Boiling in annular pipe

  • 76 Views
  • Last Post 02 April 2020
  • Topic Is Solved
ham_nola posted this 25 March 2020

Hi

I tried to simulate this case as described in the ANSYS Fluent help document! I cannot converge this case. Any help!

I hope ANSYS moderators could share the case file as in the documents a lot of these settings are missing! I simulated this exact case as a steady-state but it doesn't converge. My guess is the mass-created due to boiling is so fast that the solution diverges!!!

Thank you.

Regards

Hamed.

Order By: Standard | Newest | Votes
Kremella posted this 26 March 2020

Hello,

Could you please share the settings you used for your model? We won't be able to answer convergence related questions without the knowledge of how you set up the problem. Please provide us with some more details.

Also, which Fluent tutorial is this? Where did you find this information?

Thank you.

Best,

Karthik

  • Liked by
  • ham_nola
ham_nola posted this 27 March 2020

Hi Karthik

Thank you for your response.

The main details of my setup are:

1. Eulerian-Eulerian model is used to simulate two-phase flow inside the domain.

2. Water under saturated conditions (590 K) entering the annular domain.

3. Energy supplied at the inner wall of the annular domain with the heat flux of 1027500 W/m^2.

4. Evaporation-condensation model: thermal phase change model.

5. Saturation temperature for the phase change is constant = 590 K

5. Operating pressure of 108 bar = 1.08e+7 Pascals

6. The domain has mass flow inlet and pressure outlet.

Note: I will attach below the complete details of my setup. 

 

These snapshots I shared earlier the help I found with reference to the use of Fluent's thermal phase change model from the ANSYS customer portal. 

Thank you.

Best regards,

Hamed.

ham_nola posted this 27 March 2020

ham_nola posted this 27 March 2020

I tried the simulation with low value of heat flux at the wall like for example for heat flux = 100 and 1000 W/m^2 and it works. The numerical calculations make perfect sense with the hand calculations.

However, for the given heat flux of 1027500 W/m^2 the solution diverges!

Thank you.

 

Best regards,

Hamed.

Kremella posted this 30 March 2020

Hello Hamed,

Have you tried to ramp up the heat flux slowly (as a function of time, perhaps)? Also, what is the total input power (in W) for your system based on your higher number? Is this greater than CHF?

Thanks.

Best,

Karthik

ham_nola posted this 30 March 2020

Hi Karthik,

Yes. I tried ramping up the heat flux and the steady-state cases work for 0 W/m^2, 100 W/m^2, 1000 W/m^2. But the steady-state case for 10,000 W/m^2 diverges. Based on the hand calculations as shown in the above figures it shows converged solution in the ANSYS Fluent help!

The total input power based on the heat flux at the walls is 91029.2 Watts.

I am not sure about the Critical Heat Flux (this is done below), could you elaborate a bit further how would that affect this simulation! You mean that the vapor initially created would take up all the heat and as a result, the temperature of the vapor becomes extremely high and the solution diverges! That could be the case, but I am not sure!

Thank you for your help.

Best regards, 

Hamed.

 

ham_nola posted this 30 March 2020

Some of the questions I had, if you could kindly answer them as well:

1. My primary fluid is water-liquid and secondary fluid is water-vapor. Is that okay? It because I have saturated liquid water entering the domain.

2. I initialized the domain first by turning off the evaporation- condensation model and converge the results. Once the results are converged I kick in the evaporation-condensation model. Is this okay?

2. When defining the materials, water-vapor and water-liquid should I let the standard state enthalpy be the default values or should I change it! What I did was        --> water-liquid standard state enthalpy = 0 

      --> water-vapor standard state enthalpy = latent heat * molecular weight = 1263.2 e+3 J/kg x 18.0154 kg/kmol = 22.76 e+6 J/kmol

3. What about the "reference temperature", I define it as 590 K which is the saturation temperature of the domain.

4. What should be the outlet volume fraction! Currently, I define it as from the "neighboring cell". Do you suggest I calculate it form the mass flow of vapor at the exit (hand calculations)? How could I convert it to a volume fraction value at outlet value!

Thank you.

