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

interFoam: Setting boundary conditions for a river

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 3, 2021, 08:58
Default interFoam: Setting boundary conditions for a river
  #1
New Member
 
Deutschland
Join Date: Dec 2020
Posts: 1
Rep Power: 0
aelmoe is on a distinguished road
Hey all,

First of all: i have been looking for a solution quite a while in this forum and couldn't find a suitable answer.

I am currently setting up a case, where i want do depict the velocitys in a river where a discharge channel of an hydropowerplant rejoins the main river channel.


Presteps were blockMesh, surfaceFeatureExtract, snappyHexMesh and setFields.


I only have Input / Inlet data in m/s hence i think i have to use the flowRateInletVelocity boundary for both my Inlets (1: main channel; 2: discharge channel) in 0/U.



As i view my resuluts after the solving, it seems like everything "flow" or "velocity" is going over the atmosphere patch.

so far i have tried to just set a volumetricFlowRate and switch the additonal properties extrapolateProfile as well as the value for the volumetricFlowRate on and off.

Do you have any recommendation, so that the velocity is flowing on the soil of my mesh (i named it for projectpurposes Diff_Ref)?


My code for U ist
Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (1 0 0);

boundaryField
{
    inlet1
    {
        type            flowRateInletVelocity;
        volumetricFlowRate constant 1.4;
        //value           uniform (1.4 0 0);
        extrapolateProfile  yes;
    }
    inlet2
    {
        type            flowRateInletVelocity;
        volumetricFlowRate constant 0.6;
        //value           uniform (0.6 0 0);
        //extrapolateProfile  yes;
    }
    outlet
    {
        type            freestream;
        freestreamValue uniform (1 0 0);
    }
    frontAndBack
    {
        type            noSlip;
    }    
    soil
    {
        type            noSlip;
    }
    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    Diff_Ref
    {
        type            slip;
    }
}



my complete case can be seen here:


https://1drv.ms/u/s!AgK-q6eTTXN1xEDHd2pGFGA-l3hx?e=HHaZax


Thanks in advance,
aelmoe
aelmoe is offline   Reply With Quote

Old   January 3, 2021, 21:19
Default
  #2
New Member
 
Amirhossein Taran
Join Date: Sep 2016
Location: Iran
Posts: 27
Rep Power: 7
amirhosseintaran is on a distinguished road
Dear aelmoe , have you tried inlet-outlet bc ( for velocity and maybe alpha) for your atmospheric patch ?
amirhosseintaran is offline   Reply With Quote

Old   January 4, 2021, 03:38
Default
  #3
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 449
Rep Power: 11
Tobermory will become famous soon enough
From a quick check of your inlet boundaries, you have set the following for alpha:
Code:
    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }
    inlet2
    {
        type            fixedValue;
        value           uniform 1;
    }
i.e. setting alpha = 1 across the whole of the inlet patch. In other words, you are setting the water level to the top of the domain. The fixed volume flow boundary then controls the flow rate, and so it makes sense I think that the code fills the domain with water, from the inlets downward.

You need to do something more realistic with the water levels at the two inlets. Funkysetboundaryfield (part of swak4Foam) is a good tool for this, although you should also be able to do it with the vanilla distribution using some simple coding. Good luck.
Tobermory is offline   Reply With Quote

Reply

Tags
boundary conditions, flowratevelocity, interfoam, river

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
CFD analaysis of Pelton turbine amodpanthee CFX 31 April 19, 2018 18:02
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
Problem with SIMPLEC-like finite volume channel flow boundary conditions ghobold Main CFD Forum 3 June 15, 2015 11:14
Difficulty In Setting Boundary Conditions Moinul Haque CFX 4 November 25, 2014 17:30
Water subcooled boiling Attesz CFX 7 January 5, 2013 03:32


All times are GMT -4. The time now is 01:03.