[fkhan7]

Dear friends and CFD users,

I am currently performing a parametric study on thremocline in a tank for thermal energy storage, and I thought that it would be a good idea to start logging some of my findings for your comments and remarks. My goal is to eventually compare the CFD results to an experimental set up, which is being build right now.

the following is what I have done so far:

1. I am using Ansys CFX in 3D
2. 2D simulation was not recommended by previous literature therefore I am using a 3 D model
3. My tank is symmetrical, however modeling half or one quarter of the tank has provided faulty results
4. enabling buoyancy and gravity was a good approach to to get a thermocline to form
5. I am assuming an adiabatic wall

I was wondering if anybody else is performing similar studies on thermocilne CFD simulation where we can exchange experiences.

so far the results I am getting are very good but i have to wait for experimental validation.

thank you all and looking forward to hearing from you

Fahad

[pedroa72]

Originally Posted by fkhan7

Dear friends and CFD users,

I am currently performing a parametric study on thremocline in a tank for thermal energy storage, and I thought that it would be a good idea to start logging some of my findings for your comments and remarks. My goal is to eventually compare the CFD results to an experimental set up, which is being build right now.

the following is what I have done so far:

1. I am using Ansys CFX in 3D
2. 2D simulation was not recommended by previous literature therefore I am using a 3 D model
3. My tank is symmetrical, however modeling half or one quarter of the tank has provided faulty results
4. enabling buoyancy and gravity was a good approach to to get a thermocline to form
5. I am assuming an adiabatic wall

I was wondering if anybody else is performing similar studies on thermocilne CFD simulation where we can exchange experiences.

so far the results I am getting are very good but i have to wait for experimental validation.

thank you all and looking forward to hearing from you

Fahad

I'm working in thermocline simulations with ansys fluent (2D and 3D). I'm having problems in achieve a full thermocline (small distance between high and low temperature). In my cases, the thermocline expands to 60% of tank total height.

regards

[FluidCFD]

Hi,

I'm working on a stratified hot water storage tank for solar application or industrial waste heat (height: 4 m, diameter: 2 m). To reduce simulation time I use a slice of the cylindrical tank with a height of 1 m. The inlet stratifier is situated in the middle of the cylinder with one fluid outlet. In the real tank there are six of them distributed over the height. I'm struggling with setting correct outlet/opening boundary conditions. As the water in the real tank can flow to the fluid below the slice over the whole circular area of the tank I wanted to set this face as outlet/opening. Do I have to put a relative pressure of e.g. 100 mbar there to tell CFX there is a water layer below the simulated slice which supports it? If not how does CFX know the fluid layer won't just fall out of the tank in gravity direction? I use a transient simulation with buoyancy and turbulence, btw.

Any help is appreciated.

Regards
G.

[ghorrocks]

An image of what you are talking about would help.

[FluidCFD]

Hi,

just for visibility of the stratifier I suppressed the rest of the cylindrical tank. The water enters at the upper part of the stratifier, goes through it and leaves the stratifier at the outlet into the tank. The circular area I was talking about is at the bottom of the tank. Hope this helps to explain my problem.

Best regards
G.

[ghorrocks]

The image helps but I have no idea what it means. You are going to have to label what the important components are, and what the fluid is expected to do in it.

[FluidCFD]

Hi,

new try with new image. At the beginning, the storage tank has a uniform temperature of 26 °C. Hot water of 67 °C enters at the inlet of the stratifier and leaves it at the bent outlet. The cold water in the tank is displaced by the hot entering water and should form a hot layer at the top of the tank. The cold water leaves at the bottom of the tank. The flap is there to force the water to flow out rather horizontally than vertically to guarantee a good stratification and no mixture of the different temperatures.

I hope I made it clearer now.

Best regards
G.

[ghorrocks]

Yes, that explains what you are doing a lot better.

Some comments:
1) Is the level of the fluid free surface constant? If so can the free surface be replaced with a wall or a pressure boundary? Then the simulation is a single phase and that is far simpler. You may have already done this.
2) Fluid will not travel out the bottom boundary when it is in equilibrium with the fluid head above it. So if there is 10m of water above it you need to apply about 1 atmosphere and it should keep steady. But note with bouyant flows the pressure is modified with the hydrostatic pressure - read the documentation and the tutorials about this.

[FluidCFD]

Hi,

thanks for your reply, it's really amazing, how often you can provide help.

There is no free surface, the upper boundary is a wall, as this is the lid of the tank. So that's already done.

To check if I got you right: I have a height of 1 m, so I have to apply 100 mbar as relative pressure at the outlet/opening at the bottom of the tank slice. I checked this before the CFD forum post already, but then the absolute pressure jumps at the bottom (see image). There is 1.1 bar due to hydrostatic pressure, but the relative pressure adds on this to 1.2 bar? Is this how it should be?

G.

