Turbulence model for flow over a cylinder at Re=10000

ojha.mayank485 · June 19, 2011, 01:10

Hello,

Am trying to find the Lift coeff, Drag coeff and the Strouhal number for a cylinder in a cross flow at Re=10,000

Things I tried:
1. Created a mesh and ran cases for tstep=0.001, 0.0001 & 0.00001 using KW and SST turbulence model. The y+ for the mesh was around 3.5-4. So now I created another mesh.

2. For the new mesh, the y+ value over the cylinder surface was found to be 0.62. I ran with SST and KW at tstep=0.001 which is 2% of vortex shedding time. The time step is low enough to capture the vortex shedding.

Results:
1. My St number is 0.22 while the expected value from DNS and experimentsis 0.2~0.21
2. My Cd (average) was found to be 1.3 and expected value is 1.1
3. Lift coeff was found to be ~1 while expected value is 0.5 (which is where the real problem is). The value is almost double.

I would like to know if there is anything else I should be doing and where am I actually missing.

Thank you very much.

Ojha

ghorrocks · June 19, 2011, 07:51

Are you sure the lift coefficient is based on the correct reference area? Mixing up radius and diameter explains a factor of two.

Now that you have got a model which is pretty close (in everything except lift), if you wish to get more accurate you should do a proper convergence study to guide you into what options you have left. Consider Richardson extrapolation, grid convergence indexes and similar techniques to really squeeze the last drip of accuracy out of it. "Computational Fluid Dynamics" by Roache is the seminal textbook in this area, but a summary of some key concepts is here: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F - and the reference to JFE is highly recommended reading.

ojha.mayank485 · June 19, 2011, 13:01

Thanks Glen. Appreciate your feedback.

I had another question. I am using 5% turbulence ( i.e medium intensity) at the inlet. Should this be causing the problem ???

I realize that this problem is slightly tricky because prior to separation, the flow is laminar while after separation its completely turbulent.

How about the BSL model and the non-linear RNG k-e model ? Literature say that they have been proved to be a good estimate for near wall flows and flows with rotation (which is exactly my case). But literature also say that SST should be the best (which it does not, so far).

Right now am running an LES for this case. Lets see how it goes.

BTW what is Richardson extrapolation and grid convergence indexes ??? Looks like the library is out of Roache's txt book.

ghorrocks · June 19, 2011, 19:35

Quote:

I am using 5% turbulence ( i.e medium intensity) at the inlet. Should this be causing the problem ???

If that is not representative of the turbulence levels of the experiment you are comparing to then definitely, yes.

Quote:

I realize that this problem is slightly tricky because prior to separation, the flow is laminar while after separation its completely turbulent.

In that case you might want to consider the turbulence transition model. That is the only turbulence model which can account for transition effects.

Quote:

Right now am running an LES for this case. Lets see how it goes.

Have you checked the dissipation is correct? Made sure you are getting the correct turbulence spectrum? Defined the inlet correctly for LES? Unless you have properly set this model up for LES you are kidding yourself. You cannot just turn on the LES option and rerun it and expect to get a reasonable answer.

Quote:

BTW what is Richardson extrapolation and grid convergence indexes ???

Looks like you need to find the textbook I referenced then! Also read the FAQ link I quoted and look them up on google. There are other ways besides the library these days.

ojha.mayank485 · June 20, 2011, 14:01

Quote:

Originally Posted by ghorrocks

Have you checked the dissipation is correct? Made sure you are getting the correct turbulence spectrum?

I have never run an LES. Can I have some more details/references as to how to check for dissipation and turbulent spectrum ?

Thanks Glen.

ghorrocks · June 20, 2011, 19:47

LES is a whole field of CFD in itself, your library should have textbooks on the topic. Otherwise start with general CFD books (eg Anderson) as they often introduce the concepts of LES.

paulo · June 21, 2011, 14:17

AFAIK a Reynolds number of 10000 is not fully turbulent for external flows. Pure RANS models are not proper. Maybe LES or a transition model can give better results.

