# need suggestion on temperature simulation

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 19, 2000, 14:16 need suggestion on temperature simulation #1 Bin Li Guest   Posts: n/a I use the CFX to simulate two vertical flows(air) through some parallel dampers mixing in the HVAC duct chamber. The CFX velocity conforms with the experimental data, however temperature comparison looks poor. the experiment showed with the angle of the damper changing, the mixing flow temperature varies greatly, however the CFX didn't produce such result, it showed change, but not so big. What is the problem of it? is there anything I can do with the model? the two flow velocity is between 5-10 m/s. my group really perfer the experiment result. Thank you for your suggestion. Bin Li

 June 20, 2000, 11:19 Re: need suggestion on temperature simulation #2 Gert-Jan van der Gulik Guest   Posts: n/a Do you have strong cirulations in the main flow? Then be sure that you use a higher order differencing scheme, for example 'quick'. This makes a lot of difference. Regards, Gert-Jan

 June 20, 2000, 22:17 Re: need suggestion on temperature simulation #3 John C. Chien Guest   Posts: n/a (1). Always try to refine the mesh first. (2). And pay attention to the mesh density near the wall. (3). If your problem has flow separation in it, it is a good idea to use two layer model or low Re model. (4). Flow visualization comparison would be the ideal way to validate the simulation. (5). Internal flow with flow separations is one of the most difficult type of problem to solve.

 June 21, 2000, 03:31 Re: need suggestion on temperature simulation #4 Jan Rusås Guest   Posts: n/a When the velocities are correct and your problem is that the predictions shows a smaller spreading of the temperature than in reality, then the problem is probably not false diffusion-but try higher order differencing schemes anyway. Do investigate your mesh to see any problems in that direction as John proposed and if the flow is wall dominant look at your wall functions. The problem could also be related to that the temperature field is not well solved – depending on the problem, then the temperature fields is the last one to be finished. A good idea when calculation flows with heat transfer is after the initial calculation, where the velocity field has been probably calculated, is to do a calculation with the option ITERATIONS OF HYDRODYNAMIC EQUATIONS 0 under the program control – this forces the enthalpy and any scalar equations to be solved on a fixed flow field -. Have you checked and checked again that the inlet boundaries are the same for the CFD as in the experiment – the inlet bouundaries might have an influence on your problem – case dependant. In some cases is the reason for major differences in CFD predictions and experiments that – there is an error in the experimental measurements!!!! have you checked ? Hope it helps Regards Jan