Increasing instability for flow around as cylinder.

jgrimshaw · January 31, 2013, 10:31

I am currently attempting to model flow around a stationary cylinder at a Re=200,000 using Fluent 14. However, after running my simulation it appears my solution is too steady as no vortex shedding occurs.
I am currently using the URANS solver coupled with the K-e turbulance model and have tried running the simulation.
I originally used a 1st order upwind scheme and left the Pressure - Velocity coupling as SIMPLE. I then changed this to a 2nd order upwind scheme and used the PISO to do the pressure - velocity coupling.
I have found my wall y+ value and applied the appropriate wall function to my simulation but in doing so i coarsened my mesh.

Does anybody have any suggestions on how to create instability in the flow and hence produce vortex shedding?

RodriguezFatz · January 31, 2013, 10:51

How long have you been waiting? My experience is that you have to wait quite a long time until von Karman shows up...
Is your timestep small enough?

jgrimshaw · January 31, 2013, 11:18

My time step was originally 0.1s but I then changed this to 0.05s.

RodriguezFatz · January 31, 2013, 11:24

What is the radius of your cylinder and the velocity of your fluid?

FMDenaro · January 31, 2013, 11:25

what about your grid resolution? have you used second order accuracy in time?
check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

jgrimshaw · January 31, 2013, 11:45

My radius is 0.5m and my flow velocity is 2.364 m/s.

RodriguezFatz · January 31, 2013, 12:39

Quote:

Originally Posted by jgrimshaw

My radius is 0.5m and my flow velocity is 2.364 m/s.

Ok, that sounds ok for the time step. Now, could you post a picture of your mesh?

How many timesteps have you been waiting before you stopped?

jgrimshaw · February 11, 2013, 09:28

Sorry for the slow reply I have been out of the office for a while. I am currently running 600 time steps.

The mesh i am using is posted below, along the axis it has 96 elements with a bias factor of 10. The average element size was 0.328125m which gives a CFL=0.3602.

jgrimshaw · February 11, 2013, 09:32

Quote:

Originally Posted by FMDenaro

what about your grid resolution? have you used second order accuracy in time?
check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

The time step accuracy is second order, I have been assuming it is steady as on my Cl vs time plot (otherwise known as convergence history) I have an oscillating graph which quickly dampens wafter 20% of the time has been ran.

jgrimshaw · February 11, 2013, 09:33

Is there any good fluent literature or troubleshooting websites that either of you could recommend.

RodriguezFatz · February 11, 2013, 09:38

Quote:

Originally Posted by jgrimshaw

The mesh i am using is posted below

I dont find it...

jgrimshaw · February 11, 2013, 09:44

Sorry it is in the attachment of this post

RodriguezFatz · February 11, 2013, 09:49

What is your y+ currently?

jgrimshaw · February 11, 2013, 10:54

I do not have a exact value for the y+ around the cylinder, but the values range between 50 - 850. I have attached the plot below.

RodriguezFatz · February 11, 2013, 10:59

That means you are using wall functions. Maybe these wall functions restrain eddy shedding? Did you try to resolve the sheath (y+<=1)?

BTW: I don't think you need a turbulent inlet flow to get a von Kármán street. As I understand it, it is an instability that has in the first instance nothing to do with turbulence.

RodriguezFatz · February 11, 2013, 11:48

Are you using air? I quickly rebuild your case and I am getting a nice vortex street right from the start... Maybe you should post your settings...

Martin Hegedus · February 11, 2013, 16:33

You can try giving it just a little kick of angle of attack so the problem is not completely symmetric.

That being said, the instability should develop on it's own even if things were "symmetric" but it will take a while. The time to instability is dependent on how accurate the numerical method is. If it was "perfectly" accurate, the problem will theoretically remain symmetric. In other words, it is statically stable but dynamically unstable. However, I'm not sure what your turbulence model will do. It may dampen out the dynamic instability. This is a reason DES is used.

Martin Hegedus · February 11, 2013, 16:40

Oh, one thing to watch is lift. If it starts to oscillate from machine zero you're on your way. But, it sounds like this was zero for you? And, just to be clear, you do have two big vortices (symmetric about x axis) behind your cylinder?

arjun · February 11, 2013, 16:54

i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

RodriguezFatz · February 12, 2013, 03:08

Quote:

Originally Posted by arjun

i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

But do you think his domain looks like it is too small compared to the radius?