My two cents.

Best regards,

Paulo Rocha

wind.cfd · February 3, 2012, 21:49

Hi,
I am modelling the turbulent flow over the cylinder by fluent(k-epsilon model)
I have a basic question about defining the boundary conditions for the domain. The domain is rectangular. for specifying velocity inlet for domain, I have to define the turbulent intensity as well as hydraulic diameter, I want to know I should use the diameter of the cylinder as the Hydraulic diameter or the cross length of the inlet face?!
Thank you

Far · February 4, 2012, 06:33

You should use transition model for this Reynolds number.

hee · February 4, 2013, 04:44

Hi everyone,

I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation

The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps.

Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised?

Thanks!

Regards,
Hee

ghorrocks · February 4, 2013, 05:10

Your question is about Fluent, not CFX and this is the CFX forum. But the answer is the same: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

emreg · May 18, 2015, 21:11

Quote:

Originally Posted by hee

Hi everyone,

I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation

The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps.

Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised?

Thanks!

Regards,
Hee

is there a solution on this issue please?

ghorrocks · May 18, 2015, 22:03

My post #11 is a pretty clear response to this.

JuPa · May 19, 2015, 03:09

Is zonal RANS a thing? I.e. define two subdomains? A laminar one and a turbulent RANS one?

Jennifer Von · December 26, 2017, 09:28

Quote:

Originally Posted by hee

Hi everyone,

I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation

The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps.

Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised?

Thanks!

Regards,
Hee

I met the same problem as you met. Is there a solution?

ghorrocks · December 26, 2017, 17:29

Have you read the posts which follow it?

Jinlai · June 24, 2018, 10:44

how did you set the Re number as 10000 ?
can you show me the detail ?

karachun · June 24, 2018, 11:37

Re=u*D/ν, u - speed, D - characteristic length, ν - kinematic viscosity. Vary these three values to get Re=10000.

ghorrocks · June 24, 2018, 20:01

CFX is a dimensional solver, it does not use non dimensional numbers like Reynolds number directly. To do a simulation at a specific Reynolds Number you have to select a length, velocity and fluid properties which give the Reynolds Number you want.

February 4, 2013, 04:44		#10
hee New Member Join Date: Jan 2013 Posts: 3 Rep Power: 13	Hi everyone, I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps. Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised? Thanks! Regards, Hee emreg likes this.

June 24, 2018, 20:01		#19
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	CFX is a dimensional solver, it does not use non dimensional numbers like Reynolds number directly. To do a simulation at a specific Reynolds Number you have to select a length, velocity and fluid properties which give the Reynolds Number you want. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Modified k-e turbulence model UDF	Travis	Fluent UDF and Scheme Programming	7	November 11, 2018 21:21
question about turbulence model selection and sensitivity	karananand	Main CFD Forum	1	February 26, 2010 05:41
Centrifugal Pump and Turbulence Model	Michiel	CFX	12	January 25, 2010 04:20
SSG Reynolds Turbulence Model	Georges	CFX	1	February 28, 2007 17:15
Turbulence model	Herry	Phoenics	1	May 29, 2003 14:19

June 19, 2011, 01:10	Turbulence model for flow over a cylinder at Re=10000	#1
ojha.mayank485 New Member Mayank Ojha Join Date: May 2011 Posts: 22 Rep Power: 15	Hello, Am trying to find the Lift coeff, Drag coeff and the Strouhal number for a cylinder in a cross flow at Re=10,000 Things I tried: 1. Created a mesh and ran cases for tstep=0.001, 0.0001 & 0.00001 using KW and SST turbulence model. The y+ for the mesh was around 3.5-4. So now I created another mesh. 2. For the new mesh, the y+ value over the cylinder surface was found to be 0.62. I ran with SST and KW at tstep=0.001 which is 2% of vortex shedding time. The time step is low enough to capture the vortex shedding. Results: 1. My St number is 0.22 while the expected value from DNS and experimentsis 0.2~0.21 2. My Cd (average) was found to be 1.3 and expected value is 1.1 3. Lift coeff was found to be ~1 while expected value is 0.5 (which is where the real problem is). The value is almost double. I would like to know if there is anything else I should be doing and where am I actually missing. Thank you very much. Ojha

