CFD Online Logo CFD Online URL
Home > Forums > FLUENT

K-Epsilon for Vortex Shedding

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes

LinkBack Thread Tools Display Modes
Old   August 28, 2007, 20:15
Default Re: K-Epsilon for Vortex Shedding
Posts: n/a

First of all thanks for your replies in guiding me above.

1. I have tried SST-kw and LowReke and it seems that SST-kw is giving me better results. Right now, I am only modelling 2D but will move to 3D once I get the hang of things. In your experience, in RANS 3D modelling what is the most suitable model that predict the forces and vortex shedding accurately? How far do you usually place your first grid on the wall?

2. As shown in tutorial, I patch some y-velocity on the second half of my domain to produce some perturbation to initiate vortex shedding and I did observe vortex shedding. Is this justifiable? Will the y-velocity affect the calculation of force?

3. This might sound like a stupid question but how do we perform a time average of the Cd and Cl to get the mean value in unsteady solver? How can I get the Vortex Shedding frequency?

Thanks once again.

  Reply With Quote

Old   August 29, 2007, 02:03
Default Re: K-Epsilon for Vortex Shedding
Posts: n/a
Hi Sham,

1. I never seriously tried RANS in 3D for this specific problem, once I applied the low-Re omega-based RSM just to see the effects, and it seemed qualitatively close to LES (good vortical structure behind the cylinder, much more detailed then any other RANS model). But I did not run the simulation long enough to be able to draw a conclusion on forces. Although I must mention that the grid was almost dense enough to try LES on it...

2. The artificial triggering of physical phenomena is perfectly justifiable if the final result or the evolution are not influenced.

For example, in a gaseous mixture of methane and air, the velocity of the flame front is totally dependant on the energy of the initial impulse, and consequently the effects. For a simple spark, the flame front will move at several tens of meters per second (deflagration) and the pressure created will blow (only) the windows and doors of the kitchen (hopefully). But if the initiation is made using a blasting cap (hard to find one of those in a kitchen, but anyway), the flame front will move at hundreds of meters per second (detonation) and the pressure created will be sufficient to blow away the whole kitchen, and the neighbor's too!

Seriously now, for the vortex shedding phenomenon, a patched y-velocity will have an influence on the forces for maybe no more than a few time steps. You would understand the necessity of the patching process if you'd try to simulate the problem starting from perfectly uniform initial conditions (the time elapsed until vortex shedding occurs will be very long). Even in such conditions, the vortex shedding will still appear, even for a perfectly symmetrical grid, because of round-off errors.

3. The mean Cl is going to be 0 anyway, but for Cd, in the past I used an external program to calculate the mean value, if I wanted an exact value, or simply estimated it by eye. But you could probably use the signal processing capabilities of FLUENT (FFT). I don't know this for sure, it's just a suggestion. The vortex shedding frequency is quite easy: simply count the min or max values of Cl within a certain timeframe and scale it to 1 second, and that's it.

All the best,


  Reply With Quote

Old   August 29, 2007, 02:56
Default Re: K-Epsilon for Vortex Shedding
Posts: n/a

It is always stimulating to see replies from you. Thanks a lot for your help and hope you do not mind should I need more help later in my research.

  Reply With Quote

Old   August 29, 2007, 15:16
Default Re: K-Epsilon for Nozzle flow saparation
Posts: n/a
Hi Razvan, You can see my domain in two images (sorry for the poor quality), one is of the complete domain and the over is focoused on the nozzle outlet after the gradient adaptation.

I will increase the size of the domain as you suggest. How much can I coarsen the grid as I move away from the nozzle outlet?

Using the Rk-e model gives me a large area of high turbulent viscosity limited to 100000 along the symmetry line starting at the shock wave. Will this be resolved by the SST k-w model?

Thanks Eilon
  Reply With Quote

Old   August 30, 2007, 01:35
Default Re: K-Epsilon for Nozzle flow saparation
Posts: n/a
Hi Eilon,

The mesh seems OK inside the nozzle. But outside, you can relax it with a 1.025(L) x 1.1(H) growth ratio.

R-ke, as all high-Re k-e models, suffers from this annoying problem, extremely high levels of TVR for certain flows. K-e models are adequate away from walls, outside the B-L, but near the wall, they tend to heavily overpredict the TKE production. Shock waves are also strong TKE sources, so these two effects superimposed generate extremely high levels of turbulence, which forces TVR to grow so much.

K-w models are excellent for wall-bounded flows, especially SST-kw, so I would expect that in its case TVR should not go over 5000.

  Reply With Quote

Old   September 4, 2007, 20:22
Default Re: K-Epsilon for Vortex Shedding
Posts: n/a

You suggested earlier to use fully structured O-H grid (which is just a rectangular domain with a circle around the cylinder)instead of just O grid that I was using.

Could you tell me how does grid type can affect the simulation? Will it affect the convergence time or the accuracy of the results?

