[Rimzy]

Hello,

Description: I am simulating evacuated tube solar collector inclined at 45 degree. Its like double pipe heat exchanger. It has outer tube as glass tube and inner tube as copper. between glass and copper tube there is vacuum and its closed. inside metal tube there is fluid domain where water flows.
Meshing: nodes 35416, elements 419176, avg. aspect ratio 3.67
Solver: pressure based, steady state, including gravity effect
Model: I am using Laminar flow, energy equation on,
BCs: pressure inlet and pressure outlet. applying 1200 w/m^2 heat flux on glass tube and 1150 w/m^2 on metal tube. All other wall are by coupling.
Solution method: SIMPLE . Second order discritization

From last two days i am getting error 'divergence detected in AMG solver: Pressure correction'. I tried some answers posted but it did't work for me. Now i am exhausted. Please give me some solution. Anything wrong with my model? Please help

[vinerm]

There are a few things that you need to check.

1. Does your case have a natural convection or forced convection (in the water domain)? If it is forced, then you may or may not require gravity. If it is natural, you certainly require gravity, however, you also need to ensure proper model for water density.

2. Have you checked Re or Gr (or Ra) number before running the simulation? Are you sure it is laminar? If it is not, Fluent will not be able to converge at all.

3. From the BCs, it appears that water is flowing in and out, i.e., forced convection. Why gravity and, again, why laminar?

4. Since the simulation is steady-state, don't start your case from second-order. Always run first 200-500 iterations, depending upon the complexity of the physics and mesh, using first-order.

[Rimzy]

Originally Posted by vinerm

There are a few things that you need to check.

1. Does your case have a natural convection or forced convection (in the water domain)? If it is forced, then you may or may not require gravity. If it is natural, you certainly require gravity, however, you also need to ensure proper model for water density.

2. Have you checked Re or Gr (or Ra) number before running the simulation? Are you sure it is laminar? If it is not, Fluent will not be able to converge at all.

3. From the BCs, it appears that water is flowing in and out, i.e., forced convection. Why gravity and, again, why laminar?

4. Since the simulation is steady-state, don't start your case from second-order. Always run first 200-500 iterations, depending upon the complexity of the physics and mesh, using first-order.

Dear Vinerm, thank you for your kind response.

1. YES, its natural convection case with gravity i have put in -Z direction. For density i am using constant density of water. Now, you have pointed it out that i should have function of it. I will consider it.
2. I have not checked Re or Ra number because i do not have experimental mass flow rate or velocity of fluid. Basically, mass flow rate is problem for which i am using CFD otherwise i am getting temperatures at inlet and outlet of tube experimentally. I used Laminar model on the basis of literature review as relevant studies for natural convection in solar evacuated tube used this model. is there any other method to compute Ra/Re number?
3. YES, water is flowing in at inlet and out at outlet of tube. But, the case is not forced. Its naturally driven heated by the solar flux at outer tube surface, called thermosiphoing. Is anything worong with BCs?
4. Noted

[vinerm]

1. Gravity will not have any effect until it sees any density difference. Now, for water, Boussinesq is good enough. Do note that you have to set correct reference values for density and temperature in the Operating Conditions dialogue box.

2. You do not need any experimental data to calculate Gr. It is based on temperature difference, length scale, and properties. You can use length or diameter of the duct as length scale, maximum temperature difference expected as temperature difference to calculate Gr. If Gr > , enable turbulence.

3. BCs are good for natural convection

4. If flow rates are not very high due to natural convection, you may have to run a transient case because there could be a lot of recirculation within the domain and close to the outlet.

[Rimzy]

Thank you. very valuable information. The problem of divergence was in material properties. Basically there is vacuum between glass tube and metal tube. In fluent properties, i changed the properties of air to make it vacuum like zero density and zero specific heat. There was the problem. When i changed back into air solution was running succesfully for 200 iterations. I do not know how i ask Fluent to understand Vacuum because in vacuum only mode of Heat Transfer is radiation. but in fluent prperties there is no radiation mode. there is convective and conduction properties. Now, my solution ran successfuly as i have set bossinesq approx for density(994.67 kg/m3 as operating density and material density too at 303 K) in steady state but I am getting horrible results like 1.33m/s velocity at outlet which is impossible in this natural convection . expected is 25 to 32 mm/s. even at outlet is less than inlet may be due to recirculations. same is the case with temperature at glass tube its more than 1000 K because of poor HT from glass to next material.
For your above valuable points,

1. Used Boussinesq approx. and inserted same value of density in opt. conditions as in material properties. But i am wondering as in my case expected temperature difference is about 10 K. I am not sure Boussinesq work or not.
2. Noted. I have expected temperature difference, i think i can calculate Gr.
3. Thanks.
4. If i use transient then there will be no Boussinesq approx. then i should define new density function?

