[jpina]

Hello,

I'm carrying out a VOF simulation at the following geometry.



The velocity of the inlet is defined using a VOF wich gives a zero value at the wall and increases parabolically.

My problem is that the result gives illogical results like this for the VOF.



The entering polymer is in red and the air in blue.

Could you say to me why I receive such illogical results? My common sense says that the fluid schould advance in a normal way filling all the model, not giving this weird shapes.

If you need more information about the simulation please ask it and I will post it without problems.

Help in advance.

[hwet]

Is the right wall an outlet or a wall as well?

If you are talking about the vf in red on the left it might be due to improve initial conditions. Regarding the interface shape on the left I dont see why you think it is not right.

Probably save your solution at several timesteps as the simulation proceeds to see the flow pattern or make an animation as the solution proceeds.

From your velocity profile at the inlet the fluid at the bottom travels at a greater velocity and hence the shape, there is a dam break tutorial for VOF available on ansys portal, probably give it a go.

[jpina]

Dear hwet,

First of all thanks for your answer, I appreciate it since I’m worried about my simulation results.

The right wall is a pressure outlet which is set to 0 Pa with a backflow volume fraction for the polymer of 1. What I do not understand is why is there such a backflow of the polymer, if there is no polymer there! In any case, it should be the air giving the backflow! Should I set the backflow volume fraction of the polymer to 0?

I do not understand why you think that the shape is right. My common sense says that the simulation should show how the model is filled of polymer from left to right, without creating any weird shape. But well, maybe the reality is what is shown!

In fact, what I am simulating is a submodelling of a macro simulation. I mean, the heigth of the model is 300 nanometers, and the velocity in the inlet is obtained from a previous simulation. What we are simulating is how the fluid would fills the sinusoid shape, which emulates the roughness. Do you think I should use some other boundary conditions for simulating this?

Thanks a lot hwet!

[hwet]

The right wall is a pressure outlet which is set to 0 Pa with a backflow volume fraction for the polymer of 1. What I do not understand is why is there such a backflow of the polymer, if there is no polymer there! In any case, it should be the air giving the backflow! Should I set the backflow volume fraction of the polymer to 0?

Back flow will only be taken into consideration IF there is a reversed flow occurring. With specifying 1 as the polymer back flow fraction if there is any backflow which occurs it will be only polymer and vice versa.

I do not understand why you think that the shape is right. My common sense says that the simulation should show how the model is filled of polymer from left to right, without creating any weird shape. But well, maybe the reality is what is shown!

The picture you have shows the volume fractions of the two phases at a particular time which you specified. For the simulation to reach steady state you will have to simulate enough timesteps so that the solution does not change anymore. If you will like to see how the flow proceeds, you will have to save a picture say at every 5 timesteps for example and then use animation to see the flow building up which will connect all the pictures together. This has been discussed in this forum before so you can search about it.

In fact, what I am simulating is a submodelling of a macro simulation. I mean, the heigth of the model is 300 nanometers, and the velocity in the inlet is obtained from a previous simulation. What we are simulating is how the fluid would fills the sinusoid shape, which emulates the roughness. Do you think I should use some other boundary conditions for simulating this?

Not sure what you are asking in this. What is the objective of this simulation? Also if it is 300 nanometers is the flow even turbulent? What turbulence model are you using?

[jpina]

Back flow will only be taken into consideration IF there is a reversed flow occurring. With specifying 1 as the polymer back flow fraction if there is any backflow which occurs it will be only polymer and vice versa.

I'll change the backflow fraction to be the air, it would have more sense to have back flow of air than of polymer.

The picture you have shows the volume fractions of the two phases at a particular time which you specified. For the simulation to reach steady state you will have to simulate enough timesteps so that the solution does not change anymore. If you will like to see how the flow proceeds, you will have to save a picture say at every 5 timesteps for example and then use animation to see the flow building up which will connect all the pictures together. This has been discussed in this forum before so you can search about it.

I made this, but I wanted to show what it is, at my point of view, a weird result...

Not sure what you are asking in this. What is the objective of this simulation? Also if it is 300 nanometers is the flow even turbulent? What turbulence model are you using?

The aim of the simulation is to study how the polymer fills the sinusoid shape, which symbolizes the roughness.

I am not using any turbulent model, the velocity is very low and therefore I consider the fluid to be laminar. Am I right?

------------

I keep thinking that I obtain illogical results, I expected to obtaing something like a flow going through a pipe, and instead of this I get this shapes... It might be right though!

[hwet]

Is your simulation transient?

You have to let it run for enough timesteps for it to reach the state you want.

[jpina]

Hi hwet,

yes, it is a transient simulation.

It is currently calculating (due to the fact that I create the velocity inlet interpolating from the macro simulation results it is something slow). I'll text you when it gets to the final state.

Anyway, do you think that the boundary conditions I am using are the logical ones for the simulation I am carrying out?

Thanks a lot for your help!

[hwet]

yes they seem fine, remember you can use initialization to speed up the convergence and/or use adaptive time stepping

[jpina]

I'm already using adaptative time step.

I'll give a try with the initialization

I keep you up to date!

[jpina]

Hi hwet,

I've carried out the simulations and I do not reach the steady state because I only have data for simulating the velocity inlet for the two first seconds.

Anyway, what bothers is that the shapes I obtain are pretty weird, look at the series:



And what I expect is something like this:



I mean, am I wrong by thinking that the filling of my geometry should be like I showed in the previous image? I mean, I am simulating how the fluid goes through a region near the wall!

Thanks a lot for your help!

[hwet]

With the velocity profile you showed in the first picture it is obvious that the fluid at the bottom will flow quicker.

From the pictures you posted now of how you want the profile to be it appears that the velocity across the inlet is all the same.

