CFD Online Logo CFD Online URL
Home > Forums > CFX

need suggestion on temperature simulation

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

LinkBack Thread Tools Display Modes
Old   June 19, 2000, 14:16
Default need suggestion on temperature simulation
Bin Li
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

  Reply With Quote

Old   June 20, 2000, 11:19
Default Re: need suggestion on temperature simulation
Gert-Jan van der Gulik
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
  Reply With Quote

Old   June 20, 2000, 22:17
Default Re: need suggestion on temperature simulation
John C. Chien
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.
  Reply With Quote

Old   June 21, 2000, 03:31
Default Re: need suggestion on temperature simulation
Jan Rusås
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
  Reply With Quote

Old   June 23, 2000, 02:35
Default Re: need suggestion on temperature simulation
Duane Baker
Posts: n/a
Hi Bin,

this is fairly typical of results that have plagued the CFD community since the beginning so don't feel too bad and give up.

First, concentrate on the flow physics in the experiment and then taylor the simulation to this. Three of the main issues in a good simulation are: 1. grid (number of nodes and distribution relative to where the high gradients are), 2. characteristics of the discretization scheme 3. physical models.

In the case of parallel dampers to the flow: it is likely a nice attached flow with slow changes in the streamwise direction. This means, in terms of the grid, one can predict fairly well apriori where to put the nodes ie. denser near the walls to reslove the higher gradients there and denser near the start and end of the vanes. The flow direction will be pretty much parallel to the walls so a structured grid parallel to the walls will be well aligned with the flow. Therefore cross-stream numerical diffusion is not big problem so even a bad discretization scheme like UDS may work. The attached and slowly changing (near equilibrium) conditions in the boundary layer mean that standard wall functions will probably work pretty well. Without the complexities of recirculation zones, streamwise curvature, and adverse pressure gradients the standard k-eps turbulent model will probably be ok too.

Now, when you turn the vanes significantly, much of the flow physics changes. Recirculation zones will occur where the flow separates from the backsides of the vanes. This problem requires a much more advanced attack than the first. The grid is nolonger going to be parallel to the flow everywhere and you have to add a lot of nodes to resolve the recirculation zones. You need a good discretization scheme that minimizes streamwise and corss-stream numerical diffusion. The standard k-eps turbulence model typically under-predicts recirculation zones because it overpredics the eddy viscosity and may need some modification. So, you have some work ahead of you. Start with a systematic grid refinement see Ferziger and Peric's book for more details on error evaluation.

Good luck...................Duane
  Reply With Quote


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Conjugate heat transfer: coupled wall temperature Sarah FLUENT 7 August 12, 2013 22:36
LTCC(Low Temperature Co-fired Ceramic) substrate simulation vineeth Main CFD Forum 0 October 28, 2009 01:25
Enquiry about the flame simulation in rotary kiln hassanelattar FLUENT 0 March 25, 2009 08:41
Temperature in vessel during throttling process Astrid Main CFD Forum 2 January 31, 2001 03:34

All times are GMT -4. The time now is 06:41.