Learning Forum

[haiteng]

I am using ANSYS Fluent to simulate the experiment for natural convection of a single heated cylinder in a large water tank made of Plexiglas (approximated as thermal-insulating material), which is 1200 mm wide with a water depth of 1600 mm. Computational domain is a rectangular with the same width and depth as the experiment. The thrid dimension is neglected because it is assumed that spanwise flow field is uniform, which is reasonable. I use steady, pressure-based solver and Boussinesq approximation for buoyancy. Turbulence is modelled by transition SST. Operating temperature is set to 293 K. Density is Boussinesq at 998.92 kg/m3, which is evaluated at the operating temperature. Gravity is specified verticall downward. 

 

The major problem I have is how to set the boundary condition correctly on the four sides of the rectangular domain. I have tried two options.

 

Option 1: No-slip, adiabatic wall on left, right & bottom boundary. Zero-shear, isothermal (Tw=293 K) wall on top boundary, to simulate the free water surface. This boundary condition setting is most representative of real scenario in experiment. However, the result is non-sensible. Contour of velocity magnitude suggests buoyant plume is completely disrupted, as shown below.

Option 2: No-slip, adiabatic wall on left & right boundary. Pressure inlet at bottom boudanry. Pressure outlet at top boundary. This setting, although not representative of experimental scenario, produces sensible result. Buoyant plume show reasonable profile and velocity magnitude, as shown below.

Could anyone tell me, why Option 1 generates the non-sensible result, although it is exactly the same as experiment? Why Option 2 seems so good, although the boundary condition does not reflect the real scenario?...

[DrAmine]

What about the temperature plots especially in the corners at top? Anyhow you need to run this case transient.

[RK]

Hello, 

Please refer to the Fluent User's guide and make sure you have evaluated the density based on the model mentioned. 

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/flu_ug/flu_ug_sec_hxfer_buoy.html?q=boussinesq

[haiteng]

Hello Abenhadj, 

Temperature contour is as follows and really weird. Temeperature in the ambient is around 300 K, although it is set to 293 K in the "Operating Temperature". Near the corner of the top, it decreases to 293 K (specified temperature at top boundary) within 1 grid point.

I don't think the transient solver helps, given that steady solver, as an approximation of the system, performs so badly... 

[haiteng]

Thanks. I have read the guideline previously and followed it. I used Boussinesq approximation (commonly adopted in literature) so only operating temperature needs to be specified. 

[DrAmine]

The natural boundary condition at top should be an opening. I expect a singularity at a adiabatic/fixed temp wall. Transient solver is the way to go for further analysis.

[haiteng]

Did you mean trying transient solver (URANS or LES) by using the same boundary condition (zero-shear isothermal wall at the top & no-slip adiabatic wall on other three sides)? 

Singularity at the top corner might exist. But I don't understand why changing the solver from steady to transient help to solve this problem. Shouldn't we first debug boundary condition setting, or mesh grading near top boundary, using the less-expensive RANS steady solver? 

[haiteng]

In addition, the pressure contour is completely non-sensible as well (shown below). It increases from -12 Pa near the bottom wall to 13 Pa near the top wall. But in practice, pressure far away from the heated cylinder should be zero. 

[haiteng]

The problem is solved by switching to transient solver. thanks!