
[Sponsors] 
September 28, 2014, 23:42 
About the Reynolds Number and Yplus in external flow

#1 
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Hi, all,
I'm starting to estimate the drag force of cylinderlike body which axis is perpendicular to flow. And recently I have a basic question about the Reynolds Number and Yplus in external flow. Could you guys please kindly help me? Thank you all really. Details as below. 1) For example, flow through a finite length cylinderlike rod(the rod perpendicular to flow), how should we calculate the Reynolds number, ie use which size as length scale: diameter(D), length of rod(L) or flowfield size(W)? I think should use the diameter(D). Length Scale.jpg 2) Use above estimated Reynolds number to calculate the Yplus and calculation result gives bigger Yplus on some wallarea where has high velocity region close to wall. And according to Yplus's definition: Yplus=ro*frictional velocity*first cell height/dynamic viscosity This definition seems tell us that for a uniform first cell height, Yplus should be bigger on those wallarea which has high velocity region nearby(because this region gives bigger frictional velocity). Is this guess right? External flow.jpg 3) If this is right. Then those Yplus values on wall will vary with velocity nearby, so if we use a lowReynolds number model(Like SST) and we need a Yplus=~1, do we just need the maximum Yplus on the wall around 1 or what? If this is true, then the method we used to calculate Yplus based on Reynolds number seems not that accurate, the maximum Yplus will be obviously bigger than what we expected. Because we use a normal velocity to calculate the Reynolds number, then Yplus, but the actual flow will give local high velocity region, on those wall close to this region Yplus will be bigger. This really confused me long time. 4) And in flow simulation(like drag force estimate) do we need to guarantee all Yplus value the same as what we need on wall? This seems extremely hard to realize. Usually we can only keep the first cell height same, does this acceptable? My English is not good and expression may be not that clear, beg your pardon and really want to receive your guide. Thanks a lot all. 

September 29, 2014, 06:34 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
1) The usual parameter is the cylinder diameter.
2) The usual approach is to aim for y+=1 (approx) at the maximum y+ point. Then use a constant first mesh spacing, so then all the other points will have y+<1. 3) See 2). 4) For flows like the Ahmed body the boundary layer does not need to be integrated to the wall so you might as well use standard wall functions. Then you can use a far coarser mesh. But the complication in bluff body flows like this is you have to handle the large scale flow unsteadiness  this is usually done with LES, DES, SAS or similar approaches. These approaches have quite different demands on wall boundaries. 

September 29, 2014, 23:01 

#3  
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Quote:
Really thank you, horrocks, Thank you for your confirmation, this make me some clear on this issue. I have finished several simulation samples with the cylinderlike bodyone of them gives a some reasonable drag force value, it's about 6% compared to wind tunnel results. this sample's condition is [D=0.3m around, length L=1.4m, Domain size is large enough with 30mX20mX20m, Velocity in let with 36m/s around, SST model with auto wall function, turbulence 1%. INFLATION: first layer thickness=5e5mm, 15 layers totally]. But you can see that the Reynolds number is about :7e5, so with Yplus =1, the first layer thickness is about 0.009mm, but this 0.009mm can not give a good results. Only 5e5mm can give a reasonable drag force value, within 6%. this make me confused because this is not comply with what we know about SST model(need yplus=1 is enough). This is also not comply with the below website about the boundary layer resolving, http://www.computationalfluiddynamic...oundarylayer/ Could you please kindly give some comments, thanks a lot for your response. 

October 5, 2014, 07:41 

#4 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
I have not read that link in detail so cannot comment on it.
But I think you will find that if you refine your boundary mesh to 5e5 (which looks like y+=0.005) you are going to have round off problems and not converge well. You may have said this, but why do you say you need the first layer at 5e5? 

