[NGH]

Hi

Im simulating the flow past a cube using FLUENT LES model and encountered some issues. The flow is 0.4m/s and the cube is 0.1 m. How many flow through times do I need to get the distinct flow features? After 2 flow through time, the features are still very fuzzy. What could be the problem? Thanks


Im using pressure velocity coupling: SIMPLE
Gradient:Green Gauss Cell Based
Pressure:Standard
Momentum:Bounded Central Differencing
Transient Formulation:2nd Order Implicit

[LuckyTran]

Originally Posted by NGH

Hi

Im simulating the flow past a cube using FLUENT LES model and encountered some issues. The flow is 0.4m/s and the cube is 0.1 m. How many flow through times do I need to get the distinct flow features? After 2 flow through time, the features are still very fuzzy. What could be the problem? Thanks


Im using pressure velocity coupling: SIMPLE
Gradient:Green Gauss Cell Based
Pressure:Standard
Momentum:Bounded Central Differencing
Transient Formulation:2nd Order Implicit

Just to clarify, this is flow around a cube much like flow around a cylinder or sphere correct? i.e. some type of velocity inlet and pressure outlet? The oncoming velocity is also uniform?

For LES, the initialization is VERY important. How did you initialize your case?

For LES, typically a RANS solution using your favorite turbulence model is used. Then a random perturbation is slapped onto the solution to force it to transition to turbulence. This random perturbation is very important, if not done properly, the flow will stay laminar! Recall that turbulence is just the amplification and manifestation of small flow instabilities (so for LES you need to provide these instabilities).

After the perturbation, you need to run the simulation for enough flow through times for the effect of the perturbation to disappear, I would say 2-3 flow through times. You can run a few more to be safe. Even if the initial effects are not gone, you should be able to see distinct features by then to know your simulation is proceeding properly.

[NGH]

Hi

Do you mean that I run a RANS solution and then use the case and data file to start LES simulation? How do I introduce the perturbation that you are mentioning in FLUENT Ver 12? Thanks

[LuckyTran]

Originally Posted by NGH

Do you mean that I run a RANS solution and then use the case and data file to start LES simulation?

Yes, exactly. It is just to provide a good initial guess the same way you would initialize a flow. It is better to initialize with a good guess than a bad one, especially for LES since it is expensive. Run a steady RANS, no need to waste resources with URANS. Relative to the cost of doing the LES, the RANS expense is a joke. You do not even need to solve it well, just solve it enough to have a flow that looks decent.

Originally Posted by NGH

How do I introduce the perturbation that you are mentioning in FLUENT Ver 12? Thanks

Before you proceed, I would suggest checking your solution to see if you are having the prob of your flow remaining laminar first because the rest of my discussion may be unnecessary.

To my knowledge, this cannot be done in fluent (at least not through any feature in fluent). Maybe you can do some crazy UDF or something.

I have always exported my solution data, and then wrote a program to slap random perturbations onto the solution. You can use MATLAB, C, Python, anything programming language that supports reading a text file pretty much. I then import the data into back into fluent and start running. =)

The perturbations should not be completely random, since that would add non-physical velocities. Again, this is all just to give the solver a very good initial guess, so you want very realistic instantaneous velocity distributions to start your LES.

A good way is add a gaussian-like perturbation (normal distribution), with standard deviation proportional to the turbulent kinetic energy (or turbulence intensity). Recall the definition of turbulent kinetic energy contains velocity fluctuations. Here is where it really helps to have already solved a RANS case. Using your favorite 2-eqn model or otherwise, you would already have solved for the turbulent kinetic energy and can use that for the perturbations. This is my own way of doing it (based on a method originally developed by Jewkes).

The perturbation step is not absolutely necessary. In some cases, the flow may become turbulent without the use of perturbations. Even when perturbations are added, in many cases it is very possible for the flow to relaminarize (also very common) if the perturbations are not done well enough. Again, only worry about all this if your flow is not capable of becoming turbulent on its own.

[sbaffini]

While adding your own fluctuations is what i suggest (i used to do it by a very simple interpreted UDF) as you have more control and sometimes you can avoid the initial RANS computation, you should be aware that, if you have a RANS solution in Fluent you can:

/solve/init/init-instantaneous-vel

via TUI (or something very similar) and you get your fluctuations in the initial field which, by the way, are based on the spectral synthesizer and are not purely random.

However, i don't know the details of your simulation but for a flow over a cube initialization is probably the last problem; if you can't get reasonable istantaneous results after no more than few flow trough times (if you have distinct inflow-outflow boundaries than 1 is just enough) then i would start looking elsewhere (grid size, time step, b.c., etc.).

In contrast, if you are talking about average results (after the activation of the flow statistics), then yes, this can be a mess and you could need several tens or hundreds shedding cycles to get proper average results.

[mazdak]

hi guys
i am running ANSYS 14 to simulate turbulent backward step flow by LES.
(http://www.sciencedirect.com/science...07570403001138)

in this paper, they plotted fluid velocity in different part of channel.
i want to know how can i obtain this velocity profile? after how many seconds
should i plot the profiles?
i mean how can i find that statistically fluid is steady?
and how can i obtain fluctuation and mean velocity component by ANSYS?
THANKS

[LuckyTran]

Originally Posted by mazdak

hi guys
i am running ANSYS 14 to simulate turbulent backward step flow by LES.
(http://www.sciencedirect.com/science...07570403001138)

in this paper, they plotted fluid velocity in different part of channel.
i want to know how can i obtain this velocity profile? after how many seconds
should i plot the profiles?
i mean how can i find that statistically fluid is steady?
and how can i obtain fluctuation and mean velocity component by ANSYS?
THANKS

You need to average over enough seconds to reach statistically stationary variables. The actual time in seconds will depend on your velocity and length scale so you need to think in terms of non-dimensional time. Usually this is a few characteristic times or flow-thru times. Sorry don't have access to the paper from my current computer but that time is usually noted in most papers.

Fluent can keep track of mean and rms values, you just need to enable "Data sampling for time statistics". fluent keeps a running count of average velocity and rms values starting from the iteration when this option is enabled. It can be reset at any time that you wish to clear the average.