How do we justify using the periodic BC at the top and bottom of the domain?

Thanks once again.

  Reply With Quote

Old   November 17, 2009, 11:03
New Member
Shengyi Wang
Join Date: Mar 2009
Posts: 22
Rep Power: 10
gmwsy is on a distinguished road
Dear Razvan,

Obviously you are an exceedingly excellent expert on Fluent by reading your posts! I wonder if you are still visiting this forum. I encounter a problem with sst k-w and really want you to kindly give some help. Please drop me a line if you would like to give a help:

Thanks a lot !
gmwsy is offline   Reply With Quote

Old   November 18, 2009, 04:35
New Member
Join Date: Aug 2009
Posts: 8
Rep Power: 10
Kappe is on a distinguished road
Hi Razvan.

I am simulating a pitching airfoil.

first, I have carried out steady state runs. I have a hybrid mesh .At Re = 6 * 10^6 so that i could check the CFD results with Theory of wings ,abbott values for the CL and Cd. I used Steady state, implicit slover,I have run both K-E standard and realizable. Y+ between 40-60 with standard wall function.I checked grid independency, looked for monotonic convergence of velocity magnitude at a point int the domain.Cp values are similar at 0 deg. I cannot predict similar Cl and Cd values at angle of attack like 15 deg. I have used Turbulence intensity 0.5% and TVR 5 as the inlet conditions. I am not sure if these values are correct as they are for a wind tunnel. Can you please find where i am going wrong and suggest.

Now coming to the actual application. Hydrofoil propulsion. I have to run cases at reduced frequency 0.1-1 with varying amplitude at Re = 12000. I am using sliding mesh to oscillate the foil After going through the insightful communication going on in this thread I have come to learn K-E standard and realizable are more suitable for high Re and i must use s kw or SST kw, keeping the y+ values in the check for the low Re to capture flow separation correctly. I plan to choose 20th of the time period as a time step.

Can you suggest how can I Model this problem correctly.
What Turbulence intensity and TVR values must i give as input.
Please suggest if i have missed out any steps.
I have to calculate the time averaged values of Cl and Cd do you know how to do it. this question has been put before.


Last edited by Kappe; November 18, 2009 at 04:55.
Kappe is offline   Reply With Quote

Old   August 25, 2012, 12:32
Default Reverse flow in pressure outlet.
New Member
Join Date: Aug 2012
Posts: 2
Rep Power: 0
Sridhar thiru is on a distinguished road
Hello ppl, i had a gr8 time & understand a lot going through the discussion!!
I want to mention Mr. Razvan u hav done a gr8 job,i hav learn a lot through your replies.

This is the problem:
I am studying supersonic internal flows in ducts as a part of designing isolators, i used rectangular box domain of size 80x80x960 mm with pressure inlet and pressure outlet on front n rear faces of the 3D simple square cross section duct. but the flow in duct is not easy as i thought as it involves shock wave boundary layer interactions(SWBLI) and corner flows n really a complex domain.!!

So i modeled the flow in fluent with above boundary conditions with values as follows:
Pressure inlet: 2026500 pa
Pressure Outlet:101325 pa
( pressure ratio of 20 produces flow with Mach 2.5)
Total temperature at both and outlet: 300K
Turbulence model : standard K-e model with standard wall treatment

i used a quadrant of duct with 40x40 mm cross section to save computational effort.

i made a major mistake in choosing turbulence model n steady solver which i realised after gone through the thread,

so i got this reverse flows in 20 or 30 faces in pressure outlet zone, n residuals not converging at all, which shoots high to 10e+1after converiging to 10e-2..

The height of first cell off the wall is 1e-5m based on literature i still guess its very small.. i dunno how to compute Y+??

Also the fluent document suggested to maintain operating pressure of 0 for supersonic compressible flows but when i set to 0 it simply throws error as floating point error!! so i set to default value of 101325 pa

I need to capture SWBLI as well as secondary corner flow

so help me to overcome this problem..
Sridhar thiru is offline   Reply With Quote

Old   November 22, 2012, 09:26
Smile Help with premixed combustion model!
New Member
Hesham Khalil
Join Date: Nov 2012
Posts: 9
Rep Power: 7
HeKhalil is on a distinguished road
Dear Razfan,

i have read your posts and i am impressed with your knowledge. i wonder if you can help me with this:

I am trying to simulate flame-vortex interaction in a swirl stabilized dump plane combustor, basically the effect of vortex shedding on the flame, using the premixed combustion model of fluent. I also try to deduce the frequency of the instabilities, which is equal to the acoustic longitudinal quarter wave mode of the combustor, to compare with the experiments.
The problem is that the wall temperature is not known to me, but both the mean temperature inside the combustor and the inlet velocity are known.
I have done two trials:
1- using the adiabatic premixed model, in which i don't need the wall temperature, and set the velocity inlet and pressure outlet boundary conditions at both combustor inlet and exit respectively, along with periodic boundary conditions in the span wise direction where only a quarter section of the combustor was used. I used DES with RKE model as submodel. The continuity equation doesnot converge easily, although i started from a RANS steady state solution.(pressure based with SIMPLE algorithm used).
2- using the non-adiabatic model, with the same set-up, but applying massflow inlet at the inlet, and idealgas for density, while applying no heat transfer at the walls, i note that the solution converge so easy without the need to start from steady state solution but the temperature keeps rising in the combustor and exceeds the adiabatic flame temperature and keeps going up!!

could you please advice which is the best combustion model to use? and if periodic boundary conditions are appropriate with DES or i shall solve the complete combustor? and what type of pressure i need to monitor if i want to capture the acoustics? is it the static pressure or the dynamic one?

