Reynolds Number Similarity not applicable in Fluent?

aerospaceman · November 23, 2011, 06:16

Sorry for the dramatic title...

I'm running the same mesh, with the same time step, with the same boundary conditions, with these inlet values:

First I achieved by Re=150 by setting U=L=Miu=1 and rho=150. (As per a tutorial I found online..)

Second, I kept the real properties of air, and calculated the corresponding velocity.

For the first case, I got my vortex shedding and transient behaviour, with correct results for Cd and St when compared to the literature.

For the second case I got a steady flow...!

Does anyone know what is going on? Surely the Reynolds number similarity should be valid for these two cases.

Any thoughts?

aerospaceman · January 14, 2012, 08:37

Any thoughts?

LuckyTran · January 15, 2012, 15:27

I would love to help, but I have no idea what you are doing. Can you perhaps describe it more clearly?

aerospaceman · January 18, 2012, 08:38

Hi there,

Sorry for the lack of information.

What I was trying to do was to simulate the flow over a square cylinder in a channel. I was using reference "Numerical and modeling influences on large eddy simulations for the flow past a circular cylinder", Breuer 1998.

Simulation Details
So ran the same mesh, with the same time step, with the same boundary conditions, with these inlet values:

First I achieved by Re=150 by setting U=L=Miu=1 and rho=150. (As per a tutorial I found online..)

Second, I kept the real properties of air, and calculated the corresponding velocity.

Results:
For the first case, I got my vortex shedding and transient behaviour, with correct results for Cd and St when compared to the literature.

For the second case I got a steady flow...!

My question is that my Reynolds number is identical, yet I get very different results. This does not sound physical to me, which is why I'm trying to find an explanation for this.

Many thanks for your help in advance.

LuckyTran · January 18, 2012, 10:26

You are running LES? If so, did your solution relaminarize? The laminar solutions would produce very steady-like behaviour.

How did you setup the initial conditions?

aerospaceman · January 20, 2012, 05:09

Sorry for the lack of information again.

I was running Re=150, so definitively in the laminar flow regime.

My only guess is that there maybe some mysterious Buckingham Pi group other than Reynolds number that is being ignored here.

Or it could be a bug in the code (Ansys Fluent ), but doubt it...

The initial conditions were as normal as possible, with my inlet velocity as the initial velocity prescribed in the domain. No turbulence (Laminar flow).

Look forward to your comments!

duri · January 20, 2012, 09:00

Change in velocity would have changed frequency of vortex shedding. I guess you need to estimate frequency based on strouhal number and fix the time step.

LuckyTran · January 20, 2012, 11:12

Quote:

Originally Posted by aerospaceman

Sorry for the lack of information again.

I was running Re=150, so definitively in the laminar flow regime.

My only guess is that there maybe some mysterious Buckingham Pi group other than Reynolds number that is being ignored here.

Or it could be a bug in the code (Ansys Fluent ), but doubt it...

The initial conditions were as normal as possible, with my inlet velocity as the initial velocity prescribed in the domain. No turbulence (Laminar flow).

Look forward to your comments!

What is U (inlet velocity?), L(diameter?), Miu (dynamic visocosity) and rho(density).

As duri stated, the other grouping is Strouhal number. Since you already know the shedding frequency from your first simulation, you should be able to calculate the new shedding frequency (by keeping Strouhal number constant).

From the change in properties, it is highly unlikely that you can run the simulation again with the same time step. Your viscosity is 5-6 orders of magnitude off and density is off by factor of 150. Velocity is therefore different by 4 orders of magnitude. For the same grid, that means you would need to reduce your time-step by at least 4 orders of magnitude to capture the same flow physics in your simulation.

aerospaceman · January 22, 2012, 16:20

This is very interesting stuff!

Yeah, I think that the Strouhal number is definitively something that needs to be taken into account! Makes perfect sense now.

I'll try to run this again and see what happens.

Many thanks to "LuckyTran" and "duri" for your helpful inputs.

I foolishly thought that just maintaining the Reynolds number would be enough: clearly not.

