# Setting BCs for Riverine Flows using Interfoam

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

June 2, 2013, 06:59
manning's roughness coefficient in OpenFoam
#21
New Member

Join Date: Dec 2012
Posts: 6
Rep Power: 12
Quote:
 Originally Posted by trinath2rao Dear Foamers, I am working on dambreak flow in an open channel. can any one help me how to specify manning's roughness coefficient in OpenFoam. I checked manual and code, no success. Is there anyway to specify bottom friction in OpenFoam ? Thank You in advance. Regards, Trinath Rao
hi ,in the OF you should obtain roughness effect by Ks and Cs. you may find them in nut. for example:
walls
{
type nutkRoughWallFunction;
value uniform 0;
Ks uniform .0014;
Cs uniform .5;
}

 April 25, 2014, 11:47 #22 New Member   Benjamin Join Date: Apr 2014 Location: Zürich Posts: 27 Rep Power: 11 Hey all, I'm working at a similar problem at the moment and hope anyone could help me. I have a free surface flow channel with a narrowing. Like before I want to give the inlet velocity (here 0.5 m/s), but I need to give a predefined outlet-pressure somehow (because I need to be able to calculate for a given water elevation at the outlet). I thought I couldn't define a pressure for the whole outlet, so I chose to define it only at the bottom of the river bed (over the last m of the channel before the outlet). The idea was to be able to give a certain hydrostatic pressure at the ground, which should define the water level. Inlet: alpha = fixedValue (1), U = fixedValue (0.5 0 0), p_rgh = fixedFluxPressure (0) Outlet: alpha = inletOutlet (0), U = pressureInletOutletVelocity (0 0 0), p=fixedFluxValue (0) Outlet (bottom): p = phaseHydrostaticPressure; phaseName alpha.water; rho 1000; pRefValue 3000; pRefPoint (0 0 0); value uniform 0; I wasn't sure how to define that, has anyone ever tried this or would do it for me? Or are there other solutions? I also get problems with alpha reflecting at the outlet sometimes... Casefiles (currently negative x-axis, to avoid the problem of reflecting -.-): Thanks and have a nice WE, Benji

 November 5, 2014, 07:07 fixed depth water at outlet #23 New Member   ali naqi mohammadi Join Date: Dec 2012 Posts: 6 Rep Power: 12 for implementation of fixed depth at outlet, first you should divide the mesh block into two blocks: one with height of the outlet depth and the other for air. so we will have two outlet: waterOutlet and airOutlet. zeroGradient boundary condition for waterOutlet . atmosphere boundary condition for airOutlet. Mahmoud Abbaszadeh likes this.

 November 5, 2014, 08:17 #24 Senior Member   Albrecht vBoetticher Join Date: Aug 2010 Location: Zürich, Swizerland Posts: 236 Rep Power: 16 Hi Benji, have you tried just outlet { type buoyantPressure; value uniform 0; } for p_rgh ?

November 10, 2014, 05:49
#25
New Member

Antonio
Join Date: Jan 2013
Posts: 11
Rep Power: 12
Hi Benji,

Have you tried Kflora suggestion. I have used in some steady open flows succesfully. I would suggest to enlarge the end of the channel to reduce influence of using a uniform 1D velocity profile.

Her suggestion is to use a fixed velocity bc of water flow rate input/ water depth aim. Being it applied to all the outlet surface (water and air)

Quote:
 Originally Posted by Benji Hey all, I'm working at a similar problem at the moment and hope anyone could help me. I have a free surface flow channel with a narrowing. Like before I want to give the inlet velocity (here 0.5 m/s), but I need to give a predefined outlet-pressure somehow (because I need to be able to calculate for a given water elevation at the outlet). I thought I couldn't define a pressure for the whole outlet, so I chose to define it only at the bottom of the river bed (over the last m of the channel before the outlet). The idea was to be able to give a certain hydrostatic pressure at the ground, which should define the water level. Inlet: alpha = fixedValue (1), U = fixedValue (0.5 0 0), p_rgh = fixedFluxPressure (0) Outlet: alpha = inletOutlet (0), U = pressureInletOutletVelocity (0 0 0), p=fixedFluxValue (0) Outlet (bottom): p = phaseHydrostaticPressure; phaseName alpha.water; rho 1000; pRefValue 3000; pRefPoint (0 0 0); value uniform 0; I wasn't sure how to define that, has anyone ever tried this or would do it for me? Or are there other solutions? I also get problems with alpha reflecting at the outlet sometimes... Casefiles (currently negative x-axis, to avoid the problem of reflecting -.-): Thanks and have a nice WE, Benji

