# General CFD Question

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 11, 2002, 00:09 General CFD Question #1 sam kashan Guest   Posts: n/a 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

 June 11, 2002, 08:15 Re: General CFD Question #2 Ajay S. Parihar Guest   Posts: n/a Please make your question more clear. You want to know why we study time-averaged data field in transient flow?

 June 11, 2002, 09:01 Re: General CFD Question #3 sam kashan Guest   Posts: n/a 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

 June 11, 2002, 10:57 Re: General CFD Question #4 senthil Guest   Posts: n/a 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

 June 11, 2002, 11:01 Re: General CFD Question #5 Praveen C Guest   Posts: n/a 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.

 June 11, 2002, 11:11 Re: General CFD Question #6 Praveen C Guest   Posts: n/a 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.

 June 11, 2002, 11:48 Re: General CFD Question #7 Clifford Bradford Guest   Posts: n/a 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.

 June 11, 2002, 12:44 Re: General CFD Question #8 sam kashan Guest   Posts: n/a 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.

 June 12, 2002, 00:15 Re: General CFD Question #9 Ajay S. Parihar Guest   Posts: n/a 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.

 June 12, 2002, 14:47 Re: General CFD Question #10 sam kashan Guest   Posts: n/a Senthil: What do you mean by that? Is it a practice in industry, pleaase elaborate on that . Thanks

 June 16, 2002, 17:09 Re: General CFD Question #11 Steve Guest   Posts: n/a 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.

 June 16, 2002, 17:16 Re: General CFD Question #12 Steve Guest   Posts: n/a Correction: "time step too large"

 June 17, 2002, 05:39 Re: General CFD Question #13 sam kashan Guest   Posts: n/a 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

 June 17, 2002, 16:43 Re: General CFD Question #14 Steve Guest   Posts: n/a 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

 June 18, 2002, 08:32 Re: General CFD Question #15 Jitendra Guest   Posts: n/a 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

 June 18, 2002, 09:21 Re: General CFD Question #16 Praveen C Guest   Posts: n/a 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Jas Main CFD Forum 10 March 30, 2013 13:26 kaifu OpenFOAM 11 August 15, 2012 12:51 Alex Pope Main CFD Forum 26 April 25, 2007 11:54 Mateo Main CFD Forum 4 January 5, 2006 04:52 Frank Muldoon Main CFD Forum 7 August 3, 1998 19:04

All times are GMT -4. The time now is 09:22.

 Contact Us - CFD Online - Top