Hi,

Has anyone modeled natural convection in star-ccm+?! I have a 3D model and modelling of natural convection takes a long time!

Any feedback?!

2d takes long time..

which version do you use?

3.02

Hi, I'm doing those computations quite often as well as my students. What is your case about?

*steady state or transient?

* using radiation? which model? S2S or DO?

* what are the BC's? have you got inlet, or just pressure bc, or is it only box enclosed by walls?

* is your BC's physically correct?

*do you use coupled or segregated solver? what Courant no. or relaxation you use?

*how do you decide convergence? (i thing with nat. conv. the residuals are not enough and you should look for variables in control points, you may not achieve large drop in residuals)

*is your mesh fine enough at the walls? do you have prisms?

*do you use ideal gas model, or boussinesq approx.?

*what turbulence model you use? is your y+ correct

... do not take me wrong, those are not stupid questions, only not answering them to yourself is stupid. Even after years you can find yourself trying to compute impossible settings... that is why I'm writing them here...

matej

Thank you for your comments - here is the answers to your questions:

*steady state or transient? Steady

* using radiation? No

* what are the BC's? have you got inlet, or just pressure bc, or is it only box enclosed by walls? It's a BOX

* is your BC's physically correct? YES

*do you use coupled or segregated solver? what Courant no. or relaxation you use? Segregate Solver - relaxation= 0.75

*how do you decide convergence? (i thing with nat. conv. the residuals are not enough and you should look for variables in control points, you may not achieve large drop in residuals) I have Control Points

*is your mesh fine enough at the walls? do you have prisms? Yes, and I have Prisms

*do you use ideal gas model, or boussinesq approx.? Idea Gas

*what turbulence model you use? is your y+ correct - It's Laminar

OK, now what is the thing that makes you say the convergence is slow? what equation makes a problem? energy?, velocities?

if it is velocity, is the flow really laminar? what is the Rayleigh number at the heated or cooled wall?

if the residuals oscillate, you may wish to relax energy more.

if that does not help, the flow is probably unsteady by nature, and you need to switch to transient mode.

matej

Problem is the energy solver, as the velocity solver is frozen.

aha. now it get interesting. Could you possibly tell me what is the magic trick with which you decoupled artificially velocities from the enthalpy equation?

At least what I was told about natural convection, and what I understood from the world around is, that the nat.conv. is a flow induced by density difference which is caused by the heating or cooling of the fluid in the vicinity of the solid wall of different temperature. In such a flow, the velocities are directly coupled with the temperature (hence enthalpy) through the density (with the help of an ideal gas law). You may argue the density difference is very small, but so are the velocities. So the relative importance of the changes in the momentum equation is high.

Now stop breaking the physical laws and turn on the momentum solver, or I shall report you to the authorities ).

Or am I completely wrong here, anyone?

You are right!

natural convection is a flow induced by density difference. But freezing the momentum solver doesn't mean that we are solving only energy equation. we use constant velocity in conjugation with energy equation - Again, it goes back to your statement that velocity and density varies by the time and during the simulation.

The problem was "simulation time", and if I turned on the momentum solver it would take forever to solve the problem.

Freezing the momentum equation was an assumption to speed up the computational time only.

Ok, but then there must be something wrong. How many cells you have in your model and how many CPUs are you using? What is the time per iteration? Because when you turn the momentum equations back again, you will jump back and have to wait for convergence again, or you end up with rubbish solution.

If the temperature differences are low (say till 40K) you may try to use Boussinesq assumption instead of ideal gas which will make the solution easier.

matej