 January 11, 2016, 02:17 #26 Member   Fatemeh Join Date: Dec 2015 Location: Isfahan,Iran Posts: 39 Rep Power: 9 Hi every one! I have a similar problem. I have a 3D open channel which has a curved route. I want to enter a fully developed flow in the inlet and don't know how it will be at the outlet. can any one tell me what are the right boundary conditions for inlet, outlet and free surface? thanks a lot. Bashar likes this.

February 11, 2017, 13:50
#27
Member

Bashar
Join Date: Jul 2015
Posts: 74
Rep Power: 10
Quote:
 Originally Posted by fatemehfarshi62 Hi every one! I have a similar problem. I have a 3D open channel which has a curved route. I want to enter a fully developed flow in the inlet and don't know how it will be at the outlet. can any one tell me what are the right boundary conditions for inlet, outlet and free surface? thanks a lot.
Hi,

I am facing similar issues, I am working of flow past plate . Did you mamnge to make this work for you ?

February 12, 2017, 00:42
#28
Member

Fatemeh
Join Date: Dec 2015
Location: Isfahan,Iran
Posts: 39
Rep Power: 9
Quote:
 Originally Posted by Bashar Hi, I am facing similar issues, I am working of flow past plate . Did you mamnge to make this work for you ?

Hi! for velocity, enter flowRateInletVelocity for inlet and inletOutlet for outlet.
for Pressure, zeroGradient for inlet and fixedValue for outlet.

February 12, 2017, 00:50
Setting BCs for Riverine Flows using Interfoam
#29
Member

Bashar
Join Date: Jul 2015
Posts: 74
Rep Power: 10
Quote:
 Originally Posted by fatemehfarshi62 Hi! for velocity, enter flowRateInletVelocity for inlet and inletOutlet for outlet. for Pressure, zeroGradient for inlet and fixedValue for outlet.

Thanks a lot for the info.Will be ok for you to share the case file ?
But thanks anyway,I will try your BC.I am using single inlet patch,I saw some cases where they use two separate inlet patches,one for air and the other for water. Did you use single inlet?

Thanks

Sent from my iPhone using CFD Online Forum mobile app

Last edited by Bashar; February 14, 2017 at 14:35.

February 12, 2017, 01:23
#30
Member

Fatemeh
Join Date: Dec 2015
Location: Isfahan,Iran
Posts: 39
Rep Power: 9
Quote:
 Originally Posted by Bashar Thanks a lot for the info.Will be ok for you to share the case file ? But thanks anyway,I will try your BC.I am using single inlet patch,I saw some cases where they use two separate inlet patches,one for air and the other for water. Did you use single inlet? Sent from my iPhone using CFD Online Forum mobile app
No, I just have one inlet.

February 12, 2017, 01:29
#31
Member

Bashar
Join Date: Jul 2015
Posts: 74
Rep Power: 10
Quote:
 Originally Posted by fatemehfarshi62 No, I just have one inlet.

Thanks , I will try it .

Sent from my iPhone using CFD Online Forum mobile app

February 14, 2017, 16:18
#32
Member

Bashar
Join Date: Jul 2015
Posts: 74
Rep Power: 10
Quote:
 Originally Posted by fatemehfarshi62 Hi! for velocity, enter flowRateInletVelocity for inlet and inletOutlet for outlet. for Pressure, zeroGradient for inlet and fixedValue for outlet.
Sorry to bother you again . I have another question, if I used single inlet patch for the channel, is there away to specify the speed of the air? I am currently specifying only one speed which is the water speed.So, the water and the air will have same speed, but I want to know how I can give them different speed while using one inlet patch.

