Hi, in my results except the H-Energy all other imbalances are nearly zero. but imbalance of H-Energy is very high and converge of H-Energy is slow than others. do these reasons show wrong the heat tranfer setup?

regards

cmete

Try increasing the timestep on the energy equation (CFX-Pre, Solver Control > Advanced). If you have a very slow energy transport process such as conduction through your fluid (as opposed to convection), the energy timescale can be quite large. Setting the timestep of your energy equation to 10x or 100x larger than the fluid timescale can speed things up significantly.

Also, if your fluid properties are not temperature dependant and the hydrodynamic equations have already converged, consider turning off the solution of fluids by setting the following expert parameters:

solve fluids = f solve turbulence = f

You will find these in the expert parameters panel in Pre.

Regards, Robin

I thank you, your advice about setting the timestep of y energy equation to 10x or 100x larger than the fluid timescale was come good for H-energy converge speed.

I did not select inc. viscous work term in Heat ransfer menu. could been that option selected for good converge?

again i thank you. best regards. cmete

Hi Robin,

I saw your comment on h-energy imbalances in solids when simulating an adjacent air domain. How about transient simulations? It is normally not possible to set a different time step for solid and fluid. In my case, a free convection flow in a room enclosed by solids, high T-energy imbalances (up to value 2-10)occured in some solids (particular in the horizontal top and bottom located solids) and low h-energy imbalances in the fluid. I believe the imbalance occurs because of the different thermal time constants of the solids and the fluid on one hand and on the GGI interface on the other hand (surface mesh at interfaces are not 1:1). Is it OK to neglect the energy imbalance, if the other convergence criteria e.g. RMS=1e-5 are met? Thanks in advance for your help. Regards Tobias

Hi Tobiax,

The requirements for convergence are different in a transient simulation. It becomes importatant to converge the residuals within a timestep (this time including the transient term in the residual calcualtion), but it is no longer important to reduce global imbalances. This is not because global imbalances are unimportant, but rather because what you are trying to do is resolve the transient behavior accurately.

The difficulty with a transient CHT calculation is that the solid timescale is so much larger than the fluid timescale. To resolve the fluid behavior accurately, you must take a small timestep, but you still have to run for a long period of time to heat up your solid. The imbalance in your solid is simply indicating that it is still heating up (since the difference between what goes in and what goes out is what is accumulating in the domain).

If your fluid flow is nearly steady state, you can probably get away with a large timestep for your whole simulation. Better still, if the fluid temperature only changes slightly, you can assume constant properties relative to the temperature. In such a case it would be reasonable to solve a steady state flow and freeze this for the duration of your transient simulation. You would do this by initializing your transient simulation with the steady state solution and set the expert parameter 'solve fluids = f' and 'solve turbulence = f', leaving energy on. Your flow field would remain unchanged and you would only need to solve the energy equation, which is much cheaper, and you could use a large timestep.

Regards, Robin

Robin,

> The imbalance in your solid is simply indicating that it is
: still heating up (since the difference between what goes in
: and what goes out is what is accumulating in the domain).

this was exactly what I hoped to hear

If I understand it correctly, this means that it is OK having some imbalance in a solid domain (with high thermal mass) when going to the next time step since the imbalance does not show numerical error but only the process of heating up due to the capacity. Correct?

Thank you for your kind help, Robin.

Kind regards Tobias

Hi Tobias,

This is exactly right. The control volume equations include flux terms for quantities flowing into and out of a control volume and a transient term, which accounts for the accumulation within a control volume. If the equations are solved correctly, these should balance out, i.e. what goes in should be equal to what goes out plus what accumulates. The residual is obtained by taking the sum of all three of these. If the equations are not fully solve, the residual is not zero.

At steady state the transient term should go to zero and therefore the fluxes should balance out themselves. So in a steady state calculation, CFX does not include the transient term in the residual.

In a transient simulation, it is important to ensure the equations solved within a timestep accurately represent the transient evolution of the control volume. In this case the residual does include the transient term, because how the control volume changes is important. This is why you can converge within a timestep in a transient simulation and why the residuals are different than in a steady state.

Regards, Robin

Robin, Excellent. Thank you again! Kind regards Tobias

[happy]

Originally Posted by Robin
;79037

Hi Tobiax,

The requirements for convergence are different in a transient simulation. It becomes importatant to converge the residuals within a timestep (this time including the transient term in the residual calcualtion), but it is no longer important to reduce global imbalances. This is not because global imbalances are unimportant, but rather because what you are trying to do is resolve the transient behavior accurately.

