Conjugate heat transfer
 

Dear experts,

Did anyone do a conjugate heat transfer from a fluid (at high temperature) to the adjacent solid (at low temperature). I really need suggestions.

I've seen videos on conjugate heat transfer but every video was on solid to fluid conjugate heat transfer.

I did from fluid to solid but uncertain about the results.

Need suggestions.

Thanks in advance.

Hi Sesh,

I am not sure if I understand your question correctly. The direction of heat transfer is not something that you explicitly set! It depends on the temperature gradient at coupled interfaces.

As a sanity check, you can compare the magnitude of wall heat flux exchanged at the coupled interfaces. The magnitude of heat flux from solid to liquid should be equal (of course within an acceptable error margin) to the one from liquid to solid!

Cheers

Dear Sesh:

It does not matter which domain solver you set as master in a conjugate heat transfer study. The CFD solver is usually the parent domain because it is (usually) more resource intensive than the solid domain. Usually you need to run the fluid solver with about 50 - 100 times the iterations or more per call in the solid domain solver for the temperature field to properly develop.

Make sure the solver you intend as parent has a hook to an external solver. It is also likely that you will need to run the slave (solid domain) solver as a batch process. You could still set up both cases with the GUI (assuming there is one) but when it comes to starting and solving, you can only run the master domain in the GUI.

Another thing is that it is effectively an exchange of surface temperature and surface flux between the two domains / solvers until the discrepancy falls below some kind of tolerance. So often is the case where the fluid solver solves for the surface heat flux, which gets passed to the solid solver to obtain a new set of surface temperature for the fluid solver, where the process repeats.

There would also be some issue regarding matching locations on the surface. This is usually done at the start of the simulation by the parent solver, but depending on the solver you might need to provide the mapping explicitly. Yes, it is a pain if you have to do it yourself.

Here is a general workflow of a conjugate heat transfer problem:

1) Set up standalone fluid domain solver, using surface temperature as boundary condition

2) Set up standalone solid domain solver, using surface heat flux as boundary condition

3) In the fluid domain solver, set it to master by introducing hooks to external solver calls to obtain surface temperature from the solid domain solver

4) In the solid domain solver, set it to slave by telling it where to pick up the heat flux boundary condition from the fluid domain solver

5) Start the conjugate heat transfer job from the fluid domain solver. If set up properly, it should call the solid domain solver and wait for it to finish before continuing

6) Once the surface temperature and heat flux on both domains are about the same, the run has reached convergence. In practice this is "assumed" by having the fluid solver perform a lot of iterations per call to the solid solver

I hope this gives you a better idea on how to set it up.

Gerry.

Conjugate heat transfer
 

Dear Gerry,
Thanks for the information.

Here is my workflow. Please correct me if any of my commands is wrong.

Problem description: The entire cube domain (XYZ=79*79*65mm) having solid cylinders of 18mm in dia and these cylinders have a gap of 2mm in between. Checking the time scales of heat transfer.

Solver: density-based, transient, gravity in the z-direction
Energy equation: ON
Fluid flow: K-w SST
Species transport: ON (no reactions)
Materials: Ch4, CO2, air, and aluminum

Boundary conditions:
1. Pressure inlet: Total pressure: 1.5bar
Temperature:600K
Species: Ch4 and CO2 (Mole fraction: 0.3:0.7) and ideal gas law for 'density'
Turbulent intensity: 1%
Viscosity:1

2. Pressure outlet

3. solid-fluid interface: coupled

4. Solid cylinder wall: heat flux= zero(default), no-slip

5. All the rest boundaries: Walls, heat flux= zero(default), no-slip

6. Patch: All solid and fluid domain: 300[K]

7. Operating Conditions:
Pressure= 1bar
Density=0 (since I've used ideal gas law)

I ran the simulation and checked for the volume average temperature of a single-cylinder (9mm away from the inlet).
The result showed that there is a rise of temperature up to 3 degC in 1.4 sec.
https://ibb.co/VmY9gNz

I'm uncertain about the result because I'm new to the CFD and I doubt the conditions I gave.

Could you please check the conditions and suggest me if I missed something to add.

Thanks in advance.

Quick remarks:

1) I don't see how you define the solid (aluminum) domain, and how the surfaces of the solid pipe (I assume the inner and outer walls of the pipe) are mapped to the corresponding fluid boundaries?

