[Lapidus]

Good Day,

At the moment I am simulating the pass of an aerosol through a metallic container. This will obviously build a fluid film on the inner surface of the container by the fluid in suspension.

The simulation runs fine until it takes the fluid film into account, around step 50. They get a massive value ~1e23 (both normalized or not) and the run does not converge.

From the moment when the fluid film gets taken into account, the message
"Error: AMG solver diverged.
Turbulent viscosity limited on XX cells in Region"
gets displayed at every step. Moreover the following warnings arise every few iterations
"WARNING: Ap = 0 on multigrid level 1, nRows = XXXXX, blockSize = X
AMG coarsening halted."
"WARNING: insufficient precision on multigrid level XX, rows X
AMG coarsening halted."

Clearly something is wrong with the model, what is your suggestion on the best way to fix it? Have a better look at the prism layer?
I am runing it Steady, which permits to safe the particle´s paths in the track file for post-processing.

Thanks in advance and enjoy the weekend!

[me3840]

Is this wrapped?


It's been a while since I used fluid film, if you are using evaporation/condensation I believe there's an explicit relaxation in the physics you can apply to help calm things down.

[steve lee]

Hi,

Um... about 4 years ago, I simulated fluid film by injected fuel.
That time i also encountered divergence problem.
I solved that to control time step and mesh.

Fluid film solver require more mesh and small time step.

So, you try to control relaxation factor and mesh.

not use full model first.

try to simulate small part of whole model. And fine mesh size and relaxation factor.

[Lapidus]

It is wrapped since it was imported from a step file, @me3840.
Yet, there is no evaporation/condensation in reality, since the temperatures of the fluid and the container are pretty much the same. The energy equation has not been activated for that reason.

Everything that can be relaxed in the solver was set to 0.3 in the images attached in the Original Post, @steve lee. For now I am trying the fluid film to converge without taking into account wave stripping. I will reduce the time step, that was set at 1e-4, relax everything to 0.2 and give it another go.

[steve lee]

Is it steady? or unsteady?
If you simulate steady simulation, you should check it has reasonable condition for steady.

In my case velocity of injected fuel was about 160 m/s.
That time i used 1e-9 time step first, and i changed slowly.

[Lapidus]

Originally Posted by me3840

Is this wrapped?


It's been a while since I used fluid film, if you are using evaporation/condensation I believe there's an explicit relaxation in the physics you can apply to help calm things down.

Originally Posted by steve lee

Is it steady? or unsteady?
If you simulate steady simulation, you should check it has reasonable condition for steady.

In my case velocity of injected fuel was about 160 m/s.
That time i used 1e-9 time step first, and i changed slowly.

Hello,

Since the last post, I have refined the mesh as well as the prism layer, now standing at 18M cells.

I would like to run the simulation as steady, since this is the only way I get the particles to overwrite the track file. Also, the fluid film monitors (film continuity, X/Y/Z momentum) only appear in the residuals monitor for the steady simulation.

With this in mind, I let the simulation run as implicit unsteady and it converges nicely (no traces of the fluid film this far), at that point I switch to steady. After a few iterations in the steady mode the residuals of the fluid film appear and shoot up to 1e40+ (not normalized). Same story if I decide to simulate everything as steady from the beginning.

Am I overseeing something here? Any clue what could be messing up/missing in the simulation?
Thanks beforehand, fellas!

[tisa]

Originally Posted by Lapidus

Hello,

Since the last post, I have refined the mesh as well as the prism layer, now standing at 18M cells.

I would like to run the simulation as steady, since this is the only way I get the particles to overwrite the track file. Also, the fluid film monitors (film continuity, X/Y/Z momentum) only appear in the residuals monitor for the steady simulation.

With this in mind, I let the simulation run as implicit unsteady and it converges nicely (no traces of the fluid film this far), at that point I switch to steady. After a few iterations in the steady mode the residuals of the fluid film appear and shoot up to 1e40+ (not normalized). Same story if I decide to simulate everything as steady from the beginning.

Am I overseeing something here? Any clue what could be messing up/missing in the simulation?
Thanks beforehand, fellas!

Steady fluid film model doesn't work and it's known by Siemens. I had a lot of contact while doing my masters thesis (SCR simulation). The fluid film model is not meant to be used steady.

Edit: You !have to! activate "Stabilized Film Thickness Equation" if you want to use the Film Model in steady mode. I doubt it will help, but give it a try.

[Lapidus]

Originally Posted by tisa

Steady fluid film model doesn't work and it's known by Siemens. I had a lot of contact while doing my masters thesis (SCR simulation). The fluid film model is not meant to be used steady.

Edit: You !have to! activate "Stabilized Film Thickness Equation" if you want to use the Film Model in steady mode. I doubt it will help, but give it a try.

Hey tisa, thanks for your input! Once the "stabilized film thickness equation" is selected the fluid film residuals converge, both for impingment and wave stripping. So thanks a lot for the suggestion!

There are only two drawbacks I have noticed. The first one is about the fluid film itself. When I select to view it, the scalar representation shows me as if the whole shell was covered in a homogeneous fluid film with its thickness taking the value of the max allowed thickness in the settings (0.1m). For what is being simulated, that seems like too thick of a film and that distribution doesn´t seem reasonable´(image is attached below). Any guesses what might be going on?

The second hurdle comes written in the output box every time step.
"Volume fraction of Lagrangian phases limited to 0.75 in XXXXXX cells in Region", please note that the cell number is in the hundreds of thousands (image attached below). Does this mean my settings are limiting the amount of volume the film layer can take up in a single cell and therefore distorting the results? Would changing the value of the maximum volume fraction to 1 under the two-way couplíng options of the solver take care of this message?

Thank you once more, fellas, your support is all one can ask for

[tisa]

Originally Posted by Lapidus

Hey tisa, thanks for your input! Once the "stabilized film thickness equation" is selected the fluid film residuals converge, both for impingment and wave stripping. So thanks a lot for the suggestion!

There are only two drawbacks I have noticed. The first one is about the fluid film itself. When I select to view it, the scalar representation shows me as if the whole shell was covered in a homogeneous fluid film with its thickness taking the value of the max allowed thickness in the settings (0.1m). For what is being simulated, that seems like too thick of a film and that distribution doesn´t seem reasonable´(image is attached below). Any guesses what might be going on?

The second hurdle comes written in the output box every time step.
"Volume fraction of Lagrangian phases limited to 0.75 in XXXXXX cells in Region", please note that the cell number is in the hundreds of thousands (image attached below). Does this mean my settings are limiting the amount of volume the film layer can take up in a single cell and therefore distorting the results? Would changing the value of the maximum volume fraction to 1 under the two-way couplíng options of the solver take care of this message?

Thank you once more, fellas, your support is all one can ask for

That is exactly the problem you face with the Fluid Film model. It's broken and Siemens knows it. They said "it's not meant to be used in steady mode, because a fluid film is highly unsteady". For me it's ironic they've implemented the film model in steady mode and that they've even a option to activate (stabilized film...) even so the model doesn't work.



I've tried A LOT of different settings in my masters thesis and the conclusion I got is: Fluid Film works only unsteady, if the film is small enough (height) and it doesn't hit sharp edges.
Also the film height should never be higher than the cell where the (film) shell is located. If you want to simulate a thick film, you should use the VOF model.


Sorry I don't have better news from my side.