
[Sponsors] 
August 5, 2007, 23:43 
y+ problem

#1 
Guest
Posts: n/a

Sponsored Links
First how do you check your y+ value in post ? Do you need to create some contours or else ? I just clicked on the Default Domain and selectioned the variable y+. The max value is approximetaly 1000. How can I interpret that value? I'm using the kw SST turbulence model in a steady incompressible and isothermal flow. I created 10 inflation layer with first layer thickness 0.3 mm. 

Sponsored Links 
August 6, 2007, 09:11 
Re: y+ problem

#2 
Guest
Posts: n/a


August 6, 2007, 09:54 
Re: y+ problem

#3 
Guest
Posts: n/a

ok but how do you know what y+ value you should have ?


August 6, 2007, 10:24 
Re: y+ problem

#4 
Guest
Posts: n/a

hello
eash turbulence model amd wall function has a certain limit for the y+ cfx manual and the posts here have comprehensive information for that matter , just search here with ylus keyword regards 

August 6, 2007, 12:18 
Re: y+ problem

#5 
Guest
Posts: n/a

ok I've been reading through all the archives but I still have some questions.
I am simulating a incompressible and steady state High Reynolds number flow (10^7) with the kw SST model with Automatic Wall treatment. The max y+ value observed is 1000 (though I'm not sure if I checked the value at the good location, I just displayed the variable y+ in the default domain). I read that SST requires y+<1 in order to integrate the sub layer (no wall functions). So if my value are that high (though I don't understand because I created 10 inflation layers with first prism height 0.3mm and expansion factor 1.2 wich is practicaly the finest resolution I can get) then my nodes are not in the sublayer. Then with Automatic treatment,SST reduces to kepsilon and uses wall functions. So it means I'm not resolving the viscous sublayer but only the loglayer. Is that correct ? If I'm not resolving the viscous sublayer, and if this effect is important for my problem (I'm studying the flow that goes out of a 0.15 m side square tube through windows located on each lateral face of the tube, and what is important is the flow (mass flow rate and direction) out of these windows, wich I need to impose inlet conditions on another geometry), then my results are not that good. I would really appreciate more advices about that. Thank you all 

August 6, 2007, 18:29 
Re: y+ problem

#6 
Guest
Posts: n/a

Hi,
Not resolving sub layer with y+=1000  Correct. What y+ should you use?  Problem dependant. Do a mesh sensitivity check. I suspect you will need a finer wall resolution than that for good boundary layer resolution. Glenn Horrocks 

August 6, 2007, 20:05 
Re: y+ problem

#7 
Guest
Posts: n/a

Thanks for the answer. My question then becomes : for a Reynolds number of 10^7, can the linear sub layer have a significant effect on the flow ? And so if you're not resolving you get wrong solutions ?
More precisely, if y+=1000 then the kw SST model reduces to kepsilon and uses wall functions, does it lead to an overprediction of the turbulence ? And that would be the reason why I can't get stable values of my interest quantities after having refined the mesh 5 times (from 200000 to 10000000 elements). I'm really looking forward to an answer because I'm thinking maybe this is exactly the problem (because I already did a mesh study) Thank you 

August 7, 2007, 18:27 
Re: y+ problem

#8 
Guest
Posts: n/a

Hi,
Can sub layer have significant effect?  Yes, it is the first layer of a boundary profile. But do you need to model it (ie y+=1 approx) or can you use wall functions to model from y+>11? That is problem dependant. Most flows at Re=10^7 should be OK with the wall function approach. Wall functions do not over predict turbulence for flow over a flat plate, which is what they have been "tuned" for. They do, however have problems in separating flows, stagnation regions etc etc and that can lead to under/over prediction of turbulence and/or gross flow errors, such as not predicting a separation. Your mesh refinement study is hopefully showing a trend towards a value. If so you can use Richardson extraplotion to get a "zero sized mesh" solution. If will also give you an error estimate. What are you modelling? Glenn Horrocks 

August 7, 2007, 20:02 
Re: y+ problem

#9 
Guest
Posts: n/a

I'm modelling the flow in a control rod guide tube. Basically the flow enters at the base of a square tube wich contains very dense structures, and then exits the tube through windows that are located on each lateral face of the tube. My mesh study doesn't seem to converge to a value. What really interest me are the mass flow through the windows, because I need it in order to impose an inlet on another model. I did 4 uniforms meshes (from 200000 to 800000 elements) and the solution seemed to converge faster and faster as the elements were increased, and the mass flows through the windows seemed to converge to a value. But then I used a finer mesh (of 1 million elements) and then the solution totally changed, the convergence was slower, and the mass flows really different. With even more elements, it's still different, and in addition when I check the value of mass flows at different iterations it's still fluctuating a lot


August 7, 2007, 20:05 
Re: y+ problem

#10 
Guest
Posts: n/a

but if I'm not resolving the sublayer then my layer is only turbulent and that's why I suggested that turbulence is overpredicted, wich could explain my fluctuating values...


August 8, 2007, 07:00 
Re: y+ problem

#11 
Guest
Posts: n/a

Hi,
I assume your simulation is steady state. Did the fine mesh simulations have problems converging? It is common for a coarse mesh to successfully converge to steady state and a fine mesh to not converge as the finer mesh can resolve some transient wake shedding and other effects which the coarse mesh did not resolve. This could be a cause for a variation. Glenn Horrocks 

August 8, 2007, 08:32 
Re: y+ problem

#12 
Guest
Posts: n/a

yes that's exactly what happens. My simulation is indeed steady state and the finer meshes converge really slower and to a lower value of residual (between 1 and 2 order) than the coarse mash. But why is that exactly ? You say that with the finer meshes, more terms of the transient are resolved?


August 8, 2007, 18:40 
Re: y+ problem

#13 
Guest
Posts: n/a

Hi,
Coarser meshes have more numerical dissipation than fine meshes, so coarser meshes can damp out flow instabilities. Also if the mesh is not fine enough to physically resolve an instability it generally will occur. Hence fine meshes can go transient when a coarse mesh solution was steady state. Whether the transient is significant is significant is problem dependant  in your case it sounds like it is. If possible I would run a transient simulation of your fine case over a weekend (or maybe over a week's holiday!) and let it establish itself. Glenn Horrocks 

August 30, 2007, 15:08 
Re: y+ problem

#14 
Guest
Posts: n/a

Hi, I have the same problem as you, in finer mesh occurs instabilities nor present in coarser mash, can this avoided manipulating sw parameters?
for Gui, I think u have y+=1000 because u calculated it in the whole domain, it has to be calculated only on wall boundaries 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
UDF compiling problem  Wouter  Fluent UDF and Scheme Programming  6  June 6, 2012 04:43 
Gambit  meshing over airfoil wrapping (?) problem  JFDC  FLUENT  1  July 11, 2011 05:59 
natural convection problem for a CHT problem  SeHee  CFX  2  June 10, 2007 06:29 
Adiabatic and Rotating wall (Convection problem)  ParodDav  CFX  5  April 29, 2007 19:13 
Is this problem well posed?  Thomas P. Abraham  Main CFD Forum  5  September 8, 1999 14:52 
Sponsored Links 