[MNMK]

Hi,

I would like to model a multiphase System which has a pump. I do not want to simulate the complete pump, however, use a performance Curve instead.

May sombody guid me how to simulate it?

wishes

MNM

[ghorrocks]

Put a momentum source term or boundary condition in which has the pump performance curve set to drive the flow.

[MNMK]

Originally Posted by ghorrocks

Put a momentum source term or boundary condition in which has the pump performance curve set to drive the flow.

Thanks alot for the answer. It would be kind when you tell me more details.

regards,

[ghorrocks]

We need more detail from you first -
Is the pump inside the domain or at a boundary?
What is the performance curve data you have?
How does the multiphase affect the pump curve?
Do you just want to apply the pressure rise from the pump, or do you want turbulence, temperature or any other effects as well?

[MNMK]

Originally Posted by ghorrocks

We need more detail from you first -
Is the pump inside the domain or at a boundary?
What is the performance curve data you have?
How does the multiphase affect the pump curve?
Do you just want to apply the pressure rise from the pump, or do you want turbulence, temperature or any other effects as well?

Hi,

I appreciate your answer.

-The pump is one of my component in a system.As I said, I want to simpilify my model and prevent to simulate the pump.
-The performance curve is Massflow-Pressure. (See attachment)
-I do not know the Multiphase influence on Curve and it is not vital for me.
-Except Pressure, the temperature effects can be an interesting parameter for me.

I hope, I could clear the topic.

wishes

[ghorrocks]

OK, the easiest way to do it is:
* In your mesher, cut the domain at the location for the pump. Remesh with this new cut plane in your mesh.
* In CFX-Pre, define an interface at the cut at the pump. Make sure you correctly choose the two sides of the interface.
* In the interface tab, go to "Additional Interface Models", and select an interface model of "Pressure Change" or "Mass Flow Rate".
* Define a function for it. I just did a quick example which used the function "(massFlow()@Domain Interface 1 Side 1 - 1[kg/s])*1000[Pa]/(-1[kg/s])" for a pressure change model. This describes a linear pump performance curve which goes through (0kg/s, 1000pa) and (1kg/s, 0Pa).
* If you use a mass flow function you will need the pressure on both sides of the interface to get the pressure difference. Something like "(areaAve(p)@Domain Interface 1 Side 1 - areaAve(p)@Domain Interface 1 Side 2)" will give you the pressure difference.

You can also do it using a subdomain and a source term. It is the same concept but requires a little more thought to implement.