[ckleanth]

is the inlet and outlet fully submerged in the pond?

[Sher]

Originally Posted by ckleanth

is the inlet and outlet fully submerged in the pond?

Yes, the inlet and outlet are fully submerged and also I would like to model a position of inlet and outlet when their crown is just beneath the water surface.

Thanks for giving your time to study my problem.

[ckleanth]

two remarks
- if both inlet and outlet is submerged i'm not sure why you're trying to model air? what do you want to learn from the simulation? maybe a picture/sketch of the problem would be helpful so that people can understand what you want to achieve, and would minimize guessing.

-when the inlet is somewhere between the free surface of the phase you will need to restrict the Inlet BC according to where you defined the free surface in a similar way you created the outlet BC.

[Sher]

Originally Posted by ckleanth

is the inlet and outlet fully submerged in the pond?

Thanks for your advices. The sketch of the model is attched. Although in this sketch the inlet and outlet are just below the free surface.

[ghorrocks]

hi,

Does the free surface do much? If it stays pretty much flat then I would not do a free surface simulation at all but a single phase model with the top surface a pressure boundary, of possibly a degassing boundary if relevant. If this simplification is valid it will make things MUCH easier.

Glenn Horrocks

[Sher]

Originally Posted by ghorrocks

hi,

Does the free surface do much? If it stays pretty much flat then I would not do a free surface simulation at all but a single phase model with the top surface a pressure boundary, of possibly a degassing boundary if relevant. If this simplification is valid it will make things MUCH easier.

Glenn Horrocks

Hi thanks for your reply. Actually I have modelled as single phase model with top as a symmetry and I got very good results but as a requirement of my investigation I would like to compare these results with top as free surface. In the geometry of my model I would like to keep the inlet and outlet at 0.23 m above the bottom and free surface above this (I mean the free surface may be at 0.24m or 0.25m). Please suggest me, if possible?
regards

[ghorrocks]

hi,

A symmetry boundary is not a good choice. It can allow the pressure to deviate from atmospheric. This may or may not be important, that depends on the model. But anyway that's why I recommend a pressure boundary.

Glenn Horrocks

[Sher]

Originally Posted by ghorrocks

hi,

A symmetry boundary is not a good choice. It can allow the pressure to deviate from atmospheric. This may or may not be important, that depends on the model. But anyway that's why I recommend a pressure boundary.

Glenn Horrocks

Thanks for your help. Can you please advise me how to add pressure boundary at the top. Please advise me its step as I am new user.

Thanks

[ghorrocks]

Set the boundary as an opening, defined using pressure.

[Sher]

Originally Posted by ghorrocks

Set the boundary as an opening, defined using pressure.

Yes I did the top as opening with static pressure = zero (I was calling it a free surface in all my messages) with fluid values as:
air at 25 C ----> value=1, water --->0.

and I was tryng to compare this with my results of symmetry. But its making the problem complex and some times I get flow in reverse direction or a bad flow directions. Please suggest me, if possible for you. My geometry and .CCL file is on this forum with my previous messages

Thanks

[ghorrocks]

Hi,

No, you have misunderstood.

The pressure boundary as the liquid free surface approach should only be used single phase.

If you are running a multiphase simulation then you should raise the top boundary to always be above the surface and apply a pressure boundary to it at atmospheric pressure and reverse flow being the air phase. Then the simulation will predict the free surface level.

Glenn Horrocks

[Sher]

Originally Posted by ghorrocks

Hi,

No, you have misunderstood.

The pressure boundary as the liquid free surface approach should only be used single phase.

If you are running a multiphase simulation then you should raise the top boundary to always be above the surface and apply a pressure boundary to it at atmospheric pressure and reverse flow being the air phase. Then the simulation will predict the free surface level.

Glenn Horrocks

Yes I do but in expressions when i add volFraction of water then I need to give a reference height of water free surface which is always below the top boundary. but even then I am getting problems.

Regards

[John]

If you want to model the free surface, your geometry should be extended upward to give some space to allow "free surface" formed.

