[JackFischer]

Hello there folks,


I've met my final enemy, my David to the great Goliath... but from the beginning:


I'm doing a wading Simulation, meaning I have a car, going in and through a water trench. To do so, I use the overset mesh method, meaning, that the moving car is located in its own meshed region. That region is moved by the motion specification "Morpher" along a given path. Same is applied for the tires, which are also rotating.


To the physics:
The water is initialized by the VOF-model, namely a flat wave with a given water depth. There is no current velocity given, as the water trench is closed to all sides, more like a pond.
I used both k-epsilon and k-omega turbulence models, 1st and 2nd order, with and without resolved boundary layer, wall function, no prism layers at all, all y+ treatment and so on.. basically any sensible combination of the given choices.
Timestep is a reasonable 1e-3s and in different fine mesh approaches I used between 5 to 15 million cells in a 1:1 modell.



But here it comes: after initializing and sucessfully running the simulation for some time something weird happens. Down the trench, far from any oversetmesh or boundary condition (appart from walls) the y+ values on the wall explodes at a (seemingly) random point. Veloty magnitudes reach skyrocketting levels, resiudals go through the roof and the water litterally shoots in all directions starting from said point. There is no change in mesh size, no velocity to deal with, no phase change, nothing.


I guess (at this point, anything is just an assumption ) the turbulence modells, whichever I'm using, is struggling with the fact, that it is stillstanding water. Because of this I dont know exactly, how I should build the mesh near the walls. Using k-e and trying to be in the log layer or a resolved boundary layer with the k-w model, I have zero velocity at the wall because of the stagnant water, giving no sensible value for the first layer.


If anyone has any tips, guesses or questions to be discussed, I'm happy to share details and learn about this. I'll try to upload some pictures tomorrow as well, it's kind of tricky though because of restrictions from my company..


Anyway, have a good one, and maybe we can solve this one (=






BTW: it's actually like the JLR approach, looking like the following:

[cwl]

that the moving car is located in its own meshed region. That region is moved by the motion specification "Morpher" along a given path. Same is applied for the tires, which are also rotating.

Morpher? - Why not just Translation Motion and Rotation for wheels relative to the wheel coordinate system?

The water is initialized by the VOF-model, namely a flat wave with a given water depth.

It is advised for better stability to smoothen the initial Volume Fraction by few cells instead of setting sharp initial condition like

($$Position[2] <= 0.1) ?  1.0 : 0.0

Timestep is a reasonable 1e-3s

Courant Number?

after initializing and sucessfully running the simulation for some time something weird happens .. the y+ values on the wall explodes at a (seemingly) random point

That's why we love multiphase - #$@s up in a random cell where everything is ok %>

Did you try playing with URFs? - Like setting Velocity and Volume Fraction to 0.1:0.9?

[JackFischer]

Thanks for your insights!

Originally Posted by cwl

Morpher? - Why not just Translation Motion and Rotation for wheels relative to the wheel coordinate system?

Because its not a static motion in one direction but the direction is changing. I have to add, without the mesh motion the stability seems quite ok...

Originally Posted by cwl

It is advised for better stability to smoothen the initial Volume Fraction by few cells instead of setting sharp initial condition like

($$Position[2] <= 0.1) ?  1.0 : 0.0

Do I do this only in the initial conditions of the Pyhsics Continua or do I have to apply the same in all region physics?

Courant Number?

Thats another struggle, as stated above to find the correct wall distance with the water being at rest, the courant number tends to be zero.

That's why we love multiphase - #$@s up in a random cell where everything is ok %>

Did you try playing with URFs? - Like setting Velocity and Volume Fraction to 0.1:0.9?

I played with URF for velocity and pressure, but didnt notice that much of a difference in behaviour..

[cwl]

Because its not a static motion in one direction but the direction is changing. I have to add, without the mesh motion the stability seems quite ok...

Sure you know your case better, but
1) does it diverge if you set just a Translation Motion?
2) UserGuide says:

In fluid mechanics applications, you can move the mesh rigidly according to prescribed rotations and translations (Rotation, Translation, Rotation and Translation, Trajectory motions), or use the Morphing method that accounts for non-rigid deformations.

Maybe try Trajectory after that?

Do I do this only in the initial conditions of the Pyhsics Continua or do I have to apply the same in all region physics?

