# Bouyancy-driven flows and convergence

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

 LinkBack Thread Tools Display Modes
 March 5, 2009, 04:44 Bouyancy-driven flows and convergence #1 Marcello Caciolo Guest   Posts: n/a Dear CFD users, I am dealing with simulating a bouyancy-driven flow in a room with Fluent. When I set up the case and lauch the simulations, the residuals drop down of two orders of magnitude in the space of one-two hundreds of iterations, depending on the boundary conditions I impose. After that, residuals stop to drop down and begin to fluctuate slightly, without increasing or decreasing any more. Changing the under-relaxation factors for pressure, energy and/or turbulence variables makes the residuals drop down some few iterations, but after that they begin again to fluctuate around another value. At the same time, I monitor the value of some variables I am interested to, and they oscillate very slightly too. To give an idea, a volume flow rate at a surface of interest have fluctuations of 0.1% around its absolute value. My question is: can I consider converged the solution, even though residuals have drop down only of two orders? If yes, is it normal that residuals and solutions fluctuates slightly when reached convergence? Could this mean that a steady-state solution does not exist? Thank you in advance. Best regards, Marcello Caciolo phD student CEP - Center for Energy and Processes of Ecole de Mines de Paris

 March 5, 2009, 08:57 Re: Bouyancy-driven flows and convergence #2 Tom Guest   Posts: n/a Hi, I think you have 2 options here. It seems you will not get steady state but I think that if you average over enough iterations you will have a decent solution given that your residuals have dropped sufficiently and that your oscillations are very small. If you run for long enough you will see the solution oscillating with a certain period and average over that. You can also run it a transient simulation but you must be careful selecting time-steps and I would not say you need a time accurate solution. I maybe wrong so see what others say. Tom

 March 5, 2009, 12:18 Re: Bouyancy-driven flows and convergence #3 Jonas Holdeman Guest   Posts: n/a I have had similar experience with these flows at larger Rayleigh numbers using my own code. This leveling off of the residual can be reduced by going to even more under-relaxation. If the relaxation parameter is small enough, there is no leveling of the residual down to the level of numerical roundoff, but who is to say that it still would not level off with higher numerical precision. Probably your solution is not changing much (to engineering accuracy) as you increase under-relaxation, and you can accept the remaining residual. Though it is a stretch to accept this analogy, there is the case of evaluation of asymptotic series. As you add terms to the partial sums, the error gets smaller, up to a point where the error increases and the series diverges. The accepted procedure is to sum until the error stops decreasing and stop summation there. That is the best you can get out of this series.

 March 5, 2009, 14:27 Re: Bouyancy-driven flows and convergence #4 Ahmed Guest   Posts: n/a try increasing the mesh density

 March 6, 2009, 06:30 Re: Bouyancy-driven flows and convergence #5 Robin Guest   Posts: n/a Nah, try decreasing mesh density. It's likely that you're resolving transient flow features (big wobbly plumes). A good old bit of numerical diffusion will help to settle things down

 March 6, 2009, 11:42 Re: Bouyancy-driven flows and convergence #6 Jonas Holdeman Guest   Posts: n/a My experience with my code: this behavior is largely independent of mesh density.

 March 6, 2009, 12:31 Re: Bouyancy-driven flows and convergence #7 Robin Guest   Posts: n/a not mine

 March 6, 2009, 14:43 Re: Bouyancy-driven flows and convergence #8 Ahmed Guest   Posts: n/a Jonas Holdman wrote "this behavior is largely independent of mesh density." (I guess you refer to the stationary oscillations of the residuals). The left hand side of the Navier's Stokes equation is hyperbolic in nature, that means the advection of scalar and vectorial quantities is carried out by wave like phenomenun. Translate that to the computational grid, and a discrete perturbation analysis will show you the effect of the so called "cell Peclet Number". Good Luck

 March 6, 2009, 15:45 Re: Bouyancy-driven flows and convergence #9 Ahmed Guest   Posts: n/a Jonas, sorry I did not have this reference at hand, when I wrote my previous comment, Computational Fluid Dynamics For Engineers by Klaus A Hoffmann has some nice figures showing the nature of error.

 March 6, 2009, 16:56 Re: Bouyancy-driven flows and convergence #10 alex Guest   Posts: n/a if you stick a radiator in a middle of a room and pour some smoke to visualize air movement from buoyancy, you are not going to see some sort of a nice steady-state hot air rising, you will see a blob of warm stuff accumulating over the thing and then puff, it goes up, and then the deal repeats itself, in other words, there is no steady-state and most of the time buoyancy stuff is transient. Now, all commercial codes are full of diffusion and won't just blow up, they will converge a bit and then keep oscillating and that's what you are seeing in the residuals. So, take them and be happy, just like Jonas suggested. And, btw why would you add more diffusion with coarser mesh, to get as far as possible from an already remotely correct solution and dispersion has nothing to do with buoyancy driven stuff either....

 March 7, 2009, 07:20 Re: Bouyancy-driven flows and convergence #11 ztdep Guest   Posts: n/a how many grid sytem did you use and laminar flow or tubulent flow

 March 8, 2009, 04:34 Re: Bouyancy-driven flows and convergence #12 Tom Guest   Posts: n/a "you will see a blob of warm stuff accumulating over the thing and then puff" Are u sure about this? I know the buoyant plume is transient, i.e. it will meander/wobble like people say, but what you are suggesting is different to that. You seem to be saying that the plume stops and starts, which I don't think could be physical. Unless you have seen the plume to loop right around before rising? Maybe if you could point me to the appropriate literature that proves this.

 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 brossofor FLUENT 0 March 29, 2011 04:31 freemankofi ANSYS 0 April 8, 2010 16:59 Brian FLUENT 1 February 1, 2006 09:41 co2 FLUENT 4 May 6, 2004 11:37 Pedro Gil Main CFD Forum 3 April 25, 2000 11:34

All times are GMT -4. The time now is 11:00.

 Contact Us - CFD Online - Privacy Statement - Top