cause of Falling water surface in inlet flow?
 

hi every one
i am modeling one reservoir & spillway in ansys cfx, my results of numerical model was good agreement with experimental model, but There is a problem in my model, in inlet flow i have falling in water surface as shown figure, I do not know what is the cause, i considred total time too much in cfx-pre Unfortunately, it remains.
please guide me
thanks very much for any comments
kinf regards
hamid

This is usually caused by the inlet boundary condition enforcing a fixed free surface level, but that surface level is not valid for the flow so the simulation has to adjust the level to the modelled level. It means your inlet boundary is not properly setting the inlet free surface level.

hello dear glenn, thanks for answer
if your possible please guide me, i used CEL for setting volume fraction water & air, I did it according flow over bump in menual cfx, What do you think I who parameter wrong considered? i'm working on this model for a long time , Finally faced with this problem.
thanks in advance
best wishes

The water level in the inlet chamber is really set by the water height going over the bump. So if you define a fixed level there is always going to be a jump from whatever you defined it to be and the level the simulation finds.

One approach could be to have an inlet which is pure water which squirts into a chamber. The chamber water level is then set by the simulation, and you do not need to set a level.

dear glenn thanks for reply
Another that comes to mind It is My entrance away from of where i will to extract the results , in finally this falling in water surface will not be effective at my results, Do you mean the same thing?
unfortunately i exactly dont understand your mention about chamber, because Anyway i should defined one constant depth of water in inlet and So I'll have a constant level of water.
dear glenn , You must forgive me for not noticing your orders because I do not have that much experience you in simulation.
Did I understand correctly your mean?
yours faithfully
hamid

Here is a quick edit of your sketch to show my recommendation:

Attachment 41593

Put an inlet in the roof which is just pure water at the specified flow rate. This flows down into the chamber and the simulation can find its own level.

dear glenn thanks a lot for reply and time
i now understand your order completely , if your possible i have another question, if i defined inlet where away from i want extarcted results, Do you think there's a problem?
best regards
hamid

When you do my suggestion it means you have changed the local flow from what is really there. So you are correct - you need to move it far enough away from your area of interest such that it does not affect the true flow in your area of interest.

dear glenn
thanks so much for spending time for me.
i hope you success & health.

sorry I know it is not acceptable, to ask a question here but my problem is similar to this problem, my level of water in reservoir is falling like your case, but I sure that my inlet height of water is correct (in reservoir) because I have experimental data, and also depth of water within he model does not agree with experimental. I used normal velocity at inlet my simulation is transient (total time 10 s and time step 0.06) with initial conditions at inlet (pressure, velocity, vol.fraction)
thanks

You will have to give more detail about what you are modelling, with images, and your CCL if we are to help you.

as glenn mentioned, we need to more information of your model, but if your problem be same like me, i expressing my experience about this problem In the following:
The reason you are experiencing the problem with the CEL is because the solution has not converged to the correct water level at the inlet, as glenn also expressed Previously, you should chenged Location of inlet BC in your model, for example, put it in top of model or created one 'false wall' that protrudes a small distance below the physical free-surface which then reduces the 'fall' in the flow.
in my model, despite i have falling in water surface, but my result had good agreement with experimental model.
hope it helps

dear Glenn thanks for your reply, here all details for my model, I simulated two model transient and steady state, I used normal velocity at inlet, and one case I used bulk mass flow rate it is very easy to convergence but the results does not expected, in free surface flow is it right to use bulk mass flow rate? in flow over bump tutorial I specified all height of inlet as inlet boundary it gives a very well result (as shown in attached figure), I did same boundary for my model
thanks
https://drive.google.com/open?id=0B3...lpNemxxT0UwT1k
https://drive.google.com/open?id=0B3...EJmb1ViVXpwRlU
http://www.cfd-online.com/Forums/att...1&d=1459927200
http://www.cfd-online.com/Forums/att...1&d=1459927464
http://www.cfd-online.com/Forums/att...1&d=1459927530
http://www.cfd-online.com/Forums/att...1&d=1459928411

thanks Hamidciv for your reply
using boundary condition at the top for the case that you dont know water level at inlet ( As I said I have experimental data so, I know water level at inlet), what did you mean by (created one 'false wall') please give me more clear idea (how to create it)
thanks

dear yaseen
in first case, you should set inlet in top of model as specific flow rate that you will have surely its value.
in second case, my mean of false wall as shown in figure below
hope it helps

Thanks a lot, yes this method can maintain the US water level constant, but I think this method does not convent with free surface, because it puts velocity in reservoir is zero this is hydraulically wrong, also in this method you should enter bulk mass flow rate, so in transient simulation how can you specify initial conditions (velocity and pressure). this method give me results lower than experimental
I put the top of the reservoir as wall boundary condition as shown in attached image
http://www.cfd-online.com/Forums/att...1&d=1460026182
http://www.cfd-online.com/Forums/att...1&d=1460026199