Many thanks!

November 23, 2011, 06:16	Reynolds Number Similarity not applicable in Fluent?	#1
aerospaceman Member Join Date: Nov 2009 Posts: 43 Rep Power: 17	Sorry for the dramatic title... I'm running the same mesh, with the same time step, with the same boundary conditions, with these inlet values: First I achieved by Re=150 by setting U=L=Miu=1 and rho=150. (As per a tutorial I found online..) Second, I kept the real properties of air, and calculated the corresponding velocity. For the first case, I got my vortex shedding and transient behaviour, with correct results for Cd and St when compared to the literature. For the second case I got a steady flow...! Does anyone know what is going on? Surely the Reynolds number similarity should be valid for these two cases. Any thoughts?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] SnappyHexMesh for internal Flow	vishwa	OpenFOAM Meshing & Mesh Conversion	24	June 27, 2016 09:54
Obtaining Reynolds Number in FLUENT	Emmanuel	FLUENT	2	April 7, 2016 02:46
how to plot reynolds number vs strouhal number	bhanususarla	FLUENT	2	December 17, 2009 14:30
What is "Resolved Reynolds Stress" for LES model in Fluent?	ivanbuz	FLUENT	0	November 1, 2009 17:36
Reynolds Stress model in CFX vs Fluent	Tim	CFX	1	October 7, 2009 07:19

January 14, 2012, 08:37		#2
aerospaceman Member Join Date: Nov 2009 Posts: 43 Rep Power: 17	Any thoughts?

January 15, 2012, 15:27		#3
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	I would love to help, but I have no idea what you are doing. Can you perhaps describe it more clearly?

January 18, 2012, 08:38		#4
aerospaceman Member Join Date: Nov 2009 Posts: 43 Rep Power: 17	Hi there, Sorry for the lack of information. What I was trying to do was to simulate the flow over a square cylinder in a channel. I was using reference "Numerical and modeling influences on large eddy simulations for the flow past a circular cylinder", Breuer 1998. Simulation Details So ran the same mesh, with the same time step, with the same boundary conditions, with these inlet values: First I achieved by Re=150 by setting U=L=Miu=1 and rho=150. (As per a tutorial I found online..) Second, I kept the real properties of air, and calculated the corresponding velocity. Results: For the first case, I got my vortex shedding and transient behaviour, with correct results for Cd and St when compared to the literature. For the second case I got a steady flow...! My question is that my Reynolds number is identical, yet I get very different results. This does not sound physical to me, which is why I'm trying to find an explanation for this. Many thanks for your help in advance.

January 18, 2012, 10:26		#5
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,761 Rep Power: 66	You are running LES? If so, did your solution relaminarize? The laminar solutions would produce very steady-like behaviour. How did you setup the initial conditions?

January 20, 2012, 05:09		#6
aerospaceman Member Join Date: Nov 2009 Posts: 43 Rep Power: 17	Sorry for the lack of information again. I was running Re=150, so definitively in the laminar flow regime. My only guess is that there maybe some mysterious Buckingham Pi group other than Reynolds number that is being ignored here. Or it could be a bug in the code (Ansys Fluent ), but doubt it... The initial conditions were as normal as possible, with my inlet velocity as the initial velocity prescribed in the domain. No turbulence (Laminar flow). Look forward to your comments!

January 20, 2012, 09:00		#7
duri Senior Member duri Join Date: May 2010 Posts: 245 Rep Power: 17	Change in velocity would have changed frequency of vortex shedding. I guess you need to estimate frequency based on strouhal number and fix the time step.

January 22, 2012, 16:20		#9
aerospaceman Member Join Date: Nov 2009 Posts: 43 Rep Power: 17	This is very interesting stuff! Yeah, I think that the Strouhal number is definitively something that needs to be taken into account! Makes perfect sense now. I'll try to run this again and see what happens. Many thanks to "LuckyTran" and "duri" for your helpful inputs. I foolishly thought that just maintaining the Reynolds number would be enough: clearly not. Many thanks!