# Query on Natural Convection simulation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

December 10, 2010, 06:47
Query on Natural Convection simulation
#1
Member

Dynampally Pavitran
Join Date: Mar 2010
Location: India
Posts: 74
Rep Power: 9
Hello all,

I am simulating a natural convection problem in a differentially heated 2D enclosure(pls see the attachment for boundary conditions used). I am carrying out the simulations for varying Rayleigh numbers( Rayleigh number is based on the dimension of the geometry, L=H).

The rayleigh number relation used is: (g*Beta*delT*L^3)/(Kinematic viscosity*Thermal diffusivity)

All the air properties are taken at 75 C i.e at Prandtl no: 0.716
g :9.81 [m/s^2]
Beta: Thermal expansion coefficient : 2.87E-03 [1/K]
delT: temperature difference : 50 C
Kine.viscosity: 2.05E-05 [m^2/s]
Thermal diffusivity: 2.85E-05 [m^2/s]

therefore for L=H=0.02 [m] , the Ra No is: 1.92E+04

in CFX pre , I created material air with properties at 75 C and used laminar and thermal energy equations with Buoyancy ref temp of 50 C.

The convergence criteria for Momentum & continuity was 1E-4 and for energy 1E-6 with conservtion target as 0.01. Discretization scheme was high resolution with auto time scale.

The predicted nusselt number is about 100, whereas it should be around 2.5. and also the rayleigh no written in the out file is about 9E+01.

My question is:
1. why the rayleigh no. is coming different in the out file?
2. what may be the reason for overprediction of nusselt no.?
Attached Images
 geom.jpg.jpg (22.4 KB, 27 views)

 December 11, 2010, 06:11 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,326 Rep Power: 110 This is a standard benchmark simulation so you should be able to get very accurate answers. If you are referring to the Rayliegh and Nusselt numbers described in the output file then you should ignore these numbers. These numbers are in the output file so you can estimate what regime the flow is in to check your physics (eg laminar vs turbulent) is correct. The calculation of these numbers is based on an arbitrary length scale (the cube root of the total volume from memory), material properties (the mass average over the entire domain) and flow velocities (again I think it is the mass average over the whole domain). This means the numbers coming out from this calculation have little to do which traditional definitions of say, Rayliegh numbers, which should involve the distance the plates are apart and the temperature of the two plates. To get accurate Rayliegh and Nusselt numbers out of your simulation you need to: 1) Define a CEL expression which uses the correct definition of Rayliegh/Nusselt number and outputs that to a monitor point, AND/OR 2) Use CFD-Post to extract the quantities required to calculate the numbers with the definition you require.

September 24, 2017, 03:07
#3
New Member

Praphul.T
Join Date: Dec 2013
Location: Kochi, India
Posts: 6
Rep Power: 6
Quote:
 Originally Posted by ghorrocks This is a standard benchmark simulation so you should be able to get very accurate answers. If you are referring to the Rayliegh and Nusselt numbers described in the output file then you should ignore these numbers. These numbers are in the output file so you can estimate what regime the flow is in to check your physics (eg laminar vs turbulent) is correct. The calculation of these numbers is based on an arbitrary length scale (the cube root of the total volume from memory), material properties (the mass average over the entire domain) and flow velocities (again I think it is the mass average over the whole domain). This means the numbers coming out from this calculation have little to do which traditional definitions of say, Rayliegh numbers, which should involve the distance the plates are apart and the temperature of the two plates. To get accurate Rayliegh and Nusselt numbers out of your simulation you need to: 1) Define a CEL expression which uses the correct definition of Rayliegh/Nusselt number and outputs that to a monitor point, AND/OR 2) Use CFD-Post to extract the quantities required to calculate the numbers with the definition you require.
So does this mean that the length scale used in Rayleigh number calculation according to the Fluent user manual is the cube root of total volume ?

 September 25, 2017, 11:28 #4 Senior Member   Join Date: Jun 2009 Posts: 732 Rep Power: 15 A bit confused. You are running ANSYS CFX, and you are using the ANSYS FLUENT documentation to understand the output? Keep in mind dimensionless numbers use reference values which can be defined differently for different audiences, i.e. there is no universal definition unless it is a material property such as the Prandtl number for example. Check their definitions for each case, i.e. read CFX documentation to understand their definition. If you do not feel comfortable with their definition, feel free to evaluate the quantity using what is most convenient for your simulation.

 September 29, 2017, 09:23 #5 New Member   Praphul.T Join Date: Dec 2013 Location: Kochi, India Posts: 6 Rep Power: 6 No no. Pavithran is some other guy who asked the question initially. While reading the reply of ghorrocks to pavithrans question , i got confused and thus asked the question. I use fluent and they have defined L as the characteristic length in Rayleigh number Ra calculation. I am pretty sure they have defined Ra in the same way in cfx. Well for square domains it isn't much of a problem as L=H. But for rectangular domains what can be L ? For a text book problem , normally we use the fluid layer depth as the characteristic length. What I didn't understand was that why the cfx solver takes in cube root of total volume as length. But thanks to you , i now understand that the dimensional numbers are calculated using the reference parameters that we specify in the solver. Sent from my Lenovo A2010-a using CFD Online Forum mobile app

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post dbecker CFX 5 October 13, 2010 19:07 vidhuresh FLUENT 2 October 25, 2009 10:52 phsieh2005 Main CFD Forum 7 June 11, 2007 08:01 Greg Perkins Main CFD Forum 0 February 12, 2003 19:43 Basics CFX 3 September 25, 2002 09:42

All times are GMT -4. The time now is 03:30.

 Contact Us - CFD Online - Privacy Statement - Top