|
[Sponsors] |
atmBoundaryLayerInletVelocity - Velocity Profile not continuous through domain |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 25, 2017, 10:52 |
atmBoundaryLayerInletVelocity - Velocity Profile not continuous through domain
|
#1 |
New Member
Alwin
Join Date: Jun 2017
Posts: 11
Rep Power: 9 |
Hello,
following case: Air is flowing through a tunnel, partly over and through a geometry (a greenhouse with ventilation openings) in the center of the tunnel. I've implemented a velocity profile at my inlet (left side) to replicate the logarithmic velocity profile of atmospheric wind over a surface using the "atmBoundaryLayerInletVelocity" boundary condition for the Velocity (U) at the inlet. Taking velocity measurements at the inlet using the singleGraph sampling function confirmed the proper functioning of my velocity profile. I've attached the image - x-axis represents the domain height (ground to sky) and y-axis the velocity. I set Uref = 5 at a reference height = 1, which seems to be work according to the measurements. However, when I move inwards my domain the velocity profile seems to "disappear", as the second set of measurements show. I've taken measurements 5 meters distance from the inlet and the velocity doesn't have the logarithmic profile anymore. What did I do wrong or what did I missed by implementing the velocity profile? I would like to achieve a continuous velocity profile before the incoming wind from the inlet "hits" the geometry. Attached the two measurements graph, a screenshot of the respective area in ParaView and also my case. Thank you for any help, |
|
July 26, 2017, 06:42 |
|
#2 |
Senior Member
|
Hi,
Your ground is probably modeled as a smooth no-slip wall. For the continuation of the profile you need to have a rough wall that is corresponding with the atmospheric boundary layer. You may also need to drive your boundary layer from the top of the domain. Best regards, Tom |
|
July 26, 2017, 13:53 |
|
#3 |
New Member
Alwin
Join Date: Jun 2017
Posts: 11
Rep Power: 9 |
Hello tomf,
thank you for your answer. The bottom/ground is defined as espilon: type epsilonWallFunction; value uniform 1e-7; k: type kqRWallFunction; value uniform 1e-20; nut: type nutkRoughWallFunction; (I also tried nutURoughWallFunction) value uniform 0.0; Ks uniform 0.05; Cs uniform 0.5; U: type fixedValue; value uniform ( 0 0 0); Is this correct? What do you mean by "drive your boundary layer from the top of the domain"? To define the top of the domain is a second inlet with a velocity profile? Thank you, |
|
July 26, 2017, 17:16 |
|
#4 |
Senior Member
|
Hi,
Ks should be 20 times z0 for your nutkRoughWallFunction. You can also use nutkAtmRoughWallFunction I believe: source code For driving the top of the domain the fixedShearStress boundary condition can be used. It sets a gradient that should correspond to the logarithmic profile, taking into account the local turbulent viscosity. It is also important to have the correct turbulence profile on the inlet. Regards, Tom |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 08:38 |
UDF error - parabolic velocity profile - 3D turbine | Zaqie | Fluent UDF and Scheme Programming | 9 | June 25, 2016 20:08 |
InterFoam - Validation for velocity profile in simple channel | me.ouda | OpenFOAM Running, Solving & CFD | 0 | October 19, 2015 07:42 |
Problem with assigned inlet velocity profile as a boundary condition | Ozgur_ | FLUENT | 5 | August 25, 2015 05:58 |
[swak4Foam] groovyBC error: velocity profile (2D) >> what's wrong? | vitorspadeto | OpenFOAM Community Contributions | 4 | June 19, 2014 16:31 |