[Wolfram]

Dear all,

I am trying to reproduce the results of an experiment in order to verify the simulation for upcoming developments.

Cold air is heated by a warmed up heat exchanger like shown in the picture.

In the experiment, the outlet air flow is much warmer for the beginning and the heat exchanger cools down much faster - let us say 60 seconds.
In the simulation, the outlet air flow is colder for the beginning and the heat exchanger cools down slower - let us say 100 seconds.

CFDO.jpg

The physical properties of the solid are known and correctly set in the simulation(dimensions, density, specific heat capacity,...).

It seems like the heat transfer from solid to fluid is not captured correctly and is underpredicted. Within the heat transfer the Y+ value is around 1.

I found, that increasing the wall roughness within the heat exchanger domain, where the fluid-solid-interface is located, increased the heat transfer by approx. 10%. Are there more "parameters" in order to influence the calculated heat transfer from solid to fluid?

The heat transfer model is set to conservative interface flux.


Many thanks and best wishes

[ghorrocks]

Getting accurate heat transfer results is significantly harder than accurate flow results if the key factor is heat transfer through a turbulent boundary layer.

There is more to the mesh resolution than y+=1. You need to look at mesh resolution in the solid and in the bulk flow as well. So you should look at all these things in your mesh sensitivity study.

You should also check the other basic parameters - convergence tolerance and time step size. And for CHT simulations you probably want to add imbalances as a convergence criteria.

Other tips are here: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[Wolfram]

I varied the mesh in several directions without huge impact on the results.

Are there any specific requirements regarding time step for CHT simulations? I have to admit the timestep is pretty, pretty large regarding courant number since I have to represent 120 seconds in real life ...

[ghorrocks]

You still need to do a sensitivity study on convergence tolerance and time step size. Either of those could affect results. And adding imbalances as a convergence criteria is often a good idea for CHT simulations.

[Gert-Jan]

- Run in Double precision.
- Inflate the solid as well where it touches the fluid
- Switch on "Monitor Coefficient Loop Convergence". This allows you to monitor convergence within a timestep.
- Add more iterations within a timestep. E.g.50 in stead of default 10.
- Check all imbalances in every timestep.
- Set an additional convergence criterium on conservation: <0.01
- Add monitoring points all over and make sure you have only flatliners within each timestep. Monitor temperature, velocity, pressures, etc.
- Monitor the heat transfer through the interface. Make sure it is a flat liner as well.
- Do you use polynomes for physical properties? Make sure you have enough digits in your coefficients a0, a1, a2, etc., and clip the values at the min and max values.

[Wolfram]

Originally Posted by Gert-Jan

- Run in Double precision.
- Inflate the solid as well where it touches the fluid
- Switch on "Monitor Coefficient Loop Convergence". This allows you to monitor convergence within a timestep.
- Add more iterations within a timestep. E.g.50 in stead of default 10.
- Check all imbalances in every timestep.
- Set an additional convergence criterium on conservation: <0.01
- Add monitoring points all over and make sure you have only flatliners within each timestep. Monitor temperature, velocity, pressures, etc.
- Monitor the heat transfer through the interface. Make sure it is a flat liner as well.
- Do you use polynomes for physical properties? Make sure you have enough digits in your coefficients a0, a1, a2, etc., and clip the values at the min and max values.

Alright, many thanks. I just decided to shrink my case and determine the resulting htc depending on all the mentioned parameters.
Once it is finished, I will post it here.

I am not using polynomes. The temperature range is are around 15K.

Maybe one question prior to my DOE. Does the timestep play a crucial role in my case?

[ghorrocks]

Does the timestep play a crucial role in my case?

Your simulation is transient, so it sure does. That is why I (twice) recommended you to do a time step sensitivity check.

[Wolfram]

Originally Posted by Gert-Jan

- Run in Double precision.
- Inflate the solid as well where it touches the fluid
- Switch on "Monitor Coefficient Loop Convergence". This allows you to monitor convergence within a timestep.
- Add more iterations within a timestep. E.g.50 in stead of default 10.
- Check all imbalances in every timestep.
- Set an additional convergence criterium on conservation: <0.01
- Add monitoring points all over and make sure you have only flatliners within each timestep. Monitor temperature, velocity, pressures, etc.
- Monitor the heat transfer through the interface. Make sure it is a flat liner as well.
- Do you use polynomes for physical properties? Make sure you have enough digits in your coefficients a0, a1, a2, etc., and clip the values at the min and max values.

