Advice on open channel flow for an water intake chamber

jcox675 · August 21, 2014, 05:05

Hello, I am new to CFX and need advice on how to start/continue a simulation to do with open channel flow.
In the attached file is the setup showing what I would like. There will be an input and output of water with the free surface in atmospheric conditions.
I need to find the velocity of the water entering the chamber.

What boundary conditions and general settings would you suggest?
Which analysis type would be best?

Sorry for the really simple questions and thanks for the help!

Jonny

ghorrocks · August 21, 2014, 05:52

What do you know about the flow? What are the fluids?

jcox675 · August 21, 2014, 08:41

The fluids are water and air. The input and output flow is the same (mass flow rate 300). Thanks a lot.

Jonny

ghorrocks · August 21, 2014, 20:37

There needs to be something to drive the flow. Is the channel sloped? Pressure gradient?

What is open to the atmosphere? Does anything control the water level?

jcox675 · August 22, 2014, 04:21

The area open to atmosphere is the top face of the channel. In reality water comes from that open face and the channel is sloped, but I want to make as simple a model as possible. The water would collect in the channel and eventually due to gravity drop into the chamber. I know this won't work as I have modeled the water entering from the side face however. I just want to find out the behaviour of the water as it goes through the channel, into the chamber and out the pipe.
A valve further down the pipe controls how much water goes through the system, but i thought it would be okay just to monitor the flow in and the flow out.
What would you suggest?
Thanks again

ghorrocks · August 22, 2014, 06:53

It sounds like before you start anything you have to sort out exactly what your boundary conditions are.

You say water flows into it - you have to define this. Do you know the flow rate? If so then this is easy to define the inlet boundary.

You say the outlet is controlled by a valve. How is the valve controlled? Is it just at a fixed opening point to throttle the flow? In that case you should model the outlet as the valve discharge curve. Or is it controlled somehow - in that case how?

jcox675 · August 22, 2014, 08:56

So I have played around with some tutorials and think I would be able to do it apart from knowing what boundaries to use!

I know the flow rate going in which will be straight forward. The outlet valve will have the same flow going out as we are not modelling the valve. Trying to get a basic flow analysis done before we add more complex parts to it!

The main problem was that I wasn't sure about was the top face opening boundary conditions and the general settings for water in atmospheric conditions.
Cheers

ghorrocks · August 22, 2014, 09:28

You need to think harder about the boundary conditions. OK, so you know the flow in. But to then use the same flow as an outlet condition would be badly posed. Have a think about it - what controls the water level if the outlet flow rate is set as a constant? It means your fluid level is not controlled and this run will not converge.

The thing which probably defines your outlet flow rate is the static head applied to the outlet valve. The static head (which is your fluid level) will adjust until the flow rate in the valve matches the flow rate in. Now your fluid level is coupled to the outlet flow in a well-posed manner.

So yes, the top boundary is just an opening with atmospheric pressure. But you need to think more carefully about your outlet condition if you want this simulation to work.

jcox675 · August 26, 2014, 06:27

Yes that makes sense. How would I set the outlet condition to be dependent on the static head? Would it be similar to the equations found in tutorial 7? how would they compare? Thank you for bearing through this!

ghorrocks · August 26, 2014, 22:56

If the outlet valve is fixed then it will have a pressure drop versus flow rate curve. Then apply this curve.

If the valve moves or is under active control then you have to model the movement or control.

jcox675 · September 4, 2014, 05:17

I have tried to search how to apply this curve but have been unsuccessful. How would you apply it?

ghorrocks · September 4, 2014, 07:28

There are two options:

1) Set the outlet to be a massflow outlet. Calculate the areaAve(p)@Outlet, and use a lookup table on the massflow versus p for the valve to set the massflow.
2) Set the outlet to be a pressure outlet. Calculate the massflow()@Outlet, and use a lookup table on the massflow versus p for the valve to set the pressure.

