Default values of turbulent kinetic energy and turbulent dissipation rate
 

In an indoor airflow simulation, supply air through the diffuser comes in to the room through a rectangular duct. While setting up the velocity inlet boundary condition for the supply air, if in case the turbulent intensity is not known in prior, is it deemed okay to use the Ansys Fluent default values of K and epsilon, which is 1?:confused:

No way in hell!

By the way, there is an intensity and hydraulic diameter option that will then use some cute formulas and correlations for fully developed pipe flows to calculate some values for k and epsilon. These will work way better than using the defaults.

Thanks for your kind reply LuckyTran.
I had given a simulation run based on turbulent intensity of 10% and hydraulic diameter (2ab/a+b), where ‘a’ is width and ‘b’ is height of the duct. Based on these settings, the TKE and TDR were observed to be quite small as compared to the default values. As expected the simulation with default values of TKE and TDR had given a different flow distribution within the computational domain as compared to the simulation run based on TI and Hydraulic Diameter. Although, the residuals got converged way faster in the former case as compared to the latter case. The latter case(i.e., TI and hydraulic diameter) took around 600 more iterations to get a converged solution. What would have been the likely possibilities for observing such a scenario?

The default tke of 1 is super super high for most flow scenarios. A more typical value is like 0.1 or 0.5. The default tdr of 1 is super super super low for most flow scenarios. A more typical value is like 100 or 1000. This is a big of a gross simplification because k and tdr are very low in the core of the flow and super high near walls (k approaches infinity near walls).

Results with different inlet boundary conditions will be different.

How many iterations it takes to converge will depend on your initial condition. Normally you guess a uniform field. The actual solution will not be a uniform field and also can be very different than your initial guess (especially if you are using the default values for the guess). You can expect the same geometric case with different BC's and initial conditions to differ vastly in how many iterations it takes to converge.

[QUOTE=LuckyTran;724531] This is a big of a gross simplification because k and tdr are very low in the core of the flow and super high near walls (k approaches infinity near walls).

Thanks a lot for your valuable comments.

Would you please elaborate a bit on this comment?

[QUOTE=Manu4CFD;724586]Thanks a lot for your valuable comments.

Would you please elaborate a bit on this comment?

But, wouldn't the results of simulation run with default values of TKE and TDR serve as an initial guess for running the simulation with TI and Hydraulic diameter???

While setting the TI and Hydraulic Diameter for inlet, is it necessary to set similar settings for outlet as well? Do turbulent specifications in the outlet impact the solution in anyway??

[QUOTE=Manu4CFD;724587]For all variables... velocity, temperature, k, tdr, etc... You specify uniform profiles at inlets and initial guesses but in reality there is a profile. For example, with velocity, it is 0 at walls but some positive number away from walls (and it can be an arbitrarily high number).

At inlets this profile is often ignored for simplification. For initial conditions, you often ignore the profiles due to laziness. Because you can iterate away the initial condition and eventually get the solution anyway. It takes some more iterations to converge with a bad guess than a good guess, but because the machine is doing all the work it saves you time.

Are you talking about boundary conditions or initial conditions? They are separate things.

For boundary conditions: the default values for k and tdr (1 and 1) are absolute garbage. The default values for TI and hydraulic diameter are also garbage. You need to set it to something that makes sense for your problem. It's easy to pick a TI and hydraulic diameter that makes sense... For TI you just pick a number between 1 and 10%. And hydraulic diameter you just set to the geometric scale of your inlet. But it's a lot harder for people to pick a k and tdr that makes sense. Because they have no idea what these numbers are.

For initial conditions: Take your best guess or use the defaults. If it doesn't diverge it probably converges eventually...

At outlets, these are backflow properties (not just turbulence, but also temperature and all transported variables) for when the outlet is not an outlet but becomes an inlet because the flow is going back into the domain. You can ignore these if you don't have any reversed flow.

I was referring to the initial conditions.
It is a common practice to use flow variables obtained from steady state airflow simulation as initial conditions for running unsteady airflow simulations, as it provides good convergence, solution robustness and realistic initial values for transient case.
Likewise, I was thinking whether it is reasonable to use the flow variables obtained through steady state simulation run with default values of TKE and TDR as initial conditions for running another steady state airflow simulation with TI set as 10% and Hydraulic diameter specified through geometric scale of inlet. Would such an approach provide us with a good initial guess???

So, its safe to ignore turbulence specifications at pressure-outlet boundary conditions. Kindly correct me, if what I inferred is wrong.

Right. Unless you have reversed flow. Note that it's not just turbulence, but all transport variables (temperature for example).


Also be careful that sometimes you have reversed flow during the simulation at intermediate iterations. If you put non-sensical values into the backflow properties your solution can easily diverge. Just keep this in mind. It shouldn't matter (when everything is going well), but sometimes it does (when everything is going badly).

My case involves an incompressible flow with density approximated by using the boussinesq model. I use "Velocity-Inlet" condition for inlet and "Pressure-outlet" at the outlet. After a few iterations, I tend to get reverse flow in a few faces during the simulation run, but the analysis eventually gets solution convergence.

As I understand, after reading through posts on reverse flow conditions, the best way to overcome the reversed flow is to to set:
1) Outlet far from my region of interest. But, what if you cannot change position of outlet?
2) Change "pressure-outlet" boundary condition to Outflow".
And if we change to outflow, would the results be affected vastly or would it be marginal?
3) Lastly, like you said, it is advisable to provide realistic backflow properties?
* But how to set one? Any guidelines?

1) Moving the outlet to another location applies in some situations where the outlet can be arbitrarily moved to another location. If your boundary is where it is supposed to be, then you cannot and should not move it.
2) Pressure outlet vs outflow is a very subtle difference. Use the right boundary condition for your problem and stick with it.

These recommendations apply more to modeled situations where there is freedom in the type of BC being used. For example, flow around an airplane or a car where the BC is a natural boundary condition and not a hard constraint on any variable.

3) the guideline is to make them realistic! And sometimes this means setting the values of the stuff coming in to be the same as the stuff going out. But just to give an example. If I have a combustion problem and the outflow should be at a temperature of 2000K and I leave the backflow properties at their default of 300K... well, that would not make sense. I should probably set it to something like 2000K. There is even an option in Fluent that takes values from adjacent neighbors. You should have an idea of what makes sense for your problem and what doesn't make sense. Otherwise, what really you are doing that is different than clicking random buttons?


That is not to say that reversed flow is always a problem. Sometimes you get reversed flow in some cells but you just don't care.

Thank you so much for your insightful comments.

May I know about the option in Fluent that would enable to take values from the adjacent cell Neighbors.

And in terms of reverse flow, I guess as long as the solution convergence is achieved with proper mass balance, the concern/warning can be neglected.

Sorry I lied. Or maybe I got my software confused.


In backflow direction specification method you can choose from neighboring cell, which is something else than what I was saying. There isn't an option to take values from neighboring cells.

Thank you so much for your time and valuable comments on my queries. :)

I have also a question about the turbulent dissipationrate epsilon. In Fluent, the definition of epsilon is:



I don"t understand where the exponent comes from.