[Hale]

Hi,

I am dealing with a two phase flow problem where I need to specify a constant water level for the inlet. I do not want to do it by specifying a velocity or flux.

I tried to do it by specifying a hydrostatic pressure (rho*g*h) for p_rgh and zeroGradient for U but it blows up!

Is there any way to specify the height of the water at the inlet?

Thanks
Hale

[nimasam]

well i guess you can do it via non-uniform alpha1 (i assumed you use interFoam as solver )

[Hale]

Originally Posted by nimasam

well i guess you can do it via non-uniform alpha1 (i assumed you use interFoam as solver )

Hi Nima,

Thanks for the reply. Yes, I use interFoam. For the inlet where I need a constant water level I have defined alpha1=1 and zeroGradient for everwhere else. What did you mean with non-uniform alpha1?

[nimasam]

well you can put a non-uniform alpha
something similar this :

y < h ? 1 : 0

where h is water level

you can used:

1- code stream
2: groovyBC

to create such nonuniform BC

[Hale]

This is too complicated for me but would you please explain what will this non-uniform alpha1 do? I need a uniform water level at the inlet so why should I changed alpha1 to non-uniform?

[nimasam]

in your post #1, you said you want a constant water level!, so i assumed! a portion of your inlet fill with water! if the whole inlet is water! then specify the velocity or flux whats wrong then?

[Hale]

The problem is that I'm simulating a real life problem where the flux is not known but the water level can be adjusted. Therefore I want to specify the water level in terms of hydrostatic pressure or something else that can allow the model to find the flux/velocity by itself.

[Sim81]

I have a similar problem. I have two water tanks connected by a pipe. The tanks have two different water levels. I want to keep this difference constant but I do not know the flow rate at the inlet and outlet. Therefore I should find the BCs that allows me to keep the water levels constant in the tanks. Any help?

Thank you

[tinu80]

I have a very similar problem for open channel flows
What I need is an upstream boundary that physically behaves like there would be an unlimited reservoir of water with a fixed water level and no prescribed flow rate / velocity at the boundary. Velocity at the upstream boundary should develop as a consequence of the velocities in the model.
I have tried to fix upstream water level with groovyBC:

Upstream BC
------------------
alpha.water: pos().z <= waterlevel ? 1:0
U: zeroGradient
p_rgh: fixedFluxPressure


Downstream BC (simulating free outflow)
-------------------
alpha.water: inletOutlet, inletValue uniform 0;
U: pressureInletOutletVelocity
p_rgh: totalPressure p0 uniform 0;

Atmosphere
----------------------
alpha.water: inletOutlet, inletValue uniform 0;
U: pressureInletOutletVelocity
p_rgh: totalPressure p0 uniform 0;

These BC seem to work nicely with a very simple rectangular open channel flow. With more complicated meshes the simulation seemed to blow up, developing unphysical pressure/velocity from one point near the fixed inlet water level. I suspect the combination of zeroGradient for U and fixedFluxPressure for p_rgh at inlet is not stable.
Any ideas which combinations for p_rgh and U could work when fixing the inlet alpha.water level with groovyBC?
Hints are highly welcome!
Tinu

[Bashar]

Originally Posted by tinu80

I have a very similar problem for open channel flows

What I need is an upstream boundary that physically behaves like there would be an unlimited reservoir of water with a fixed water level and no prescribed flow rate / velocity at the boundary. Velocity at the upstream boundary should develop as a consequence of the velocities in the model.

I have tried to fix upstream water level with groovyBC:



Upstream BC

------------------

alpha.water: pos().z <= waterlevel ? 1:0

U: zeroGradient

p_rgh: fixedFluxPressure





Downstream BC (simulating free outflow)

-------------------

alpha.water: inletOutlet, inletValue uniform 0;

U: pressureInletOutletVelocity

p_rgh: totalPressure p0 uniform 0;



Atmosphere

----------------------

alpha.water: inletOutlet, inletValue uniform 0;

U: pressureInletOutletVelocity

p_rgh: totalPressure p0 uniform 0;



These BC seem to work nicely with a very simple rectangular open channel flow. With more complicated meshes the simulation seemed to blow up, developing unphysical pressure/velocity from one point near the fixed inlet water level. I suspect the combination of zeroGradient for U and fixedFluxPressure for p_rgh at inlet is not stable.

Any ideas which combinations for p_rgh and U could work when fixing the inlet alpha.water level with groovyBC?

Hints are highly welcome!

Tinu

Thanks for sharing the BC.I am simulating flow past plate with free surface.I will try your BC.



Sent from my iPhone using CFD Online Forum mobile app

[burbur]

Originally Posted by tinu80

alpha.water: pos().z <= waterlevel ? 1:0

Hi Tinu,
I am trying to define flow depth as boundary condition for an open channel model. This suggestion of yours seem reasonable. However, I could not find out how to apply this in the alpha.water file. Can you or anyone help on this issue?

Thanks.

[Tobermory]

Originally Posted by burbur

Hi Tinu,
I am trying to define flow depth as boundary condition for an open channel model. This suggestion of yours seem reasonable. However, I could not find out how to apply this in the alpha.water file. Can you or anyone help on this issue?

Thanks.

Tinu80's post is using the (fantastic) swak4Foam utility by Bernhard Gschaider (which is now integrated within v2021 I believe, if you are using that branch of OF). I heartily recommend that you check that out if you are planning to use OpenFOAM a lot, since I find it a really useful tool, and it provides a quick and intuitive method for applying BCs.

Failing that, as someone at the start of the thread mentioned, you can do the same with some pretty codeStream coding. Check out the following:
http://www.wolfdynamics.com/wiki/pro...streamINIT.pdf