Dear Astrid

On my last thread about splitting the eqns. (energy and momentum) you told me to run first solve fluids t, solve the keps f and solve energy f and afterwards run keps and energy. How can it run the fluids eqns without the keps eqns. when the problem is turbulent? Do you understand what I mean?

Sincerely,

Dimitris

Dimitris,

The solver calculates only the momentum and pressure equation with the present k and eps field. These are not changed during the iteration. In fact, you uncouple the system of PDE's.

Astrid

Interesting,
Suppose that you're starting a simulation from the scratch. I've noted in a simulation using Reynolds Stress, that the turbulence only starts to be solved in the third or fourth iteration. Now using standard k-epsilon, are you saying that if you turn off tke and epsilon equations, and start your simulation, CFX-5 will use the initial fields for these variables, which I believe its default are 1.e-04. Is that it ?

Regards, cfd guy

- Turbulence start on iteration 5 if you have smart start on.

- I think the solver will act as you say.

- In practice I only turn off the momentum and turbulence equations if I have a fairly good solved solution (mass balance is below 0.1 %) but a terrible enthalpy balance (say above 30%). I don't use it for the imaginary test cases you mention, although it might help you.

Astrid

Yes but I start my simulation solving the fluid eqns and after reaching my residual target I restart with the fluid eqns off while the keps and enrgy eqns are on. Is it the wrong way to go or is it OK?

I would never accept a final solution with

Solve fluids FALSE
Solve energy TRUE
Solve Tke eps TRUE


Always provide a final solution with all equations solved simultaneously because the equations are coupled!!!!
Switching on and off the separate equation classes can help in cases like:

- as I mentioned before when global energy and mass balance differ a lot, run with only the energy equation with a large timestep.

- when your domain contains to much fluid, that leaves the domain during the iteration process, you can win some time by only solving the fluids equations. When your mass balance is within 0.1% you might consider solving all equations.

- when you want to perform some passive scalar mixing simulations, you only have to solve the scalar equtions of course.

Can anyone provide more examples?

Astrid

Well...in some cases I've run I don't get convergence while running all equations simultaniously...but if I start with only fluids and then restart with energy and the k-eps it works...but as I mentioned before I don't have an idea if it's proper to do so or not...

In all cases, the turbulence equations should not be solved separately from the mass-momentum equations (other than in an effort to get convergence started in extreme cases). Although only mass and momentum are strictly coupled, the turbulence solution provides the turbulent viscosity for the mass-momentum equations and will thus change the solution.

As for energy, if the the solution is incompressible, buoyancy is not of concern and the Thermal Energy energy equation is used, the energy equation will have no effect on the fluid solution. If you wish to investigate the heat exchange effectiveness in such a case, you could solve the fluid flow and turn fluids = f to go through several different scenarios.

Alternatively, in this sort of case, one could kill many birds with one stone. Since the Thermal Energy equation is just a diffusion equation, you could solve for several alternative heating scenarios in one shot by creating multiple additional scalars, one for each scenario, and solve them all at once!

Sometimes I think I spend too much time thinking about these things

Regards, Robin

Hmm,

I could see justifying turning off fluids if the residuals and % balances for u,v,w and p are reasonable. Then, if energy k and epsilon are not good enough, you could set "solve fluids = f" and pound in the others. However....

Keep in mind though that pounding in k and epsilon without fluids on is probably meaningless because normally the turbulent viscosity is fed back into momentum. If you have "solve fluids =f" then the extra iterations on k and epsilon are somewhat meaningless

Converging in energy is a different story as you may be running a case where enthalpy conduction matters more than advection. So, in that case turning off fluids makes sense, so that you can use a huge time step to pound in the energy residuals. You'll have to use your judgment to decide which is the case.

Note, you can control energy and k/eps with "solve energy = t/f" and "solve tke eps = t/f".

Neale

On second thought, it's probably not a good idea to solve Temperature as an additional scalar.

OK...I'm actually first solving the fluid equations together with k-eps, and when they've dropped to a level that I find resonable I stop the run and restart it with fluids an k-eps eqns. off, that is, running only with energy eqns. But when the run is finished and I postprocess the 2:nd resultfile it is, according to the vector plots, constant velocity throught the entire domain, which is impossible. Am I doing something wrong here? I mean when I ran similar problems with CFX4 I could do like I've written above and it showed according to postprocess the different velocities in the domain. How come?

No no no...

1:st run : solve fluids t, solve Thekeps t and solve energy f.

2:nd run (restart of 1:st): solve fluids f, solve Thekeps f and solve energy t.

So in my restart I only run energy.....is that OK?

Dimitris,

You have defined your initial values as "Value", rather than "Automatic with Value". The "Automatic" settings will use the existing solution if it is available, otherwise it will use the default or user specified value. If you did not choose one of the automatic options, your existing solution will be overwritten with the initial guess.

The "Default" and "Value" options are provided to allow you to re-initialize a variable. For initial guesses, you should always choose the "Automatic" or "Automatic with Value" option.

Robin

Ahh, sorry for the mistunderstanding. Yes, that is probably fine as long as you are running thermal energy (low speed flow), so that the energy transfer is mainly diffusion driven rather than advection driven, which would be the case with higher speed flows.

Why are you doing it this way at all? Is there a reason? i.e., are you having convergence difficulties when runing u,v,w,p,k,eps and h all at once?

Neale.

Yes...the K-eps stops dropping after some time and of course influences the rest...but this behaviour becomes clearer when I use finer mesh...for coarser mesh with the same parameters I get convergence running all oft the simultaniously...

Ehhhh.....OK? Wait a minute....let's see if I understood what you meant...

1. I run first fluids and k-eps

2. I restart the run with a modified definition file (fluids and the k-eps are off and energy are on) and my initial value file is the result file from the first run.

Now my question is...where and when do I alter something to auto....I don't have a clue where to find and to do that...

The modified definition file used to start the second run should use either the "Automatic" or "Automatic with Value" setting for the initial value options. This will allow the solver to pick up the solution fields from the res file from the first run. If you use "Default" or "Value" then the solution fields from the first run won't be picked up, a default value or the value specified will be used instead. You select these settings in CFX-Build from the initial values forms. It would be better to use "Automatic with Value" when setting up the first run though - that way you can specify a value that will be used when no initial values file is present, but when an initial values file is present the solution fields from it will be used. It also means less modifications are needed in the second definition file. This is all explained in the documentation.

Yes, I got it and it works great. The reason to why it didn't work the first time was because I changed some of the values, that I knew, like inlet velocities, so I changed it from automatic. That's why, because if you don't touch it, it's automatic from the start (default by the software).

Thanks alot!!!

Dimitris,

Are you trying to solve a case with heat transfer between a solid/wall and the fluid? If yes, then which turbulence model do you use and do you perform any verification with experiments?

Astrid

I have a cylinder in crossflow that has the diameter D and length 2*D. I only create 1/4 of the cylinder because I use symmetryplanes. The walls of the cylinder have a const. heat flux (2000)and the fluid flows in the axial direction of the cylinder. The velocity of the fluid, which is air, is subsonic and is of room temp. The turbulence model I use is K-eps and I want to calculate the temperature of the front, back and the circumference of the cylinder walls because I want to compare it with an experiment to verify my code. Is this enough info for you or do you want more details?