Solar Heating for Swimming pool

[kadenlh]

Hey Guys,

Would you guys kindly give me a hand on my simulation.

I need to simulate a swimming pool (50mX17m,2.5m deep) with inlets and outlets inside the pool under solar heating condition for 24 hrs.

I search over the google page and also the CFD tutorial but found nothing relevant to my case.

*you may find the model above for your information

I would like to know:

1.Is it actually possible to simulate this case in autodesk CFD?

2.As I can't make an air box surrounding/above the pool (error: dissimilar fluids in contact), how should I simulate the fluid circulation and also the solar radiation properly?

Please would anyone help me on this.

Thanks a lot.

[Jon.Wilde]

Hi,

We should be able to do this, yes. What do you have set as inlets and outlets? Make sure you don't over constrain the model.

For the solar loading, how about a solid 'window' material on the top surface with air above it? Thought that might be a nice work around.

Thanks,

Jon

[kadenlh]

Hi Jon,

Thanks for your prompt reply.

Please find the attached file for your information.

I think i didn't set too much constraints to the inlet&outlet (only volumetric flow rate is applied to the inlets while the outlets are kept under P=0).

However, I still don't understand much about the solar heating.

No temp difference has been observed after simulation.

Please would you guide me on this. Thanks again.

[Jon.Wilde]

Hi,

You have no thermal boundary conditions to set an ambient temp so CFD will not be able to work thermally. What temp is the water entering at, what is the ambient air temp?

Test the difference between a surface and solid piece of glass - not sure if you might need a solid here.

Also, don't forget to increase the conductivity so that it isn't preventing heat being lost to air.

Thanks!

Jon

[kadenlh]

hi Jon,

Sorry that I missed to include the temperature, actually I set the air temperature of the air to IC = 35degC before, but I didn't see any effect from the solar for both the air and water.

Now I change it to BC with velocity = 3m/s into the air, and the water inlet temp  =20degC, but still, i can't see any temperature variation in the water.

(would you kindly guide me more in detail?)

And there are some other issues to be solved:

1. Actually the inlet water temperature should not be specified since the water will be recirculated after gaining solar heat, the temperature at the inlet and the outlet should be recalculated with the solar heating. (so should I assign IC for the water in this case?)

2. I changed the temperature of the air to a transcient scale as I want to simulate the solar variation within a day. But the simulation kept diverging, how should I set an transicient solar simulation with aambient temperature varying? would you please give me an example?

[Jon.Wilde]

1. OK then you need initial conditions (Temp) and to run this as a transient study. All parts will need an initial temperature. The outlets would also need to be connected to the inlets - if the water is recirculated (try an internal fan material)
2. Did you set a temp to the incoming air?
3. What time step size are you using within the Solve Window?
4. Also, have you run through our tutorial models?

[kadenlh]

Dear Jon,

Please find the 2 cases below for your information.

Case 1 refers to my original model,all parts included (I would like to use the solar function in solver window).

Case 2 refers to the model with air and the recirculation volume removed (heat flux BC is used to replace the solar function, transicient simulation applied) However, the result temperature during afternoon raised above the expected value (I believe this is because heat loss is not included?)

Please would you suggest which case I should keep if I would like to see the 24 hr temperature variation for a pool under solar heating?

And to reply your msg, 

1.I tried the internal fan material before, but as shown before, the flow will be in opposite, firstly Y direction and then the Z direction. But all the pump/fan functions can cater only one direction right?

2. 35 degC incoming air is used.

3. For Case 1, I still can't simulate the transcient case yet. As from Case 2, 864sec is used with internal interval =10 

4. Sure Jon, I went through all the relevant tutorials already, I believe I understand the use of transcient as you may see from Case 2, however I still don't know how to apply that into the solar radiation model. There is not much guide about solar simulation in the tutorials, please would you give me a more insight into this?

I am frustrated with the solar function and the case 1 result. Please help Jon  Thanks.

[kadenlh]

hi all,

I am still not getting any progress for days

please would anyone help me on this?

Thanks a lot

[Jon.Wilde]

I can try to help here.

Case 2 has no temperatures on the water inlets

Your time step size is too large, are you running flow first as Steady State to get the velocity converged and then running heat transfer only as transient? This is the best way I think. With a 864s time step, CFD is not going to establish a flow field, you would need something closer to 0.5s.

Even when you run the heat transfer only transient model, use something like 5s or 10s.

Case 1 has too many Boundary Conditions, just have flow going in one direction, or as it is nearly zero, use the guide I shared before and model proper natural convection in the air.

Your air is set to fixed, is that OK? There will be no natural convection taking place right now.

We need to avoid internal Boudnary Conditions - so ensure that they are all on model 'boundaries' and not embedded inside. You can suppress adjacent parts to help you do this, then it is OK for them to be within the model, so long as they are attached to a suppressed volume.

Both of these should run OK if you follow the guidelines I shared before and what I listed here.

Thanks,

Jon

[kadenlh]

Hi jon,

Thanks for your reply.

I understand your points ,however, I think the problem now is I am still not clear with the main way to find solution, not even close one...

please let me clarify my situation now again:

I have a swimming pool with 1. recirculation of the water 2. under solar heating for 24 hrs

I would like to know how will the temperature of the swimming pool and water in the recirculation vary for 24 hr under the solar heat. 

The water recirculating is assumed to be same temp as the lower level pool water (near outlet).

We are expecting to see a higher temp(~37) near the pool surface. 

