CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   LES feasible on desktop for this problem? (http://www.cfd-online.com/Forums/cfx/83302-les-feasible-desktop-problem.html)

mullenc525 December 22, 2010 18:46

LES feasible on desktop for this problem?
 
1 Attachment(s)
Iím 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. Iíve 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 5-10 cm, and height (y) 0.5-2mm.

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 200-800 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,0.5-2mm,50-100mm] for the pin field or [20mm,0.5-2mm,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?

ghorrocks December 23, 2010 05:09

Quote:

I can't use a laminar model since there is gross flow separation
Incorrect. The choice of laminar or turbulent has nothing to do with flow separation. The choice is based on Reynolds number and therefore the flow is mainly laminar or mainly turbulent.

Quote:

Turbulent models don't relaminarize for example after the lateral web in the rib design
Correct, but I doubt this is important in your case.

Quote:

Turbulent models with transition are custom tailored for external flows and therefore not appropriate
Generally correct, but if the transition is important it is still your best bet.

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?

mullenc525 December 23, 2010 14:12

Thanks for your reply Glenn.

Re is 200-800 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?

ghorrocks December 23, 2010 21:30

Assuming Re=200-800 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.

mullenc525 December 24, 2010 14:33

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.

ghorrocks December 25, 2010 05:06

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.

ghorrocks December 25, 2010 05:07

Oh yes, and this forum post is very informative: http://www.cfd-online.com/Forums/flu...t-laminar.html


All times are GMT -4. The time now is 20:11.