[mrkmrk]

Hi All
I want to simulate fluid flow inside two deformable computational domains that are connected to each other by one interface using ANSYS CFX. The problem is that due to the deformation of elements, at some points during the simulation some elements of the surface located on one side of the interface separates from those of the other side because of using “unspecified” option for the mesh motion scheme. This is not logical and causes many divergence problems.


Is there any way to make two sides of the interface, stick together throughout the simulation, i.e. is there any way to make elements located on one side of the interface copy the motion of those that are located on the other side?



In order to provide more details,
-----------------------------------------

it should be mentioned that I cannot use “Parallel to boundary” option for the mesh motion scheme because the whole interface itself is moving in a direction which is approximately normal to the interface. In other words the mesh motion around the interface consists of movement of the interface and the deformation of elements located around the interface. Moreover, the movement of the two surfaces of the interface is unpredictable so I am unable to use a specified displacement or location scheme for this purpose. Attached is a 2D schematic figure that shows what is happening in my 3D problem.
-----------------------------------------


Best

[ghorrocks]

Why do you need an interface here at all? It appears to be in a critical part of the flow which is not a good place for an interface anyway.

What motion does this interface require? This will determine what options you have for defining the motion.

A final suggestion (which is only occasionally successful) is to try adjusting the mesh smoothing parameters. For instance try difference mesh displacement diffusion coefficients.

[mrkmrk]

Hi Glenn


Thanks for your prompt attention. I really appreciate it.


In reality the two deformable walls move toward each other until they touch their counterparts and obstruct the fluid flow. I want to simulate this problem by using ANSYS CFX 2-way fluid-structure interaction method. The main difficulty in modelling such problem is that the wall motion splits the computational domain of the fluid flow. As you know re-meshing feature is not available in ANSYS CFX FSI method so in order to circumvent this problem, I want to let the two deformable walls to only get too close to, but not touch each other, and then place a wall in the existing gap between them to obstruct the fluid flow. By using your help, I found that interface boundary condition has a feature that enables me to place a wall in the fluid flow domain at a specific time interval during the simulation. So this is the only reason behind using an interface boundary condition in that location.


About the interface mesh motion, the two deformable walls move based on the pressure difference between the flow inlet and outlet boundary conditions and ambient pressure. As I said in the previous post, the interface moves in upward and downward directions while it is expanding or shrinking. So I cannot provide it with a specified displacement expression. However I wondering if we could define an expression for the mesh motion of one side of the interface to force its elements to move and deform in a way that their counterparts in the other side of the interface are moving and deforming. Please let me know if this idea is applicable?


Thanks for your suggestion, I am testing it now and will inform you about the result.


Best

[ghorrocks]

Another way of doing this would be to model it as one single domain but with a momentum source term in a small region in the throat. Normally you can set the source term to zero so it does nothing, but when the throat constricts and gets close enough to closed that you want to shut the flow off you can activate the momentum source term to stop the flow.

[mrkmrk]

Hi Glenn

Sorry for my late response.

Altering the elements smoothing parameter worked! Thank you very much.

About the momentum sources term; if I got it correctly, you are suggesting the use of a sink so as to suck the flow up. I think it will change the flow pattern in a different way that placing a wall will do. However, it can obviate the interface problem because in this case there is no need to use two different computational domains.

Best

[ghorrocks]

No, I did not propose a momentum source to suck up the flow. A momentum source cannot do that anyway, that would require a mass source term. I was proposing to use a momentum source term to make the velocity of the fluid in the throat zero, which will stop the flow.

And yes, the point of this suggestion is that it means you do not need the interface in the throat.

[mrkmrk]

Um, it will act like a Dirichlet boundary condition. This solution will work like a panacea for my problem!
However I don't know how to implement it yet. I am going to give it a try in this week.

Thanks a lot.

Warm wishes.
David

[ghorrocks]

This solution will work like a panacea for my problem!

I know, That is why I suggested it . But I won't take credit for it, it is a well known way of dealing with meshes which close up and pinch off the flow. It is just when you have been in CFD for a long time you learn a few tricks.

You implement it with a small source region defined in the throat. Set the momentum source terms to what is defined in eqn 1-16 here: https://www.sharcnet.ca/Software/Ans...iSourType.html

where u/v/w (spec)=0. Then put the source term in an if statement so you can turn it on and off. Set the source term coefficient and it should work fine.

[mrkmrk]

Hi Glenn

I am really sorry for my late response.

Your help is highly appreciated. I really didn't expect it.

Best regards,
David.

