CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Timestep study (http://www.cfd-online.com/Forums/cfx/74553-timestep-study.html)

ijk April 3, 2010 05:52

Timestep study
 
Hi all,

I am simulating an axial fan. It is stalled and steady state will not converge. I have tried various timesteps with transient. I set the pressure rise and monitor the mass flow.

What I have found is that there are high frequency oscillations in the mass flow for early iterations which reduce in frequency as the simulation progresses. Please could someone explain why this happens - does it mean my timestep is too big? I am looking for a timestep that, when I reduce it, the results do not change.

Please could someone advise on how to approach the timestep study. Should I start all simulations from the same file? Should this file be a really small timestep as I think it matters what file I start from?

Thanks,

ijk

farzola April 3, 2010 11:13

Hello,
I suggest that it is neccesary to begging tunning the steady simulation, you can start with smaller mass flow rate and grow up this value progressively. The same thing you can do when you will start transient simulation, wherever is recommendable start using a frozen rotor sim. The angular velocity of the rotor can be increase progressively also.

I hope it can help you...

ghorrocks April 4, 2010 07:38

Have you looked at:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

ijk April 7, 2010 05:26

Thank you both for your responses.

Glenn - I have looked at that particular document and tried all the things suggested. I have vortex shedding from the blades. No matter what timescale I use it doesn't converge.

My main concern is how to approach the transient timestep study, as it seems the timestep I have been using is too large and damps out high frequency oscillations in my mass flow plot. Does anyone know why this happens and how to correctly approach the timestep study?

Fidel - I will try speeding up the fan and perhaps also starting from lower loads to see if it makes a difference.

ghorrocks April 7, 2010 18:36

If you know you have transient shedding happening then your only choice in a steady state simulation is to use a very large physical timestep - much larger then the eddy turnover time of the transient feature. If this does not converge then you will not be able to use a steady state model and have no choice but to use a transient simulation.

If you use a transient simulation I recommend you use adaptive time stepping, homing in on 3-5 iterations per time step. Then the simulation will find its own time step size easily. The timestep size which comes out of this should be pretty close to time step independent, but it is still wise to check it to be sure.

If you want to accurately resolve the shedding you will need to use second order time advancement. If you use first order it will blurr out the vortex a bit - but this may be a good thing depending on your application.

ijk April 9, 2010 05:38

Glenn, thank you once again for your response.

I tried large physical timesteps with steady state but it diverges after a few iterations.

The adaptive timestepping works well. Will it find the same sort of timestep value for all mesh resolutions or will the timestep get smaller with finer meshes?

ghorrocks April 9, 2010 07:38

Quote:

I tried large physical timesteps with steady state but it diverges after a few iterations.
Then you timestep is too large. Try a bit smaller than that. Also you can only increase the time step dramatically once you are in the monotonically converging section. If you do it before then it will probably diverge.

Quote:

Will it find the same sort of timestep value for all mesh resolutions or will the timestep get smaller with finer meshes?
Depends on the simulation. Generally a finer mesh will result in a finer timestep (roughly keeping the Courant number the same) but with implicit solvers this is not necessarily the case.


All times are GMT -4. The time now is 09:05.