[cTaH]

Hello everyone,

As a part of my uni work I was suggested to look into the possibility of implementing relative motion in a steady state simulation in CFX. Basically I have a 1 mm thick 2D channel with top and bottom non-slip walls created using sweep mesh option. The inlet velocity was specified as 0.5m/s and it is a laminar flow.
Also there is a constant heat flux to the bottom of the wall.

1) I run the simulation 1st time and export the achieved outlet velocity profile to the inlet to get fully developed flow throughout the length of the channel.

2) I run simulation one more time and then export the outlet temperature profile and using dimensionless temperature difference and the equation Q=h(Tw-Tm) I am finding the approximate temperature profile for inlet and exporting it there. Getting pretty constant result for heat transfer throughout the whole channel.

3) Now I subtract the mean flow velocity from the inlet velocity profile. AND I AM MOVING BOTH WALLS IN DIRECTION OPPOSITE TO INLET WITH THIS MEAN VELOCITY. ( I am using openings at both sides)

As I was suggested this should work but in fact I am not getting any reasonable results and it seems that CFX is just trying to reverse the flow. And now there is a larger temperature at the inlet instead of the outlet.

I am attaching screenshot of the channel and the graphs of temperature before and after moving the walls. Can somebody suggest if what I am trying to do is possible and actually makes sense? I am doing to in order to progress with the further step.


I also attached the screenshot of what I am trying to do. I am trying to simulate a disturbance wave in an annular flow. An since in that configuration I cannot give the wave a velocity I have to move the bottom wall at the negative wave velocity and put the film inlet from the opposite side. But I was trying to make it work for so long I am not sure this is possible. So crying for help

By saying I am trying to make it work I am saying I am trying to get same or at least close results in heat transfer to the normal motion case.



Thanks for your attention.

[ghorrocks]

I think what you are trying to do is to use a translating frame of reference at the velocity of the wave so it becomes a steady state flow. Is that right?

This will be difficult as even a tiny numerical difference in the conditions will mean your flow is not exactly the velocity of the wave. This means the wave will move and it will never converge as it is not steady state.

If I understand you correctly a better approach will be to just most a stationary frame of reference and allow the wave to move at its own velocity.

[cTaH]

Originally Posted by ghorrocks

If I understand you correctly a better approach will be to just most a stationary frame of reference and allow the wave to move at its own velocity.

Thank you for you reply. I was trying to move the wave along without the air present but I was not able to able to achieve any reasonable results for translational motion. what I was doing.

1) Set up regions of mesh deformation specified for the wave. Set up a displacement in the x direction for the wave outer boundary. And also select a parallel to boundary movement option for the interface.

2) Then in the domain initialization I gave the velocity in x direction to the wave.

However, when I was trying to run it it could move along sometimes but there was no flow in the film present and the values of velocity shown for the wave were huge like something *10^12. So something was crashing. Also sometimes it just gives an overflow error.

I am sure simple translational motion along the boundary without deforming the mesh should be possible. I just wasn't able to implement it. So if you could suggest what is the procedure for that that could be great.

Thanks.

[ghorrocks]

This sounds very strange and I do not understand what you are doing. Why do you need moving mesh? Why don't you use a multiphase model to capture the wave?

[cTaH]

Thank you for your reply.

Sorry, I am trying to move the wave across the film and not getting the appropriate results. What would be another option to implement this without using a deforming mesh?

Deforming mesh doesn't work for me anyway. I am giving wave boundaries a displacement. And then a velocity to wave domain. However this is producing no result as it was mentioned previously.

The main idea here is that the film is slow and the wave has to move fast across. E. g. film has a velocity of 0.5m/s. Then I specify top wall of the film as no slip and trying to move a wave along it with velocity of 3m/s. I didn't find any description of how I could apply this kind of translational motion in CFX. Is there a special interface setting I need to set?

Basically if I could leave the film as just a film with inlet and outlet and then somehow slide this wave on top of it along a straight line that would solve all my problems. Is it possible? I am sorry for my bad explanations I am really new to CFD.

[ghorrocks]

Is this a two fluid flow? So air and a liquid? So are the film and wave are the same fluid?

[cTaH]

Originally Posted by ghorrocks

Is this a two fluid flow? So air and a liquid? So are the film and wave are the same fluid?

Yes, the wave and the liquid is the same fluid. Just specified as 2 different domains which need to have different velocities. (wave should slide along the film on top of it and the film is just with inlet and outlet really)

Ideally I would also want air domain as it was shown on the drawing. But for now I guess moving the wave along the film domain is the main task. (simple translational motion in the X direction)

Thank you.

By the way in order to create the air domain I had to disable constant domain physics in beta features.

[ghorrocks]

OK, I understand what you have done now.

It would appear the way to simulate this would be with a free surface multiphase model. Then the entire domain is a single domain, and the mesh does not move. From your geometry it looks like the mesh will just be a rectangular box so meshing is trivially easy.

Then the motion of the wave, film and everything else will just be modelled as motion of the free surface.

Or is there some reason why this approach is not suitable?