This is a tricky problem. Top and outlet boundary conditions should be carefully selected, since both could significantly affect the result.

[Sher]

[QUOTE=John;223813]If you want to model the free surface, your geometry should be extended upward to give some space to allow "free surface" formed.

This is a tricky problem. Top and outlet boundary conditions should be carefully selected, since both could significantly affect the result.[/QUOTE
Thanks John,
Yes, the top and outlet really significantly effect the results. This problem is making me mad. I have tried many times this problem with a little variation of free surface height (or the hydrostatic pressure at the outlet) all the time flow patter become different. Now i am fighting with this issue. I have extended the geometry 0.1 m above the free surface and below the free surface the depth of pond is 0.23m. I have applies the hydrostatic pressure at the outlet as a function of rising height of water upto the free surface (0.23m height of water). I have modelled the top as opening with zero static pressure and the relative pressure of the domain is 1 atm.

please advise me if you have any suggestions to improve this modeling.

I thanks youe once again for your help

[Sher]

Originally Posted by ghorrocks

Hi,

No, you have misunderstood.

The pressure boundary as the liquid free surface approach should only be used single phase.

If you are running a multiphase simulation then you should raise the top boundary to always be above the surface and apply a pressure boundary to it at atmospheric pressure and reverse flow being the air phase. Then the simulation will predict the free surface level.

Glenn Horrocks

Hi ghorrocks, I was reading all your suggestions and what I understand now is that I should model the flow as single phase whith the only fluid i.e water with the following BCs:
Inlet: Speed or mass flow
Outlet: pressure outlet with static pressure -->Density of water*g*(H-y)
Top opening with static pressure Zero

Please advice me if still I am approximating something wrong. Please also advice me that top (opening) should be given static Presure=0 or atm Pres= 1, Will any one of them make difference or they will make the same results. I will wait your suggestions, please.

Regards

[John]

[QUOTE=Sher;223829]

Originally Posted by John

If you want to model the free surface, your geometry should be extended upward to give some space to allow "free surface" formed.

Originally Posted by John

This is a tricky problem. Top and outlet boundary conditions should be carefully selected, since both could significantly affect the result.[/QUOTE
Thanks John,
Yes, the top and outlet really significantly effect the results. This problem is making me mad. I have tried many times this problem with a little variation of free surface height (or the hydrostatic pressure at the outlet) all the time flow patter become different. Now i am fighting with this issue. I have extended the geometry 0.1 m above the free surface and below the free surface the depth of pond is 0.23m. I have applies the hydrostatic pressure at the outlet as a function of rising height of water upto the free surface (0.23m height of water). I have modelled the top as opening with zero static pressure and the relative pressure of the domain is 1 atm.

please advise me if you have any suggestions to improve this modeling.

I thanks youe once again for your help

Just some thoughts:

1. Your air space above water should be high enough to avoid the impact of top "open" boundary.
2. The outlet Boundary condition should be phase dependent, and should be a function of height and volume fraction.
3. Your mesh on the unknown water/air interface should be very fine to capture the interface


Again, this type of problem should always include validation study. withough validation process, you may have to do some traditional hydraulic calculations to judge the result--see if it is in the reasonale range.

[Sher]

Thanks all of you, John,ghorrocks and ckleanth for my help.
I really got much more understanding of free surface from your suggestions. Thanks for this. Now I have done the free surface which is below top (opening) and now I am getting very good results.

The only problem which I am facing now is that the velocity at inlet varies from 0.1 m ^-s to 3.2 m ^-s. The case in which velocity is higher (3.2 m s^-1) is giving very nice results now but the case with low velocity (0.1 m s^-1) is not giving good results and shows lumpyness flow pattern and also flow start from outlet to inlet. I am wondering why is this happening as the case of high velocity giving good results which have every thing same as the high velocity case except velocity at inlet. May be it is due to hydrostatic pressure at the outlet?
Can somebody advice me in this regard, please.
thanks again
cheers

[mechovator]

Dear Glenn Horrocks
You solved my problem.
Thanks alot