# Reynolds Number Similarity not applicable in Fluent?

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

 November 23, 2011, 06:16 Reynolds Number Similarity not applicable in Fluent? #1 Member   Join Date: Nov 2009 Posts: 36 Rep Power: 10 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?

 January 14, 2012, 08:37 #2 Member   Join Date: Nov 2009 Posts: 36 Rep Power: 10 Any thoughts?

 January 15, 2012, 15:27 #3 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 1,919 Rep Power: 26 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 Member   Join Date: Nov 2009 Posts: 36 Rep Power: 10 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 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 1,919 Rep Power: 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?

 January 20, 2012, 05:09 #6 Member   Join Date: Nov 2009 Posts: 36 Rep Power: 10 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 Senior Member   duri Join Date: May 2010 Posts: 160 Rep Power: 9 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 20, 2012, 11:12
#8
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,919
Rep Power: 26
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.

 January 22, 2012, 16:20 #9 Member   Join Date: Nov 2009 Posts: 36 Rep Power: 10 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!

 Tags fluent, fluid mechanics, reynolds number, similarity

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 24 June 27, 2016 08:54 Emmanuel FLUENT 2 April 7, 2016 01:46 bhanususarla FLUENT 2 December 17, 2009 14:30 ivanbuz FLUENT 0 November 1, 2009 17:36 Tim CFX 1 October 7, 2009 06:19

All times are GMT -4. The time now is 00:05.