CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Unsteady flow around a rectangular building

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 3, 2006, 05:25
Default Unsteady flow around a rectangular building
  #1
EA
Guest
 
Posts: n/a
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
  Reply With Quote

Old   March 3, 2006, 12:47
Default Re: Unsteady flow around a rectangular building
  #2
Ahmed
Guest
 
Posts: n/a
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
  Reply With Quote

Old   March 4, 2006, 02:19
Default Re: Unsteady flow around a rectangular building
  #3
EA
Guest
 
Posts: n/a
Thanks for your reply. I used hex element to mesh the grid. Should I use SIMPLEC or PISO for pressure-velocity coupling?
  Reply With Quote

Old   March 4, 2006, 12:32
Default Re: Unsteady flow around a rectangular building
  #4
Anindya
Guest
 
Posts: n/a
Use Piso for unsteady simulations. But it will take more time compared to Simplec.

Anindya
  Reply With Quote

Old   March 5, 2006, 01:41
Default Re: Unsteady flow around a rectangular building
  #5
changkiang
Guest
 
Posts: n/a
maybe you should consult the HELP, there are many useful information i think.

changkiang
  Reply With Quote

Old   March 5, 2006, 23:32
Default Re: Unsteady flow around a rectangular building
  #6
EA
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 5, 2006, 23:45
Default Re: Unsteady flow around a rectangular building
  #7
EA
Guest
 
Posts: n/a
Should I use "Use Frozen Flux Formulation" also?

Thanks
  Reply With Quote

Old   March 6, 2006, 07:38
Default Re: Unsteady flow around a rectangular building
  #8
edi
Guest
 
Posts: n/a
I would suggest to stay with PISO algorithm and definitely reduce your time step, at least 2 orders of magnitude.

Hope this helps

Edi.
  Reply With Quote

Old   March 6, 2006, 11:14
Default Re: Unsteady flow around a rectangular building
  #9
Anindya
Guest
 
Posts: n/a
reduce your time step to around 10^-5 range.
  Reply With Quote

Old   March 6, 2006, 23:23
Default Re: Unsteady flow around a rectangular building
  #10
EA
Guest
 
Posts: n/a
I tried to reduce to 0.001s but got a malloc error. What should I do?
  Reply With Quote

Old   March 7, 2006, 00:31
Default Re: Unsteady flow around a rectangular building
  #11
EA
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 7, 2006, 05:35
Default Re: Unsteady flow around a rectangular building
  #12
edi
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 7, 2006, 09:36
Default Re: Unsteady flow around a rectangular building
  #13
EA
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 7, 2006, 10:55
Default Re: Unsteady flow around a rectangular building
  #14
edi
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 8, 2006, 04:32
Default Re: Unsteady flow around a rectangular building
  #15
EA
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   March 8, 2006, 05:51
Default Re: Unsteady flow around a rectangular building
  #16
edi
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   March 13, 2006, 11:01
Default Re: Unsteady flow around a rectangular building
  #17
EA
Guest
 
Posts: n/a
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.
  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Periodic boundary in unsteady flow ac2011 FLUENT 0 September 26, 2011 06:52
Incompressible, Unsteady Cylinder Flow startingcfd Main CFD Forum 1 March 15, 2011 02:12
Compilation error OF1.5-dev on Suse10.3 darenyang OpenFOAM Installation 0 April 29, 2009 04:55
Unsteady Flow in FLUENT Vidya Raja FLUENT 0 November 1, 2005 18:54
Solving unsteady compressible low speed flow atit Main CFD Forum 8 July 31, 2000 13:19


All times are GMT -4. The time now is 11:25.