
[Sponsors] 
December 22, 2010, 18:46 
LES feasible on desktop for this problem?

#1 
New Member
Join Date: Dec 2010
Posts: 26
Rep Power: 8 
I’m doing some heat exchanger design, and would like some advice on turbulence modeling. I run on a PC with 4gb ram and a quad 2.4 ghz processor. I’ve attached an image with example geometries  flow field elements on top and 'periodic repeated' mesh volumes on bottom.
The length of the channels (streamwise, or x) will be about 20cm, width (z) about 510 cm, and height (y) 0.52mm. In the pin field, pins are ~1mm dia on 3mm spacing. In the rib design, ribs are 1mm square with 4mm z spacing, and the lateral support webs are 0.25mm in y and 2mm in x, spaced 20mm in x. In both geometry cases, I want to understand the effects the blunt bodies in the channel have on turbulence and heat transfer. The fluid is air at ~6m/s, so Re are 200800 based on height. I'm happy to assume fully developed flow along the length of the device, so that makes the repeating units quite small [3mm,0.52mm,50100mm] for the pin field or [20mm,0.52mm,20mm] for the rib design. From my limited understanding of CFD: 1. I can't use a laminar model since there is gross flow separation 2. Turbulent models don't relaminarize for example after the lateral web in the rib design 3. Turbulent models with transition are custom tailored for external flows and therefore not appropriate However, the Re is low and domain is very small. Will LES be feasible for this, and is this the best choice for me? 

December 23, 2010, 05:09 

#2  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Quote:
Quote:
Quote:
The choice of laminar or turbulent model should be made purely on how turbulent the flow is. What is the Reynolds number? Does it have upstream turbulence sources? 

December 23, 2010, 14:12 

#3 
New Member
Join Date: Dec 2010
Posts: 26
Rep Power: 8 
Thanks for your reply Glenn.
Re is 200800 at max flow. As far as upstream turbulence sources, I have chosen to ignore the manifold leading to the plates at this point. For most of the flow, I understood the first few rows of pins or webs would be a source of terrific turbulence. How could the laminar model capture this? Would an unsteady simulation capture the vortical motion? I've used the SST transition models in a test duct of 3cm dia to 1 cm dia with laminar reynolds numbers upstream and turbulent numbers downstream, and the solution it gives has a velocity profile skewed toward the turbulent duct profile everywhere, leading me to believe it wont have the fidelity I need. Is LES feasible at this reynolds number and domain size or are there even more pitfalls there for an inexperienced user? 

December 23, 2010, 21:30 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Assuming Re=200800 is from cylinder diameter and a sensible representative flow velocity then the flow is strongly laminar. So use a laminar model.
Sounds like you are confused between separations and turbulence. They are completely different things  time to read a textbook so you know the difference. Yes, a laminar simulation is the one to use. You may require transient, maybe steady state, don't know you would have to fidn out for your case. Forget LES, SST and transition. You flow is laminar. 

December 24, 2010, 14:33 

#5 
New Member
Join Date: Dec 2010
Posts: 26
Rep Power: 8 
I have a fairly good grasp of separation, transition, and turbulence  though it wasn't until recently I was corrected that large scale flow unsteadiness such as a karman vortex sheet is not necessarily turbulent.
Glenn I understand from your forum history you are an expert in this field, but this paper did a DNS study of a similar geometry, and they found transition reynolds numbers in the low hundreds based on channel height (same basis as my Re). http://www.2shared.com/document/ImDC..._patterns.html Are you still certain a laminar model is appropriate? That paper as well as others studying similar geometries have stated wall effects were small in their DNS or LES simulations. To me this sounds like I can use a relatively coarse (grid size > yplus=1) LES simulation and still get good results. 

December 25, 2010, 05:06 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
I have not done flow over a cylinder for a while and yes, you are right  you are in the region where turbulence is going to start. My apologies for misleading you.
But having said that, the amount of turbulence is going to be small. Flows just above transition are always a challenge to model so you are unlikely to find a turbulence model which behaves well. You can do this with LES, but modelling transition with LES is still very tricky. I would do this by a purely laminar model. This will capture the laminar section correctly, and if you use an upwinding differencing scheme the small amount of numerical dissipation will provide a bit of damping for the turbulence. Note I am talking about a second order upwinding scheme here, not a first order scheme. This may sound crude but soemtimes it is as good as a RANS turbulence model or a "real" LES model. I use this technique in my PhD thesis and give a more detailed justification and analysis of it: http://hdl.handle.net/2100/248. And yes, it gave surprisingly good results. If you are talking about LES with y+>1 then you are going to have plenty of numerical dissipation and I suspect you will find the technique I describe above as good as anything. 

December 25, 2010, 05:07 

#7 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Oh yes, and this forum post is very informative: http://www.cfdonline.com/Forums/flu...tlaminar.html


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
problem about numerical scheme in LES.  libin  Main CFD Forum  4  July 1, 2004 04:32 
LES combustion problem  Salvador  Main CFD Forum  0  August 28, 2003 09:52 
Problem with interpolation  Ramu  Main CFD Forum  0  August 7, 2003 03:37 
extremely simple problem... can you solve it properly?  Mikhail  Main CFD Forum  40  September 9, 1999 09:11 
Is this problem well posed?  Thomas P. Abraham  Main CFD Forum  5  September 8, 1999 14:52 