Also, what setting should alpha.water get, i.e. BC.

Bashar

Last edited by Bashar; February 22, 2017 at 11:00.

 September 13, 2018, 08:18 Channel Flow Depth outlet BC - resurrected #33 New Member   Jeff DeGraff Join Date: Apr 2018 Posts: 3 Rep Power: 7 An old post with a lot of good information. I am modeling a river and would like to know if there are any additional tips on setting the downstream flow depth. I used Kflora's work around for simple rectangular channels but would like to know if there are work arounds for irregular shapes. Last edited by jdegraff; September 13, 2018 at 09:23. Reason: Wrong title

 September 13, 2018, 09:26 #34 Member   Honza Höll Join Date: Mar 2016 Location: Brno, CZ Posts: 33 Rep Power: 9 Maybe a good option is to make river a little bit longer (to the point where results from new cross section dont influence results in the initial location of downstream BC) and there use regular shape.

 September 18, 2018, 15:13 #35 New Member   Jeff DeGraff Join Date: Apr 2018 Posts: 3 Rep Power: 7 indy07cz - Good suggestion. That worked for most cases. Now what I am finding is that there isn't a constant inlet flow. I tried setting the inlet alpha to 0 (all water) but found that I still get "separation" in the stream. Does anyone have any suggestions?

September 20, 2018, 12:35
#36
New Member

Jeff DeGraff
Join Date: Apr 2018
Posts: 3
Rep Power: 7
Quote:
 Originally Posted by indy07cz Maybe a good option is to make river a little bit longer (to the point where results from new cross section dont influence results in the initial location of downstream BC) and there use regular shape.
This was a good idea which lead me to another idea. OpenFOAM V2 does not appear to be "good" at determining a proper inlet and outlet boundary condition (fixedFluxpressure, Volumetric Inlet flow) for complex geometries. But it does a decent job for simple geometries such as a rectangle. Thus I added a rectangular channel far enough upstream and downstream so that it doesn't effect the solution. Once I feel comfortable with the results, I will post them.

Again, if there is a better way of defining boundary "open channel flow" boundary conditions, please let me know. I feel that there is a lot of Foamers that deal with this issue.

 October 19, 2021, 11:38 #37 Senior Member   Albrecht vBoetticher Join Date: Aug 2010 Location: Zürich, Swizerland Posts: 236 Rep Power: 16 In case you are using atmosphere boundary conditions for the top, make sure the water does not contact it. Single drops are OK but interFoam can't handle the water/air density difference at the atmospheric boundary condition.

October 19, 2021, 11:44
#38
Senior Member

Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 236
Rep Power: 16
Quote:
 Originally Posted by jdegraff This was a good idea which lead me to another idea. OpenFOAM V2 does not appear to be "good" at determining a proper inlet and outlet boundary condition (fixedFluxpressure, Volumetric Inlet flow) for complex geometries. But it does a decent job for simple geometries such as a rectangle. Thus I added a rectangular channel far enough upstream and downstream so that it doesn't effect the solution. Once I feel comfortable with the results, I will post them. Again, if there is a better way of defining boundary "open channel flow" boundary conditions, please let me know. I feel that there is a lot of Foamers that deal with this issue.

By the way, I use fixedFluxPressure with complex inlet geometries, combined with fixedValue at the inlet and inletOutlet at the outlet for U. For the atmospheric top I use totalPressure with the corresponding settings and pressureInletOutletVelocity. It works well for mountain torrents

July 27, 2022, 07:51
#39
Member

Mahmoud
Join Date: Nov 2020
Location: United Kingdom
Posts: 43
Rep Power: 5
Quote:
 Originally Posted by ali naqi for implementation of fixed depth at outlet, first you should divide the mesh block into two blocks: one with height of the outlet depth and the other for air. so we will have two outlet: waterOutlet and airOutlet. zeroGradient boundary condition for waterOutlet . atmosphere boundary condition for airOutlet.
Have you tried this actually? This has not solved the problem in my case

 Tags interfoam, openfoam, river, vof