Turbulence boundary values
Hi!
I need your suggestion which kind of turbulence boundary condition to be used. I calculate flow field and mixing between heated rod bundles. I already have a result file, and I would like to set the inlet turbulence parameters for a new run on the basis of the outlet results of this previous calculation. I use the kOmega turbulence model. I can export the following turbulence parameter values: Eddy Viscosity [kg /m/s] Shear Strain Rate [1/s] Turbulence Eddy Dissipation [1/m2/s3] Turbulence Eddy Frequency [1/s] Turbulence Kinetic Energy [1/m2/s2] And I can set as input parameter the followings: Turbulent Intensity and Eddy Viscosity Ratio [dimensionless], [dimensionless] k and Epsilon [1/m2/s2], [1/m2/s3] Turbulent Intensity and Eddy Length Scale [dimensionless], [m] My problem is that I have a detailed result, but I can set only AVERAGE values. And for example in case the Turbulence Kinetic Energy (k) the values near the wall is much different than it is in the main flow. Which type of setting should I use? And how can I calculate these parameters from the parameters, which can be exported? (For example Eddy Viscosity Ratio = Eddy Viscosity/Dynamic Viscosity) Thanx: LEGO 
Re: Turbulence boundary values
You do not need to only set the average
If you use CFX4.4 you can set a value in each cell face with usrbcs. You can export the data you have to I file and read it in USRBCS If you are using CFX5 I think I recall that it is possible to do this very easy, it is possible to use the vaules from another calculation as input. Try to search the forum. Was the fantastic LEGO toys named after you :) 
Re: Turbulence boundary values
You won't belive...
There is no possibility to set an exported field as inlet boundary condtion in the CFX5.5. I have a direct contact to the support and they informed me. There is only a cloud interpolation method, but this method takes into consideration in every point the all other data point with a 1/r factor. So it blurs the field, and corrupts conservativity. They said me that their object to make possible to solve great problems (for example 8 000 000 volume elements) in one piece. They suggested to buy greater hardver... Yeah, I'm the LEGO's grandpa 
Re: Turbulence boundary values
This is not fully accurate as you can set the tolerance for the DWA method and switch to a "local node" approach ie take only the neibourinhg nodes into account for the interpolation to improve things (avoid spikes) I believe.

Re: Turbulence boundary values
It would be perfect for me because the meshes of the exported outlet and the inlet to be import are exactly the same.
I asked the support whether I can set or change the source of the cloud interpolation that it takes into consideration only the nearest nodes, but they said, it impossible. (I think DWA and cloud interpolation is the same... On the other hand I think this DWA method is a fool method, because the 1/dr weight function has singularity at dr=0. And I have data set with dr=0 in every points...) Do you know or only belive that setting local node approach is bossible in case of CFX5 (CFX5.5.1)? Because I could not find this mode. 
Re: Turbulence boundary values
... which is why I am saying there's a tolerance value to be adjusted via an env variable so that when dr <= tol, the interpolated value = the nodal value.

Re: Turbulence boundary values
Sorry if I made a mistake, I would though not be concerned about "bluring" it.
I once had a problem in the old CFX4.3 with periodic boundaries for a cylindrical problem, there was a bug in CFX for my problem so it was not possible to use the periodic boundaries. The answer to my problem was that CFD is so fast today that I should just solve it in 3D :))) making my mesh in this case 60 times bigger !!!! If you are LEGO's grandpa then you should have no problem in just getting more hardware. 
Re: Turbulence boundary values
Actually, if you have nodal data the distance is never zero, since boundary values are applied at the faces, not the nodes.
Robin 
Re: Turbulence boundary values
Yes, and it means, that in my case the weight factor depends on the last digits of the coordinate values...

Re: Turbulence boundary values
No. Face coordinates do not coincide with node location (see documentation for details). So in your case, you are not dealing with the last digits of the coordinate value.
If you have a grid for the upstream run, why not GGI them together and run the whole thing? Robin 
All times are GMT 4. The time now is 02:47. 