CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   just calculating the energy equation (http://www.cfd-online.com/Forums/cfx/72796-just-calculating-energy-equation.html)

peterle February 18, 2010 06:01

just calculating the energy equation
 
Hey guys,

I'm working on a simulation of a heat sink. As I have only small temperature variations in the heat sink, I consider the physical properties to be constant -> one-way coupling between Navier-Stokes and energy equation.

I finished to simulate the hydrodynamics of the system and want to add the thermal analysis. I don't want to solve the N-S equations again. How can I tell CFX 12 to use my result from the hydrodynamic analysis and just calculate the energy equation? What do I have to consider regarding names of domains and boundary conditions? Are they supposed to be the same? What happens if I change the grid (Perhaps the grid has to be finer for the thermal analysis)? Before I was just modeling the flow channels, now there is a massive domain of solid material involved? Is there a problem due to the fact, that I add domains to the simulation?

It would be nice if someone could share his experiences with this kind of two-step approach in CFX

JDA April 21, 2010 16:48

If I understand you correctly, you solved the Navier-Stokes equation without regard to heat transfer. Now you want to solve both the fluid flow and the heat transfer, but don't want to start from scratch, is that right?

What you need to do is edit your .def file and include the energy components (both solving the heat transfer and including heat transfer BCs, the default heat transfer BC is adiabatic wall). Write a new .def file (probably want a different name to keep things separate) and setup a new run. In the define solver run window, check the initial conditions box and browse to your .res file from the fluid flow. You can use a different (more or less refined) mesh and it will interpolate the values onto the mesh. I don't think you can add a domain, but it's worth a shot to give it a try. I usually model all the domains and just apply walls to the solid surfaces if heat transfer is not being studied initially.

ghorrocks April 21, 2010 22:32

An alternate approach is you can use expert parameters to turn the fluids solver off and continue running. This way you will only solve the heat equation with the fluid field fixed so the simulation will proceed much faster.


All times are GMT -4. The time now is 02:09.