Regards

Hamed.

ham_nola posted this 31 March 2020

Dear Karthik,

The Critical heat flux (CHF) is 4.118 MW/m^2. The heat flux provided at the inner wall is 1.0275 MW/m^2. Thus, the critical limit is not exceeded!

Kremella posted this 31 March 2020

Hello,

Why are you running a steady state model? Could you please try transient?

Also, what is the end goal of your simulation? Are you looking to evaporate water and generate steam?

Here are some answers.

1. yes.

2. What are your initial conditions? Where is your interface located? What happens when you run the model with evaporation - condensation model turned on?

2. Yes, this is okay.

3. Yes, it is okay to use Tsat as Tref.

4. Outlet VF comes into effect in case of backflow. You should pick your boundary in such a way that in the event of a backflow, you only have a single phase flow across (either liquid or vapor).

Please help us understand your end goal here so we can help better.

Thanks.

Best,

Karthik

  • Liked by
  • ham_nola
abenhadj posted this 01 April 2020

you want account for boiling in the annulus? Perhaps I might overlook the settings but are you enabling the boiling model. The first picture you posted is from some work I adjusted a couple of months ago.

Best regards, Amine

  • Liked by
  • ham_nola
ham_nola posted this 01 April 2020

Hi Amine,

Thank you for your response.

Yes, I want an account for how the model was set up to get the required results as shown in the help from ANSYS (shown above).

No, I am not using the boiling model. The evaporation-condensation model is used instead! I am exploring how the evaporation-condensation model operates!

Thank you.

 

Regards
Hamed.

ham_nola posted this 01 April 2020

Hi Karthik & Amine

Thank you for your responses!

Initial condition

The domain is initialized with standard initialization from the inlet. The domain is initially filled with saturated water liquid and a velocity of 0.29 m/s (calculated from the mass flow rate of 3 kg/s at the inlet). The vapor volume fraction initially is zero.

I define the inlet static gage pressure as 0 Pascal (I tried running cases with 15 Pa as well).

The operating pressure is1.08e+7 Pa.

 

Solution

Fortunately, I got the result of the volume fraction of vapor I was trying to do. Below is the vapor volume fraction contours in the domain.

My problem was I didn't consider that the density of water vapor at 1.08e7 Pa should be 61.223 kg/m^3. Also, I had to correct the enthalpy and give is values as explained above.

The vapor mass flow rate at the outlet is 0.0701 kg/s which is less but comparable to 0.072 kg/s calculated by hand-calculations!

ISSUES

(1). The issue I have is regarding the pressure inside the domain. It is negative pressure at the inlet!

My question would be that does that make physical sense? Here are the contours.

(2). Also, why is the static temperature of the liquid and vapor much much higher than the wall adjacent temperature? Please see contours below

Thank you.

Best regards,
Hamed.

 

abenhadj posted this 01 April 2020

First of all your are looking into gage pressure check absolute pressure values. The values you are showing the maxima correspond to the wall temperature. If you disable node values and show the values again they would correspond to the phase values: Node values at wall are wall temperature

Best regards, Amine

ham_nola posted this 01 April 2020

Thank you for the prompt response!

I plotted the absolute pressure values (see below). My issue was not just with negative static gage values. Why is the inlet pressure less than the outlet pressure, the flow is from left to right! 

About temperature contours, you are right that if I turn off the node values the wall adjacent temperature and static temperature correspond to each other.

My question would be what value to report? Static temperature or wall adjacent temperature, could you elaborate, please!

Thank you.

Best regards

Hamed.

abenhadj posted this 01 April 2020

Static temperature. Regarding pressure it does not make sense. Check surface integral of absolute pressure and set operating density to zero.

Best regards, Amine

ham_nola posted this 01 April 2020

Perfect, it works with operating density set to zero!

Thank you Amine and Karthik!

Best regards,

Hamed

ham_nola posted this 02 April 2020

Hi Amine

I had a final question regarding the temperature. Below are the static temperature of vapor with and without node values. I'm confused as to which value to report? The temperature of 1737 K with node values ON, is a huge number!!

From what I understand

Thank you.

Best regards,

Hamed.

 

abenhadj posted this 02 April 2020

you always report cell values. Do not show here plot with node values or do not use global range.

Best regards, Amine

ham_nola posted this 02 April 2020

Thank you Amine. 

Regards

Hamed.

Close