Hi, My problem is that in my simulation I am not able to get unsteadiness (in many papers they claim that they have obtain unsteadiness). I will be thankful if some one give me guidance to obtain vortrex shdding. Does sombody simulated this case of flow behind a bluff body square or cylinder one and obtain the vortex shedding frequncy using URANS. Please help me this is urgent pp

hi u have to give some petrubation to solution eg. by rotating the bluff body for a short period of time or give disturbance in velocity field itself. that might(definitely) work.

This is kind of cheating since then your triggering your stable solution to make it unsteady. The papers which I was talking about mentioned that they have obtained unsteadiness without using any such triggering. any suggestions. pp

I have studied 2D bluff bodies and I found the same unsteadiness that you.

If you are trying with a steady solver, try an unsteady solver. It worked for me. I hope it works for you.

Remember that flow behind a bluff body is unsteady depending on reynolds nunmber and maybe you should be getting unsteady results

godd luck

Miguel

I am using both unsteady solver and steady solver. But I do not see any unsteadiness? Can you describe what did you do special when you simulated your geometry and what type of geometry you are simulating in details. Please respond quickly as this is urgent. pp

really, the question is what are you doing?; which boundary conditions, which viscous model, Y+??? etc

I tested bodies like bullets;data from Hoerner.and results showed and error<7%

I am simulating flow behind triangular bluff body. I am giving you two refernce. 1)"Numerical simulation of Vortex Shedding past triangular cylinders at high Reynolds numbers Using a k-epsilon Turbulnce Model" Stefan H. Johansson. Lars Davidson and Erik Olsson in Internation Journal For Numerical Methods in Fluids Vol. 16 859-878 (1993) 2)Unsteady simulations of turbulnet Flow Behind a Traingular Bluff Body by R.K. MadaBhushi, D.Choi and T.J. Barber in AIAA 97-3182 Now I am doing this simulation since I do not have the information about there grids I am using my grids and doing an unsteady calculation and steady calculation. I notice that unsteady solver convergence to steady state condition and lift coefficient is assume to be constant so this means that I am not able to capture the unsteadiness of the problem which in the papaer they claim that they have obtained unsteadiness. I will be thankful if you guide me accordingly. I hope the information is enough for you to give me some guidance. pp

You might have "data sampling for time averaging" turned on... this will cause the solver to average each cell over time and give a "steady state" solution when using the unsteady solver. Another problem is that vortex shedding is a function of an instability. In a perfectly symmetrical mesh there shouldn't be any instability, even with a bluff body. You may want to patch a high pressure onto one of the vertices to create your instability. I've run into the same problem on a dodecahedron where I couldn't get the model to form any vortices... I patched an uneven pressure onto the model and that started the vortices.

Hope this helps, and goodluck, Jason

Thanks I have data sampling for time statistics enabled. I will correct and rerun the case. But these could not be the problem as I am running this case in other cfd software which gives me similar results where ther is no such option of data sampling and all You said that for perfectly symmetrical mesh there will not be any instability can you expalin me the reasons why is that so. By patching the pressure you are actually making the solution to become unsteady this is not a good idea I think. pp

CFD is just a numerical approximation of the flow. If the model is perfectly symmetrical, then CFD doesn't see any difference between that and if you actually used a symmetry boundary condition. In real life vortex shedding is started by a couple factors... one reason is that no model is perfectly symmetrical... but the main reason (imho) is that the flow isn't perfectly symmetrical, especially when the flow is starting up. There's all kinds of turbulence in the flow (flow irregularities tend to be highest when starting the flow) that establishes an instability on the body, which starts your vortices... these vortices then continue once they're started.

It may be possible to start the vortex shedding by increasing your Turbulent Kinetic Engergy on your inlet (I'm not sure though, I've never tried this). Another possibility might be to initialize the flow at 0ft/s before iterating. My thought is that this might act like starting up a tunnel where you get a lot of mixed flow when the high speed air hits the stationary air. I've never bothered with these though, I've always forced the instability. It won't take long for this artificial pressure to be worked out and the system will reach it's natural frequency.

Goodluck, Jason