[katty17]

Hi all,

I want to simulate the water flow inside a cubic duct. This is a case study prepared for the final complicated simulation. In the middle of duct I placed a subdomain to obstruct the fluid flow at the time t_c by using the method described in the aforementioned posts. The inlet boundary condition is set to opening pressure with the magnitude of 60mmHg and the outlet boundary condition is set to entrainment with the magnitude of 80mmHg. All the specific components of general momentum source are set to zero. By using an expression the value of source term coefficient (C) is gradually increased from -10^5 to -10^450. The problem is increasing the value of this parameter to such a huge value does not obstruct the fluid flow at all. However by using another set of boundary condition, i.e., using velocity inlet with the magnitude of 0.001m/s as the inlet boundary condition and using entrainment boundary condition with zero magnitude static pressure as the outlet boundary condition, a value of -10^14 for the parameter C can stop the fluid flow.

Please help me to fix this problem.
Best.

[ghorrocks]

The source term coefficient does not affect the flow in a converged solution, it only affects convergence. The source terms are the ones which affect the flow.

[katty17]

Hi Glenn,

Thanks for your consideration.

Based on the post #8, in the general momentum source tab, I set the values of U_spec, V_spec, W_spec to zero and by using a expression increased the value of momentum source coefficient gradually. Do you mean that I should enable the continuity option and then set the values of source terms including mass flow source and velocity components (U,V,W) too?

Best

[ghorrocks]

No. Momentum sources and continuity sources are totally different.

Can you post your CCL or output file?

[katty17]

The attached file contains CCL file. Due to the size limit of forum I uploaded the output file into a website which its link is also attached. Please take a look at them. The utilized expression modifies the value of source term coefficient as is shown in the attached figure.

Many thanks in advance.

Attachment 63590

http://s000.tinyupload.com/download....18373583129189

[ghorrocks]

In your momentum source term you have set the XYZ sources to zero but set a momentum source coefficient. Why have you done this? This will do nothing as the source terms are zero.

I suspect you actually want to set the X source terms to -C*(u-0), or in other words -C*u; and the Source Term Coefficient to C, and then set C to 1e6 or something like that. This will set the u velocity to zero in the source region. Is this what you wanted to do?

[katty17]

Thank you Glenn. I really appreciate your time and consideration.

I am really sorry for this awkward mistake. Without considering the units, I thought we should enter the values of specific momentum velocities.

Best wishes,
Katty

[ghorrocks]

No problem, the forum is here to help sort things out.

Have a look at the CFX documentation (Theory guide) for where the source terms come from. This will give the background about how the source terms fit into the modelled equations and will hopefully make things clearer.

[katty17]

Hi Glenn,

Yeah, sure. Thanks for your valuable information.

Best wishes,

Katty

[katty17]

Hi All,


I want to model a transient water flow inside a straight tube. In the middle of this tube there is a valve that closes the fluid flow path at a particular time point during the simulation by using the general source term of a subdomain which is positioned in the location of the valve. The inlet boundary condition is set to opening pressure inlet, and the outlet boundary condition is opening pressure outlet with Entrainment option selected for its mass and momentum option along with the specified static pressure waveform. There are two problems with this simulation.


1. During the valve closure phase, when the value of the general momentum source term coefficient is increased gradually to 10^(10) [kg/(s*m^3)], a big pressure pulse is induced in areas located between the inlet boundary condition and the location of the valve. I know this may be a correct response of the flow to the sudden decrease in its velocity, but the magnitude of the pulse in something very bigger than what is happening in the reality (Reality: 80mmHg VS. simulation: 120mmHg).


2. After that the valve is fully closed, the pressure pulse oscillates unstably and this oscillations end up with an overflow divergence error. I studied the forum page: https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F, I am sure this error is not arising due to the mesh quality, initial condition, and time step size or double precision calculations. About the simulation set up; except the subdomain which is located in the location of the valve, all other settings are what we can observe in the real physics of the problem in hand. It should be mentioned that around the location of tiny subdomain there are two adjacent areas with high pressure value difference (about 22000 Pa).

Any suggestion and information in this regard will be highly appreciated.
Best,

[ghorrocks]

1) This pressure pulse is exactly what does happen. If the magnitude of the pressure pulse is incorrect then consider the accuracy of your valve model (ie the momentum source), the accuracy of your fluid domain and boundary condition location and whether pipe deformations need to be considered.

And once you have considered those issues, do a sensitivity analysis on convergence criteria, mesh size and time step size.

2) I have modelled water hammer and transient compressible waves many times so I can assure you CFX can model this type of flow well. If you are getting overflow errors then you need to check your mesh quality, time step size, convergence criteria and boundary conditions.

What does your comment about a tiny subdomain mean? I do not understand this.