The difficulty with a transient CHT calculation is that the solid timescale is so much larger than the fluid timescale. To resolve the fluid behavior accurately, you must take a small timestep, but you still have to run for a long period of time to heat up your solid. The imbalance in your solid is simply indicating that it is still heating up (since the difference between what goes in and what goes out is what is accumulating in the domain).

If your fluid flow is nearly steady state, you can probably get away with a large timestep for your whole simulation. Better still, if the fluid temperature only changes slightly, you can assume constant properties relative to the temperature. In such a case it would be reasonable to solve a steady state flow and freeze this for the duration of your transient simulation. You would do this by initializing your transient simulation with the steady state solution and set the expert parameter 'solve fluids = f' and 'solve turbulence = f', leaving energy on. Your flow field would remain unchanged and you would only need to solve the energy equation, which is much cheaper, and you could use a large timestep.

Regards, Robin

Hi Robin,,
After the energy equation is convergenace how I can get my overall solution. I mean the flow field solution and enrgy solution.
please help me ASAP.
Best Regards
CFD user

[ghorrocks]

Robin has not been sighted on this forum for years.

My preferred method of getting CHT simulations to convergence is by using a solid time scale factor. For typical air/steel systems (for example) a time scale factor of 1000 would be a good starting point.

Your comment suggests you have miunderstood robin's comment. You only freeze the fluids equation after it is converged.

[happy]

Originally Posted by ghorrocks

Robin has not been sighted on this forum for years.

My preferred method of getting CHT simulations to convergence is by using a solid time scale factor. For typical air/steel systems (for example) a time scale factor of 1000 would be a good starting point.

Your comment suggests you have miunderstood robin's comment. You only freeze the fluids equation after it is converged.

Hi again
yes, I did it after I post my question.
Actually, the fluid field solution is remained and has been used to complate the convergance for energy equation within solid domain. After, it get convergance, the complete solution will be together within res file.
great hint
Bye

[bemomb]

Hey everyone,


I have a question concerning the topic: In my case, there is a cylinder filled with oil (created the material by myself) in a big box simulating the atmosphere (air). Thus I have two fluids. What I don`t understand is why the imbalance for the oil that is in an enclosed area goes down (light blue)?



Thanks in advance

[ghorrocks]

Most likely it is because your simulation is not converged.

[bemomb]

Hey glenn,

Thanks for your answer. If i check the other residuals as well as my monitor points, the solution seems converged:/

[ghorrocks]

The imbalances are saying it is not converged. There are many simulations where residuals and values suggest it is converged but the imbalances do not. Simulations which show this are usually ones with something which acts on a slow timescale relative to the rest of the simulation - examples are a big block of material which slow heats up to temperature, or a large tank whose contents slowly rises until it gains equilibrium.

You should add imbalances to the converge criteria so you have this covered.

[bemomb]

Good morning glenn,

In fact, in my case, there is a thick disk in the cylinder that slowly heats up. I read in another thread that in such a case you should increase the solid timescale, so I increased it to 1000 s. I did the simuöation before with a mixture of air and oil inside the cylinder and there were no problems with the imbalances, only when I changed the fluid inside to pure oil I got the result as shown in the picture above. However, I will try to let the simulation calculate further and see what happens with the imbalances.


regards
Benni

[bemomb]

Is it possible that I have to increase the fluid time step as well due to the fact that the fluid is now oil instead of air and thus also needs more time to heat up?

[Gert-Jan]

Better use the the expert parameter "Solve fluids = f" and "Solve turbulence = f" for several iterations with a large timestep. Then the energy equation is solved solely. This allows temperature to propagate through the fluid fast. You can do this 'on the run'.

This is only useful if the coupling between fluid and energy is weak.

Look at point 2 using the following FAQ-link:
https://www.cfd-online.com/Wiki/Ansy...gence_criteria

[ghorrocks]

Hi Gert-Jan

In CHT simulations the coupling is strong - the issue is the timescale of the heating is orders of magnitude slower than the fluids time scales. So a timescale which converges nicely in the fluid is very slow in the solid and you have to do zillions of iterations. I would recommend using solid time scale factor (for steady state runs only) as a better approach than turning equations off as it can greatly accelerate the solid progression yet still update the coupling to the fluids as it goes.

If it is still converging slowly with a time scale factor of 1000 then use a bigger time scale factor.

[bemomb]

Hey guys,


Thanks for your answers. @glenn yes that's exactly what I did. I increased my solid time scale factor and everything went well with the steel-air combination. But when I changed my fluid to oil, the fluid-imbalance became problematic even with larger solid time scale factors. So I basically want to know if it makes sense to increase the fluid time scale as well (lets say 1000 for solid and 10 for fluid) or does that make no sense?