Well .. if you do not set any Region-specific Initial Conditions - i.e. Initial Condition settings from Physics are applied to all Regions, then just set it in Physics only.
The idea, once again, is to smoothen the initial liquid-air interface.
Can't guarantee that it will help - but it's a good practice anyway.

Thats another struggle, as stated above to find the correct wall distance with the water being at rest, the courant number tends to be zero.

Zero is ok where the liquid is still.
I meant more like maximum and average Courant number where motion of phases happens.

I played with URF for velocity and pressure, but didnt notice that much of a difference in behaviour..

I'd say - in multiphase simulations Volume Fraction URF is the one affecting stability the most.

[JackFischer]

Originally Posted by cwl

Sure you know your case better, but
1) does it diverge if you set just a Translation Motion?
2) UserGuide says:

Maybe try Trajectory after that?

Well I do not have any deformations becaus of the overset method, a mesh is moved through anoter mesh, being interpolated at the interface. I'd really like to stick with that approach, as I have exactly the movement I want and need. Dont know how to get to that with trajectory or any of the other.

Well .. if you do not set any Region-specific Initial Conditions - i.e. Initial Condition settings from Physics are applied to all Regions, then just set it in Physics only.
The idea, once again, is to smoothen the initial liquid-air interface.
Can't guarantee that it will help - but it's a good practice anyway.

I think I didnt get that right. In Physics -> Initial Conditions -> I have Volume Fraction -> Composite and put the equation you suggested in both phases. That produces an Error, I have to check my initial volume fractions in the regions, but no matter what I put in there doesnt work

Zero is ok where the liquid is still.
I meant more like maximum and average Courant number where motion of phases happens.

Ok, but how would I calculate the first cell height with zero velocity? Is it iterative, check solution and change cell height accordingly? I'll check the solution and come back for the Courant numbers.

I'd say - in multiphase simulations Volume Fraction URF is the one affecting stability the most.

Alright, do you mean the URF under Segregated VOF -> Single Step?

[cwl]

I think I didnt get that right. In Physics -> Initial Conditions -> I have Volume Fraction -> Composite and put the equation you suggested in both phases. That produces an Error, I have to check my initial volume fractions in the regions, but no matter what I put in there doesnt work

What I mean is - usually initial conditions for Volume Fraction is set like two Field Functions:

$$InitialVolumeFractionofLiquid
($$Position[2] <= 0.1) ?  1.0 : 0.0

$$InitialVolumeFractionofAir
($$Position[2] <= 0.1) ?  0.0 : 1.0

Which is discontinuous. What is recommended:

Ok, but how would I calculate the first cell height with zero velocity? Is it iterative, check solution and change cell height accordingly? I'll check the solution and come back for the Courant numbers.

Wait, Courant number is:

Thus - it can be calculated in cells based on your velocity, mesh size and time step and show how "good" your time step is, since target CFL (Courant number) is adviced to be ≤ 1.
Given mesh cells sizes and given velocity distribution (driven by physics and process) - one can estimate a target time step.

Alright, do you mean the URF under Segregated VOF -> Single Step?

Exactly. Try setting them to 0.1 and 0.9 .. might help.

[JackFischer]

I really appreciate your help here!

Originally Posted by cwl

What I mean is - usually initial conditions for Volume Fraction is set like two Field Functions:

$$InitialVolumeFractionofLiquid
($$Position[2] <= 0.1) ?  1.0 : 0.0

$$InitialVolumeFractionofAir
($$Position[2] <= 0.1) ?  0.0 : 1.0

Which is discontinuous. What is recommended:

I put these into the initial conditions for the physics contiuna, but no matter what I choose for the Volume fractions of the boundaries in the regions, the error "Please check your initial values for "Volume Fraction" in the following regions: ... " I seem to oversee something here..

Wait, Courant number is:

Thus - it can be calculated in cells based on your velocity, mesh size and time step and show how "good" your time step is, since target CFL (Courant number) is adviced to be ≤ 1.
Given mesh cells sizes and given velocity distribution (driven by physics and process) - one can estimate a target time step.

So far so good, of course I know about the Courant number, how its calculated and that for certain turbulence models/boundary layer treatments it should be less than one. But what I'm struggling with, is the fact that I cant calculate it for zero velocity, can I?