I believe you have gravity on? Then why shouldn't the fluid move downwards as well?

To get what you have in the picture, i think you should turn of gravity and have another look at the inlet velocity profile, i dont think the profile you have will give you the results you want.

Again, the solution is an iterative process after all, you should get what you have been getting until you reach a steady state unless you provide the solver enough details so it can have a jump start.

Also, check your fluid densities as well. What is the density of the polymer you are using? Check the orientation of the axis. Which way is the gravity acting? are you sure that the gravity is acting in the same direction the gravity should be acting on the geometry in the simulation (dont just assume it will be acting downwards).

these are just some troubleshooting ideas, other things could be wrong as well. But again I dont see why you shouldn't get what you are getting by the inputs you have given the solver. I would expect that unless you force the solution to be how you actually want it by changing the parts I have mentioned above.

Also make sure, the top boundary is a wall, maybe you have made it an outlet too.

[jpina]

Dear hwet/everybody,

let me ask you the following:

Wonder a fluid entering a pipe. How is it supposed to fill the pipe if the velocity on the walls is zero? Using a parabollic inlet velocity profile (the one of a developed flow), wouldn't it fill only the center region?

Thanks a lot!

[hwet]

The wall is not moving and hence theoretically the fluid molecules right next to the wall have 0 velocity. This is happening at microscopic level, away from the wall the fluid velocity increases dramatically.

In cfd since we know that at the wall the velocity is actually 0 and increases going away from the wall exponentially so we used wall functions instead of having an extremely small mesh at the wall which will be able to capture the fluid right next to the wall (which is not possible computationally).

The fluid fills the pipe as the velocity is 0 at the wall only and not elsewhere. This is more of a general concept which you can make up in your mind just imagining what is going on. The parabolic velocity profile you normally see is greatly exaggerated to explain/show the idea. It doesn't mean that half the pipe has 0 velocity.

Also, were you able to sort the previous problem out?

[jpina]

Dear hwet,

I haven't solved the problem... I am trying to understand why using a inlet exported from a macro simulation I doesn't fill my model. In the reality, the interphase has a zero velocity in the wall and increases in the center and even though fills the model.

[Jehosh]

Did you ever check hwet suggestion about gravity being on? Also, it makes sense to me that it would only fill the middle first as there is no resistance there, especially with the parabolic velocity profile. I was getting similar stuff in some work I am doing on a laminar falling liquid film trying to track the free surface. I had to use a wall adhesion model to get it the initial setup to work. Do you know the contact angle of your polymer? I think without that, the fluid will just be forced away from the no-slip condition. Just a thought. Let us know if that works. I am keen to know as well. Having a rough surface like you have is the next step in my research.

[jpina]

Dear Jehosh,

I turned gravity on and it has little or no effect on the simulation result.

Maybe I should use wall adhesion and see if it makes a difference.

I'll keep you up to date.

Thanks a lot!

[jpina]

Hello,

I tried turning on surface tension and wall adhesion but the simulation crashes because the Courant number increases suddenly.

I have tried different surface tension constants (0.1, 1... N/m) and different contact angles, but crashes whatsoever.

I am actually carrying out a submodeling simulation, so I am interested in really simulating the flow without wall functions. How could I do this?

@Jehosh, I understand that you think that turning on wall adhesion the polymer would fill all the model?

Thanks a lot!

[Jehosh]

I'm not sure. I am a bit of a newbie to this simulation world myself, just what you are doing looks very similar to my setup that I got to work. A few more things you could try and if it converges, build back up:

1. Make the wall slip so see if that is the problem.
2. Use implicit formulation (which is bounded, not limited by Courant number). There have been some updates recently that make implicit as accurate or more accurate that explicit if you use the right settings. I have been using a presentation from Ansys by Jinwon Seo as a guide titled "Multiphase Flow Modeling with Free Surfaces Flow". Has excellent best practices. If you can't find it, I can attach it to the next correspondence. Not sure if I am allowed, though, by the forum rules...
3. Use water instead of your polymer to see if viscosity is the problem. Water surface tension ~0.072. In my reading, high viscosity needs special treatment. Again, i'm no expert.
4. decrease your URFs? Decrease you time step? I had some issues with adaptive time step. Start with 1e-5s

Just some thoughts. Keep me updated.

[jpina]

[*]Make the wall slip so see if that is the problem.

No difference.
[*]Use implicit formulation (which is bounded, not limited by Courant number). There have been some updates recently that make implicit as accurate or more accurate that explicit if you use the right settings. I have been using a presentation from Ansys by Jinwon Seo as a guide titled "Multiphase Flow Modeling with Free Surfaces Flow". Has excellent best practices. If you can't find it, I can attach it to the next correspondence. Not sure if I am allowed, though, by the forum rules...

I tried it some time ago and dismissed it because the implicit method doesn't give a sharp interface.
[*]Use water instead of your polymer to see if viscosity is the problem. Water surface tension ~0.072. In my reading, high viscosity needs special treatment. Again, i'm no expert.

Using water the results are somehow different but essentially the same.
[*]decrease your URFs? Decrease you time step? I had some issues with adaptive time step. Start with 1e-5s

In order to avoid this I use adaptative time step with Courant number limited to 2.

[Jehosh]

The implicit method does give a sharp(er) interface if you have the right settings. In Ansys' own documentation (that presentation), it looks sharper to my eye. Although, I haven't played around with explicit too much because it was working with implicit and I do have a sharp interface.

About the time steps, until you have a solution that converges well, I like having control, i.e. not using adaptive time steps. Adaptive time stepping has caused me problems in the past for initial cases before I understood the physics completely. I could have been using it wrong, though.

If you are desperate, you could send me your case file and I could have a look at it.