2) Is this a segregated (each domain has its own case file) or a coupled (all domains in a single case file) CHT simulation?

3) you should not be using zero heat flux. This defeats the purpose of running a CHT in the first place. Using a heat transfer allows heat transfer between the domain.

It seems like a fairly basic CHT study. There should be a similar tutorial available for your CFD software.

Gerry.

Solid time step in CHT
 

https://ibb.co/vP6v1B6

Dear Gerry Kan,
please have a look at the image (above url). The 16 solid domains and the cube as fluid.

2. It's a coupled simulation (CHT)

3. I understood the mistake and changed it.

Now, I got stuck with another problem 'time step' both physical and solid time step.

I have a 2mm pressure inlet (1.5bar)at one side of the cube. From the previous simulations I read the velocity is too high (600m/s) at this pressure inlet, so I've used a physical time step of 1e-6 and a solid time step as 1e-4. I assumed this would take longer and reduced the domain. I tried to play with 'solid time step'. When I was using a solid time step of 0.1, the temperature was increasing very fast, and when I use the small time step, the increase in temperature was very low. Here, I'm confused. How to find the correct solid time step?
Please help.

Dear Sesh:

The "time steps" for solid and fluid are relaxation factors which allows one phase to adjust to changes in boundary condition without the other taking too many iterations. Usually you set the fluid time step much smaller than the solid time step (say, 50x smaller than the solid time step). It is the same as the number of iterations I mentioned in one of my earlier responses.

As for the problem you described, it could be twofold:

(a) incorrect boundary conditions in the fluid region, especially if it is compressible. In this case make sure it runs alone (i.e., without the CHT) and reaches convergence easily. If it is incompressible this should not be the issue but it might be a good exercise to double check.

(b) Problem with heat flux mapping at the solid/fluid interface in your coupled CHT. It is a much trickier problem, especially when the interface mesh densities are very different in the adjacent domains. If you could get away with it, run it in segregated mode (i.e., as parent-slave simulations). It will save you a lot of headache.

Hope that helps, Gerry.

P.S. - You did not leave the link to your image in your thread.

Dear Sesh:

I managed to locate your image. It was on my CFD-online notification e-mail, but not in the message. I don't know why.

You can merge all your cylinders into one solid domain, if they are made of the same material. This will simplify your problem a lot more.

In the meantime, I read through your settings. I assume that it is a steady compressible flow problem. In the case it is advisable to first solve the fluid side alone until an initially steady solution has been reached before turning on coupled (or segregated, recommended) CHT.

My hunch is that your fluid side BCs are not correctly prescribed. I don't know what your outlet (static) pressure is, but it does not take a high pressure drop to get a large flow velocity. If you could do it, I would fix the mass flow rate at the outlet, which will allow the simulation to converge a lot easier.

Gerry.

CHT settings, temperature rise as a step
 

Dear Gerry Kan,

Thanks for your suggestions.

I've changed the mesh size to be uniform (2mm both in fluid and solid region).

I've changed a couple of settings
1. Pressure based solver
2. I changed the outlet to a mass flow outlet instead of a pressure outlet and can see the solution is converging.
3. I changed the pressure-velocity coupling method to SIMPLEC
4. I used incompressible ideal gas for the fluid, assuming the change of density is only due to temperature variation.

*** I do not want to merge all the solid cylinders into a single domain because I want to monitor the temperature of each solid cylinder w.r.t flow time.

*****************************
In another thread I asked about the rise of temperature as a step.
Mr. Alexanderz replied me but I couldn't manage to understand him.

His reply: in fluent interface check zone ID of your solid.

With UDF find temperature of that solid zone using loop over cells in that thread (in other words in that zone)

If criteria is met, change temperature in solid zone.

-- I have no idea how to implement this. Do you have any suggestions for this?

Thank you.

Dear Sesh:

I have no idea who Mr. Alexanderz is, and I am not familiar with running CHT with Fluent. You should ask him.

Gerry.

Dear Geryy,

Thank you very much for all your immediate responses.
I wish the suggestions you provided will solve my issues in the simulation.

I'll get back once I finish the simulation to share my results.

In addition: I just ran a quick simulation for a small geometry and I've seen no difference in using only physical time step and as well as both physical and solid time step.
The temperature profiles in the solid region look the same in both cases.
Any comment on this?

Thank you.