[Franke]

Hello,
I am completing a project using Ansys Fluent and could really do with some help. A few details first;

I am modelling a multiphase domain around a body, I have used symmetry to half the domain and body, it is multiphase flow of both air and water with an inlet speed of 1.03m/s and using a pressure outlet. The body is set as a wall, the lowest surface is wall and other than inlet or outlet the rest are symmetry.

I am trying to study the drag force and coefficient acting on the body, I plan to do this several times for slight alterations on the body to see how they compare. however I have run the simulation and the values i'm so far recieving to drag coefficient are around -6x10^13, and for drag force around -3x10^13. these are very clearly incorrect.
My contour plot of the phases is also showing very abnormal results which are not desired at all.

Please if anyone can help this is a report due very very soon. thank you

[vinerm]

In a multiphase flow, the only boundary that can act like a symmetry is one with its normal perpendicular to the gravity vector. So, first aspect you need to ensure is that any other boundary is not taken as symmetry.

Secondly, if you have only one inlet, is it liquid coming in or gas? In case it is VOF, you cannot have both coming in. If it is mixture or Euler-Euler, then it is alright. You also have to ensure that the operating conditions are properly set, i.e., the operating density, this should refer to the density of the lightest material, and reference location for the operating pressure, this has to be the highest point of the domain.

[Franke]

Hi, thanks for the quick reply.
I was wanting an inlet of both air and water to be entering the domain, opposed to this the key fluid is the water.
Would it be correct to change from VoF to Eulerian and then multi-fluid vof model? I want the surface of the water to be at -0.075m.

I have now changed the upper boundary to wall.

thanks

[vinerm]

Whether free-surface model is better or dispersed depends upon the real situation. If it is air carrying water droplets or water carrying air bubbles, then dispersed models (Euler-Euler or Mixture) are good. Otherwise, use VOF. If height of the water is more or less fixed, then you can use open channel flow.

[Franke]

It is meant to be a body on the surface of water with air above, i.e. simplified body of water. do you this the problems were all from incorrect use of symmetry? Should i still change the model or remain vof?

Thank you!

[Franke]

or is there a simplified way for me to change this to keep the domain size and have only water flowing through? The air is a non-essential part of it however i am interested in the changes in water surface as it meets the body also

[vinerm]

If the body is floating and the objective is to predict the forces due to the air flow on the body, then you can simply neglect the water and the part of the body submerged in the water, until the forces from the air are strong enough to make the body move within the water. In that case, you have to use Moving Mesh.

If it assumed that body position within the water is not disturbed by the air, then you can assume water surface as solid surface and only consider the part above the water for the body. Then, the case becomes single phase.

[Franke]

Thanks, very similar but I am actually studying the forces from the water. I intend to keep the body still and the flow of water over it. I do also want the water to be able to move as it meets the body so that the wake field can be shown. Do i simple turn off the multiphase model? Will this 'empty' the upper area?
I have been having some problems with this in different ways for a while and feel I have just gotten myself more confused over it

[vinerm]

If the objective is to consider the forces from the water, then you have to use VOF. This is because when water moves relative to the body, it rises up and dips down. In this case, you should separate the inlet into two boundaries. Use upper one for air inlet and lower one for water inlet. That would resolve the issue.

[Franke]

Is there an easier way to do this or do I have to go back and remake them as 2 seperate domain areas?

[vinerm]

You don't have to go back. You just need to separate the inlet into two boundaries. This can be easily done within Fluent. You can use Adapt > Iso-Value to mark the cells using the vertical coordinate and then use that register to separate the boundary into two.

[Franke]

Thank you so much for all your help, I will try this now!

[Franke]

Hi, sorry I don't have iso-value as an option, if I go to adapt i can only use refine/coarsen, ansitrpoic refinement or geometry... none of which seem to give me an option similar to what you have suggested

[vinerm]

Refine and Coarsen are available after selecting the option. However, if you click on Adapt Menu, and if the case is initialized, then you will see the option IsoValue.

https://www.afs.enea.it/project/nept...ug/node852.htm

[Franke]

So I think that I have managed it however the domain now won't patch through, so the interior is appearing as fully water... I used hybrid initialisation from the water inlet and patched through the water phase using a volume fraction of 1 on the fluid domain and the region that I created to split the inlet (this should cover all the water area)

I split the inlet at the level but both phases are still set as mixture.

Should I also separate the entire domain area? or will this prevent the water to be able to move around the body


My velocity inlet is only about 1 times the body away from it, does this seem far enough? It is a circular body made from pipes so while a large total area it does not take up as much space. I am kind of using the maximum of the student software so don't want to make it any bigger but could maybe reduce in other areas

[vinerm]

Do not use hybrid initialization with multiphase flows. You need to initialize using standard settings and then patch the secondary or primary phase. Keep the cell zone as one; only inlet had to be separated into two. Now, you can assign only water inlet at lower inlet and only air inlet at higher inlet. For patching as well, you can mark the cells using Adapt and then patch the register instead of cell zone. For this, you do not need to separate; just mark and then patch the register.

[Franke]

Hi,
So when I try to initialise the console is not updating with anything.
If I follow this with patching I am being told that 'zone not slit' and '0 cells marked' any advice on this? Thanks

[vinerm]

Let me explain using an example. I am assuming a geometric model with z-axis representing its vertical axis and minimum and maximum values for z are 0 and 1 m. If water is primary phase and its height in the domain has to be 0.35 m, then process is as follows

1. Initialize > Standard Initialization with Gas Volume Fraction as 1.0
2. Adapt > Iso-Value > Mesh > Z-coordinate. Compute. Use minimum 0 and maximum 0.35, and click on Mark.
3. Go to Patch, select the register in the right column. Do not select the cell zones. Choose Gas under Phase and then volume fraction. Use value of 0 and click Patch. This will patch gas volume fraction as 0 within the cells defined by register, i.e., cells with z-coordinate 0 to 0.35. A 0 volume fraction of gas implies 1 of water.

[Franke]

Thanks, I have the patching now I believe!

When I try to run the simulation I am getting a warning about my solution diverging and the global courant number is over 250. it suggests to reduce the timestep however my time step is already at 0.01s, the mesh i have is modelled to be quite large in some areas then further refined in particular areas of interest. Should I make my meshing more refined?
Thanks in advance

[vinerm]

It depends on the velocity as well. If you refine the spatial mesh, you will also have to refine the temporal mesh, i.e., you will have to use a smaller time-step. Even with current mesh, 0.01 s may be high.