Thanks for your help. it is greatly appreciated.
HeKhalil is offline   Reply With Quote

Old   July 10, 2015, 21:13
New Member
zeeshan latif
Join Date: May 2011
Posts: 7
Rep Power: 8
zeeshan latif is on a distinguished road
Hi Razvan
I am Zeeshan. I am doing work on fluent. I need your help. If yes, then will send you my problem and questions
Zeeshan Latf
zeeshan latif is offline   Reply With Quote

Old   September 18, 2015, 16:04
New Member
Join Date: Jul 2015
Posts: 3
Rep Power: 4
divyemalik14 is on a distinguished road
Hi Razvan,

I am new to CFD and analyzing the wind flow around 2-D square cylinder. Since you know a lot about modeling can you please guide me with the problem I am facing.

Flow Re=100 (unsteady) and I have modeled it in ADINA. Computational domain is 8D upstream, up and below the body and 18.5D behind.

But I cannot see the vortex shedding?

Divye Malik
divyemalik14 is offline   Reply With Quote

Old   March 8, 2017, 01:12
Default strouhal no
New Member
Join Date: Sep 2016
Location: India
Posts: 5
Rep Power: 3
shirlin is on a distinguished road
i am reading the comments i am able to gain good info,,i am trying to capture the vortex shedding phenomenon of a bridge deck for a Re 10^5,,firstly i used rke and i was not able to obtain any fluctuations in the lift then i used sst kw and im getting pretty good fluctuations and my strouhal value came out to be 0.04 but the expected value is 0.1,,where did i go wrong,,could anyone pls help me to get the correct strouhal value.
shirlin is offline   Reply With Quote

Old   March 29, 2017, 05:48
New Member
Join Date: Mar 2017
Posts: 5
Rep Power: 2
qianquan is on a distinguished road
Originally Posted by Razvan
Hi Sham,

1. skw or SST-kw (no "transitional flow" option activated) = y+>30

skw or SST-kw + "transitional flow" = y+ near 1 (2.5 is still OK)

Low-Re omega-based RSM is similar.

All low-Re k-epsilon models are designed for y+ near 1.

2. v2f is an excellent turbulence model, good for vortical flows also, but it needs y+=1 meshes. I also needs separate licensing, which could be a problem...

3. Practically all engineering flows are 3D, turbulence itself is a 3D phenomenon. The 2D assumptions work only for RANS models and only for a very small number of problems. Vortex shedding is NOT a 2D phenomenon, so the 2D calculations cannot predict it very accurately.

RSM is essentially a 3D turbulence model. It does not work very well in 2D, and if you remember, I recommended it to you for 3D calculations!

What you are doing is correct, starting from RANS to "get the feeling" about turbulence, and then going to LES. But only from a certain POV. There are several BIG differences between RANS and LES:

- LES meshing is extremely difficult, it requires a LOT of skill and time (this does not mean that RANS meshing is easy, but there are several restrictive conditions to obey with LES);

- LES is always 3D and unsteady, wich means very high computational resources are needed (grids are always bigger, required time steps are very small);

- instantaneous LES results are useless most of the times, so you need to perform time-averaging, which also translates into very long computational time.

Yes, it is going to be really hard. But do not give up, it's very rewarding and full of satisfaction once mastered! And remember: LES is the future!


Razvan, recently, i did circle cylinder flow simulation with les , and the re 140000, y+=1, wall BL is 50, the domain is 800*1200*130, max grid size is 4, however the Cd is 0.8, whats the matter with my setting? thank you advance.

Sent from my iPhone using CFD Online Forum mobile app
qianquan is offline   Reply With Quote


Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
SimpleFoam k and epsilon bounded nedved OpenFOAM Running, Solving & CFD 16 March 4, 2017 09:30
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
How to get reference to k and epsilon in the epsEqn and kEqn cfd_explorer OpenFOAM Programming & Development 0 March 10, 2011 11:16
How to get reference to k and epsilon in the epsEqn and kEqn cfd_explorer OpenFOAM 0 March 10, 2011 10:58
SimpleFoam k and epsilon bounded nedved OpenFOAM Running, Solving & CFD 1 November 25, 2008 21:21

All times are GMT -4. The time now is 09:55.