[shanheplus]

Hello guys, I am struggling for this problem for a long time, need for help.

I'm working on that the fluid(R134a) flow from the inlet with the saturation liquid,

then heating by the wall surface with constant heat flux,

then after transfer mass and heat in the two-phase (gas and liquid R134a),

finnally to the superheated outflow.

The flow channel is microchannel (a layer of plate heat exchanger), used for the battery cooling.

However, as the freshman, I don't know my model is right or not? And, after my simple culculation,

it's very easy to divergency, and hard to goes down the residual to a certain level.

Maybe you have some experience which can help me, please.

Thanks a lot!

---------------------

The FLUENT configuration is shown as following:


Model: RNG k-epsilon; Mixture two-phase without body force; No gravity; Steady;

The two-phase transfer UDF is defined as this logic, if t>t_sat ... else ...;

B.C.:
Inlet: R134a liquid under the saturation state in 0.3MPa. --- Mass flow inlet with 0.21 kg/s.
Outlet: R134a superheated state in 0.3MPa. -- Pressure out.
Wall: Heat flux = 12000 W/m2.
Other is no heat transfer.

--------------------

Thanks!
If there need any other data, please contact with me.

[vinerm]

There are a few important things that need to be taken care of

1. A multiphase flow should ALWAYS be run with gravity enabled. This is because there is usually a significant density ratio across the phases.

2. Material properties for vapor phase are important. Prefer using ideal gas for its density

3. A simple UDF of might invoke huge mass source term and cause divergence. Prefer using inbuilt model for mass transfer, such as, Lee model. Or include latent heat of vaporization in your UDF.

4. Since you are running a steady-state simulation, do not enable mass transfer in the beginning. Run without it and see if the flow and thermal energy conservation as well as numerical convergence is achieved. Once that is done, then enable mass transfer.

[shanheplus]

Firstly, thanks a lot.
Then,I want to simulate a steady results, which the refrigerants boil in the channels. The difficulty is the boiling two-phase process.

So, I don't know what multiphase model is correct or appropriate.
For point 2, I just used the polynomial kind to define the gas and liquid R134a. Should I use the idea-gas for its density?
And, this UDF is what I search from the Internet. Maybe I can show you. I don't understand what is the inbuilt model. Maybe I should see some tutorial.

Thanks again,
Best wishes.

[vinerm]

A tutorial would certainly be a better idea. However, first you need to look at the expected morphology for the conditions you have. Boiling of a liquid usually have multiple regimes and those depend up on the temperature difference between wall and saturation temperature. If this value is very high, it could lead to wall or film boiling. Then you will have to use wall boiling models available under Euler-Euler. If the temperature difference is not very high, then you can use Lee model or Thermal Phase Change Model. Both of these are available under Mass Transfer. Once you enable, say VOF multiphase model, these models are available under Phase Interactions > Mass Transfer; right where you have hooked the UDF.

[shanheplus]

Originally Posted by vinerm

A tutorial would certainly be a better idea. However, first you need to look at the expected morphology for the conditions you have. Boiling of a liquid usually have multiple regimes and those depend up on the temperature difference between wall and saturation temperature. If this value is very high, it could lead to wall or film boiling. Then you will have to use wall boiling models available under Euler-Euler. If the temperature difference is not very high, then you can use Lee model or Thermal Phase Change Model. Both of these are available under Mass Transfer. Once you enable, say VOF multiphase model, these models are available under Phase Interactions > Mass Transfer; right where you have hooked the UDF.

Thanks.
In this project, firstly I use 'mixture' model. And, assume it boling in the saturation temperature. So I just use the UDF. The UDF is at the end.

And, maybe further the real condition is that another side fluid's tempeture is 20C. This side R134a is 3C. So maybe this difference make it use Euler-Euler model- Wall boiling model?

I'm nervous because Im NOT familiar with multiphase flow model.
Thanks again.

