CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   CFX Cable Tunnel Modelling (https://www.cfd-online.com/Forums/cfx/75666-cfx-cable-tunnel-modelling.html)

 ibrahim.mohamed May 2, 2010 15:01

CFX Cable Tunnel Modelling

1 Attachment(s)
Here is a description of a modelling problem I am currently working on.
A hot cable is installed concentric to a circular tunnel. Air at 25oC is blown at 15m/s (x-direction) through the tunnel for cooling. Please see the image attached.

The objective is to find the variation of temperature from the cable surface to the tunnel wall and find the rate of heat transfer from the cable to the surrounding air and tunnel wall.

Problem: Currently the tunnel is 10m long. This is to allow the incoming flow to develop a fully developed profile. The issue is the tunnel may be not long enough.

Proposed Solution: Apply periodic boundary conditions such that the outlet flow is the inlet flow

How do I do this? How to I apply a periodic boundary condition in this case?

I am relatively new to CFX and I am using version 11.0. Any help you can offer would be highly appreciated.

 ghorrocks May 2, 2010 17:31

Firstly I see you have meshed the wire. You have defined the wire as a fixed temperature so there is no need to mesh the wire. It can be a fixed temperature boundary condition on the air domain.

If you are only worried about the fully developed heat transfer then periodic boundaries make sense. You can do this is CFX V11 using a domain 1 element thick with periodic boundaries on both sides, but I think you need to use a momentum source to move the flow along. This is much easier in V12 as periodic boundaries have been improved to make this type of modelling easier.

 ibrahim.mohamed May 3, 2010 07:32

Quote:
 Originally Posted by ghorrocks (Post 257229) Firstly I see you have meshed the wire. You have defined the wire as a fixed temperature so there is no need to mesh the wire. It can be a fixed temperature boundary condition on the air domain. If you are only worried about the fully developed heat transfer then periodic boundaries make sense. You can do this is CFX V11 using a domain 1 element thick with periodic boundaries on both sides, but I think you need to use a momentum source to move the flow along. This is much easier in V12 as periodic boundaries have been improved to make this type of modelling easier.
Thank you very much ghorrocks.

The geometry is just an extrusion of two circles. So, when I ask CFX-Meshing to generate a surface mesh and a volume mesh to generate the complete mesh it does generate a mesh for the cable too. Also, I am going to apply a fixed heat flux instead of the fixed temperature once I figure out the periodic BCs. I guess meshing the cable is not an issue that can effect the results.

Thank you very much once again for the reply, I really appreciate it.

Ibrahim

 ibrahim.mohamed May 3, 2010 07:44

Quote:
 Originally Posted by ghorrocks (Post 257229) If you are only worried about the fully developed heat transfer then periodic boundaries make sense. You can do this is CFX V11 using a domain 1 element thick with periodic boundaries on both sides, but I think you need to use a momentum source to move the flow along. This is much easier in V12 as periodic boundaries have been improved to make this type of modelling easier.
Would be great if you could tell me whether to use translational periodicity or rotational? To my understanding rorational periodicity is for circular geometries. Correct me if I am wrong.

 ghorrocks May 3, 2010 07:49

OK, so in CFX-Pre then do not put the wire into any domain then it will not form part of the simulation.

Keep in mind that specifying the external wire temperature means simulating the wire is pointless (as it will just all be at the defined temperature) but if you impose a volumetric heat source in the wire then you will a temperature gradient in the wire. If you only specify the wall heat flux then, again, there will be no temperature gradient in the wire so no point simulating it.

And you will be looking for translational periodicity in the flow direction. If the flow has nothing to depart from axial symmetry then you can use additional symmetry planes to reduce the simulation down to 1D - and for simple 1D simulations it is often better to just write your own solver. But you can get CFX to do 1D stuff if you want.

 All times are GMT -4. The time now is 18:32.