[cTaH]

Originally Posted by ghorrocks

OK, I understand what you have done now.

It would appear the way to simulate this would be with a free surface multiphase model. Then the entire domain is a single domain, and the mesh does not move. From your geometry it looks like the mesh will just be a rectangular box so meshing is trivially easy.

Then the motion of the wave, film and everything else will just be modelled as motion of the free surface.

Or is there some reason why this approach is not suitable?

Thank you for your reply.

Sorry, are there any tutorials explaining how to model a free surface? And also the problem is if I model this as a free surface how would I specify the movement of the wave the film and the air separately. I could exclude air for now and try to just simulate the wave movement.

And the idea is to model the wave geometry. So I could move it along. If divide the inlet into 2 parts with air flow and film flow I would get some flow it would not have the wave to analyse. I am trying to see what effect waves have on heat transfer compared to the case with no waves. From the concept of free surface I would have film and air at inlet but I have no idea how to incorporate a wave shape into that.

Could you please elaborate on how to move these parts with different velocites and define their geometry in this free surface domain.

Is there absolutely no way to slide the wave domain along the film?

Thank you.

[ghorrocks]

The free surface flow over a bump CFX tutorial is an example of a free surface simulation.

The answer to your other question depends on what you want to do. I suspect that this flow will automatically form waves of its own accord. So the case with no waves is artificial, it does not exist. Also your wave geometry is artificial, I am sure the real geometry is more complex than that and will evolve with time. So you are asking what is the heat transfer difference between an assumed artificial wave shape and an artificial flow when the waves which would form are suppressed. This question appears to be of academic interest only - I would concentrate on what really happens rather than making assumptions on what happens.

But if you really want to model your assumed flow, I would use moving mesh to move the assumed wave shape, but use a GGI at the top of the film to attach the top air/wave region to the bottom film region. So the mesh motion is just a translation, no other complex motion is required.

[cTaH]

Originally Posted by ghorrocks

The free surface flow over a bump CFX tutorial is an example of a free surface simulation.

The answer to your other question depends on what you want to do. I suspect that this flow will automatically form waves of its own accord. So the case with no waves is artificial, it does not exist. Also your wave geometry is artificial, I am sure the real geometry is more complex than that and will evolve with time. So you are asking what is the heat transfer difference between an assumed artificial wave shape and an artificial flow when the waves which would form are suppressed. This question appears to be of academic interest only - I would concentrate on what really happens rather than making assumptions on what happens.

But if you really want to model your assumed flow, I would use moving mesh to move the assumed wave shape, but use a GGI at the top of the film to attach the top air/wave region to the bottom film region. So the mesh motion is just a translation, no other complex motion is required.

Thank you. But the problem is even when using GGI I cannot move the wave along and get reasonable results. When I specify wave dispalcement it moves the way along but no motion of cluid occurs in film domain and the wave speed is very 3X10^12 instead of 3m/s. Should the top wall of the mesh set as non slip? Or what type of interface would allow moving the wave.

[cTaH]

Originally Posted by ghorrocks

The free surface flow over a bump CFX tutorial is an example of a free surface simulation.

The answer to your other question depends on what you want to do. I suspect that this flow will automatically form waves of its own accord. So the case with no waves is artificial, it does not exist. Also your wave geometry is artificial, I am sure the real geometry is more complex than that and will evolve with time. So you are asking what is the heat transfer difference between an assumed artificial wave shape and an artificial flow when the waves which would form are suppressed. This question appears to be of academic interest only - I would concentrate on what really happens rather than making assumptions on what happens.

But if you really want to model your assumed flow, I would use moving mesh to move the assumed wave shape, but use a GGI at the top of the film to attach the top air/wave region to the bottom film region. So the mesh motion is just a translation, no other complex motion is required.

So this is what I am trying to do. Move the box along by 20mm with a speed of 3m/s but it is either giving an overflow error or moving the box along but removing all liquid from film domain and velocity of the box is shown then as 3*10^12 something.

[cTaH]

While the previous question still stands I am trying to use free surface approach. Any suggestions which turbulence model would give best convergence and possibly create a wavy interface?

[ghorrocks]

The moving mesh method of doing this is contrived, artificial and I can't see why anybody would want to do it. That is why you are finding it difficult to implement

Viscous action in the wave/film is what controls the wave speed. Your suggested approach means you need to work this force out for yourself or the wave will zoom off at ridiculous speed (as there is no force to act against the air pushing it, and in a steady state flow an unbalanced force means things accelerate to ludicrous speed straight away).

So if you want to do a lot of development work in this feel free to try to develop a model for this force to react against the air force. Sounds like a waste of time to me.

Multiphase model: Only implement a turbulence model if the flow actually is turbulent. What is the Re number this is running at? That will tell you if it is turbulent or not.

And I think you will find that waves will automatically form on the interface when you are correctly modelling it. That is how ocean waves work, when the wind blows the waves just start forming.

[cTaH]

Thank you for your reply! Now I see why the translation wasn't working for me =) I will try to implement a free surface approach and will see what results I will get. Might as well look at the flow as a whole instead of modelling the waves separately if it works fine.