real' ". I don't know what this error means. I've tried searching about this on different forums but never got any useful answer. Can you please help me out. The program is given below.

#include "udf.h"
#include "sg_mphase.h"

DEFINE_MASS_TRANSFER(mass_transfer,c,t,i,j,n,m)
{
real m_dot_grad=0.0;
real T_c = 647.0, T_sa = 298.18, H_sa = 2257.0, mw = 18.0152, ma = 28.996;
real V_s,C_s,h_fg,p_ratio,conc,temp_interface,term1_1,t erm1_2,term_1,term2_1,term_2,term3_1,term_3;

temp_interface = C_T(c,t);
term1_1 = (H_sa/UNIVERSAL_GAS_CONSTANT);
term1_2 = ((temp_interface-T_sa)/(temp_interface*T_sa));
term_1 = term1_1*term1_2;
term2_1 = log(temp_interface/T_sa);
term_2 = 0.38*term2_1/T_c;
term3_1 = temp_interface-T_sa;
term_3 = 0.118*term3_1/(T_c*T_c);
p_ratio = (exp(term_1-term_2-term_3));
C_s = 1.0/(1.0+((ma/mw)*(1.0/p_ratio)-1.0));
conc = C_UDSI_G(c,t,0);
V_s = 2.88e-5*conc/(1.0-C_s);
m_dot_grad += C_VOF(c,t)*V_s*C_R(c,t);
return m_dot_grad;
}

[`e`]

The C_UDSI_G macro returns the gradient of the UDS in each direction (vector quantity represented with an array). An example in the UDF manual calculates the magnitude of this gradient with NV_MAG, but you could use the components if that's what you're after.

[abhinayiyer2408]

Hi 'e',

Yes, I need the y-component of the gradient at the interface thread alone. What is the macros for obtaining the y-component gradient ? UDF Manual doesn't provide these information properly. It is very brief and very easy to lose track. Again, Thank you so much for the help.

[`e`]

The syntax should follow the other gradient macros (C_U_G for example); then the y-component would be: C_UDSI_G(c,t,0)[1] (the 1 corresponds to the y-direction, 0 would be for x and 2 for z).

[abhinayiyer2408]

Hi 'e',

I tried the one you said, but when I use that I get "ACCESS_VIOLATION" error for both coordinate specified gradient and NV_MAG of the gradient. Is there any other way to use the gradient of a UDS function? Can we add the gradient as another UDS and use that UDS in the expression?

[`e`]

Have you enabled the user-defined scalars? This won't be the cause if you're only getting errors with the gradient macro, and not the normal UDS macro.

There are reported issues with using the gradient on the first time step because the gradient hasn't been calculated for this first step. This problem is not only for UDS, but for other variables as well. Have a read of this thread for details and a solution for UDS gradients.

[abhinayiyer2408]

I have enabled the user-defined scalars. Since I'm working on a multi-phase problem, I'm using 2 UDS for both phases separately and the number UDS matches the condition.

I'm using a steady state model so there should not be any issue with time steps. Just in case, I've used a User-Defined Memory location in my main program which saves the gradient of the UDS. I run the program for 5 iterations and later hook the gradient term on to the solution. Even after that, I get an ACCESS_VIOLATION error when I start to iterate. Does the User-Defined Scalar Gradients have these kind of problems?

[abhinayiyer2408]

Hi 'e'

Let me explain you the problem statement. Probably you could help me doing it in a different way.

A thin-film is flowing inside a channel along the wall at a prescribed velocity. Air flows adjacent to it at a higher velocity compared to the liquid. The wall of this channel is heated just below the boiling point of the liquid so that it evaporates. I have formulated heat and mass transfer equations at the interface. My aim is to track the liquid-gas interface.

I've attached an image of the problem that I want to solve. Here, I know the initial thickness of the liquid film but I don't know the profile of it. The profile depends on mass transfer at the interface. The equation of mass transfer is as shown in the image.

I tried using Species Transport equation directly and calling the y-direction species transport gradient in my Mass-Transfer UDF. I get an ACCESS_VIOLATION error due to that. I can only call the species transport but not the gradient. So I decided to write a diffusivity UDF for the species transport for both the phases separately and call the gradient of this UDS. When I do that, the solution never converges. But, the fluid starts to evaporate from the inlet point and at the end, the fluid stays as it is. The UDF for my mass transfer is given in the attachment. Now, I don't know where I've gone wrong or what mistake I commit. Please help me out.