CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Query on Natural Convection simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2010, 06:47
Default Query on Natural Convection simulation
  #1
Member
 
Dynampally Pavitran
Join Date: Mar 2010
Location: India
Posts: 74
Rep Power: 9
pavitran is on a distinguished road
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
File Type: jpg geom.jpg.jpg (22.4 KB, 27 views)
pavitran is offline   Reply With Quote

Old   December 11, 2010, 06:11
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 14,326
Rep Power: 110
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   September 24, 2017, 03:07
Default
  #3
New Member
 
Praphul.T
Join Date: Dec 2013
Location: Kochi, India
Posts: 6
Rep Power: 6
praphul is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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 ?
praphul is offline   Reply With Quote

Old   September 25, 2017, 11:28
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 732
Rep Power: 15
Opaque is on a distinguished road
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.
Opaque is offline   Reply With Quote

Old   September 29, 2017, 09:23
Default
  #5
New Member
 
Praphul.T
Join Date: Dec 2013
Location: Kochi, India
Posts: 6
Rep Power: 6
praphul is on a distinguished road
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
praphul is offline   Reply With Quote

Reply

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
CFX Natural Convection, please help. dbecker CFX 5 October 13, 2010 19:07
natural convection vidhuresh FLUENT 2 October 25, 2009 10:52
model natural convection? phsieh2005 Main CFD Forum 7 June 11, 2007 08:01
Approximate Mixing due to Natural Convection Greg Perkins Main CFD Forum 0 February 12, 2003 19:43
transient simulation: natural convection problem? Basics CFX 3 September 25, 2002 09:42


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