Thanks

[vinerm]

You need to specify the vacuum as vacuum; Fluent will not understand that on its own. Nor will it understand 0 pressure and 0 density. Vacuum implies no fluid, i.e., do not create a domain where vacuum exists. Then the boundaries will become outer wall boundaries and you can apply radiation boundary. Furthermore, for radiation to be available inside a domain, you have to enable the radiation model; Surface-to-Surface for vacuum.

Boussinesq is meant for the conditions where density variation is very small, say, less than 5% over the temperature range in the system. And you can use it for both steady-state as well as transient. There is no limitation on that.

[Rimzy]

Dear Vinerm,

I did't understand the sentence ' do not create a domain where vacuum exits'. Do you mean that in Design modeler, i should not create this domain by using Fill command, as i did or it means something else?Please make me more clearer. It would largely help me to deal with this problem of vacuum.

Thank you,

[vinerm]

Yes, that's what I meant. Since it does not include any fluid, you do not want Fluent to solve anything in that domain. Simpler solution is not to create it. When the domain does not exist, its boundaries will become external and you can apply radiation boundary condition.

[Rimzy]

Noted but i have little concern. If i do not create a domain by using Fill. Then, in meshing tool, ANSYS would not create mesh in that domain too. When there would be no mesh between glass tube and metal tube(that region is vacuum) then how solver solve the equations of fluid dynamics and heat transfer in that domain? My concern is appropriate? The second thing is now my solution is running till 100 iteration but after that divergence in pressure correction occure. May be that vacuum is causing problems.

Thank you so much,

[vinerm]

Muhammad, the vacuum is not governed by the equations that are solved in a standard CFD too. Therefore, you do not need to solve any equations in the vacuum region. However, radiation is important. So, there are two ways. Lets assume you have three regions, one containing fluid 1, second one has vacuum, and third one contains either fluid 1 or fluid 2. Another assumption is that there is not transfer of the mass from region 1 to region 3. There are at least two ways to solve it

1. Create region 1 and region 3 but not region 2. This implies region 2 does not have a model, hence, no mesh. Fluent only receives mesh and not the geometric model. So, it would not know about any region 2. You have to create boundary conditions between region 1 and region 3 for transfer of energy.

2. Create all three regions. Enable surface-to-surface radiation model. Fix the velocities to 0 in region 2; this is doable under cell zone conditions. This will ensure that there is no heat transfer by convection. You also have to ensure that the thermal conductivity in the region 2 is very very low because that's how a vacuum will behave (statistically, if we can define vacuum statistically which would be absurd ). To set conductivity to a very low value, you have to create a new material. Other properties for this material could be same as air or water or fluid 1 that you have, but set its k to be 1e-18. Do not set it to 0.0. Use this fluid for region 2.

[Andrea1984]

Hi Rimzy,

hi this paper I have simulated a heat exchanger operating in a way similar to how your solar collector works: https://www.sciencedirect.com/scienc...29549313002446

I went with option 2 in the post above by Vinerm, i.e. the two fluid regions containing the two "moving" fluids participating in the heat exchange process are separated by a third fluid region representing the vacuum. Actually, in the paper I was also considering conjugate heat transfer between the fluids and the pipe walls and conduction within the pipe, but I am not sure if you are seeking to do that. In order to mimic vacuum behaviour I have set both density and thermal conductivity of the fluid in this region to very low values (do not use zero, numerical codes don't like zeroes in general and is likely that you will end up with a floating point exception). The value of 1e-18 suggested by Vinerm will do. You can also de-activate the solution of the momentum equation within the vacuum fluid region. If the fluid inside the vacuum is not moving and its thermal conductivity is practically zero, the heat transfer can only occur via radiation. Also, by definition of vacuum, it is safe to neglect the participation of the "vacuum" fluid region to the radiative heat transfer, and hence you can use the surface-to-surface radiation model in Fluent to simulate the radiative heat transfer between the two solid walls encompassing the vacuum fluid region. In my case these two solid surfaces were the two finned walls, i.e. the outer walls of the inner pipe and the inner wall of the outer pipe.

Hope this helps,
Andrea

[Rimzy]

Thank you Dear Vinerm.
I am going for option no 2. i have already created a pseudo vacuum from fluent material data base. now i will set the properties as mentioned after enabling surface to surface radiation model.

Thank you very much for help

[Rimzy]

Dear Andrea, Thank you for providing link of the paper. I have downloaded it. I will see in detail. in my case, i am performing radiation heat transfer from glass tube to copper tube(this copper tube contains water that need to be heated by radiation). I am not using fins but i can cite your paper in my research work as we have similarities. you are right about zero density previously i was setting it zero and it was giving pressure correction error.

