Question about heat transfer simulation convergence
 

Hi,

Heat transfer convergence usually takes much more time than the velocity convergence. For fluid dynamics simulation, when the velocity residual and mass flow residual is very small, then we can basically say that the simulation has already converged.

But for heat transfer simulation, this convergence criteria may not work. I'm wondering what could be the convergence criteria for the heat transfer simulation?

Transient or Steady State? How are the equations being solved? What exactly do you mean by convergence?

Are you using a commercial code or something you wrote youself?

It's steady state conjugate heat transfer simulation. NS equations and total energy equations are solved by FVM. Convergence means the heat transfer rate doesn't change a lot anymore even thought the residual is still reduced. CFX is used.

If the physical parameter you are interested in, ( a heat flux), is converged to a level that is good enough for you then stop there. There residual does not directly reflect how far your solution is from the correct solution, it tells you how accurately you are solving the equations. Also because the flow depends only weakly on the temperature it make sense that it will converge quickly, the temperature field depends strongly on the velocity field so that a small update to the velocity field can cause a large change to the convective terms in your heat equation. But I would say that if you flux is not changing by much then your answer is probably good enough and running the simulation for longer will not give you much more accuracy.

CHT simulations commonly have this problem where the residuals are well converged but the imbalances are not and converge quite slowly. The problem is caused by the different time scales in the solid and fluid regions - the solid region is much slower than the fluid region, so a sensible time step for the fluid region only advances the solid region very slowly.

The answer is to use a solid time scale factor. This accelerates the time step in the solid region. As the equation solved in the solid region is just the heat equation and it is linear and well-behaved you can accelerate it by a large amount - I typically use factors like 100 or 1000. This usually makes the solid region converge just as fast as the fluid region and speeds up CHT simulations many times.

And this is also why it is vital that CHT simulations have convergence criteria on both residuals and imbalances. If you just use residuals or look at the convergence of parameters of interst you can get answers which are wrong by miles.

1) What do you mean by 'factors like 100 or 1000'?

2) Is there a way to setup to change the time step during the simulation running automatically? Then I can use large time step firstly then change to small step. I really need a automatic way to do this time step shifting. Because I have more than 300 this kind of simulations to run. I can't change the time step manually every time.

3) Could I setup a simulation stopping criteria like 'the outlet temperature doesn't change a lot anymore' in CFX? So that the simulation can be stopped by this criteria automatically and in this way the next simulation can be started earlier. This can save some computation time.

4) How to decide the length of the time step I need to use at the beginning to solve the solid temperature distribution?

I agree! Just compare solid time scales to fluid time scales and you quickly appreciate why the imbalances don't reduce as much as you want to! (And it's usually the energy equation - no suprises there!)

However in transient simulations surely you can't set a timescale for the solid region, and a different time scale for the fluid region?

Using your method described above (coincidentally is the same method I use) you're restricted to steady state calculations using "false" physical timesteps.

Yes, the solid time scale factor is only applicable to steady state runs. In transient runs you have to model it with the physical time step the same in both regions.

Shoushou:
I mean set a solid time scale factor in the range of 100-1000.

You do not need to change the time step during a run. You can start it with this high factor.

For CHT simulations I recommend using the residuals AND imbalances as convergence tolerances. Do a sensitivity study to check your settings are OK and then use that setting on all your runs.

Setting time step size: Just try it out and see if it works. It is goes slow then make it bigger, If it diverges then make it smaller.

What is the imbalance convergence? Conservation target? Does it mean RMS T-Energy and H-Energy?

I didn't find the answers of it on the user manual. Thanks.

No, I mean using the global imbalances as an additional convergence critereon. This is described in the documentation. It does not mean RMS T-Energy or H-Energy, it is a global imbalance.

In your case, Glenn is talking about the balances of all the heat. For example when you stop a run, CFX will report out in tablular format T-ENERGY-*** for each of your solid domains. It will also report out H-ENERGY-*** for each of your fluid domains.

It also tells you what the balance (or imbalance) is (for a SS run Heat in should = Heat out). All of your boundarys and sources are listed in this table.

If you desire, during a run, you could monitor all of your heat (make sure you include the fluid inlets and outlets and losses), see what is going where, and determine from that whether your heat solution is converged.