So I tried many different ways for  Modelling and also BC conditions

For modelling

1.Case 1 with air box above and with water box connecting the inlet and outlet of the pool, glass added between water and air

(yes this will create internal BC but I thought u said if I need to simulate recirculation, I need to connect the inlet and outlet together?)

2.Case 2 just the pool itself

(I didnt specify the inlet temperature since it is not fixed, it will follow the pool heat gain as mentioned before)

3.Case 3 that I attached, no air box, just recirculating system.

(But internal BC still exists)

So actually which one should I use/none of above, for my case?

Is it really possible for autodesk to solve this? 

and what's more,

Please would you tell me which one I should use below to simulate the solar heat gain:

1. solar heating in solver (never succeed as the water temperature never rise)

2. heat flux in BC (results:temperature on surface rise above expected)

These two cases both can't meet the result, and seems like heat loss from water surface and pool wall cannot be simulated (I used film coefficient and it gives error)

Please would you give me the direction first?

I don't think I am even on the right track

[Jon.Wilde]

Hi,

If your inlet temp needs to be the same as your outlet - shouldn't they be connected with a pump to drive the flow? (Not an internal BC)

If you do not have an inlet temp - the water will not change in temperature as CFD doesn't know what temperature to start from - you must have some temperature assigned to the inlet, or have it connected to the outlet. It is similar to me asking you to calculate the temperature of a room that has incrased by 10C but not telling you the initial temperature 🙂

Yes, this should be simple. Avoid internal boundary conditions if you need the inlet temperature to match the outlet temperature and just model the system.

Run a steady state simulation initially to get a flow field.

Reset the initial conditions and run transient from that point onwards.

Personally I would lean towards the solar loading option, but only as it might give you a more accurate heat loss as the air moves.

Please also use the natural convection guide I shared before to model the air box above the water.

Thanks,

Jon

[kadenlh]

Dear Jon,

Really thanks a lot.

so getting back to the pump issue, as mentioned before, I tried the internal fan material, but as shown on the first post, the flow will be in opposite direction, firstly Y direction(both +/- ) and then the Z direction. But all the pump/fan functions can cater only one direction, how is it possible to set it?

For case 2 I tried to apply an initial temperature to the inlet or the water volume, but still no use for the heat simulation, the temperature still didn't change for solar function. 

Sorry I am confused, if simulating recirculation needs to connect both inlet and outlet together, then those BC must become internal BC right? 

and also, which model should I use for my case actually? Case 1/2/3 would be better?

[Jon.Wilde]

All volumes need Initial Temperatures

The inlets need a Boudnary Condition of flow and temp (OR to be connected to the outlets so there is a constant recirculation)

Using a fan material is fine - each would be assigned the right direction - so you would assign each side separately.

Fans need a good uniform mesh with 4-5 elements from inlet to outlet - use Advection Scheme 5.

Does that help?

[kadenlh]

Dear Jon,

As shown below, this is the section for my model, I modelled two fans at the two sides, but the problem is the bottom one, if I separate it in the middle as shown, error comes up. Should I also model the bottom box as fan as it contains two directional flow.

Also, do I need that air box for solar simulation? is it necessary? Can you please let me know which case, Case 1 or Case 3 is the better one?

[Jon.Wilde]

If one option works and one fails - pick the one that works 🙂

The choice on air box is really yours - depending on how much information you wish to capture and the goal of the analysis. If you are only adding heat to the model then a heat flux should be OK. I am not sure if this will work with a film coefficient to allow heat to escape though, which is where an air box might be better - it will allow the water to lose heat more accurately.

[kadenlh]

Hey Jon,

I tried like fifty times for different models, none of it is even close to the result...

I think accurancy is not the major concern for me, I don't even need to be too accurate right now, I just want a successful trial.

I tried the most simplified way, even just a pool without any inlet, inital temperature = 30degC, under solar for 24 hrs.

NO temperature change is observed. Would you kindly provide any example for Autodesk CFD to cater for water heating under solar?

It just doesn't seem like the solar function is working.

[Jon.Wilde]

Please share this simplified model with me and I will take a look

[kadenlh]

Dear Jon,

Attached please find the model.

For a single time solar simulation using steady state->no temperature change

For a 24 hr solar simulation using transcient with large/small timesteps (tried both)-->Error appear

Please help, Thanks.

[Jon.Wilde]

I would expect this behaviour. You could run this with a heat flux on the top surface but for the solar model, you need an air dome/box modelled as you had before.

Your mesh needs a lot of refinement too - at the moment there is only one element from the top to the bottom of the volume. Start with something like a uniform mesh refined down to 0.7 for example (I tested this, it's a little coarse still).

Turn off radiation (no air and only one part so no need for it), I also turned off flow and turbulence as a quick example, it runs fine:

Animation of it heating up here (obviously this isn't going to be realistic but it gives you an idea).

Hope that is useful

Jon

[kadenlh]

Dear Jon,

Thanks a lot for the simulation.

I am having the same thing currently.

But I got another problem now, I can't see the saved iteration.

My setting for the solver is:

Time Step Size = 10

Inner Iterations = 1

Results Output (Under Save Intervals) = 864

Continue From = 0

Time Steps to Run = 8640

This is to run 86400 seconds for 24hrs simulation.

However, I used either the table/ result under the save intervals option, I was not able to get the result for intermediate steps for both methods, what is wrong with this?

I already simulated the case for a few times without getting the profile at last...