I found that the speed of FLUENT 6.2 is so slow, especially for the unsteady state. It took much longer time to converge than 6.1, and sometimes it diverge.

i agree with you, 6.2 seems to be slower than 6.1, but fluent claims 6.2 is faster.

I think there maybe some bugs in FLUENT 6.2. Now I change it back to 6.1 It took several days to run my program, which before I just need to spent several hours on.

Are there any things you can elaborate on? Which models do think could be problem? Solution schemes? Grid types?

I have recently switched to 6.2 from 6.1 and have run several cases for boiler simulations. I haven't seen any issues (other than with UDF names described previously) and although 6.2 went on a new workstation, the speed-up with the new system was as expected.

i also prefer to run it on 6.1 as much as possible, but in my case we are mostly using les models those are not available in 6.1, so sort of stuck, for example for a case with 3 million cells i used to get results in three days , but now with 4 million and using three 64bit (4gb ram each) linux machines, its been 4 days and job is still 40 percent done.

i have observed that when i run the 6.2 on parallel machines its performance is inferior to 6.1 but on single machine its difficult to notice , but this thing can really be confirmed if other users also feel the same.

Hi zxaar,

Could you please briefly outline the steps in les simulation using fluent? I tried using 6.1 for an impinging jet with about 2 million cells, but I find the results are not what I should get. Also when I see the vector fields of velocity, the instantaneous and the time averaged results look to be the same. But when I see them as contours, they look diferent (as it should be).

So if possible please outline the steps that you follow both in 6.1 and 6.2 starting from the initial run and ending with clicking the button for time averaged data.

Thanks a lot.

Anindya

i am afraid the steps are as simple as just enabling the LES models, however i can write my observations about the results i obtained:

my case is highly separated flow, and the prediction of drag and lift coefficients are pretty difficult in this case.

1. of all the models, rng les has given me best results with prediction of drag and lift coefficients within the error bound of +/-5percent.

2. with other les my results sometimes differ as 10-15percent, but still i take them as good results as its so difficult to predict drag and lift in my cases.

3. two equation models give me results as off as 30 percent from experimental values. i have tried k-e and k-w models, even with enhanced wall treatment (that is keeping yplus less than one). (here for k-w model enhanced wall treatment is enabled by putting transition option on).

4. contrey to popular belief, i have mostely got better results using tet meshes than hex or prism meshes. this could be explain as this the region where there are lot of small vortices, the flow does not have a finite direction and hence prism meshes lose their advantage there, and tet meshes give better results. To check this, we had a very fine mesh completely made up of prisms (with quad elements) and other parts were just cartesian mesh. the mesh size was 4.5 million cells and we used rng les with it, the results were off by 20 percent from experimental values. now consider this another case it is only 1.3 million cells, with tet in the turbulent region (and very thin layer of prisms near to wall, extending to yplus 30 or so), and some cart mesh in far regions , we got the results with in 5 percent from experimental values, using rng les). so you can see, that the mesh size does not matter (after a limit) if mesh is based on the nature of flow you have.

5. i am still running DES and SA models with the same meshes and i have only one or two calculation with them so can't much comment on them , but results were between the les and 2 equation models.

6. time step and number of steps you perform at each step are crucial, for me i get best results at 1E-05 or 5E-05, smaller than this is too small, and larger than this i get bad results.

in summery:

use very small prism meshes near walls , and if you have a region where you have lot of vortices then use tet meshes there, and try to keep meshes as fine as possible, the far region mesh could be coarse, use small time step with number of iteration per time steps around 7-8 (i use 1.0E-05 and 7 iteration perstep), first few steps (around 5 are with 1E-06 and 10 iteration perstep, you can call it initialisation). and yes for the initialisation steps do not use time sampling option for averaging).

Thanks for your detailed information.

Could you please let me know a few more things?

1) How do you enable rng-les? I did not find it. I am running 6.2 on a linux box.

2) How long (how many time steps)do you run your simulation to get time averaged results (when you collect data using a time step of 1.0E-05 ? And how many processors do you use?

3) So instead of using default 20 iterations per time steps, you set it to about 7-8?

4) So you are not using NITA scheme in 6.2 ?

5) Do you use perturb the inlet velocity?

Thanks for your help.

1. i myself do not know how to enable rng les, it once happend accedently, and i am not able to find the way to do it. my superior asked fluent support (he is not cfd man) they told him its not present in GUI because it is not a good model. (funny reply but that is what they told him). Anyway if you have to enable rng les, do give me your email, i willsend you a small case you read that case first that will enable rng les and put it on GUI and then read your case, (i created the case from the first calculation i did and now that is how i enable it).

2. i am usually going till 2000 time steps or more, usually i plot Cd and Cl and that tells me whether i have got the Cd and Cl values and based on it i stop the calculations.

3. yes i use around 7 iterations per time step, since my time step size is very small.

4. i treid using NITA but could never get converged results, it always comes out with some error like floating point or divergence.

5. in my case the inlet flow is very much laminar, i can safely assume so, so i usually do not perturb the inlet flow, but perturbing inlet won't change much, considering the way fluent does this.