October 9, 2014, 02:11 

#5  
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Quote:


October 9, 2014, 06:03 

#6  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Quote:
Quote:
* Single versus double precision * Big changes in mesh size, time scale, velocity, pressure in a simulation. Quote:


October 9, 2014, 09:48 

#7 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 512
Rep Power: 12 
Going back to your first cell estimate and your body geometry. You stated that for 36m/s inlet and a 1.4m long body or D=0.3m, your first cell hieght for y+=1 is ~0.009m. Are you running this in air?
I think you miscalculated first cell height. I think your first hieght should be about 1e7m to 1e5m (you need to choose and appropriate travel length your BL will see), which is even smaller than the 5e5m that you started seeing good values for Cl and CD. Did you plot your y+ on your body in Post? I would expect you might see values above 500. Glenn, I have used first distant hieghts in the 1e7m to 1e9m range before. This is needed in supersonic+ flow with SST model in order to capture the aerodynamic coeffs correctly and to get the heat transfer nailed down. Another important thing will be the total height of your prisms (if you used them). You need enough hieght and enough nodes in order to capture what that link you posted is telling you about. 

October 9, 2014, 18:02 

#8  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Quote:


October 10, 2014, 03:31 

#9  
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Quote:
Quote:
And I got a good value of drag force with first cell height=5e5mm,totally 15 layers[Call this simulation sample as case#1], I plot the y+(Use variable 'Yplus') on body wall in Post and the max value is about 0.0361(Should be 5e5/0.009*1=0.0056). You can see that the y+=0.0361 is too small for SST, so I think if I want y+=~1, I should use first cell height=1/0.0361*5e5mm=1.38e3mm, take it as 1.25e3mm for simplification and I finished another simulation[We call this as case#2]. This gives about half of the drag force, y+ is about 0.325(Not ~1), and flow field is different from case#1 obviously as below. Case#1.jpg Case#1 y+.jpg case#1 Case#2.jpg Case#2 y+.jpg case#2 The max velocity near to body is different(43 versus 76), and flow separation is also different. In case#1 separation is early and there is lots of eddy near the body's side, in case#2 only eddy behind the body's back. Obviously at least one case is very wrong, or both are wrong. What we know now is that case#1's results is good anyhow, and horrocks said this may have big round off error or not converge well, need to check. Because of the capacity of my computer I don't want to try LES or other advanced turb model, I think SST may be enough for my drag force estimate(10% gap compared to wind tunnel is acceptable). For SST we need y+=~1, but I can't get a proper result. With y+=0.0361 I got the good value, is this really irrational??? but I think the flow in case#1 is some reasonable.
++  Average Scale Information  ++ Domain Name : Default Domain Global Length = 1.4422E+01 Minimum Extent = 1.0000E+01 Maximum Extent = 3.0000E+01 Density = 1.1850E+00 Dynamic Viscosity = 1.8310E05 Velocity = 1.9385E+01 Advection Time = 7.4399E01 Reynolds Number = 1.8094E+07 Is this info above useful? For example the 'Reynolds number'=1.8e7, according to my calculation it's=1.2*36*0.3/(17.9e6), about 7e5. And the 'global length', what dose this mean?


October 14, 2014, 04:54 

#10 
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Hi,
Glenn and Singer, could you please give me some advice about above simulation, I have been really confused on those results for a long time. Any comments from anyone are deeply appreciated. Thank you. 

October 14, 2014, 05:19 

#11  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Quote:
Quote:
Calculation of drag on a body like this will depend greatly on the Reynolds number. At low Re the flow is laminar. After turbulence transition the flow sheds a vortex street and so you should model this with SST and try to resolve the vortex street. As the Re increases then the vortex street gets more chaotic and a DES/LES approach may be required. And as the Re increases again the vortices become small enough that a standard RANS turbulence model becomes applicable. So the turbulence model you use  and the entire modelling approach  depends on what flow regime you are in. Have you established what flow regime you are in and what level of resolution you need to model the regime correctly? 

