[octavyo]

Hi everyone,

I am modelling an absorber tube for CSP. The geometry is very simple: two coaxial cylinders and the gap between them is filled with H2. Inside the inner cylinder molten salt is flowing.

I would like to make a conjugate heat transfer and I created two domains: a fluid domains representing the gas between cylinders and a solid domain representing the inner tube. Since there are two different domains I had to crate a Solid -Fluid domain interface.

I have an experimental data about the distribution of the radiative heat flux on the absorber tube and I would like to apply this heat flux to the inner tube as a profile boundary condition. Since I used the same surface to create the domain interface, CFX solver does not work.

Does any one have an idea how to apply the heat flux to the absorber tube?
Please help

If the problem is not clear enough, please let me know.

[joey2007]

At home I have no CFX to check, at work I have no time left for such things. If I remind correctly:

In CFX-Post there is a feature to export 3D profiles. Do it for an arbitray result. You will get an csv-file wich is readable with an editor. You can change the header and write in your data in the same format. Then go to CFX-Pre and use initialize profile data. This procedure introduces a CEL function. This can be used to set a boundary source on your interface or something like that.

Hope I mixed nothing up with other codes I used already.

[octavyo]

Thanks for your reply joey2007, but the problem is not about the data profile file. I created a data file and loaded it to CFX-Pre.

The problem is that I need to implement this boundary condition to the solid-fluid interface but since I used the surface, which I would like to implement the profile boundary condition, to make up the solid-fluid interface, Ansys does not allow me to use the same surface because it already formed another boundary condition.

I think, I will add a 2D boundary source term to the surface and use a Fortran routine to define the data profile.

BR

[topsedar]

Hi dears !
I am also modeling absorber tube of a PTC. and also i have the same problom.

What should i do to solve the problem??

[octavyo]

Create 2d boundary energy source on the surface and define the energy source by using the distribution data you already have.

If you are working on a comprehensive thermal model, you should take into account the radiation between the surfaces, solar radiation absorbed and reflected by the glass envelope, radiation emitted and reflected by the coating of the absorber tube along with the conduction and convection.

[topsedar]

Thanks Dear octavyo
Do you mean i should use Fortran subroutines ?

If yes, Could you plz introduce(send) me help of creating Fortran subroutines? and an sample of 2D profile That you created for modeling absorber tube for CSP?

and a general question:
in which domains should i active the Radiation Models?
(the following picture shows my domains)



did you suppose the glass as a gray material or not?
Have U tried to model an Ideal Vacuum Space between absorber tube and glass envelope or not? if yes, how???

Thanks in advance For your attention and help

[ghorrocks]

What is a PTC?

[topsedar]

PTC means parabolic trough collector ...

[octavyo]

There is no need to use Fortran, an excel file is enough. In my model, I created 2D boundary energy sources on the surface of the glass vacuum jacket and the absorber tube to model the absorbed non-uniform solar heat flux. If you have the distribution data, you are able to enter the location and magnitude of the heat flux into CFX.

I never activated the radiation model, instead, I formulated the radiation heat transfer between the surfaces with net radiation method and modeled it by defining 3D energy sources within the solid domains, glass vacuum jacket and absorber tube. Because CFX does not allow radiation to escape from the boundary of the solid domain to the environment. In case of the solar receiver, some radiation emitted at the surface of the absorber tube escapes to the environment through the vacuum jacket. Moreover, CFX does not allow defining the radiative properties of a surface if the surface is opaque.

I implemented the gray-band approximation for radiative properties of the glass and absorber tube because radiative properties of the surfaces are heavily wavelength dependent.

In reality there is no absolute vacuum within the gap but very low pressure gas exists eg. 0.05 Pa. So I defined low pressure gas with very low conductivity for the vacuum.

[topsedar]

Originally Posted by octavyo

There is no need to use Fortran, an excel file is enough. In my model, I created 2D boundary energy sources on the surface of the glass vacuum jacket and the absorber tube to model the absorbed non-uniform solar heat flux. If you have the distribution data, you are able to enter the location and magnitude of the heat flux into CFX.

Yes It Really Works. Thanks For Your Help

Originally Posted by octavyo

I never activated the radiation model, instead, I formulated the radiation heat transfer .....
I implemented the gray-band approximation for radiative properties of the glass and absorber tube because ...

1- do you mean, you used Stephan Boltzmann equations?
coluld you plz Write an example expression?

2-IF you didn't active Radiation Model, I think there is no need to set Radiation Properties for glass and absorber tube .
What is necessity of this act?

Originally Posted by octavyo

In reality there is no absolute vacuum within the gap but very low pressure gas exists eg. 0.05 Pa. So I defined low pressure gas with very low conductivity for the vacuum.

I tired to set different pressure gas for vacuum domain but there is no difference between the results !!
any Idea? what is the reason?

[ِAbdullah]

Dear all
Please how can I find the thermalboundary condition, non-uniform solar heat flux distribution around the absorber tube in parabolic solar concentrato to set as Boundary Condition in Ansys cfx. (If you have any tutorial )

Best regards,