Natural Convection in Cavity with Cu-Water NanoFluid
 

Hello Friends

i'm new in fluent. can some one help me to solve this simulation with fluent:

The flow field is a square enclosure with an aspect ratio of unity and length of 1 meter. The horizontal walls of the cavity are assumed to be insulated while the vertical walls are maintained at constant and uniform temperatures. The temperature gradient between the two vertical walls is maintained at a constant value of 20K (283K for cold wall and 303K for hot one). The cavity is filled with a nano-fluid made up of water and copper nano-particles (Cu).

My questions:

- What's the best meshing method and size?
- In material edit, with option should be selected for Density?
- What's the best Solution Method for momentum and energy

Thanks in advance.

It's very hard to predict a good grid size without experience of the particular problem. It's much faster to just make any mesh, run it, and then update the mesh if needed. It's customary to try several meshes.

Density should be a function of temperature. At the minimum, and I recommend to start this way, you should use a linear function between the two temperatures. You can refine it later if needed.

By the way, Fluent also supports REFPROP if you want access to a built-in, extremely detailed, and accurate database. You simply need to type in some commands to activate it. But only do this after you have familiarized yourself with Fluent. However, it only has common fluids and not nano-fluids.

For solver settings, most of the defaults are ok. You should focus on the mesh, boundary conditions, and initial conditions.

Use the pressure-based solver. Don't use the density-based solver because your problem is incompressible.

The SIMPLE scheme should work (also default).

For discretization, the defaults are okay. But you can go ahead and use the 2nd order upwind method for everything and use the higher order term relaxation option. Most of the defaults are already 2nd order.

Make sure you have a good initial guess!

Hello Dear LuckyTran and thanks for your answer.

I ran my simulation with below conditions:

- density: piecewise-linear
- Solution methods: (Pressure: 2nd Order, Momentum and Energy: 2nd Order Upwind; all same as Ansys Fluent 18 Defaults)
- Relaxation Factors: Same as Defaults (0.3, 1, 1, 0.7, 1 respectively for Press. , Density, Body Force, Momentum, Energy)
- Initialization:
-- Standard Initialization
-- Compute from: Hot Wall
-- Initial Values: 0 , 0 , 0 and 303K respectively for Gauge Press. , X , Y Velocity and Temp.

After Running the simulation, the residual plot didn't converge and it had oscillation (as shown in attached) and contour of Temperature is seems not to be correct.

Please let me know my mistakes and help to improve results.

Thank you some much for your attention.

The settings look fine. The residuals are not that bad. If you don't like them, you can lower the urf for energy down to 0.9 or so.

You are using the laminar flow model right?

Check the velocity vectors and see if they make sense.
Check the direction of the gravity vector.

The temperature looks odd yes. I would expect the temperature to be pretty much linear. You can try disabling gravity and running again to see if you can this linear temperature profile (pure conduction case).

Btw I just realized that since this is a closed domain, there will be a global mass conservation issue later on. I don't think that is the problem you are having right now though. You really should be running a transient case. In a closed domain with a steady solver, you can't conserve the global mass. You have to run a transient case, with an initial temperature profile that gives a starting value for density so that you have some global mass, and this global mass gets conserved in the transient simulation. You can run super large time-steps, it's not a problem.