Wall Function
Hi there, this is a really novice question: would one specify the friction acting against the fluid flow in the wall function specification? That is, for some given patch specified in the wall function file, would one specifiy the friction in the 'value' field?
Thank you for taking the time to read this. 
Hello Pooven,
From what I understand of the Wall function treatment of OpenFOAM (nutWallFunction) the wallShearStress is derived from: tau_wall = rho * (nu + nut) * mag(grad(U))_w with nut = nu * ((y+ * k) / ln( E * y+)  1) With tau_wall you can then determine the friction coefficient. I don't know exactly what you mean with wall function file? Could you explain that. I hope that helps a little, Hagen 
Thank you for your reply Hagen. It's much appreciated. By wall function file I was referring to the 0/nut file (for incompressible RAS). This is where the wall function is specified right? So for example for:
movingWall { type nutWallFunction; value uniform 0; } Would I specify the friction coefficient in the value field? I've been trying to get more familiar with CFD, but I'm obviouly not doing such a good job; you said that I could determine the friction coefficient from tau_wall but wouldn't I actually need to know what the friction coefficient is before running the simulation? Thank you once again for lending me some of your time :) 
Quote:
Hope this helps Best Regards V. 
Hi V, thank you for explaining that. Is there a way to determine the most optimal initial value for nut? I suppose 0 would be okay for all simulations (since the initial value is arbitrary) then?
If I may, I have another two questions: how does one know which of the wall functions to choose? nutWallFunction, nutRoughWallFunction, nutSpalartAllmarasStandardRoughWallFunction, nutSpalartAllmarasStandardWallFunction and nutSpalartAllmarasWallFunction are mentioned in the documentation but I suppose the CFD user would need to know when they are applicable... perhaps there's some resource I could read to better understand how to choose the correct function? So where would I specify the friction coefficient (or friction force)? My initial approach was to define it in the /0/U file: within the boundaryField subdictionary, for the value field of the patch, I'd specify the friction coefficient. Would this be correct? Thank you again for the assistance. 
Quote:
Quote:
Quote:
V. 
Hi, Friction Coefficient is used in DarcyWeisbach phenomenological equation. This coefficient is not used in lawofthewall models because it is completely modeled by them.
Regards. 
Hi again V :)
You've been extremely helpful, thank you! I'm trying to model air flow at the boundary level and I'm a bit unsure as to where I'd model the friction effect caused by the ground. I estimate the friction velocity from the logarithmic velocity profile and I'm wondering if it would be okay to specify this in the /0/U file? 
Quote:
Regards V. 
Thanks for taking the time to reply. It took me a while to understand, but I think it finally makes sense... the friction would depend on the fluid speed anyway so it would change as the iterations progress...
Yes you are correct V, I want to model the airflow over solid ground. For both options (thank you for that again), how would I then take into account the land cover? I mean, it would change from area to area and that would have a bearing on the friction right? Also, I only have a wind speed reading at 1 point, so I initialize U by filling the mesh with that 1 wind speed reading  would this be okay? 
Quote:
In the second case you MUST define the ground surface very carefully and then use a very fine surfacefitted grid (first node away from the wall at a nondimensional distance y+ of about 1) to solve the boundary layer properly: in this case, with a sufficiently accurate geometry and grid definition, the solver will do all the "hard work" (but, of course, at a very high computational cost) and there will be no need to use a simplified modeling approach (such as the roughWallFunction approach). Quote:
Hope this helps V. 
Thank you V, you've been a tremendous help :) Outstanding really. Things make much more sense now! Thank you all.

Hi All,
I am wondering what is the range of values for Reynolds number to be considered low or high turbulent from this formula, turbulent Re = (rho*k^2)/(epsilon*mu)? Also, why can't I use wall functions if I use RAS/KE LaunderSharma? so far I've set of all my walls (bottom, outer, top, and wall) conditions as zeroGradient but getting rather a not very good result. Your feedback will be very appreciated. Thanks and regards, Robert 
Quote:
Since for a given flow k and epsilon assume different values in space and time, this formula can return only local informations about the turbulence level of the flow itself (which means that you can have a relatively low global Reynolds number but with locally high levels of turbulence somewhere in your domain). However, about the distinction between High and LowRe turbulence models, LowRe simply means that the model can be consistently integrated in regions where the local level of turbulence (and thus the local turbulent Reynolds number) is "damped" by viscous and/or wallblocking effects (i. e. very close to a solid wall). On the other hand, HighRe models are usually derivated assuming fully developed turbulent flows (flows with high levels of local turbulence), which render them not reliable in LowRe regions of the flow. Quote:
Very low (fixed) values for k and epsilon (something like 10^10 should be appropriate)  No slip condition for the velocity field [fixedValue (0 0 0)]  zeroGradient condition for p Hope this helps V. 
Hi Vesselin,
Thanks very much for your helpful feedback. Is there a way to check yPlus values with low Re Launder Sharma model? although there is a code available in here http://www.cfdonline.com/Forums/ope...usvalues.html And since I should be more concerned with the distance normal to the wall, does that mean I should only consider the top wall yPlus average value? Also, I've got a slightly modified energy equation to the laminar one. I added the turbulent kinetic equation ((mu*(gradU + gradU.T()) && gradU)/(rho0*Cp0)) and rate of dissipation (turbulence>epsilon()/Cp0) on the RHS of the TEqn.H and I left the pEqn.H and UEqn.H as they were for the laminar case from porousSimpleFoam. Do they look right to you? Thanks once again and with regards, Robert 
nutWallFunction in OpenFOAM
Hi Hagen,
Do you have any idea about where the following nut equation for wall treatment (nutWallFunction in OpenFOAM) comes from? I mean which paper. nut = nu * ((y+ * k) / ln( E * y+)  1) Thanks, Jie 
Hi Jie,
You will find a good summary in Int.J. of Heat and Fluid flow 23 (2002) 148160. (Craft, Gerasimov, Launder, Iacovides) I think you will need the following relation in order to derive the OpenFOAM wall function: tau_w = rho (nu + nut) gradU I hope this will help a little bit. Good luck, Hagen 
Thanks Hagen, Progress in the generalization of wallfunction treatments is a helpful paper.
However, from that paper, nut near wall is calculated as nut = nu * Cmu * Ct * (yPlus  yPL) (if yPlus > yPL ) where Cmu=0.09, Ct=2.55, yPL=10.8 It is quite different from the expression nut = nu * ((yPlus * k) / ln( E * yPlus)  1) (if yPlus > yPL) where k=0.41, E=9.8 Thus, I think there must be some other paper talking about this. Thanks very much, Jie 
Hi Jie,
thanks for your response. The formulation for nut you refer to is used for the new wall function approach, which is introduced in this paper. Forget about this part. OpenFOAM does not use this generalized wall function. However, this paper provides a good overview over the conventional wall function approach in the first and second section. It has been a while since I derived this myself but I think you can the derive the OpenFOAM wall function from the expression for tau_wall in the paper. Good luck, Hagen 
Hi All,
If anyone has useful information about the new wall treatment used in OpenFOAM 1.7.x and later version for nut (i.e nutWallFunction), please post here. Thanks in advance! Jie 
All times are GMT 4. The time now is 09:07. 