I tried those methods. But the H-Energy still converges slowly. May I ask how is H-Energy defined? I didn't find its definition in the user manual.

What documentation is the global imbalances defined? I searched for it in the Ansys help but found only very limited information about it. What is the definition of the 'global imbalances'?

See attached Picture. The arrows point to the imbalance. The items above are all the heat sources for your each of your domains. All of those numbers are in watts.

I assume you put in heat as either a surface flux, or volume generation. You know the watts of your imposed sources.

You can check the balances for all locations using this information. Adding up all the numbers should be about 0 (give or take a resonable variance).

So the 'global imbalance' is defined as the overall heat conservation in a domain. Right?

And how is H-Energy and T-Energy defined?

You first question answer is correct.

By H-Energy and T-Energy, I assume you mean the Solver Manager convergence RMS (or MAX) plot that you see when the job is running?

That is just the residual of the Energy Equation.

If you mean H-Energy and T-Energy precisely then that is the energy equation:

Energy In - Energy Out + Energy Stored = Total Energy.

In simple terms Energy In would be: Volume Intergal of all your volumetric heat generation+surface integral of All your heat fluxes+mdot_fluid_in*enthalpy

You can do the other terms in similar manner.

If this is not what you mean, I do not understand the question.

Yes. That is what i mean. Thanks.

Which of them is the residual of energy equation? H-Energy or T-Energy? What is the difference between them?

One pertains to a fluid domain, the other a solid domain.

If you run just fluids you will only see H-Energy.

hey,
I have convergence problems too in my single-phase simulation with thermally stratified tank which has an inlet, three outlets, free slip surface and other no-slip walls. Water flow into the domain having a varying density with temperatue (temperature changing with depth).
Considering temperature transport, H-energy RMS reduces very slowly, even increases somewhere. The Imbalance is strange too. what's the problem?
Could you give some suggestions for this? Thank you so much.

FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thanks for your reply

Transient heat transfer simulation - convergence
 

I write in this thread as it is more related in what I am doing. I am doing a transient heat transfer simulation. I have the simulation run as charging and discharging cycles. regarding solver convergence: I checked residuals and Imblances in fluid and solid region. The residual graph looks good until 350(iterations) and after that it started increasing as shown.. Why is this?

The global imblances are with in 1% . I checked the yplus value near the fluid and solid interface and it is 30+ for 70% of the area and 80+ for 30% of the area. I use SST model.

What can be the reason for this residual graph shoot up after 350 iterations:confused::confused:?

Without knowing what you're simulating it's hard to give a proper answer.

It could be due to a poor mesh, poor choice of model, both, or something else completely.

To me it might look like the simulation is resolving some evolving flow physics (maybe vorticies which grow as a function of time?).

Start a new thread and give a detailed description of what you're doing.

Also I'm sure Ghorrocks will be around to tell you to read the FAQ - so do that too.

Sadly, I don't think an FAQ covers this one :(

I agree with Mr CFD's comments: First check for numerical problems (mesh, models), and if they look OK check for transient flow starting up, such as vortex shedding or gross flow instabilities.

Thank you. I m starting a new thread:)

okay,Ghorrocks. I ll try to create new thread with more details on this regard.

Convergence Issues-CHT for Turbomachinery
 

Hello! Thank you all for this useful thread, it helps a lot in CHT related topics.



I am trying to simulate a multistage axial turbine throw CFX to account later for the temperature field on turbine blades by thermal analysis.



To succeed more acqurate results i implemented in my model Conjugate Heat Transfer with a loose couple (different mesh between fluid region (TurboGrid) and solid region (Ansys Meshing) through CFX.



When i applied CFX to only the second rotor stage (to check if it works fine with my settings (interfaces etc.)) it results with good convergence both from residuals side and global imbalance as well.



However, when i tried to add mesh for another stage then RMS-T Energy for the previous stage is diverging like in the attached image.


Timescale for fluid domain is set as 1/omega through an expression (as suggested by CFX-manual)



I used different Timescales for the solid domains like 1000, 100, 10 and 1s but it tends to give similar results in all cases.


I would be grateful if you could make me aware of what is the possible cause of that.



Again, Thank you!


Residuals' Plots:

https://ibb.co/Btk2PMn
https://ibb.co/zh2sPQy
https://ibb.co/PjrqPpY