[ghorrocks]

Your domain is closed so you don't know what the pressure is at the top of the tank. So the pressure at the bottom of the tank is 100mbar above an unknown number - so that is unknown.

Can you explain to me how this flow is driven? I don't mean your simulation, but the real device - what pushes fluid in the inlet and what happens after it leaves the outlet?

[FluidCFD]

I set the reference pressure of the domain to 1 bar and define the top of the tank as the ref location, so both pressures are actually known. Now the question is whether to put 0 or 100 mbar as the relative pressure at the opening at the bottom of the tank?

The water is pumped into the tank. According to the density of the entering fluid which depends on its temperature it will leave the stratifier at the appropriate outlet. All this is done just by physics, not with valves.

If the tank is not yet stratified (the containing water has a low temperature) and hot water is entering, it will leave the stratifier at the topmost outlet. If there are already different temperature layers it will leave the outlet where the upper layer is hotter and the lower layer is colder than the entering fluid. The perfect result now would be that a mid-layer between the existing layers is established where the entering temperature is preserved and doesn't get mixed with the other temperatures. So the outlet has to be designed in a way that this is reached as perfectly as possible.

If the tank is used as a solar tank where solar collectors deliver the hot water the aim is to make this hot water available for domestic hot water immediately by storing it just in the upper part of the tank without having to heat up the whole tank first.

[ghorrocks]

If the tank is closed then you do not know the pressure at the top. Assigning that point the reference point does not fix the pressure to zero relative pressure.

The pressure will be regulated by some mechanism. It might be a pressure relief valve, it might be a free surface, or it might pressurise the entire tank so the elasticity of the tank determine the pressure. Which one is it?

[FluidCFD]

Ah, the tank is pressurized up to 3 bar, then the safety valve opens.

[ghorrocks]

So the pressure ramp up can be modelled with the safety valve closed (ie a wall) and the open period as a pressure outlet.

But linear buoyancy models do not care about the absolute pressure, the buoyancy only comes from temperature differences. So you have to decide whether this 3 bar pressure is important for what you are modelling.

[FluidCFD]

What do you mean with open period?
And to come one last time to my first question: Do I have to put 100 mbar as relative pressure at the outlet or not?
Any further advice for this setup and simulation?

And thanks a lot for your help!

[ghorrocks]

To answer whether you need the pressure on the bottom I need to know a little more about what you are doing:

Is the image on post #7 the full simulation domain? Is there anything else you are modelling?

What buoyancy model are you using?

In the real device, what is below your bottom boundary condition? Is there a wall, more tank or some other structure?

In the real device, when fluid flows into the tank what happens? Is the tank enclosed and the same amount of fluid flows out? Or does the tank level rise? Or does something move?

[FluidCFD]

Post #7 shows the full simulation domain (3D of course as can be seen in #5).

Buoyancy model is "Buoyant", so I guess it's the full buoyancy model.

Below the bottom BC is more tank, i. e. 3 m of water with the rest of the stratifier.

The tank is enclosed, so the same amount of water flows out. In this case to the water layers below the simulated slice. The tank is rigid, nothing moves, no free surface.

Attached a CAD model so you can see how the real device looks like. The outer tank is not relevant for this simulation it holds the insulation.

[ghorrocks]

In that case I would not put a pressure boundary on the bottom surface. I would just model the entire tank with its external wall, that is include the botttom half of the tank as well. Then there is no doubt what type of boundary condition to use. And you can mesh it with a coarse mesh so it does not add too much to the simulation time. In fact convergence will be much easier with the full tank model and it may well run faster than the top half model with a boundary condition with numerical stability problems.

Then you only have to put boundaries on the inlet and outlet and that should be straight forward.

[FluidCFD]

Sounds like a good idea.

Greetz to Aussieland!

[FluidCFD]

Now I have done some simulations with low mass flow which I can compare with experimental data. Using k-epsilon-model which was found out to be the best turbulence model for such tanks by experts on this topic, yields too much mixing of the fluid and therefore too low temperatures in the hot layer of the tank. I know from visual tests that the flow in the experiments is turbulent, at least for small scales, because schlieren are visible.

Doing the same simulation with laminar conditions I can reproduce the experimental data. Calculating the Re number with those results shows that there should be turbulence in the near region at the outlet of the stratifier.

The aim of my simulation is actually to find out what happens at high mass flows (e.g. 2-4 m³/h) because there are no experimental data available for this setup. To do this I need to know when it is necessary to use turbulence models to correctly describe my problem.

Conditions are: free stream with mixed convection (forced and free convection), high density gradients. I would like to know the Reynolds and Rayleigh numbers that define the transition from laminar to turbulent for this case.

Anyone had the same experience? Switching on turbulence seems to mean that if there is a laminar flow, it can't be computed. Help is much appreciated although I know the question is just partly CFD stuff!