Natural Convection Boundary Conditions
 

Hi all,

I am simulating 2D natural convection in an open vertical channel of high aspect ratio (12.5) with both sides isothermally heated by ΔT = 5K with water as the operating fluid. I have modelled the regime with large spaces on top and bottom of the channel to visualise inlet and outlet flow.

Gravity of 9.81 m/s^2 is applied in -Y direction. I have used Boussinesq approximation for density since β.ΔT<<1. Initial values of velocity and pressure in the regime are zero.

The boundary conditions I have specified are, as shown in figure 1, isothermal no-slip for the channel walls, adiabatic no-slip for the adjacent and side walls, velocity inlet with v=0, p=0 for the bottom edge and pressure outlet p=0 with flow normal to boundary for the top edge. The simulation performed is transient and laminar, using SIMPLE solver.

Am I correct in using the mentioned boundary conditions? The result agrees with experimental data with ±7% error of Nusselt number and averaging out minimises it to ±2%. I am confused as to why a pressure boundary condition is required for solving natural convection problems with Boussinesq approximation since the approximation takes out the pressure terms in Navier-Stokes equation and energy equation. The reduced set of equations are described in the Fundamentals of Heat and Mass Transfer by Incropera and Dewitt, shown in figure 2.

Wouldn't the velocity field and temperature field be enough to solve the set of equations implicitly?

Incompressible flows (with Bousinnesq) requires BCs for velocity and temperature, the Dirichlet value for the pressure equation is not necessary.
However, if you fix the pressure outlet value, you have to let free the BC for the velocity. The pressure equation determines a pressure field up to a function of time.

Note that fixing a value for the pressure is a "trick" sometimes used to let the iterative method to converge but if the compatibility condition

I tried using pressure inlet and pressure outlet (both p=0) but the velocity diverged to a large value after a few time steps to overwhelm buoyancy driven flow. In that case, temperature gradient near the hot wall was almost non-existent.

Yes, your "trick" certainly worked. The combination of velocity inlet + pressure outlet sort of fixes the direction for the solution to proceed towards actual solution and the flow is similar to experimental data.

But I'm confused why pressure inlet + pressure outlet won't work and why velocity inlet + pressure outlet works.

You can set pressure inlet and outlet (leaving free the velocity) but you have to prescribe a pressure difference between inlet and outlet that, for buoyancy-driven flow depends, on the temperature difference that induces the flow.
Have you tried using Neumann condition for the pressure everywhere?

But isn't the pressure difference between inlet and outlet handled by specifying gravity, thereby specifying the hydrostatic pressure difference hρg? I don't see any other form of pressure other than hydrostatic, and the buoyancy-induced localized pressure difference.

No, I did not specify Neumann condition for pressure anywhere directly. The no-slip BC at the walls imply a zero normal pressure gradient. Other than that, inlet is a Dirichlet of velocity and pressure, outlet is a Dirichlet of pressure alone.

Thermaly driven flow
 

Hi i am facing problem with my ansys fluent simulation. I have a 3d pipe titled at a 45* and water as a fluid. I want to know how much water rises and its temperature and velocity contour when specific lenght of pipe wall is given a temperature (localized heating). I want to know to proper boundary conditions in order to evaluate velocity flow bcz of temperature. Consider it as thermally driven flow by allowing gravity and buoyancy factors to be involved. Kindly help me in this problem.
Regards.