[ali naqi]

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;
}

[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 -.-):

• 0
• constant
• system

Thanks and have a nice WE,
Benji

[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.

[vonboett]

Hi Benji,

have you tried just
outlet
{
type buoyantPressure;
value uniform 0;
}
for p_rgh ?

[avigrod]

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)

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 -.-):

• 0
• constant
• system

Thanks and have a nice WE,
Benji

[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.

[Bashar]

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 ?

[fatemehfarshi62]

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.

[Bashar]

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

[fatemehfarshi62]

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.

[Bashar]

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

[Bashar]

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

[jdegraff]

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.

[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.

[jdegraff]

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?

[jdegraff]

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.

[vonboett]

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.

[vonboett]

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

[Mahmoud Abbaszadeh]

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