Boundary Condition for Natural Convection

  • Last Post 19 February 2020
cha10 posted this 08 May 2018


I want to simulate air flow around heated/cooled body due to the natural convection. I am not really sure how to put the boundary conditions.

Here are what I think

1. Assign the temperature to the body, 2. no heat flux to the ground, 3. Pressure-inlet at the top boundary, pressure-outlet at the side. 

Are these fair boundary conditions? 

Thank you!

Order By: Standard | Newest | Votes
Raef.Kobeissi posted this 13 May 2018

Yes but you need to make sure that the ideal gas is selected and also the Boussinesq Parameter is set up. Please see figures below:

Raef Kobeissi

  • Liked by
  • gishnutr
  • peteroznewman
gishnutr posted this 24 May 2018

Hi, Raef

       I your comment above, you mentioned to use ideal gas as material. I have three doubts in this.

  1. The incompressible-ideal gas also have same values in the given tab. Is it just a incompressible fluid/ flow version of ideal gas model or is there any other explanation for using these two?

2. If Boussinesq parameter is set up in Operating conditions tab, then what is the use of the Boussinesq term in Density model selection under Edit Material  tab? 

3. In Operating conditions tab the operating density id given as "0". By default the value is 1.225. Why is it changed to 0?


Thank you.

Kremella posted this 24 July 2018


To answer your questions:

1. An incompressible-ideal gas law is used to estimate the density of an INCOMPRESSIBLE fluid using the ideal gas law (check out section 7.3.6., Fluent User's Guide).

2. The density drop down in the material property panel allows you to choose the Boussinesq approximation model and it uses a constant value of density by writing the buoyancy term as a function of operating temperature (section, Fluent User's Guide). You will also have to specify thermal expansion coefficient (beta).

3. Operating density is non-zero because it appears in the body-force term of the momentum equation. When Boussinesq approximation is used, this value becomes irrelevant and therefore need not be specified. Care should be taken while specifying the operating density (section, Fluent User's Guide).

I hope this helps.

Best Regards,


NicholasS posted this 19 February 2020

How about the other settings?

Should it be Pressure or Density based?

What kind of solution methods?


If I activate the 'Specified Operating Density' I always obtain an unrealistic velocity field even when the 'warm' surface is at the same temperature as its surroundings. When I turned it off, at least  in the case of zero difference in temperatures, the velocities drop realistically to ~0.


rwoolhou posted this 19 February 2020

If the system is sealed you need ideal gas. Operating density should be the mean value in the domain (near enough) in that case. I assume you did turn on gravity?