Fluent: convergence problem, help
I am having a problem getting my solution to converge. I tried everything in the users manual to no avail.
Here is the set up: I have a tank with water in it, and a heater in the center, and a capped off pipe coming off of it. It is kept in a fairly cold room, and the temperature difference causes natural convection flow within the tank. I am trying to simulate this experiment using FLUENT. I am fairly certain I set up the boundary conditions correctly, and my mesh seems OK. I am running the coupled explicit solver for realizable kepsilon viscous model. I have the courant number set to 0.1 right now, because that seemed to be the thing to do initially for my problem, according to the users manual. It was converging (excruciatingly slowly) but at least it was. Then it seemed to get "stuck" before reaching the convergence criteria. So I tried many different ways to get it unstuck (changing courant number, changing multigrid settings, volume adaption, underrelaxation). All I have succeeded in doing is cause it to start to diverge again. I need some serious help. Can someone point me in the right direction please? 
Re: Fluent: convergence problem, help
It is difficult to converge natural convection problem. There is a set of relaxation factors to converge your problem and (as you know) there is no absolute way to find your own relazation factors except continuous trial.
P.S. Do you have any special reason to use coupled solver? As I know, coupled solver solves governing equations simultaneoulsy. Probably that maks your problem more difficult to be converged. (Just my personal opinion) 
Re: Fluent: convergence problem, help
Buoyancy can be difficult sometimes. Assuming your mesh is OK and all your fluid properties are OK, here are some suggestions. First, I don't like to use the Boussinesq approximation. If you're using it, try specifying a temperature dependent fluid density. Second, try the segregated solver. It's not "better" than the coupled solver, just different, but it might help. Third, try starting with a lower gravity (say 2.0 m/s^2) and let the solution partially converge, then increase the gravity force in small steps (say 2.0 m/s^2 each step) and partially converge in between.

Re: Fluent: convergence problem, help
Thanks. I ran this first as a 2d problem using the segregated solver and could'nt get it to converge, so I changed it to the coupled solver, then it converged. The results weren't that accurate, but I didn't expect as 2d problem that it would come out close to my 3d experiment. When I ran the 3d case I kept the coupled solver. I will try all of your suggestions one at a time and see what happens.

Re: Fluent: convergence problem, help
For your problem, a good idea of what bouyancy model to be used is necessary. In Fluent, I suppose you can only use Boussinesq approximation for liquid or you need to provide some kind of function yourself. So make sure that the temperature dependent fluid density is correct. Also, you may like to refer to User Manual Chapter 8 regarding bouyancy model for further details.
I deal with bouyancy model everyday. My experience on bouyancy model is to use segregated solver and switch the run to transient even you are looking for steady state solution. It is usually the only way to get converge result for bouyancy driven flow. To speed up the run, you can first start the run as steady state and switch it to transient later. 
Re: Fluent: convergence problem, help
Well, I've been trying... Using the segregated solver does not help. Continuity diverges and causes a floating point error. I have tried changing gravity. It is converging, but very slowly still. I haven't had much luck changing from boussinesq to temperature dependent density, but that may be because I set up the temperature dependence wrong. Trying to solve as an unsteady problem does not appear to speed up the process at all, but at least it is still converging. I have been consulting chapter 8, and I thought I was doing what I was supposed to. Any more suggestions?

Re: Fluent: convergence problem, help
Can you describe you model with further details? Eg. axisymmetric, 2D, or 3D; the dimensions, etc. I think I can try it and see whether I can come up with something.

Re: Fluent: convergence problem, help
its a 3d symmetric problem. The tank (made of plexiglas) is 30 inches wide X 30 inches long X 40 inches tall, with a 4.5 inch ID pipe, 22 inches long coming off the side at 30 high along the centerline. It is filled with water (with boussinesq density). A heater is in the center of the tank, 12 inches from the bottom, 18 inches tall, attached to a 1 inch ID copper pipe along the length of the center of the tank. The plane of symmetry is along the centerline of the tank, heater and pipe. I used GAMBIT to make the mesh. It is set to maintain a constant temperature of 93 F, and the room temperature is a constant 60 F. I initially tried to just simply set the boundary condition at the walls to a constant temperature of 60 F. Also, I had kept it as a laminar flow problem. It converged, but the values for velocity were several orders of magnitude different from the experimental results. I changed the boundary conditions to convective heat transfer, with the heat transfer coefficient calculated by using an assumed outside wall temperature of 70 F (not entirely a guess, I have some thermocouples on the outside surface of the tank as well) and the free stream temperature at 60 F. That may not be the right way to do it. I also added turbulence. I wasn't sure if I needed to, because the reynolds number I calculated using the experimental flow rate is kind of low, but visually, it looked like there might be some turbulence, so I added it to the model. Using the segregated solver, this diverges (continuity residual). With the coupled solver it starts to converge, but the residuals get stuck before meeting the convergence criteria (default settings). This has been plaguing me for months. I hope someone can help.

Re: Fluent: convergence problem, help
In Seggregated solver : try high relaxation(0.7) for pressure and low relaxatation for velocity(0.3) after few iterations with default values(0.3 pressure, 0.7 vel). See if it works.

Re: Fluent: convergence problem, help
Thank you so much. That did the trick! It has converged!
Cindy 
Re: Fluent: convergence problem, help
I had the trial run converage with seggregated solver. In fact no specific solver setting is required and the modelling is very straight forward. The key points are using Boussinesq model and transient simulation for convergence. Pls advise me if you would like to have the case file for a look.
Regards, KH 
Re: Fluent: convergence problem, help
If its not too much trouble, I would like to see your case file. thank you.

Quote:

I haven't tried that to see if it works, but so far I've only been modelling convection with temperature differences of around 70K so the boussinesq model is fine.
I struggled to begin with, but I finally got my problem sorted when I reduced the gravity to 9.81e3 and went up by orders of 10 after the convergence rate dropped. Took around 2000 iterations per model though  but I'd of expected that because of the complex geometry in my model. Other models should converge quicker. 
Hello all!
I had the same problem in a room containing 10 people and lamp. I got a very smooth converge without considering Buoyancy. After getting converge I impose the gravity to apply Buoyancy. then I got diverge (divergence detected in AMG solver pressure correction) or the residuals jump over the zero and didn't come down. I run with Ke RNG, Simple C, Incomprehensible ideal gas, inlet speed 0.28 m/s I read whole the posts, But I cannot come up with the conclusion? Is there anybody here can draw a conclusion? How can I check if the temperature dependent fluid density is correct? Thanks. 
Hello all!
I had the same problem in a 1m 2d square, 10 degrees different for two sides, and Ra is about 1e+09 with air. I can get the solution by using g=0.000981m/s2, that is making Ra<1e+5, but as I increase g I can't get it converge! Is there anyone can help? Thanks! 
All times are GMT 4. The time now is 23:19. 