[biro]

Hello again,

I have some problem by changing the turbulence modell from k-epsilon to k-omega-SST.

When I use the k-epsilon modell I get a steady state solution for my problem. Now I have to change the turbulence modell to k-omega-SST and when I use "advection scheme: upwind" and "turbulence numerics: first order" i get a converged steady state solution, too.
But I read, that for final results I should use the "high resolution" option for both.
When I use the high resolution option my residuals will decrease within the first 100 timesteps, but then they increase to the value 1e-3 and the values on my monitor points are oscilating.

Can I use the first order and upwind option ?
Do someone know the problem and a solution for it ?

[ghorrocks]

Not all simulations are sensitive to tight convergence of the turbulence equations. I would do a sensitivity study to see if it makes a difference in your case. Loose convergence of the turbulence equations may be irrelevant, making it unnecessary to converge tighter.

Also this FAQ may help:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

[biro]

I read the FAQ, but I don't find an item, which can help me.

Can you give me a short explain, what kind of sensitive study you mean ? I don't know this time what you mean.



Maybe my explanation are not exacty: all my residuals increases, not only the residuals for turbulence

[ghorrocks]

The big tip on the FAQ is try a bigger time step. Have you done this? Also improved mesh quality ALWAYS helps.

Sensitivity study: Do a simulation at one convergence value (1e-2 maybe) and another to a significantly tighter value (say 1e-3) and compare the results for a value of interest to you. If it has not changed significantly then it you can be confident you are OK and can stop there. If it has changed then you need to try tighter again (1e-4) and keep going until it converges.

If you can't do this using high order turbulence (you might not get tight enough convergence) then it should be OK to do the sensitivity study on low order turbulence and use that result for the required settings for the high order turbulence simulation.

[biro]

Sorry for my answer there was no item in the FAQ! I wasn't concentrate enough, but my time is runing out for thesis. And slowly I get panic


I have varied the timestep size from residence time (rt) over rt/2, rt/3 to rt/4.
You will see, that the convergence is even better and the monitor point iss steady state. But the convergence of the turbulence rms is still bad.

In the last picture you will see a stagnation region after a tear-off edge. I need the tear-off edge to slow down the stream to reach the velocity profile I need. I think, that the stagnation region is responsible for bad convergence ?! But with the k-epsilon model there was no problem ?! And I use the same mesh (y+ = 50-80). I thougt (with automatic wallfunction) the solution has to be similiar with both models.

My plan was to change turbulence modell (with same mesh as k-epsilon) and then to refine to y+ ~1


One more question: your said "... then it should be OK to do the sensitivity study on low order turbulence and use that result for the required settings for the high order turbulence simulation."
Which settings do you mean ?

[ghorrocks]

Also try time step size larger than the residence time.

If you do the sensitivity study I suggested using low order turbulence (so you get tight convergence) then you can use those settings on the high order turbulence simulation. It might be tricky to get the high order turbulence to converge tighter so it is best to know if you need to before you do it.

[biro]

By using timestep larger residence time I became worse convergence than I use rt/4.

I have problems by doing the sensitivity study:
When I use convergence criteria 1e-2 or 1e-3 the criterias are reached after the first respectively after the second iteration. But my values of interests can't adjust within 2 iterations.
What can I do ?

[evcelica]

You clearly have transient flow, so It is very difficult to converge the numerical residuals using a steady state solver. But that doesn't mean that you don't have a good solution, if your result of interest isn't changing then you should be good. I'd concentrate on sensitivity analyses and grid refinement and check to see if your result of interest isn't changing. Don't worry about the value of the residuals.

[biro]

Thank you for your answer evcelica.

I will do refine-mesh-study and show on the value of interest.
But I don't know how to do a sensitivity analysis, can you give me a short explanation how to do?

[biro]

I try to execute a transient simulation. After 40 timesteps everything went well and every variable has a good value.

But the adaptive timestep algorithm falls back to a timestep of 6.5e-5 [s] so I think, the timestep iss to small to see anything ?!
And the Courant-Number (RMS) has a value of 131.5 (max Courant Number 999.99). I thougt Courant Number should have be a value of about 1.

So I think I simulate a kind of rubbish ?! Can everybody help me ?

[ghorrocks]

Use adaptive time steps homing in on 3-5 coeff loops per iterations. Do not use Courant number adaptive and ignore the Courant number reported. It is not relevant for many flows.