Hello! I'm studying transition of heat across steel plate to the water. From experimental setup we determined the 2D velocity field of the problem. I have created the same geometry in CFX (with nodes on the same place as the velocities from the experiment are). The problem arised when I had to implement the obtained velocities in to CFX before solving. Probably this requires the use of Fortran subroutine but I've never done it. Can anybody give me some clues on how to do it? Thank's in advance! Matjaz

Hi,

If you are using CFX-4, you will need to write a fortran for this!

If you are using CFX-5.6/5.7 you can directly import the experimental data and apply the same on the boundary. This can be done using the User functions. You can either create a 1D or a cloud interpolation function.

You can contact your CFX-support people who would eb able to provide you with examples.

Let me know if you require any further inputs.

Regards, test

Later I've figured uot that initial conditions can be predetermined usig *.csv files which are actually excel files using comas beetwen values. This csv file can be later imported in to CFX. I will give a detailed description on how to do it later.

Matjaz

After almost giving up I finally solved the riddle. I'm giving a detailed description on how to implement Velocity field in the initial condition. As mentioned the problem occured when I had to determine heat flux thru steel plate to water with known velocity fied. I figured out that this can be done using *.csv files. I've found some directions in tutorial Tut03Inject_Mikser and by reading InjectMikser.pre both located in CFX5.7/exsamples directory. Here is how I've done it:

After defining boundary conditions specify not to solve fluids. Go to Create - Expert Objects - Expert Parameter - Model Overrides, Check solve fluids and set it to f (false). - OK.

Go to Tools - Initialise profile data. Browse for the csv you want to import. If the file is accepted you should get in the same window parameters Coordinates, Values and Units. - OK In the Physics - Library you should see CFX Expression Language - fx (name of the surface where the condition applies) - Data Field:Velocity u, v, w in my case

Define Initialisation by cliking on Global initial conditions for fluid domain. Check domain initialisation - check Initial conditions - Velocity Type set to Cartesian and specify for U, V, W: "Surface where the condition applies".Velocity u(x,y,z) "Surface where the condition applies".Velocity v(x,y,z) "Surface where the condition applies".Velocity w(x,y,z) - OK If every thing is ok no errors will be displayed.

The csv file should look like this:

[Name] Surface where the condition applies

[Spatial Fields] x,y,z

[Data] x [ m ], y [ m ], z [ m ], Velocity u [ m s^-1 ], Velocity v [ m s^-1 ], Velocity w [ m s^-1 ] Here down comes the data separated by comas.

I suggest you read tutorial and look at the pre file to see how it is defined. Good luck

Matjaz