Thank you

[Rimzy]

Hello Andrea and Vinerm,

I applied S2S radiation model with vacuum properties as mentioned by both of you. In my case, there are two concentric tubes, outer tube is glass tube and inner tube is metal tube having vacuum region between two tubes. Ideally, solar radiations falling on the outer surface of glass tube would transmit to vacuum as radiation heat transfer and then falling on inner metal tube where conduction through copper tube would heat the water inside metal tube. In addition to S2S radiation model, i also applied solar load model as ray tracing because solar is my only energy source.In radiative participating zones, I inserted outer wall and inner wall of glass tube, wall vacuum and outer wall of metal tube. set the both walls from glass and vacuum as transparent and metal tube outer wall as opaque. in Boundary conditions under thermal, initially i put glass wall as 'heat flux' wall and all other walls as 'system coupling'. when i run the solution for 200 iterations, i get 5000 K facet average temperature at glass tube, 1.33 K temperature in interior vacuum and 303 K temperature at metal tube. At inlet is same as set by Bc thats 303 K but it increases at outlet as 311K with fluid domain temperature as 314 K. when i see animation then flow is going against gravity. i do't know its happening due to natural convection or due to static pressure difference.

So, my point is Whats the possible reason for so much higher temperature difference between glass tube and metal tube? It means no heat transfer is occurring there? If no heat transfer then why temperature at outlet and in fluid domain is increasing and velocity of water is 3.38 m/s? when i calculate the solar radiation flux for glass tube and metal tube it shows zero. In residuals, energy and continuity is also going upwards means they have no intention to converge at larger iterations. Can you please point out me where i am wrong? My supervisor is asking for results and i am struck.

[vinerm]

First, where is the system coupling coming from? This option is meant for FSI, i.e., when Fluent is connected with Ansys Mechanical simulations for thermal stress prediction in the solids. Is this the scenario for your case? If not, set it to proper condition, such as wall.

Between liquid and copper, it should be wall-wall-shadow pair. Similarly, between copper and vacuum, and vacuum and glass tube. Furthermore, solar model is not really necessary if your domain is small and you know the incident radiation from the sun on to the glass tube. Then, just apply wall heat flux on the outside of the glass tube. For S2S, I hope you have calculated view-factors properly. Otherwise, this might lead to error or divergence.

Flow would be the direction opposite to the gravity if the settings are not proper. Ensure that gravity value has appropriate sign and applied along correct coordinate. If Boussinesq model is used for water, apply proper density value in materials panel. Similarly, apply proper reference temperature and reference density in the Operating Conditions panel.

[Rimzy]

Yeah, system coupling does not make sense then. As you mentioned that solar loading should be replaced with heat flux at glass wall. so i will replace 'via system coupling' with 'heat flux'.
NO. I have no wall-wall shadow pair. I only have wall-glass tube, wall-vacuum, wall-metal tube and wall-fluid domain. Apart from this, I have 2 extra walls which i have defined as named selection during meshing. these walls are wall-outer-side-glasstube, wall-inner-side-glass tube and wall-outer-side-metal tube. Basically these 3 walls and Wall-vacuum are the walls which i have defined as participating zone for S2S radiation. Is it correct.

No, flow direction is what i want mean against the gravity. Gravity is -9.81 for Z direction which is correct. But the velocity and temperatures are not what i expect.

[Rimzy]

At the start, i was receiving error of 'segmentation fault'. I read a thread where it was mentioned that remove the contact regions under 'connections' in Meshing. So i deleted all contact region. So this is the reason of absence of wall-pair shadows?

[vinerm]

Contacts at the meshing level are really really bad for CFD. Those are alright if you use Mechanical simulation or if you want moving interfaces in CFD. Otherwise, those must be removed so that a conformal mesh is maintained across all domains. You also need to ensure that all the bodies belong to same part. You can check that in Meshing tool under Geometry. If that is not the case, then you will have to go back to you CAD tool, DM or SCDM and ensure that all bodies have shared topology.

Yes, this is the reason that you have extra walls that should be there but as shadow pairs.

[vinerm]

You need to ensure that there is only one part. This part can have multiple bodies but if you have more than one part then that will lead to non-conformal mesh, and hence, interfaces. This is required only with moving mesh. Otherwise, ensure that geometry contains only one part. For DM, you need to select all the bodies in the tree, right-click, and then select Form New Part. For SCDM, you need to go to Workbench tab in the ribbon, select Share, and then the green-tick icon. If even after this Meshing shows contacts, delete those. But do check at Meshing level that it shows one part and not multiple parts.

By private content I mean something that you do not want to share in the Forum for any reason. I do not charge. Helping is my payout.

[Rimzy]

Thank you so much. Your help really appreciated from core of my heart.