Pump Station Simulation
Hello to everybody;
I have done a simulation in CFX 11 but the results seems to be not realistic.
I´ve done the tutorials and I have read the post of the forum but I cant solve the simulation. So I ask you for help and recomendations.
I am trying to study the velocity profile in a Pump Station(PS) in order to demostrate that the velocities at any point of the Pump Station is not too high. The porpuse it isnt study the velocity at the inlet of the Pump Suction Bell, but to study the velocity profile in the chamber of the Pump Station(PS).
I have attached an image of the PS (this is the model with the walls. In the CFX I have modeled the "negative"..just the water).
The Inlet will be always submerged
The Outlet are the five cilinders (Pump Suction Pipes)and also will be always submerged. The Pump Suction Pipe are 800 mm separated from the bottom.
The BC I have set are:
Location = Pipe InletOutlets =
Location = Bottom face of each cylinderOpening =
Location=Top of the PS.Walls =
Location= All the peripherial faces incluiding the lateral faces of the cylinders.Questions:
1-Which domain definition is the most suitable for this problem? Multiphase or Single Phase?.
2-How Should I define the Outlets? I guess that are not correctly defined.
3-In case the inlet wasnt submerged and I want to model the free surface, Which BC of multiphase domain do I have to set (using the expression of tutorial 7)?
PS definition attached file
Sorry the file wasnt attached.
Do a single phase simulation if at all possible.
What do you mean by "define the outlets?"
For the dual phase inlet you will need to set an inlet velocity or pressure, and then specify the volume fraction of the incoming fluid. The volume fraction should be set to water at the bottom and air at the top with a transition at whatever water level you wish to model.
Thank you very much ghorrocks for you reply.
> Do a single phase simulation if at all possible.
I have already done a single phase simulation. The matter is that almost all the flow streamlines goes up to the opening boundary(the top face) and only few streamlines goes to the Suction Pumps. The behavior is like the opening face were at lower pressure. But this is not the case because the opening boundary pressure is set at 1 atm (and the domain reference pressure is set at 0 atm).
I have attached an image.
So why this behaviour? What its happening?
> What do you mean by "define the outlets?"
I mean the setting of the face location of the outlet and the boundary details.
>For the dual phase inlet you will need to set an inlet velocity or pressure, >and then specify the volume fraction of the incoming fluid. The volume >fraction should be set to water at the bottom and air at the top with a >transition at whatever water level you wish to model.
I have tried it but I am doing something wrong.
The inlet pipe is full of water.
The waterlevel in the pump station chamber depends of the flow of the pumps and the simulation time (if the pump discharge is higher than the inflow, the water level will decrease with time).
So I dont know which level of water do I have to set at the inlet boundary details: at the crown of the pipe? At the water level of the Pump station? In case the last one...which level?
Thank you very much in advance
Alternately, if you replace the pressure outlet with a slip wall then the flow won't go out. It might generate regions of high pressure - you will need to check this assumption is valid.
Thanks again ghorrocks
>Then obviously your implicit assumption that the free surface is at the >pressure outlet location is wrong. If the free surface level is not very flat >then you are best to do a multiphase simulation.
Sorry Ghorrocks, I dont understand it very well.
I have set a opening at the top of the Chamber and 5 outlets and the end of the chamber. The opening is set at 1 atm (reference pressure = 0 atm). The outet is set at a fixed flow.
So you mean that the free surface isnt at the atmospheric pressure?
Because the only pressure I have set is for the top Opening (P=1 atm) and for the domain (Pref= 0 atm). The 5 outlets pressures are calculeted by CFX.
Now I am bit confused. Please Ghorrocks, could you help me a bit more?
>You need to put all boundaries at locations where the variables you >define are known. Right at the outlet there will be significant gradients in >pressure and velocity across the flow, so it might be better to move the >boundary upstream to where the flow is simpler and the variables can be >defined more accurately.
But the only variables I know are
1-Chamber Geometry (the top is open)
2-Inlet Flow and location
3-Outlets flows and location
How I can set other boundaries and where?
>That means there will be some sort of control system to keep the water >level within limits. Then the response of this control system needs to be >incorporated in your model somehow.
You are right ghorrock I didnt thought on it. Thank you! So I have to set the free surface at a level that depends on the pumps regulation.
Ok ...if I fix the free surface at a convinient level... is correct to set variable UpH(tutorial 7) at this free surface level or at the crown of the pipe inlet?
I mean for a filling tank problem, where you define the variable UpH...at the crown of the pipe? at the initial water level of the tank?
Thanks in advance
That is why I recommend using a slip wall instead of a pressure boundary. Then there is no way fluid can be created or destroyed at the boundary.
|All times are GMT -4. The time now is 09:00.|