CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

atmBoundaryLayerInletVelocity - Velocity Profile not continuous through domain

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 25, 2017, 09:52
Default atmBoundaryLayerInletVelocity - Velocity Profile not continuous through domain
  #1
New Member
 
Alwin
Join Date: Jun 2017
Posts: 11
Rep Power: 8
sdfij6354 is on a distinguished road
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,
Attached Images
File Type: png velocity_paraview.png (61.0 KB, 77 views)
File Type: png velocity_at_inlet.png (12.5 KB, 51 views)
File Type: png velocity_5_meters_after_inlet.png (12.5 KB, 40 views)
Attached Files
File Type: gz velocity_profile.tar.gz (35.6 KB, 19 views)
File Type: txt U bundary condition.txt (1.7 KB, 25 views)
sdfij6354 is offline   Reply With Quote

Old   July 26, 2017, 05:42
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 638
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
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
tomf is offline   Reply With Quote

Old   July 26, 2017, 12:53
Default
  #3
New Member
 
Alwin
Join Date: Jun 2017
Posts: 11
Rep Power: 8
sdfij6354 is on a distinguished road
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,
sdfij6354 is offline   Reply With Quote

Old   July 26, 2017, 16:16
Default
  #4
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 638
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
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
tomf is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 07:38
UDF error - parabolic velocity profile - 3D turbine Zaqie Fluent UDF and Scheme Programming 9 June 25, 2016 19:08
InterFoam - Validation for velocity profile in simple channel me.ouda OpenFOAM Running, Solving & CFD 0 October 19, 2015 06:42
Problem with assigned inlet velocity profile as a boundary condition Ozgur_ FLUENT 5 August 25, 2015 04:58
[swak4Foam] groovyBC error: velocity profile (2D) >> what's wrong? vitorspadeto OpenFOAM Community Contributions 4 June 19, 2014 15:31


All times are GMT -4. The time now is 22:36.