Hi,

I want to use fluent to model vortex shedding effect around a rectangular building. The detail are as follows

building size: B=0.1125m D=0.075m H=0.45m

domain size: B=3m D=6m H=1.8m

coordinate x=-1.5 to 4.5 y=-1.5 to 1.5 z=0 to 1.8

The base of the centre of the building is at the origin

velocity profile: power law u=14.7*(z/1.5)^0.15

turbulent model: RNG k-epsilon

I used fixed time step = 0.004s with SIMPLEC for velocity coupling and QUICK for covective transport.

I used the same mesh to calc steady flow and there is no problem and I just changed the setting in fluent from steady to unsteady.

I failed to obtain a periodic fluctuation in lift force. Is there an error in setting?

Thanks

You will benefit from reading the tutorial (6) Flow past a circular cylinder www.studentfluent.com QUICK scheme is excellent if the stability is maintained

Thanks for your reply. I used hex element to mesh the grid. Should I use SIMPLEC or PISO for pressure-velocity coupling?

Use Piso for unsteady simulations. But it will take more time compared to Simplec.

Anindya

maybe you should consult the HELP, there are many useful information i think.

changkiang

I have tried PISO with time step=0.004s but continuity still does not converge after 100 iterations at the start

Should I further reduce the time step size?

Thanks.

Should I use "Use Frozen Flux Formulation" also?

Thanks

I would suggest to stay with PISO algorithm and definitely reduce your time step, at least 2 orders of magnitude.

Hope this helps

Edi.

reduce your time step to around 10^-5 range.

I tried to reduce to 0.001s but got a malloc error. What should I do?

I changed the time step to 0.001 sec. It converges in 30 iterations but I got a out of memory error. Should I change back to SIMPLEC or use a single precision solver instead? If I use a single precision solver, is the convergence limit of 1e-5 appropriate?

Thanks for your help.

The memory error should be related much more with the dp solver than that with the algorythm, so try to keep PISO (that reduces the iterations per time step a lot, believe me...) and move to single precision. The convergence limit of 1e-05 (at least for continuity) sounds appropriate.

Hope this helps

Edi.

Thanks for your suggestion. I started unsteady calculation with steady solution. In order to 'start' vortex shedding, I modify the inlet B.C. such that v=0 for y<0. But then I got the message "Reversed flow in ### faces on outflow". Is this message important? How to avoid this message?

Thanks again for your help.

It simply means that in some cells of the outlet boundary the flow is coming in instead of going out (as it is supposed to be for an outlet boundary). Basically it is due to the position of the boundary, if you have put a pressure boundary too close to the building the flow could not be fully developed and in order to satisfy the boundary condition reversed flow appears.

If it disappears after some iterations (before proceeding to the next TS) it's acceptable, otherwise consider to extend your domain past the building.

Hope this helps

Edi.

Thanks for your reply. I found out that when I change the velocity field at inlet, the first few timestep did not converge. Would it affect the solution of subsequent timestep?

Yes. First time steps are usually a bit more difficult to converge. Consider augmenting the n° of iterations per TS until a converged solution is reached.

Hope this helps.

Edi.

I tried PISO with single precision solver. But I found out that the residue continuity did not fall below 1E-05 but oscillate around 2E-05. I know that it may due to numerical diffusion. I also tried SIMPLEC with double precision solver. I started with steady state solution and patch the static pressure on one side face to start vortex shedding. Although the lift force is sinusoidal with decreasing amplitude, the result is wrong. The Strouhal number is 0.01, which is 10 times smaller. The amplitude is also very small, about 0.00014N. What should I do? Thanks for your advice.