Hi,
as mentioned before I shrinked my case and evaluated the impact of the mesh and observed the imbalances.

In my DOE I varied the
- volume mesh size
- fluid inflation layer heigth
- fluid number of inflation layer
- volume mesh size in solid
- solid number of inflation
By choosing the mesh with the maximum heat transfer, I was able to increase it by 12%. The area averaged Y+ Value is around 0.05??

Furthermore I had to increase the inner loops to 15 in order to achieve 0% imbalance regarding heat transfer.

Although, the heat transfer was increased and each timestep converged, I am far from the measurements.

[ghorrocks]

It is good that you have investigated the effect of your mesh. But as I have said several times in this thread, there is more than just the mesh you need to check. You also need to check:
* Your convergence is tight enough (residuals AND imbalances in your case as it is a CHT simulation
* Time step size

Check the convergence criteria and time step size and let us know how accurate it is.

[Wolfram]

Hi,

here are screenshots of the imbalances and residuals. The timestep is pretty large regarding courant number. It is my approach to reproduce approx. 240 seconds in real time for a huge mesh.
gh1.jpg
gh2.jpg

[ghorrocks]

Courant number does not have much relevance to CFX. You certainly cannot tell your time step size is OK merely by Courant number. It is better to do a time step sensitivity check to get the time step size correct.

Plots of residuals and imbalances are not what I have been talking about. You need to do a simulation where you converge to (say) residuals 1E-4, and then another run at 1E-5. If the two simulations are the same then 1E-4 is OK for a convergence tolerance. If they are different you need to run again at 1E-5 and keep going tighter until it does converge.

Likewise for the time step size you should decrease the time step size by factors of 2 until it converges.

[Gert-Jan]

The momentum residuals should easily drop down below 1e-4 and beyond in a transient analysis. Since they don't, it looks like there something wrong in your physical propperties, setup or mesh.
I would advice to save the residuals to the results file (=setting in Output Control in CFX-Pre) and look in Post where they have the highest value. That might indicate where the problem is.

[Wolfram]

Hi,

I meanwhile reduced the transient timestep by factor 30 without an impact on the residuals and overall heat transfer.

The momentum residuals are below 1e-4 unless really really small regions with bad mesh elements. Interestingly the porous domains show the highest momentum residuals.

The region comprising fluid and the ceramic solid (function as heat accumulator) is completely unremarkable regarding any residuals (this is where the finest mesh is applied).

The screenshot shows isovolumes for H energy residuals above 0.001. The colored isovolumes are downstream of the ceramic heat accumulator and downstream the fan ( the alternating flow direction is achieved by reversing the direction of rotation)

cfdo.jpg

[ghorrocks]

Porous domains? You did not mention that before.

Porous domains have a number of issues which can affect convergence. Have you looked at all the porous domain options in the solver tab and documentation?

[Wolfram]

cfdo2.jpg

here you can see the domains.

The settings in the porous domain regarding pressure drop where adjusted in order to match my measurements of the air performance curve

[ghorrocks]

I am sure you have adjusted the porous domain to match the performance curve. But what I was referring to was the convergence and accuracy options available in the solver tab relevant to porous domains. They can have a strong effect on convergence for porous domains.

[Wolfram]

Originally Posted by ghorrocks

I am sure you have adjusted the porous domain to match the performance curve. But what I was referring to was the convergence and accuracy options available in the solver tab relevant to porous domains. They can have a strong effect on convergence for porous domains.

No, I am not aware of this kind of options! Could it be also related to heat transfer?

[ghorrocks]

I am not familiar with what effect porous domains can have on the heat equation. But there are a number of options for the momentum equations to improve convergence with porous domains so it is likely they will affect the heat equation as well.

The Rhie-Chow option is certainly one to look at, but there are many others.