[Tasos]

Hi all,
I have some questions about the start values of k and ε for internal and boundary field.
a)Why do we need start-values for k and ε in a k-ε model? For example if i put 0 in the start values i have an error, why is that happening?
b) How can i find the start values for k and ε for my simulation? Is there any equations for that reason or do i have to took the decision by comparing the results with the experiment data? For example i made some tests for k and ε values (0.000001 , 0.0002 and 0.2), and the best results were for the 0.2 value. I wanna know if the correct way to take the start values for k-ε is the way that i took or there is another way? To be more specific, while i was doing my tests i used the same start values both for the internal field and boundary field.

P.S. i used interFoam solver and i have a dam break problem, so i don't have start value for velocity.

Thank you very much i would appreciate any help.

Regards,

Tasos.

[jhoepken]

Have you checked this site: http://www.cfd-online.com/Wiki/Turbu...ary_conditions ?

[Tasos]

First of all, thank you for your reply. Yes i saw this yesterday, but the thing is that i have a dam break problem. So i don't have a start value for velocity (inlet).
The boundary conditions that i have are :
leftWall, downWall, atmosphere and at the right side outlet. Any ideas?

[Phicau]

Hi Anastasios,

since the case starts from rest I would initialize k and epsilon to very small values (but not zero to avoid zero division error). No velocity means 'zero' turbulent kinetic energy and dissipation rate, and will yield 'zero' turbulent viscosity.

If your turbulence is not producing the results you expect there are a number of elements to take a look at: interface compression, mesh, turbulence model constants...

Best,

Pablo

[Tasos]

Hello Pablo,

Thank you for your answer. As i said before, i had put 3 start values for both k and ε. (k and ε 0.2, 0.0002, 0.000001). One would expect that closer to the experimental results would be the simulation with the start value 0.000001 but this didn't happen. The best results was for the start value 0.2. Thats why i am concerned. What do you think?

Best regards
Tasos

[wyldckat]

Greetings to all!

@Tasos: I got the PM you sent me and I've given a quick read to this thread.

From my experience, the solver usually tries to tell you during the simulation what each turbulence-related field should have for a specific flow situation. It will either crash or have really weird values (e.g. 1e15) if the values are very bad.

In addition, the turbulence-related fields are mostly theoretical/empirical models, whose values don't necessarily equate to something physical, since they simply are sort-of of a modelling approximation to how turbulence behaves. In other words, your mileage may vary, depending on your own case. I believe this is explained on the wiki page that jhoepken indicated. And Phicau also gave a good brief answer

My take on the initial questions:

1. Turbulence-related fields, such as k-epsilon, usually cannot not have 0 values or negative values, because they will eventually equate to a viscosity term. This means that if the value were to be 0, the fluid would essentially not exist, since it had no viscosity. If negative, it would be a sentient fluid
   Although in reality, the equations will use k-epsilon values in the denominator part of fractions, leading to a division by zero, namely SIGFPE: http://en.wikipedia.org/wiki/SIGFPE
2. My advice is to play around with the tutorial "incompressible/simpleFoam/pitzDaily". If you change the U value at the inlet and run the simulation for several iterations, you'll see what happens to the turbulence fields inside the simulated domain. If the U values are very low, these fields will essentially be very smaller than the initial values defined at the inlet.
   For example, the inlet value for "k" is 0.375, but when U is not the original 10.0 m/s, but in fact 0.001m/s, the simulation will result in the "k" field to reduce to something like "1e-6", even though the inlet is injecting k=0.375. This is sort-of like the solver is trying to tell you that the actual "k" values are a lot lower.

How can you know when the k-epsilon fields are correct? Well... technically, you can't... at least not according to my personal experience, but I'm not a CFD expert either .
But AFAIK, technically only with experimental results can you try and find which values better approximate the simulation to the experimental results. Of course you will also to need to take into account the fact that you need to be careful regarding which turbulence model you're using and if you're using a steady-state solver or transient solver and so on...

I guess the easiest way to explain this is: first solve a known and simple experimental case, such as a 2D or 3D cylinder inside a flow, to see the vortices developing behind the cylinder; for example:

1. With laminar flow, it's unlikely you'll see any vortices.
2. With excessive turbulence flow, it'll be too chaotic and probably non-physical.

Then you'll gain the necessary experience and confidence to adapt your newly gained experience to your current case.

Best regards,
Bruno

[Tasos]

Thank you very much Mr Bruno and all of you, i appreciate your answers. Helped me a lot