Applying heat transfer boundary conditions
 

Greetings!

I have a solid containing a fluid (water tank, 100% filled). My question pertains to the heat transfer between the tank and its environment. Is there a way to apply boundary conditions like convection and solar radiation?

heat flux from where to where?

For instance, on the top surface of the tank we have heat gain from solar radiation (heat flux) and heat loss to the environment via convection. From what i understand, we can't apply two boundary conditions on the same surface. How should i approach this? Haven't found any example or tutorial where we have both convection and heat flux on the same surface...

Edit: I just realized that you cannot use a surface as a boundary condition and as an interface at the same time, something that perplexes things. I really need a comprehensive example.

It is pretty simple maths to derive it and use CEL expressions to apply it.

Do you mean the free surface? That is inside the domain, not on a boundary - that is why you cannot apply a boundary condition on it :)

Thank you for your answer!
Lets us ignore the first part of your answer for the time being. I'll figure out the specifics about CEL expressions later.
What i've done so far is define a solid and a fluid domain, as well as their automatically generated solid-fluid interface. If i go ahead and insert a boundary condition in a surface, that surface will be subtracted from the solid-fluid interface. Naturally, if i do this (add boundary conditions) for all the surfaces within the interface, i'll end up without interface. Weird huh?
On top of that, i have NO heat transfer between the domains. I've been "tinkering" for quite some time without results...

Not really. You are replacing the interface condition with a boundary condition. So the interface disappears. It does not seem weird to me :)

You can add heat fluxes to the interface boundary condition. This allows you to have an interface with additional heat input. I think this is what you want. Have a look at the interface boundaries on the domain level (not the interface condition by itself).

I see....Each domain's interface provides a heat source option. How do i make the domains convect heat? I don't want just a steady heat flux.

you have heat flow and heat flux option.
You can set one domain as heat source or select some faces and set them as heat source. Then you need buoyancy setting enabled for the fluid.
For domain you can set heat as kW per m^3 and for a surface kW per m^2.
Or you can specify a temperature.
It is a good idea to create named objets in the mesher. I.e. name the domain or the surfaces in question something descriptive like heat source. Then they are easier to identify in the Preprocessor

I apologize for taking a long time to answer. I' d like to thank both of you, for pointing me to the right direction. I have successfully run simple simulations (at least i think so), both steady and transient. Now my problem lies in simulating a partially filled water tank. Including a second fluid certainly perplexes things...

Hi, I have the same problem. when I combine heat flux and convection into one equation, FLUENT does not accept that equation, because the derived equation is related to time (due to heat flux) and temperature (due to convection). I do not know how to solve the problem.
Any help will be appreciated!

Try the fluent forum.

Thanks a lot for your quick respond. I could not find anything to solve my problem. Since you did kindly suggest up in this threat that "It is pretty simple maths to derive it and use CEL expressions to apply it", I derived the equation, but does not work. Therefore I would appreciate if you or any body else kindly have any idea to solve the problem. Thanks in advance

Convection is Flux = h(Twall - Tambient)

So if you have a heat flux you wish to apply on top of that the Flux = h(Twall-Tambient)+A where A is your additional heat flux.

Thanks again for your kindly respond. I did so, but as I already mentioned, since I am applying the solar heat flux for a whole day (24 hours) which is based on time, the final derived equation is related to time (due to solar heat flux) and temperature (due to convection). Therefore when I use "DEFINE_PROFILE" to write the corresponding UDF, FLUENT does not accept it. I think here is the reason from the FLUENT manual "Note that DEFINE_PROFILE allows you to modify only a single value for wall heat flux". I was wondering if there is any other way to approach to this problem. Thanks again

Switch to CFX and it will work fine. Otherwise refer to post #11.

This is what I do ready need, but how can I add heat fluxes to the interface boundary condition? Thanks in advance

Let me quote post #11 for you:

This is the CFX forum. For details on Fluent try the Fluent forum.

Hi all. Hey Steffen I have made double pipe heat exchanger with hot water fluid domain inside, an inner pipe and then an outer cold water fluid. There is no heat transfered along the length of the pipe when I opened CFD-Post the same inlet temperatures run through all contours for both pipes. If I define heat as kW/m3 would ay heat transfer take place then. Also I wanted to ask how can I define heat as kW/m3 for a a domain as I don't see any option for that when I select Thermal Energy In Option in Heat Transfer in Fluid Models in Domain:Hot water (or Cold water). I have searched a lot to define a heat in kW/m3 but couldn't find anything. Would be grateful for reply. Thanks.

Either the no heat transfer result is correct or you set the simulation up wrong.

If you are in a flow regime when very little heat transfer occurs then it is correct that you don't see much heat transfer. This could be the case if the intermediate material has high thermal resistance or specific heat or many other factors.

If the simulation is wrong then you set it up wrong. The most obvious thing is whether the interfaces between the fluids and solids are correct. If they are wrong it will stop heat transfer. Have a look at the non-overlap % reported in the output file.

Also what do you mean by heat as kW/m3? Do you mean there is a volumetric heat source in there somewhere? Or is that the heat content of the incoming fluids?

Thanks a lot Mr. Ghorrocks. Actually there is no volumetric heat source inside the Hot water fluid domain. I thought without that no heat transfer takes place but I was wrong. I just want to study basic heat transfer due to temperature difference between hot and cold fluid. Also you mentioned "heat content". How can I include "heat content" and will it allow heat transfer to take place or is it altogether irrelevant to heat transfer. Another thing what is non-overlap% reported in out file. The detail for Fluid Fluid Interface is as follows:


Discretization type = GGI
Intersection type = Direct
Non-overlap area fraction on side 1 = 3.56E-04
Non-overlap area fraction on side 2 = 1.58E-02

Would be grateful for explanation. God bless you. Thanks.

