I am running what i thought was a fairly simple heat transfer problem in Fluent (v6.3) but i have been running into some issues and i hope someone has done similar and is able to help.

My problem consists of air-flow passing through an open ended rectangular box, the bottom surface of the box is a heated plate at 923K. A small pipe carrying running water cuts through the sides of the box perpendicular to the air-flow. I have the results from a rig experiment to give me results for the temperature rise of the water in the pipe. I am running the problem steady state, segregated, implicit solver. I have the energy equation switched on. I am using the k-e turbulence model with standard wall treatment.

I started the solution with the gravity turned off, the operating pressure at 101325pa (1bar) and both the water and the air set to constant density. The solution converges after about 1000 iterations and gives a reasonable temperature rise in the pipe that isn't a million miles of the rig results.

I next switched the air to ideal gas - this was the only change i made at this time but i do plan to switch on gravity and radiation. This time the solution does not converge properly, the residual for epsilon in particular is relatively high and all residuals have a degree of fluctuation. When i looked at the flow behaviour i could see that the flow of the water at the start of the pipe had some high velocities and pressures and the flow was reversing in some places. After a short distance the flow returns to normal and the temps/pressures/velocities in the rest of the pipe look typical.

I think this is caused by the operating pressure, and the use of ideal gas for the air and constant density for the water. I cannot figure out how to setup this problem in order to get rid of the anomolies on the water inlet?

I'd appreciate any ideas, Cheers.

What are your boundary conditions at the inlet and exit?

Air Inlet - Mass Flow inlet 0.18Kg/s at 404K. Air Outlet - Pressure Outlet 0 pa gauge. Water Inlet - Mass Flow inlet 0.001Kg/s at 300K. Water Outlet - Pressure Outlet 0 pa gauge.

I set this problem up to match the rig, i have been provided with with mass flows of the two fluids. The two outlets on the rig just vent to atmosphere, hence 0pa gauge given my operating pressure.

Is your model multiphase or multispecies?

Model is multispecies. Air and Water are completely seperated. The water is always between about 25 and 50 DegC so is never a gas or solid.

I think that this result was just Fluent messing up though, it appears that the change from Constant Density to Ideal Gas conditions was a bit to much of a jump for it to handle in this problem. I've since tried air as incompressible ideal gas and the solution has converged perfectly. The pressure differences in the air are fairly small hence the use of Ideal Gas was a bit unnecessary anyway as the density changes will be dominated by the temperature differences.

Now i'm turning on the gravity to get the correct bouyancy effects of the air passing over the hot plate. I'm running this steady state, but manuals seem to suggest that if you are not using the Boussinesq approximation for density (which i can't because of the quite large temp differences in the air!) then you have to run the solution transiently.

I was just wondering if anyone has any thoughts on the above as opinion seems to be split with my colleagues?

Cheers Jon

Hi..

I have few suggestions and few questions

"air-flow passing through an open ended rectangular box, the bottom surface of the box is a heated plate at 923K" - do u have a developing length for the flow in your air domain entry?

"Air Outlet - Pressure Outlet 0 pa gauge" - if the outlet face is so close to the water tubes, the wake shed by the tubes will intersect the outlet boundary, and i hope this will cause the soln to fluctuate. - I hope ur expt rig has a downstream passage for hot air, which probably u might have omitted, for computational convineance

- whether the mesh is aquequate to capture the sudden gradients in the flow properties. whether u have used a Boundary Layer mesh?

- i guess since the bottom plate temp is > 900K, u may need to involve natural convection also, which may be a dominating mechanism near the wall

- what is the pressure velocity coupling scheme u use.

- have u tried the case with a different inlet turbulence intensity (by default, it is 1%)