

August 31, 2018 at 6:40 pmJosé MantovaniSubscriber
Hello guys!
So I have some doubts to do a good way in a Large Eddy Simulation and with a quick search in google I found a pdf with sometips to make this in ANSYS FLUENT. In respect regarding the mesh process I have some knowledge and my doubts is around the solution process. I give some image below with the data that I found in this pdf which I got in google. To make it clear, I do not have a supercomputer at my disposal and my package is student (some limitations).
Doubts can be seen in the two comments below, it did not fit all in one post.

August 31, 2018 at 6:42 pmJosé MantovaniSubscriber
At first point, it's ok, as make a fully converged solution is easy I consider to use a fully converge steady RANS solution by a turbulence model of my preference.
The second point, Is it really necessary to impose this turbulence synthesizer? What happens if I do not?
The third and fourth point it's ok.
For the fifth point, I tested a approach which I found in a Power Point file gived by dear friend Raul that have a way to speed up the solution which talks to use a very small time step size with a large iteration for the initial solution and decreasing across the solution, but I make some test with this and I obtained results, say, unsatisfactory, I think that for the case of the time step must be really small and as it has been calculated an amount of time to decrease the number of iterations per step of time but maintaining its size. (If anyone wants to comment on this, I'll be happy.)

August 31, 2018 at 6:42 pmJosé MantovaniSubscriber
For the sixth and seventh point is ok, for the the last (7th) I think that is in respect to create a Calculation Activities compatible with CFDPost, per exemple.
In the eighth point, I want know: What does it mean when say you get a statistically stationary state? Is it to follow the convergence residues in order to stop the solution when they obtain a "linear" behavior?
The ninth point ok.
In the tenth point, this point I need make after the solution be statistically stationary state or I need to configure the data sampling in the FLUENT area where I run calculation from the beginning of the solution?
For the eleventh point, How I calculate the flowthrough times? What is L in the formula L/Uo as we can see in the image above?
And the twelfth point is also ok.
So, here have many doubts about the LES solution procedure, but I think that it can be useful for someone which take a look in this thread. I will be very grateful to those who have the knowledge on this subject and can share their knowledge here in order to solve these small doubts. I'm here waiting!
Thanks for attetion.
Mantovani.

September 2, 2018 at 2:58 amraul.raghavSubscriber
2. Superimpose initial synthetic turbulence: This is required so you can achieve relatively faster convergence of the LES simulation (Vortex method over Spectral Synthesizer)
5. Timestep size: It is recommended to estimate the local timescale information from the precursor RANS simulation. You can create a custom field function (CFF) to evaluate the local timescale, dt = cellvolume^(1./3.) / (V + 0.00000001). Plot this CFF at multiple planes across your geometry to get an estimate of the min dt value. Ansys also suggests to use a timestep size of 0.5 * dt, which means that you set your timestep in such a way that you aim for a Courant number of 0.5.
8. Statistically stationary state: This step is essential to eliminate the initial condition effects. The turbulent instabilities that are developed due to the initial conditions provided (either a RANS simulation or user assigned initial conditions) has to be convected out of the fluid domain. Since LES is computationally expensive, it is important to detect problems right from the beginning. You can monitor velocity across certain regions of your domain and if a repetitive pattern is noticed, then you can say that the simulation has reached a statistically stable state beyond which you can start timeaveraging and sampling your data. This could take a minimum of 1 through flow cycle.
10. Sampling the data and 11. Sample for a sufficiently long period of time: Once you've reached a statistically stable state, you can start sampling your data for several flow through cycles until you achieve a timeindependent average solution. This could be anywhere between 525 through flow cycles (as Ansys reports). Mean values are reported to converge after 5 through cycles whereas the rms values can take between 1025 cycles. The length scale (L) in the equation is the length of the flow domain. For a simple pipe flow, it would be the length of the pipe and not the diameter.
There is a lot more to LES that cannot be covered over a post. The grid requirements are expensive for LES and with the student package you might be limited in certain aspects. Good luck Jose. Let us know how your simulation goes.

September 2, 2018 at 6:25 am

September 2, 2018 at 11:05 pmJosé MantovaniSubscriber
Very thanks Raul, I will make the simulation through this procedure and soon I share here my results. I try to do the simulation of BFS in LES approach because I tested several ways to converge the graphs of Cp and Cf and also the reattach point, but I get good results for Cf and rettach point but the Cp overpredicts the experimental data in all ways... Look the charts in image below.
The discussion of this simulation stay here, I don't now if you looked this thread: https://forum.ansys.com/forums/topic/understandingthebehaviorofthesolutionresultsbyfluent/ If you can give some comment about or some tips I will be very grateful.
Like me, other friends here in the community, found it very funny that the Cf graph and reconnection points are close to the experimental but the Cp near the reconnection overpredicts the experimental value. I have tested several models and meshes but, for example, when I improve the reconnection point the graph Cf is further from the experimental and for the graph of Cp I always get this values higher close to x / h = 5 ... I am happy for being able to "validate" my simulation, but only this detail of the Cp chart is missing. So I decided, within my limitations, to take an LES approach.
A while ago you made available to me the community a file, which even has this formula to find the size of the time step. And at the end of the file, there is a slide with this image, I do not know if I can access the Customer Portal with the login here in the community. Could you pick up and make this file available to me? (in the image below). If you can comment on my RANS results for BFS and because I always get an overpreditc on the Cp chart I will be very grateful as I am already for your huge help.
One more time, very thanks for your attention and helping! I will try make the LES approach and soon I give my results here.
Best Regards,
Mantovani.

September 3, 2018 at 4:42 amKeyur KanadeAnsys Employee
Hello,
With student version, you have limitation on no. of cells. With LES, you will very fine mesh which will go above limit. So with student version you may not able to do LES perfectly. You may want to continue with RANS.
You will get more description at following link. Please check problem size limits.
https://www.ansys.com/enin/academic/freestudentproducts?utm_source=studentcommunity&utm_campaign=studentcommunity&utm_content=Studentproduct&utm_source=studentcommunity&utm_campaign=studentcommunity&utm_content=Studentproduct
Regards,
Keyur

 You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Suppress Fluent to open with GUI while performing in journal file
 Floating point exception in Fluent
 What are the differences between CFX and Fluent?
 Heat transfer coefficient
 Getting graph and tabular data from result in workbench mechanical
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error in cfd post

2524

2066

1279

1096

457
© 2023 Copyright ANSYS, Inc. All rights reserved.