They are just two different ways of doing the same thing. But I suspect you will find the first is more numerically stable than the second.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Question on the boundary condition for open channel flow, please help!	ripperjack	OpenFOAM Running, Solving & CFD	0	September 13, 2013 11:44
Gravitational water flow in closed channel.	Szymon85	CFX	7	September 3, 2013 16:28
Open Channel Flow Boundary Conditions	TWaung	STAR-CCM+	2	October 7, 2011 00:37
Open Channel Flow	forsumit	FLUENT	0	October 1, 2009 02:01
VOF modelling open channel river flow	Matthew Roberts	FLUENT	6	July 31, 2009 12:52

August 21, 2014, 05:52		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	What do you know about the flow? What are the fluids?

August 21, 2014, 08:41		#3
jcox675 New Member Jonny Cox Join Date: Aug 2014 Posts: 6 Rep Power: 11	The fluids are water and air. The input and output flow is the same (mass flow rate 300). Thanks a lot. Jonny

August 21, 2014, 20:37		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	There needs to be something to drive the flow. Is the channel sloped? Pressure gradient? What is open to the atmosphere? Does anything control the water level?

August 22, 2014, 04:21		#5
jcox675 New Member Jonny Cox Join Date: Aug 2014 Posts: 6 Rep Power: 11	The area open to atmosphere is the top face of the channel. In reality water comes from that open face and the channel is sloped, but I want to make as simple a model as possible. The water would collect in the channel and eventually due to gravity drop into the chamber. I know this won't work as I have modeled the water entering from the side face however. I just want to find out the behaviour of the water as it goes through the channel, into the chamber and out the pipe. A valve further down the pipe controls how much water goes through the system, but i thought it would be okay just to monitor the flow in and the flow out. What would you suggest? Thanks again

August 22, 2014, 06:53		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	It sounds like before you start anything you have to sort out exactly what your boundary conditions are. You say water flows into it - you have to define this. Do you know the flow rate? If so then this is easy to define the inlet boundary. You say the outlet is controlled by a valve. How is the valve controlled? Is it just at a fixed opening point to throttle the flow? In that case you should model the outlet as the valve discharge curve. Or is it controlled somehow - in that case how?

August 22, 2014, 08:56		#7
jcox675 New Member Jonny Cox Join Date: Aug 2014 Posts: 6 Rep Power: 11	So I have played around with some tutorials and think I would be able to do it apart from knowing what boundaries to use! I know the flow rate going in which will be straight forward. The outlet valve will have the same flow going out as we are not modelling the valve. Trying to get a basic flow analysis done before we add more complex parts to it! The main problem was that I wasn't sure about was the top face opening boundary conditions and the general settings for water in atmospheric conditions. Cheers

August 22, 2014, 09:28		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	You need to think harder about the boundary conditions. OK, so you know the flow in. But to then use the same flow as an outlet condition would be badly posed. Have a think about it - what controls the water level if the outlet flow rate is set as a constant? It means your fluid level is not controlled and this run will not converge. The thing which probably defines your outlet flow rate is the static head applied to the outlet valve. The static head (which is your fluid level) will adjust until the flow rate in the valve matches the flow rate in. Now your fluid level is coupled to the outlet flow in a well-posed manner. So yes, the top boundary is just an opening with atmospheric pressure. But you need to think more carefully about your outlet condition if you want this simulation to work.

August 26, 2014, 06:27		#9
jcox675 New Member Jonny Cox Join Date: Aug 2014 Posts: 6 Rep Power: 11	Yes that makes sense. How would I set the outlet condition to be dependent on the static head? Would it be similar to the equations found in tutorial 7? how would they compare? Thank you for bearing through this!

August 26, 2014, 22:56		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	If the outlet valve is fixed then it will have a pressure drop versus flow rate curve. Then apply this curve. If the valve moves or is under active control then you have to model the movement or control.

September 4, 2014, 05:17		#11
jcox675 New Member Jonny Cox Join Date: Aug 2014 Posts: 6 Rep Power: 11	I have tried to search how to apply this curve but have been unsuccessful. How would you apply it?

September 4, 2014, 07:28		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,700 Rep Power: 143	There are two options: 1) Set the outlet to be a massflow outlet. Calculate the areaAve(p)@Outlet, and use a lookup table on the massflow versus p for the valve to set the massflow. 2) Set the outlet to be a pressure outlet. Calculate the massflow()@Outlet, and use a lookup table on the massflow versus p for the valve to set the pressure. They are just two different ways of doing the same thing. But I suspect you will find the first is more numerically stable than the second.