power law code
 

hi,how can take the fluent code for power law?(i know that fluent simulate the power law fluids)

Re: power law code
 

yes, you can configure it in the Define-->Materials panel. You can select "non-newtonian power-law" instead of "constant" for viscosity properties. When you select Edit, you can enter the consistency, the power-law index, the maximum and minimum value for viscosity. Note that Fluent enables the energy equation. If you are not interested in the solution of the energy equation, you can deselect "Energy" in the Solve-->Controls-->Solution panel and Fluent won't solve this equation. I hope I answered to your question.

Antoine

Re: power law code
 

thanks Antoine, power law in fluent defined as : k exp(T0/T),but i need to change the power law define to : k exp(T0/(T-T1)),then i need the know how to change the source code of power law fluid in fluent,if can you help me PLEASE help me.

majid reza

Re: power law code
 

Sorry to give an answer so late; I'm interested in customizing laws for viscosity too, and I tried with your case without succeeding very well.

So, you can modify the law for viscosity in Fluent using an UDF DEFINE_PROFILE. This UDF is called in the "Material panel" in Fluent selecting "user-defined" for viscosity. In this UDF, you will define your variable for viscosity (ex: mu_app) and define a law for this variable. Then with the line "return mu_app", Fluent will consider the calculated value in the UDF as a value for the viscosity. When you define the law for viscosity, you have to access the shear rate variable and the temperature variable calculated by Fluent. This can be done using C_STRAIN_RATE_MAG(c,t) and C_T(c,t).

Now I will give you the UDF I've done. It works but the problem is that the user-defined viscosity is not initialized correctly: when you select in Fluent the classic non newtonian power law, apparent viscosity is set to the value of k at initialisation. But when you initialize Fluent with your UDF (defining mu_app=k), apparent viscosity is set to the max value (because shear_rate=0), even if you hook a DEFINE_INIT macro. So results calculated with this method are not correct.

I'm sorry to have written so much but if you find the way to initialize correctly this function, please tell me. Here is the UDF:

#include "udf.h"

real mu_app;

real k;

DEFINE_INIT(init_mu_app,d)

{

cell_t c;

Thread *t;

thread_loop_c(t,d)

{

begin_c_loop_all(c,t)

{

k=1;

mu_app=k;

}

end_c_loop_all(c,t)

}

}

DEFINE_PROPERTY(user_power_law,c,t)

{

real visc_dyn_min=0.0001;

real visc_dyn_max=10000;

real index_n=0.9;

real T0=0;

real T1=0;

real temp=C_T(c,t);

real shear_rate=C_STRAIN_RATE_MAG(c,t);

real mu_temp;

mu_temp=(-k)*pow(shear_rate,index_n-1)*exp(T0/(temp-T1));

/*!!1/pow(--)is correct only if index_n < 1; this is written like this only to set mu_app to visc_dyn_max when shear_rate is equal to 0*/

if ((mu_temp>=visc_dyn_min)&&(mu_temp<=visc_dyn_max))

{

mu_app=mu_temp;

}

else if (mu_temp>=visc_dyn_max)

{

mu_app=visc_dyn_max;

}

else if (mu_temp<=visc_dyn_min)

{

mu_app=visc_dyn_min;

}

return mu_app;

}

Re: power law code
 

Hi Antonie, Thank you very very much, i try to find it and then tell you again,thank you

mahjoob

Re: power law code
 

I've finally found the causes of the problem. To initialize correctly the apparent viscosity, I used the current iteration number macro N_ITER, so when it is < 1 (computation is not launched) apparent viscosity is set to a fixed value. Also, in my previous udf, I defined -k because I'm used to see a minus sign before k in the definition of the shear stress. But the apparent viscosity is positive so the minus sign is a source of error because mu_app always took a negative value < visc_dyn_min... I've also modified some lines of the last version of the udf because they finally weren't necessary. Now the udf works fine, I tested the case of a simple power-law and I obtained errors below 0.5% compared to the fluent integrated power-law. Here is the tested last version of the user defined power-law. Even if I don't find problems anymore, you should test it before launching important computations.

#include "udf.h"

DEFINE_PROPERTY(user_power_law,c,t)

{

real visc_dyn_min=0.0001; /*Define the minimum limit for the value of viscosity*/

real visc_dyn_max=10000; /*Define the maximum limit for the value of viscosity*/

real index_n=0.9; /*Define the power law index*/

real k=1; /*Define the consistency index*/

real T0=0; /*Define the reference temperature T0*/

real T1=0; /*Define the fixed temperature T1*/

real temp=C_T(c,t); /*Define the access to the temperature calculated by Fluent through the temp variable*/

real mu_app; /*Define the variable for the apparent viscosity which will be returned to the solver*/

real mu_temp; /*Define a temporary variable to stock the user defined apparent viscosity*/

mu_temp=k*pow(C_STRAIN_RATE_MAG(c,t),index_n-1)*exp(T0/(temp-T1));

if (N_ITER<1)

{

mu_app=k; /*Initialize mu_app to the value of k*/

}

else if

((N_ITER>=1)&&

(mu_temp>visc_dyn_min)&&

(mu_temp<

visc_dyn_max))

}

mu_app=mu_temp; /*Replace the value of mu_app by the calculated user-defined temporary viscosity when the computation has been launched*/

}

else if ((N_ITER>=1)&&(mu_temp>=visc_dyn_max))

{

mu_app=visc_dyn_max;

}

else if ((N_ITER>=1)&&(mu_temp<=visc_dyn_min))

{

mu_app=visc_dyn_min;

}

return mu_app; /*Set the value of the user-defined viscosity in Fluent*/

}

Best regards

Antoine

Thanks...this is very helpful