CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   General CFD Question (http://www.cfd-online.com/Forums/main/4817-general-cfd-question.html)

 sam kashan June 11, 2002 00:09

General CFD Question

I have this general CFD question.

How can we value (credit or discredit) the steady state solution obtained for a flow that is known to be transient in nature (vortex shedding).

for example. The calculated steady state pressure coefficeint (Cp distribusion or Cp toal) along a flow past a circular cylinder. In literature these values are reported as the time averaged of a transient solutions. I appreciate your feedback

 Ajay S. Parihar June 11, 2002 08:15

Re: General CFD Question

Please make your question more clear. You want to know why we study time-averaged data field in transient flow?

 sam kashan June 11, 2002 09:01

Re: General CFD Question

In simulating the flow past circular cylinder (Re is in the subcritical range i.e <400k),the pressure coefficient Cp is obtained by time averaging from a transient solution. You know that the calcualted variables, including the pressure over the cylinder wall, will exhibit some how a periodic variations due to the vortex shedding.

I simulated this problem (using Fidap) as a steady state solution and obtained the Cp which show qualitative agreement with time averaged solutions obtained using a transient simulation( Using RNG turbulence model).

My question: Do you think that the solution obtained using the steady state solution is relevent or representative in any way for the problem.

or in other word: Do you see any value of the solution obtained using a steady sate solution ? thankyou for the response

 senthil June 11, 2002 10:57

Re: General CFD Question

I depends on wat u r interested in. if you are interested in time averged quantities like cp or average vel...steady state prediction will help you. ypu can believe them. it helps. senthil

 Praveen C June 11, 2002 11:01

Re: General CFD Question

If you are getting a converged solution for a problem that you know is unsteady, then there should be cause for worry and I wouldn't trust such a solution even if it looks correct. The reason for such a behaviour is excessive dissipation which is killing all the unsteadiness. I suppose you are performing the calculations without using time-accurate integration. If your code is right then you should not get a steady solution even if you are using local time-stepping and such things. You should still get a oscillating residue which shows the periodic nature of the flow.

 Praveen C June 11, 2002 11:11

Re: General CFD Question

There is one case when you can trust a steady state computation even if the solution is unsteady (but periodic). Consider the equation in the form du/dt = L(u) where L is some LINEAR operator. If U is the average solution which could be defined as a long-time average and if you average the above equation, you get L(U) = dU/dt = 0 So it might make sense to directly solve L(U)=0 or use pseudo-time integration to reach the solution U. But this argument does not hold when L is non-linear.

 Clifford Bradford June 11, 2002 11:48

Re: General CFD Question

The steady state solution is not relevant. In a flow with such large scale unsteadiness it is only coincidence that your results are close to each other.

In fact you should expect not to get a converged solution for such an analysis because of the large scale unsteadiness.

 sam kashan June 11, 2002 12:44

Re: General CFD Question

Raveen, you said: The reason for such a behaviour is excessive dissipation which is killing all the unsteadiness.

I will appreciate you elaporate on this.

I obtained a converged steady state solutions using both a commercial FE code and my Fv code. You are right, the residue is oscillating but after fallen within a reasonably small range.

 Ajay S. Parihar June 12, 2002 00:15

Re: General CFD Question

Dear All, What i feel that steady state solution of any transient problem can not give realistic results. If a problem is not steady state problem and even then you are solving it as steady state so you won't get correct flow field like Cd, Cl or Cp because you are assuming that there is no vortex sheding. As transient problem is marching in time direction so all quantities are varrying and hence there is no importance in saying that this is Cl or Cd at this particular time. To see average effect of any variable we do time averaging. You can't say that time-averaged data will be similiar to steady state solution of that problem. It could be same in some special cases atleast not in case of high Reynolds no flow. And it will be very difficult to get converged solution of transient problem if you are sloving it as steady state.

 sam kashan June 12, 2002 14:47

Re: General CFD Question

Senthil:

What do you mean by that? Is it a practice in industry, pleaase elaborate on that . Thanks

 Steve June 16, 2002 17:09

Re: General CFD Question

As mentioned, excessive dissipation is a possible reason for you non-physical steady state results. This would be due to either your grid being to coarse, your spatial interpolation scheme being low order, your time integration being low order, or your time step too small.

However the most immediate problem that you have is that you are using the "RNG turbulence model". Of course the flow will be steady if you use a turbulence model - eddy viscosity will both delay separation and damp unsteadyness. You mentioned yourself that the flow is subcritical. Turbulence models are renowned for giving nonsence around tansition Reynolds numbers let alone 2 magnitudes below.

 Steve June 16, 2002 17:16

Re: General CFD Question

Correction: "time step too large"

 sam kashan June 17, 2002 05:39

Re: General CFD Question

Steve:

The issue is not that i am using a transient simulation that leads to a steady state solution. It is That I am using a steady state simulation ( steady state RANS and rng k-e equation) that leads to results that compare reasonably with the time averaged solution that would be obtained using a transient solution. If course we are missing the physics of vortex shedding and all inherited transient behaviors. I would appreciate any comment about that. Thanks

 Steve June 17, 2002 16:43

Re: General CFD Question

In my opinion it must be a fluke. Especially considering you are using a turbulence model when the boundary layer is laminar.

The unsteady solution should have more drag than a steady solution (large dynamic wake). Perhaps the turbulence model is compensating somewhat by pushing the separation points further aft.

You could try doing a grid dependence test. i.e. If you double (or half) the grid density do you get the same answer? This process will eliminate numerical dispersion as a source of error. You may find that the solution will go unsteady (periodic residual behaviour, periodic forces) if you refine the grid. However it is the turbulence model that is causing the false steadyness, so perhaps disipation is negligible.

Steve

 Jitendra June 18, 2002 08:32

Re: General CFD Question

Praveen,

You said that,

"If your code is right then you should not get a steady solution even if you are using local time-stepping and such things. You should still get a oscillating residue which shows the periodic nature of the flow."

Do have any literature which showes/proves such behaviour or its your observation. It would be helpful if you can clarrify little bit on that.

Jitendra

 Praveen C June 18, 2002 09:21

Re: General CFD Question

You cannot prove that you always get reasonable results but sometimes you can extract useful information of an unsteady flow using a computation which is not time-accurate. See the following paper

Efficient numerical simulation of buffet for airfoils in transonic regime, T Renaud, C Corre and A Lerat

In this paper the authors want to find the Mach number at which the buffeting sets in. For this you have to calculate the flow at different Mach numbers till you arrive at the buffet Mach number. They have used local time stepping (LTS) and still found that they can locate the Mach number at which buffeting occurs. Even with LTS they obtain oscillating lift coefficient. But if you want more quantitative information like the oscillation frequency you have to use a time-accurate calculation. I do not know where this paper was published. You can mail to Christophe Corre

<Christophe.Corre@paris.ensam.fr>

 All times are GMT -4. The time now is 14:12.