Non-overlap area fraction is the amount of the interface which has not intersected. In your case the % is low (max 1.5%) so most of the interface correctly intersects. I would still have a close look at this to check it is OK.

Regarding heat transfer:
You should apply the flow conditions to match what you are trying to model. Likewise, you should measure the performance on the simulation using a parameter which is of use in your situation. I do not know what you are modelling so cannot say.

But I can guess that most heat exchangers work with a hot fluid coming in at a known temperature and a cold fluid coming in at a known temperature, and you want to know how much heat comes out of the hot fluid and how much goes into the cold fluid. In this case I would use massflowAve of temperature at the inlets and outlets to get the heat gained and lost.

Hi all. Thanks a lot Glenn. I am attaching pics of my double pipe counter flow heat exchanger (2nd image). Why don't I see a change of temperature colors along the length of the pipe as in the first image of a similar tutorial setup in ANSYS Fluent even when I changed the inlet speeds from 5 m/s at the hot and cold inlets to ~.8-.9 m/s (I thought decreasing the speeds will increase the contact time and make the heat transfer more enhanced/prominent along the length of the pipe). Also I will apply your recommendation of using massflowAve at the inlets and outlet boundary conditions (but I converted my outlet boundary conditions from outlet to opening type because of a message of wall being placed and suggestion of conversion from outlet to opening type in out file). Should I change boundary conditions at outlet back to Outlet type? Would be grateful for review and recommendation. God bless you. Thanks.

Hi all. Dear Glenn, I have a few questions.

First of all to insert a massflowAve(T)@ expression at an outlet do I need to define mass flow rate (instead of Average Static Pressure or Normal Speed) in Option in Mass and Momentum in Boundary Details in Boundary:Coldwateroutlet (but for that I need to change boundary condition at outlet from Opening to Outlet? Should I do that? Similarly should I do that for Boundary:Hotwateroutlet)?

Second inserting a massflowAve(T)@ expression for inlets would mean I am not defining static temperatures at the inlets which is usually the norm and like you suggested for a heat exchanger problem. Also for this to happen do I need to define Mass Flow Rate in Option in Mass and Momentum in Boundary Details in Boundary:Coldwaterinlet and similarly for Boundary:HotwaterInlet?

Third irrespective of inlets or oulets do I need to insert massFlowAve(T)@ expression as "Static Temperature" in Option in Heat Transfer in Boundary Details in Boundary?

Would be grateful for reply. God bless you. Thanks.

I suspect the heat exchanger in image 2 is not working very effectively. All the heat transfer takes place at the entrance and nothing much happens after that. You need to get the flow rate and temperature difference in a proper operating range for the heat exchanger to function correctly.

Second Post: You apply the boundary conditions to match the flow conditions. Then you look at the best way of monitoring it. You could also use a massFlowInt(T) or cp*T to give an input/output heat flux.

Thanks a lot Glenn. I followed your adice and played around with boundary conditions. First I changed the speeds of the inlets but nothing happened. Then I changed the temperature of inlets, again nothing happened. Then I changed the "Speed" Option in Mass and Momentum in Boundary Details in Boundary:Coldwaterinlet (and Boundary:Hotwateroutlet) to "Mass Flow Rate" with a value of 25 kg/s and then in CFD-Post I saw some change of temperature along the length of the pipe but now I am faced with the problem of no convergence of heat transfer and mass and momentum graphs. How to solve this? Would be grateful. God bless you. Thanks.

The convergence problem is an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Can you post attachments as image files or text files? Word files are a pain to view on some machines.

I recommend you do a simple hand calculation on your heat exchanger before you start CFD work. That way you can find a sensible operating point to start at quickly. There are several methods to approximately size a heat exchanger in heat transfer textbooks. I recommend you use these methods to get a starting point.

Thanks a lot for the feedback Glenn. Is the change of temperature along the length of the pipe correct in your opinion? Basically I am a Mechatronics Engineer by profession and also I have studied a full semester course in heat transfer and another one in thermodynamics in my Bachelors of Engineering. Now I am doing Masters and had taken a summer course on CFD and now am applying CFD code ANSYS for my thesis. But I need your help brother. Usually while designing a heat exchanger on paper/theoretically Mass Flow Rate is chosen/given in problems, but here in CFX-Pre there are six options including "Normal Speed" in Mass and Momentum in Boundary Details in Boundary:Inlet. Why are results so different when I use speed as compared to when I use Mass Flow Rate. Also please find an attached jpeg file for easier view. Sorry about loading word files earlier. God bless you. Please forgive me. Would be grateful. Thanks.

Mass flow rate and velocity are the same boundary condition. Are you sure you are specifying them correctly?

I have no idea what the correct temperature change along the pipe is as I do not know what you are modelling. And even if you told me I do not have time to work it out for you - you will have to figure that out for yourself. But I will try to help you as much as I can.

Hi Glenn
I did switch to CFX, so I already made my geometry along with meshing by CFX. However when I run the model, it does not even start. It says:"In Analysis 'Flow Analysis 1': No domains have been defined."
Any help will be appreciated

The error sounds obvious - define a domain.

Have a look at the CFX tutorials for examples of how to set things up.

As I see at following links which show two examples of CFX on youtube, after making geometry and meshing, when you click on setup, your geometry pups up and you can go on and proceed your modeling. However in my case, when I click on setup, my geometry does not pup up.
Please note that all manuals I found, have no example to look at.
Thanks for your help.

https://www.youtube.com/watch?v=Xu8rJGOFWok

https://www.youtube.com/watch?v=ymGQIA_Rv3Q

Try the CFX tutorials which come with CFX, under the help/documentation. They come with all the files required to run them.