[mrkmrk]

Hi Everyone,

I am trying to model an incompressible fluid's flow through a pipe with a sliding valve in the middle. I asked about my question on the Fluent forum but haven't heard any response yet. Since this seems to be a general CFD question, please permit me to ask it here as well.

In the pipe shown in the figure below, the pressure inlet and outlet profiles are applied to the inlet and outlet of the pipe. The pipe's walls are deformable. Flow is modeled using FSI simulation.

From t=0 - 10 s, the valve is fully closed. The problem is that in this time interval, the flow velocity in the left part of the pipe increases to 0.7 m/s, while since there is no outlet for the left portion of the pipe, the velocity in this part should be near zero.

It should be mentioned that to avoid splitting the computational domain, a small gap is left between the valve and the lower wall. Flow cannot pass through this gap because it is modeled using Fluent's Gap model, and it is defined that when the sliding valve gets closer than a predefined value to the lower wall, it shouldn't let flow pass.

Und1.jpg

I would appreciate any help you can provide.

[Opaque]

Not certain what you are trying to achieve in the early transient of your model.

If the valve is closed, and you have an incompressible fluid you can only assume the initial velocity is 0 (patch it), the static pressure is the total pressure at your inlet, and the valve must be fully closed.

Once the valve is partially open, regardless of the amount, the fluid MUST move through (pure physics) and the flow on the left side will start to move.

If the pipe is elastic, and you increase the pressure the walls should bulge out and the fluid velocity should increase from 0 to whatever the physics is. Once the valve opens, depending on how fast the valve is open the wall may retract or continue bulging out.

[mrkmrk]

Dear Opaque,

Thank you for your help.

If the valve is closed, and you have an incompressible fluid you can only assume the initial velocity is 0 (patch it), the static pressure is the total pressure at your inlet, and the valve must be fully closed.

This is exactly what I expect to get but the velocity on the left side of the valve increases with time. I think this is a convergence issue as my continuity residuals are increasing by time (at the end of the 20th time step the continuity residual converges to 10! ). I think considering a slightly compressible fluid should improve the residuals. Do you suggest any other method to solve this problem?

[ghorrocks]

It is always best to model the actual physics of what is really happening rather than trying to make up some physics which might work.

So how does the actual device operate in the phase when the valve is shut? The pump or pressure source will have some form of system characteristic, so if you dead head it (which is what you are doing) then you are going to go to some extreme points on the system characteristic. But it will tell you what really happens in this initial phase.

[mrkmrk]

Dear Glenn,

Thank you very much for your help.

Yes. I understand that this is not a physically reasonable condition. However, I need to prestress the valve considering these pressure profiles because, in real physics, the pressure values on the left side of the valve never get below 10000 Pa, and that of the right side will always be more than 100 Pa. On the other hand, we cannot apply the final pressure values (10000 Pa) to the wall as a step function because this will distort the structure elements.

Do you know any trick to impose these pressure values while preserving the fluid velocity near zero (initial condition)?

Thank you.

[Gert-Jan]

Is "FSI with deforming mesh" possible to combine with "immersed solids" in CFX?
In that way it would be possible to use a pressure inlet and outlet while using the immersed solid as a valve to open and close.

I have used the immersed solid method succesfully, in a pipe with a ball valve. Since the pipe wall was fixed, I did not have to use FSI with deforming mesh.

[mrkmrk]

Dear Gert-Jan,

Thanks for your help.

I am using Fluent to perform the FSI analysis.

The valve senses the deflection's direction. If the pressure on the upstream gets higher than the pressure on the right side of it, then the valve deforms toward the downstream and this triggers a mechanism that closes the valve.

[Gert-Jan]

You mentioned earlier that the the pipe can deform and the value can slide up and down, as sketched in your picture. Now you mention that the valve can deform as well. So, it can do multiple things? I'm lost.

To me it is unclear what exact question you want to answer when doing this CFD-study. The title of your query is: "Flow in a flexible pipe with a valve". But that isn't the whole story? Is it the deformation of the pipe? The valve? Both? Pressure drop? Flowrate? Fluent testing? FSI testing?

[mrkmrk]

Dear Gert-Jan,

Thank you very much for your attention.
I am sorry for not being able to disclose the exact mechanism of this valve. I think we can simplify the problem to a cylinder and piston. We want to increase the pressure inside the chamber without changing the velocity of fluid particles. Considering deformable walls for the cylinder, this should be possible. Please let me know if I am not on the right track.

As Glenn mentioned, this is not a physically valid problem. If we consider the cylinder and piston problem without opening an outlet, the pressure will rise when the piston compresses the air inside the cylinder. So the system will reach an extreme point. Since we have only one inlet for a very limited time interval, the only way to model this problem is to include the transient effects, which I am neglecting here.

Thank you again!

[ghorrocks]

If your system is not physically possible then you cannot model it as CFX models physical systems. You have some scope to bend reality in a simulation but not much.

In an incompressible flow, for a given velocity field it will define the one and only pressure field which goes with it. But note the pressure field is really just a pressure variation from a reference pressure - you can change the reference pressure and offset the whole pressure field up and down. But you cannot change the pressure variation from that reference pressure.

So your question of how to "increase the pressure without changing the velocity" can be answered by changing the reference pressure to increase or decrease the pressure level, but the pressure variations from that reference pressure are set by the defined velocity field and never change.

[mrkmrk]

Dear Glenn,

Thank you very much. Changing the reference pressure should work!

I hope I can define an expression for it so that in the beginning I can increase it linearly with respect to time.

[ghorrocks]

No, you cannot change the reference pressure. Once set it must be fixed for the entire run - otherwise it is not much of a reference pressure, is it?

But for an incompressible flow changing the reference pressure during the run (if it could be done) would do nothing anyway. As I said, for an incompressible flow it is only pressure VARIATION which is relevant, the absolute pressure level has no effect.

[mrkmrk]

Dear Glenn,

I agree that the reference pressure should remain constant throughout the simulation.
Fortunately, the fluid is incompressible, and I can confirm that I could successfully define a time-dependent profile for the reference pressure, and it worked very well!

Your help is much appreciated!

[ghorrocks]

I did not know you could do that. You learn something every day.

[Opaque]

Originally Posted by mrkmrk

Dear Glenn,

I agree that the reference pressure should remain constant throughout the simulation.
Fortunately, the fluid is incompressible, and I can confirm that I could successfully define a time-dependent profile for the reference pressure, and it worked very well!

Your help is much appreciated!

Hope you meant a "time-dependent value for reference pressure". There is no way to make a profile (where profile means a no-time dependent distribution)

[mrkmrk]

Originally Posted by ghorrocks

I did not know you could do that. You learn something every day.

We have the privilege of getting help from omnipotent scholars here which makes learning new things in CFD straightforward. Thank you!

[mrkmrk]

Originally Posted by Opaque

Hope you meant a "time-dependent value for reference pressure". There is no way to make a profile (where profile means a no-time dependent distribution)

Dear Opaque,

Thanks for letting me know. Yes. I meant a function that defines the relationship between pressure and time.