October 14, 2014, 21:38 

#12  
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Glenn, thank you very much.
Quote:
Quote:
Re [0~a] [a~b] [b~c] [c~d] Model [laminar] [SST] [DES/LES] [standard RANS] And my Re is about: Re=ro*U*L/dynamic viscosity =1.2*36*0.3/(17.9e6)~=7e5, what model should I use??? 

October 14, 2014, 22:01 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
You will have to research this yourself to find the transition Re numbers. It also depends on what you are trying to do  if you are looking for high accuracy and you have lots of computer resources you might tend towards LES, if you are limited in resources you might tend towards RANS.
Also note SST is a RANS approach. This paper (http://ctr.stanford.edu/ResBriefs01/wang.pdf) describes some modelling of Re=10^6 flows which looks close to your application. It suggests your Re=7e5 is in the regime where they used LES as you are above the region with a coherent wake structure, but the individual turbulent eddies are still big enough to have significant effects. I would start your work using RANS (ie SST), and possibly a turbulence transition model. See how close you get to the correct result and then consider LES/DES/SAS. 

October 14, 2014, 23:13 

#14  
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Thank you Glenn.
I'm not that familiar with CFD theory, and what do you mean by 'turbulence transition model', is that a certain turbulent model??? Quote:
Do we have a common order of those items above to do a systemic sensitivity analysis? Firstly with which one and secondly with which one...? I think the order should be like: Domain size>Mesh density>turbulent model>First cell height. Really appreciated for your guide. 

October 15, 2014, 05:32 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
Turbulence transition model is and addon model to the SST model which allows it to model laminar to turbulent transition.
It is not too important which order you do the sensitivity analyses in, it is very good you are doing them  you will learn a lot. It is especially useful if you have a good benchmark experimental or simulation result to compare against, so you know when you are on target. The paper I quoted might be good for that. 

October 31, 2014, 05:35 
Residauls go to flactuate, what's may be the solution?

#16 
New Member
Mason
Join Date: Sep 2014
Posts: 22
Rep Power: 4 
Hi,
I use a 2Dlike(i.e. extrude one layer) simulation to estimate the drag of an rod in CFX. The residuals(include the turbulent residuals) continue to fluctuate like below picture. But the drag went into a steady state. WP_20141031_00_52_27_Pro.jpg WP_20141031_00_52_18_Pro.jpg What's maybe the reason for this? Mesh? Time step? I changed time step within a large region, but no big difference. Can some one give me any suggestion? Thanks, any comments and tips are highly appreciated. 

October 31, 2014, 05:36 

#17 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 

November 10, 2014, 19:29 

#18  
Member
Join Date: Mar 2013
Posts: 42
Rep Power: 5 
Quote:


November 10, 2014, 19:37 

#19 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,832
Rep Power: 100 
The temporal study needs to be able to resolve the important flow features. So the mesh needs to be fine enough that the important flow features are resolved. So the process is iterative  you do a temporal study, then you do a mesh size study. Then your initial temporal study may need updating on the new mesh, so you repeat the temporal study.... and then you consider if this has implications for your mesh.
So theoretically they are all coupled, but in reality the coupling is fairly weak. So you can usually home in on a good mesh/time step/convergence criteria fairly quickly, and once you have found that you can do the studies about that point and check it is OK. Likewise, for your question about regimes  you need to repeat the study whenever new flow phenomena occur, or they occur on significantly different length or time scales. 

Tags 
external flow, first layer thickness, reynolds number, yplus 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
decomposePar no field transfert  Jeanp  OpenFOAM PreProcessing  0  June 20, 2014 05:59 
decomposePar pointfield  flying  OpenFOAM Running, Solving & CFD  28  December 30, 2013 16:05 
Reynolds number in pressure driven flow  Many  Main CFD Forum  1  October 1, 2013 13:00 
Low Reynolds Number Flow over a Flat Plate  Go  FLUENT  4  August 28, 2013 05:19 
airFoil2D  Calculating / Printing Reynolds number of flow  akku  OpenFOAM Running, Solving & CFD  5  April 7, 2013 17:12 