June 19, 2011, 07:51		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	Are you sure the lift coefficient is based on the correct reference area? Mixing up radius and diameter explains a factor of two. Now that you have got a model which is pretty close (in everything except lift), if you wish to get more accurate you should do a proper convergence study to guide you into what options you have left. Consider Richardson extrapolation, grid convergence indexes and similar techniques to really squeeze the last drip of accuracy out of it. "Computational Fluid Dynamics" by Roache is the seminal textbook in this area, but a summary of some key concepts is here: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F - and the reference to JFE is highly recommended reading.

June 19, 2011, 13:01		#3
ojha.mayank485 New Member Mayank Ojha Join Date: May 2011 Posts: 22 Rep Power: 15	Thanks Glen. Appreciate your feedback. I had another question. I am using 5% turbulence ( i.e medium intensity) at the inlet. Should this be causing the problem ??? I realize that this problem is slightly tricky because prior to separation, the flow is laminar while after separation its completely turbulent. How about the BSL model and the non-linear RNG k-e model ? Literature say that they have been proved to be a good estimate for near wall flows and flows with rotation (which is exactly my case). But literature also say that SST should be the best (which it does not, so far). Right now am running an LES for this case. Lets see how it goes. BTW what is Richardson extrapolation and grid convergence indexes ??? Looks like the library is out of Roache's txt book.

June 20, 2011, 19:47		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	LES is a whole field of CFD in itself, your library should have textbooks on the topic. Otherwise start with general CFD books (eg Anderson) as they often introduce the concepts of LES.

June 21, 2011, 14:17		#7
paulo Member Paulo Alexandre Costa Rocha Join Date: Mar 2009 Posts: 71 Rep Power: 17	AFAIK a Reynolds number of 10000 is not fully turbulent for external flows. Pure RANS models are not proper. Maybe LES or a transition model can give better results. My two cents. Best regards, Paulo Rocha

February 3, 2012, 21:49		#8
wind.cfd New Member cfd Join Date: Oct 2011 Posts: 17 Rep Power: 15	Hi, I am modelling the turbulent flow over the cylinder by fluent(k-epsilon model) I have a basic question about defining the boundary conditions for the domain. The domain is rectangular. for specifying velocity inlet for domain, I have to define the turbulent intensity as well as hydraulic diameter, I want to know I should use the diameter of the cylinder as the Hydraulic diameter or the cross length of the inlet face?! Thank you

February 4, 2012, 06:33		#9
Far Senior Member Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,558 Blog Entries: 6 Rep Power: 54	You should use transition model for this Reynolds number.

February 4, 2013, 05:10		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	Your question is about Fluent, not CFX and this is the CFX forum. But the answer is the same: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

May 18, 2015, 22:03		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	My post #11 is a pretty clear response to this.

May 19, 2015, 03:09		#14
JuPa Senior Member Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 15	Is zonal RANS a thing? I.e. define two subdomains? A laminar one and a turbulent RANS one?

December 26, 2017, 17:29		#16
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,867 Rep Power: 144	Have you read the posts which follow it?

June 24, 2018, 10:44		#17
Jinlai New Member Jinlai Zhang Join Date: Jun 2018 Posts: 11 Rep Power: 8	how did you set the Re number as 10000 ? can you show me the detail ?

June 24, 2018, 11:37		#18
karachun Senior Member Join Date: Nov 2015 Posts: 246 Rep Power: 12	Re=u*D/ν, u - speed, D - characteristic length, ν - kinematic viscosity. Vary these three values to get Re=10000.