[Jiricbeng]

Hello,
I have transient analysis in CFX including heat transfer - fluid and solid domains are presented (conjugate heat transfer model). The calculation simulates 10 hours during the day, the temperature distribution during the day is the goal of the analysis. Some solids are source of heat flux and the value of their heat flux is changing during the day (parabolically - from zero to maximal value and then to zero again).

The question is:
In terms of numerics and "quality" of the results is it better to have:
1) Timestep 1 hour (10 timesteps) with 40 iterations per timestep
2) Timestep 0.25 hour (40 timesteps) with 10 iterations per timestep

I think that becuse the conditions (heat flux from solid) are changing, it should be more convinient to choose option 1. In fact in each timestep, there is a new boundary condition (new value of heat flux), so the numerics needs more iterations to converge. Moreover, I think that both timesteps 1 hour and 0.25 hour are "big enough" to damp some flow phenomena. In another words I think a relatively big number of iteratons should be needed in both cases. Therefore in this case I think that having less number of timesteps with more iterations could be better for "quality" of the results.
Can someone add some opinion? Thanks in advance.

[Opaque]

It seems there is a confusion on what these two parameters do.

The goal of any simulation is to obtain meaningful accurate results. To do so, you discretize space-time and solve the equations of interest. The equations must be solved "exactly" or to a certain level of tolerance (residual convergence criteria).

The timestep gives the accuracy, and the iterations within the timestep give you partial control of not overworking a timestep. The goal of the timestep is to converge it correctly (user's criteria). The number of iterations within the timestep is irrelevant if the equations are converged to the level of interest.

Did I make sense ?

[ghorrocks]

With Opaque's background in mind you should be able to see that the answer to your question is neither 1 nor 2 is appropriate. CFX works best for most transient simulations when you have 3-5 coeff loops per time step. So use adaptive time stepping homing in on 3-5 coeff loops to find whatever time step size that results in.

[Jiricbeng]

Thank you both very much for the reply. Well, I think I understand the principle.
Just to clarify the situtation again - the transient analysis simulates 10 hours. There are heat sorces and flowing air from air condition. The velocity of the air at the inlet is about 10 m/s. Based on this, the proper timestep should be very little, something like 0.1 s. It is "impossible" to calculate 10 hours with such small timestep. So I have to increase the timestep to a bigger value. And I think that if you increase timestep to 15 minutes or 1 hour, both 15 minutes and 1 hour are just big values, so the numerics does not differentiate if it is 15 or 60 minutes, because in both cases the change of the boundary conditions (heat flux from solid) is not small, so the numerics needs a relatively enough iterations to converge...
I think it would be meaningful to have small time step (e.g. 0.1 s, 0.5 s or 1 s). And if the timestep is "big", it does actually not matter if it is 10 minutes, 15 minutes or 60 minutes because the flow phenomenons are damped anyway. Because the goal of the analysis is temperature distribution during the day and of course my effort is to decrease computational time.

What are your opinions?
Thank you very much.

[ghorrocks]

Based on this, the proper timestep should be very little, something like 0.1 s.

I don't follow. Why does that imply the time step should be 0.1s?

The rest of your comment shows a fundamental misunderstanding of CFD. You need to have a time step small enough to resolve the things you need to resolve. You can't just use a bigger time step and think that you will still get useful results.

You have to start from determining what the appropriate time step is, and then you get appropriate computing resources for the simulation which results from it. You cannot do it the other way around.

I recommend you:
* Activate adaptive time stepping, homing in on 3-5 coeff loops per iteration.
* Run the simulation and you will find the appropriate time scale. I cannot say whether it is going to be bigger or smaller than your estimated 0.1s, it could be either
* When you find the timestep size then you can work out an estimated simulation time. If this is too long you can:
- get more parallel machines and licenses
- decide the simulation is too complex, so simplify it
- decide the simulation is not worth the cost

[Jiricbeng]

Thank you for letting me know I have fundamental misunderstanding of CFD. Sure, only those who do the code can say they understand it. 0.1 s is just a rule of thumb based on maximum velocity and geometry.

Well, I think you know the term "industrial convergence" and all the issues you must come across to deliver the results in time although CPU resorces are not infinite.

[ghorrocks]

Yes, sometimes near enough is good enough, that is very true. But there is a minimum amount of resources you need to achieve even that level of accuracy and if you don't have that amount of resources it is better to say that the simulation is impossible and not attempt it - then you can focus your attention on areas where your effort is going to be more valuable. Rather than to cut too far and end up with a totally misleading result.

Regarding time step - CFX is an implicit solver and so the time step required for accuracy and convergence is not a simple function of velocity and geometry. This is the case for explicit solvers, but not implicit solvers. For implicit solvers the time step should be selected based on a sensitivity study, or the ease of convergence I described before.