January 31, 2013, 10:31	Increasing instability for flow around as cylinder.	#1
jgrimshaw New Member James Grimshaw Join Date: Jan 2013 Posts: 8 Rep Power: 13	I am currently attempting to model flow around a stationary cylinder at a Re=200,000 using Fluent 14. However, after running my simulation it appears my solution is too steady as no vortex shedding occurs. I am currently using the URANS solver coupled with the K-e turbulance model and have tried running the simulation. I originally used a 1st order upwind scheme and left the Pressure - Velocity coupling as SIMPLE. I then changed this to a 2nd order upwind scheme and used the PISO to do the pressure - velocity coupling. I have found my wall y+ value and applied the appropriate wall function to my simulation but in doing so i coarsened my mesh. Does anybody have any suggestions on how to create instability in the flow and hence produce vortex shedding?

January 31, 2013, 10:51		#2
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	How long have you been waiting? My experience is that you have to wait quite a long time until von Karman shows up... Is your timestep small enough? __________________ The skeleton ran out of shampoo in the shower.

January 31, 2013, 11:24		#4
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	What is the radius of your cylinder and the velocity of your fluid? __________________ The skeleton ran out of shampoo in the shower.

February 11, 2013, 09:49		#13
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	What is your y+ currently? __________________ The skeleton ran out of shampoo in the shower.

February 11, 2013, 10:59		#15
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	That means you are using wall functions. Maybe these wall functions restrain eddy shedding? Did you try to resolve the sheath (y+<=1)? BTW: I don't think you need a turbulent inlet flow to get a von Kármán street. As I understand it, it is an instability that has in the first instance nothing to do with turbulence. __________________ The skeleton ran out of shampoo in the shower.

January 31, 2013, 11:18		#3
jgrimshaw New Member James Grimshaw Join Date: Jan 2013 Posts: 8 Rep Power: 13	My time step was originally 0.1s but I then changed this to 0.05s.

January 31, 2013, 11:25		#5
FMDenaro Senior Member Filippo Maria Denaro Join Date: Jul 2010 Posts: 6,849 Rep Power: 73	what about your grid resolution? have you used second order accuracy in time? check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

January 31, 2013, 11:45		#6
jgrimshaw New Member James Grimshaw Join Date: Jan 2013 Posts: 8 Rep Power: 13	My radius is 0.5m and my flow velocity is 2.364 m/s.

February 11, 2013, 09:28		#8
jgrimshaw New Member James Grimshaw Join Date: Jan 2013 Posts: 8 Rep Power: 13	Sorry for the slow reply I have been out of the office for a while. I am currently running 600 time steps. The mesh i am using is posted below, along the axis it has 96 elements with a bias factor of 10. The average element size was 0.328125m which gives a CFL=0.3602.

February 11, 2013, 09:33		#10
jgrimshaw New Member James Grimshaw Join Date: Jan 2013 Posts: 8 Rep Power: 13	Is there any good fluent literature or troubleshooting websites that either of you could recommend.

February 11, 2013, 11:48		#16
RodriguezFatz Senior Member Philipp Join Date: Jun 2011 Location: Germany Posts: 1,297 Rep Power: 27	Are you using air? I quickly rebuild your case and I am getting a nice vortex street right from the start... Maybe you should post your settings... __________________ The skeleton ran out of shampoo in the shower.

February 11, 2013, 16:33		#17
Martin Hegedus Senior Member Martin Hegedus Join Date: Feb 2011 Posts: 500 Rep Power: 19	You can try giving it just a little kick of angle of attack so the problem is not completely symmetric. That being said, the instability should develop on it's own even if things were "symmetric" but it will take a while. The time to instability is dependent on how accurate the numerical method is. If it was "perfectly" accurate, the problem will theoretically remain symmetric. In other words, it is statically stable but dynamically unstable. However, I'm not sure what your turbulence model will do. It may dampen out the dynamic instability. This is a reason DES is used.

February 11, 2013, 16:40		#18
Martin Hegedus Senior Member Martin Hegedus Join Date: Feb 2011 Posts: 500 Rep Power: 19	Oh, one thing to watch is lift. If it starts to oscillate from machine zero you're on your way. But, it sounds like this was zero for you? And, just to be clear, you do have two big vortices (symmetric about x axis) behind your cylinder?

February 11, 2013, 16:54		#19
arjun Senior Member Arjun Join Date: Mar 2009 Location: Nurenberg, Germany Posts: 1,285 Rep Power: 34	i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
flow over a cylinder urgent!	kevin	FLUENT	8	August 11, 2015 14:00
benchmark: flow over a circular cylinder	goodegg	Main CFD Forum	12	January 22, 2013 12:47
Incorrect Drag and Drag Coefficient for flow over a cylinder	ozzythewise	Main CFD Forum	8	June 13, 2012 07:24
[blockMesh] Specifying boundary faces failes in blockMesh	blaise	OpenFOAM Meshing & Mesh Conversion	0	May 10, 2010 04:56
rotating cylinder using sliding mesh	Tim Daly	FLUENT	1	November 10, 2008 00:02