CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   calculate heat transfer coefficient in repeated geometry (http://www.cfd-online.com/Forums/cfx/83239-calculate-heat-transfer-coefficient-repeated-geometry.html)

mullenc525 December 20, 2010 18:34

calculate heat transfer coefficient in repeated geometry
 
Hi,

I am doing some flow field design for a heat exchanger, and want to calculate the relative heat transfer coefficient and pressure drop for many geometries. These geometries will all be repetitive in nature along a channel in the heat exchanger.

I understand I can use a periodic BC at the 'inlet' and 'outlet' of the repeating geometry to solve the fluid flow, but does this work with heat transfer? Is it possible to solve the fluid flow without heat transfer, then calculate what the heat transfer coefficient would be if the geometry was not repeated and the wall temperature was different than the bulk temperature?

Thank you

ghorrocks December 21, 2010 05:09

I have not checked but I think you can include heat transfer in periodic boundaries like you suggest. But note that the heat transfer may not be periodic in that it is often driven by convection and that is proportional to (T-Tboundary), and will change as the flow proceeds. If the Tboundary is massive compared to T then it would be OK.

If heat transfer is decoupled from the flow (in that the temperature does not affect buoyancy, density or anything else significantly) then you can solve the fluid only, then freeze the fluid flow (using expert parameters) and get the heat transfer from one row and just multiply it out (subject to the convection caveat mentioned above).

joey2007 December 21, 2010 14:57

Glenn is right and his suggestion is the simplest approach to solve the issue. Some additional remarks on periodic flows. A periodic flow field can be modelled with translational periodic interface. It is possible to set a pressure offset at the interface which balances the pressure losses in the chanel. In the result the pressure profile plus offset is equal on both sides of the interface.

If you solve enthalpy equation in such setup, the enthalpy profile is periodic. For solving your issue it would be required to setup the temperature analogously to the pressure. With some limiting assumptions it is possible to formulate such a boundary condition. This implemented in Fluent but not in CFX.

You may realize by formulating some boundary sources for the enthaply with CEL. The boundary source has to balance heat flows in the domain.

We discussed this already under http://www.cfd-online.com/Forums/cfx...tml#post283314


All times are GMT -4. The time now is 13:35.