UDF:

#include "udf.h"
#include "sg_mphase.h"
#define T_SAT 273.8221
#define LAT_HT 198091.4

DEFINE_SOURCE(liq_src, cell, pri_th, dS, eqn)
{
	Thread *mix_th, *sec_th;
	real m_dot_l;
	mix_th = THREAD_SUPER_THREAD(pri_th);
	sec_th = THREAD_SUB_THREAD(mix_th, 1);
	if (C_T(cell, mix_th)>=T_SAT)
{
m_dot_l=-100*C_VOF(cell,pri_th)*C_R(cell,pri_th)*fabs(C_T(cell,mix_th)-T_SAT)/T_SAT;
dS[eqn]=-100*C_R(cell,pri_th)*fabs(C_T(cell,mix_th)-T_SAT)/T_SAT;
}

else {
m_dot_l = 100*C_VOF(cell,sec_th)*C_R(cell,sec_th)*fabs(T_SATC_T(cell,mix_th))/T_SAT;
dS[eqn]=0.;
}
return m_dot_l;
}


DEFINE_SOURCE(vap_src, cell, sec_th, dS, eqn)
{
Thread *mix_th,*pri_th;
real m_dot_v;
mix_th = THREAD_SUPER_THREAD(sec_th);
pri_th = THREAD_SUB_THREAD(mix_th, 0);
if(C_T(cell,mix_th)>=T_SAT)
{
m_dot_v = 100*C_VOF(cell,pri_th)*C_R(cell,pri_th)*fabs(C_T(cell,mix_th)-T_SAT)/T_SAT;
dS[eqn] = 0.;
}

else {
m_dot_v = -100*C_VOF(cell, sec_th)*C_R(cell, sec_th)*fabs(T_SATC_T(cell,mix_th))/T_SAT;
dS[eqn] = -100*C_R(cell, sec_th)*fabs(C_T(cell,mix_th)-T_SAT)/T_SAT;
}
return m_dot_v;
}


DEFINE_SOURCE(enrg_src, cell, mix_th, dS, eqn)
{
Thread *pri_th, *sec_th;
real m_dot;
pri_th = THREAD_SUB_THREAD(mix_th, 0);
sec_th = THREAD_SUB_THREAD(mix_th, 1);
if (C_T(cell, mix_th)>=T_SAT)
{
m_dot= -100*C_VOF(cell, pri_th)*C_R(cell, pri_th)*fabs(C_T(cell,mix_th) -T_SAT)/T_SAT;
dS[eqn] = -100*C_VOF(cell,pri_th)*C_R(cell,pri_th)/T_SAT;
}
else
{
m_dot =100*C_VOF(cell, sec_th)*C_R(cell, sec_th)*fabs(T_SAT -C_T(cell,mix_th))/T_SAT;
dS[eqn] =100*C_VOF(cell, sec_th)*C_R(cell, sec_th) / T_SAT;
}
return LAT_HT*m_dot;
}

[vinerm]

You have to find multiphase regime diagram for R134a. Each fluid has its own regimes. For water at 1 atm., even 110 can cause wall boiling, i.e., vapor bubble formation. For R134a, this could be different. You can use the UDF but do note that in the UDF, saturation temperature is considered as 0 C and latent heat is NOT as per R134a. So, you have to provide correct numbers in the UDF before compiling. For the beginning, just use the UDF. This will work because it is using Latent Heat in its formulation.

[shanheplus]

Originally Posted by vinerm

You have to find multiphase regime diagram for R134a. Each fluid has its own regimes. For water at 1 atm., even 110 can cause wall boiling, i.e., vapor bubble formation. For R134a, this could be different. You can use the UDF but do note that in the UDF, saturation temperature is considered as 0 C and latent heat is NOT as per R134a. So, you have to provide correct numbers in the UDF before compiling. For the beginning, just use the UDF. This will work because it is using Latent Heat in its formulation.

Thanks. I will consider and study more.
Best wishes!

[vinerm]

Sure. Studying will be a good idea. In the mean time, you can certainly work with the UDF. Just use appropriate numbers in the UDF as per the fluid you have.