CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

How to fixed water height in outlet

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

Like Tree1Likes
  • 1 Post By So_LL

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 2, 2019, 18:51
Default How to fixed water height in outlet
  #1
New Member
 
Marcos
Join Date: Mar 2019
Posts: 3
Rep Power: 5
MDietrich is on a distinguished road
Hi everyone.
I am modeling an natural river with a bridge. A am using interfoam for solver. I want to know how to fixed the water height in outlet to force the model to have that height at outlet. I want to know which Boundary Conditions must use. Tranks for you help.
MDietrich is offline   Reply With Quote

Old   December 17, 2020, 14:37
Default
  #2
Member
 
Grivalszki Péter
Join Date: Mar 2019
Location: Budapest, Hungary
Posts: 39
Rep Power: 5
GrivalszkiP is on a distinguished road
Hi!

I have the same problem, did you get any solution?

Thanks,

Péter
GrivalszkiP is offline   Reply With Quote

Old   January 25, 2021, 10:43
Default
  #3
New Member
 
Marc
Join Date: Oct 2017
Posts: 10
Rep Power: 7
mcgoldba is on a distinguished road
Same here. Any solution?

Thanks,
Marc
mcgoldba is offline   Reply With Quote

Old   January 25, 2021, 13:13
Default
  #4
New Member
 
Federico
Join Date: Jan 2021
Posts: 13
Rep Power: 3
Federico_ is on a distinguished road
I posted something in similar below in which I use variableHeightFlowRate but I'd like to understand more about it. It should fix same values of alpha of the inlet with the mass conservation
Federico_ is offline   Reply With Quote

Old   January 25, 2021, 15:22
Default
  #5
New Member
 
Marc
Join Date: Oct 2017
Posts: 10
Rep Power: 7
mcgoldba is on a distinguished road
Hi Federico,

Thank you for the reply. I have tried something similar with the variableHeightFlowRate, however it didn't seem to work for me. I am attempting to simulate a water channel with something similar to an infinite reservoir at the outlet (with a fixed water level). However, the water level drops as the simulation progresses with the variableHeightFlowRate specification. I am now trying with a codedFixedValue boundary as follows. However, I am questioning whether or not it is a numerical issue since my mesh is somewhat coarse.

Code:
 
fixedWaterLevel                                              
 {                                                            
     code                                                     
     #{                                                       
         const vectorField Cf = patch().Cf();                 
         scalarField& field = *this;                          
                                                              
         forAll(Cf, facei)                                    
         {                                                    
             field[facei]=(Cf[facei].y() <= -1.68584 ? 1 : 0);
         }                                                    
     #};                                                      
 }
Here -1.68584 is the constant water level I want to specify, and gravity is acting in the "y" direction.
mcgoldba is offline   Reply With Quote

Old   March 4, 2022, 07:50
Default
  #6
New Member
 
Sophie
Join Date: Jan 2021
Posts: 11
Rep Power: 3
So_LL is on a distinguished road
Hi

Did you find a solution to this need?

I've seen elsewhere to fix the velocity of the outlet to V=Qinlet/Achannel for the depth you require, but this leads to a significant impact from the downstream BC on the modeled velocity. And if running LES, the need to extent the mesh further downstream is quickly overwhelming computationally.

Did you find a more elegant solution?
Mahmoud Abbaszadeh likes this.
So_LL is offline   Reply With Quote

Old   July 26, 2022, 05:44
Default
  #7
Member
 
Mahmoud
Join Date: Nov 2020
Location: United Kingdom
Posts: 37
Rep Power: 4
Mahmoud Abbaszadeh is on a distinguished road
Quote:
Originally Posted by So_LL View Post
Hi

Did you find a solution to this need?

I've seen elsewhere to fix the velocity of the outlet to V=Qinlet/Achannel for the depth you require, but this leads to a significant impact from the downstream BC on the modeled velocity. And if running LES, the need to extent the mesh further downstream is quickly overwhelming computationally.

Did you find a more elegant solution?

Hi. Have you found any solution?
Mahmoud Abbaszadeh is offline   Reply With Quote

Old   July 28, 2022, 03:32
Default
  #8
New Member
 
Tobias
Join Date: Jul 2022
Posts: 7
Rep Power: 2
dalasrevo is on a distinguished road
I am working on a similar problem:
I have a section consisting of a basin open to the atmosphere at the top, fed by a lateral inlet. Then follows a piping (closed at the top, so a section under pressure, because the water level before and after the piping is higher), followed by a basin open to the atmosphere at the top.
The model is fed by a constant volume flow Q at the inlet. In reality, there is a flap at the outlet which keeps the water level in the lower basin constant at the desired level.
At the inlet I work so far with
inlet
{
type variableHeightFlowRateInletVelocity;
volumetricFlowRate 0.5;
flowRate 0.5;
alpha alpha.water;
value uniform (0 0 0);
}

But how do I keep the water level in the lower pool constant?
I have my patches open to the atmosphere with

top1
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

defined.

Someone gave me the tip to "lower the model area by x cm", with x as the desired water level, but I can't figure out how to do that.
dalasrevo is offline   Reply With Quote

Old   September 13, 2022, 03:55
Default
  #9
New Member
 
Kate Bradbrook
Join Date: Nov 2015
Posts: 8
Rep Power: 9
KateBradbrook is on a distinguished road
Hello, you can try the following:
make sure the file hRef exists in constant director with a line "value ***;"
Where *** is your desired outlet water level.

Then try the following outlet boundary conditions:
p_rgh
outlet
{
type totalPressure; //fixedValue also possible for static pressure
rho rho;
p0 uniform 0;
value uniform 0;
}

U
outlet
{
type inletOutlet;
inletValue uniform (0 0 0);
value $internalField;
}

alpha.water
outlet
{
type zeroGradient;
}
KateBradbrook is offline   Reply With Quote

Old   September 21, 2022, 05:13
Default
  #10
New Member
 
Tobias
Join Date: Jul 2022
Posts: 7
Rep Power: 2
dalasrevo is on a distinguished road
I solved my problem with a different approach, namely by calculating the expected flux for my water phase at the outlet (using the area to determine the expected velocity) and then using the following boundary condition in U:

Code:
    

outlet
    {
        type       outletPhaseMeanVelocity;
        Umean  XXX;
        alpha     alpha.water;
        value     uniform (0.312 0 0);
    }
dalasrevo is offline   Reply With Quote

Reply

Tags
boundary conditions, interfoam

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
Fixed water level BC alexvhn OpenFOAM Running, Solving & CFD 0 July 2, 2017 18:58
help: choosing density for water height flow_CH FLUENT 0 August 2, 2013 03:18
adjointShapeOptimizationFoam fixed outlet sailor79 OpenFOAM Running, Solving & CFD 14 December 6, 2011 09:55
Water vapour condensation in CFX-5.7.1 hdj CFX 1 November 27, 2005 08:15
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 10:11


All times are GMT -4. The time now is 18:31.