CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Fluent Multiphase (http://www.cfd-online.com/Forums/fluent-multiphase/)
-   -   Eulerian Wall Film model with Eulerian disperse phase (http://www.cfd-online.com/Forums/fluent-multiphase/118057-eulerian-wall-film-model-eulerian-disperse-phase.html)

michujo May 20, 2013 12:01

Eulerian Wall Film model with Eulerian disperse phase
 
Hi all, I am trying to simulate the water droplets impact on a solid wall and the formation of a liquid wall film. The continuous phase is air and the disperse phase is liquid water (I use the eulerian approach for the multiphase flow, not DPM). The wall film is taken care of using the Eulerian Wall Film model. The Fluent version I'm using is the 14.5.7.

Following indications from the on-line documentation and customer support engineers I set up a dummy DPM injection with the name of material the same as the material of the disperse phase, to which the string "-particle" is attached. Finally I initialize the film variables in Models/Eulerian Wall Film and hit calculate.

I observe max_cfl=0 in Fluent console during the calculation and I obtained null values of all the film variables (thickness and velocity). The model is not collecting any mass from the eulerian dispersed phase.

Has anyone else come across this problem and knows how to proceed?

Thanks a lot in advance.

Cheers,
Michujo.

menjya June 12, 2013 16:36

Hi, Michujo,

I am also trying to use Eulerian Wall Film model in Fluent v.14.

But, each time, I got warning as below:

Warning: Unable to initialize Eulerian Wall Film model

I do not understand why you need a dummy DPM injection ?

Could you please give me some explanation how to initialize EWF model successfully?

Thank you very much!

menjya

michujo June 13, 2013 07:25

Hi, my model is finally running (having contacted Ansys customer support numerous times though). Here are some tips:

- Go to Boundary Conditions and:
1) Go to the wall where you set the EWF
2) Go to the Wall Film tab
3) Enable the wall film
4) Change the default "Boundary condition" to "Initial condition" and set all to zero.


- Go to Models/EWF and hit initialize, otherwise the film won't do it.

- Bonus hint: in Models/EWF set the minimum film thickness to zero. Otherwise you might get null values of the film variables all the time. I spent a large amount of time figuring this out until I finally discovered it by chance.

The dummy injection is necessary in case you want to account for the detachment of the liquid film from the solid surface into discrete droplets. That's why you need to enable first the lagrangian droplets model.


Cheers,
Michujo.

menjya June 13, 2013 11:50

Thanks for your good advice, Michujo.

My model is working now.

Far June 13, 2013 12:17

Good Info. Thanks for sharing.

Marbau July 8, 2013 09:47

Hi,
I also try to simulate the impact of water droplets on a solid. Like you, I use the Euler-Euler model, with air as the primary phase and water-liquid as the secondary phase (diameter 5e-06 m) and the Euler Wall Film model. Also if I follow the guideline you posted no wall film occurs.
Could you please explain step-by-step how you set your simulation up or at least the most important steps?

Thank you!!

michujo July 8, 2013 10:16

Hi, what do you mean "no wall film occurs"? Do you mean that you get null values of the wall film variables (film velocity and thickness)?

Cheers,
Michujo.

Marbau July 8, 2013 10:19

Yes, that's what I wanted to say.
Sorry for that bad formulation.

michujo July 8, 2013 16:30

No worries. Did you try the procedure proposed above? specially the part where you set the minimum film thickness to zero?

Cheers,
Michujo.

Marbau July 10, 2013 05:08

I did it like you described it. But probably I made a mistake. That was my procedure:
1. transient calculation
2. enabling Euler-Euler approach
3. enabling Euler-Wall-Film (at this point it is the only thing I did)
4. defining the phases (air primary phase, water-liquid secondary),
Interaction: universal-drag, surface-tension-modeling with enabled wall adhesion (surface tension coefficient: 0.07941)
5. setting the boundary condition at the wall where I want to investigate the wall film (turning on Eulerian Wall Film, switch to initial condition with all values as 0)
6. at models (see point 3) I set the wall film material "water-liquid" and minimum film-thickness to 0. Then I initialize.
7. defining the inlet boundary (velocity-inlet)
8. then solution initializing and starting the simulation

Well, I have to admit that I don't really know what functions I have to enable at Euler-Wall-Film, or rather what the single functions really do. So I kept it simple and used the default options.
And I also don't get how the interaction between the flow and the boundary takes place. Do I need the wall adhesion or does the Eulerian Wall Film Model already contain a wall-flow-interaction? As far as I understand there is just a momentum-coupling....

Many questions... Thank you very much for your help!!

Cheers,
Marbau

michujo July 10, 2013 05:27

1 Attachment(s)
Hi, you need to enable the Phase Accretion option in the Eulerian Wall Film window (see attached figure). This accounts for the droplets impact on the wall. If this option is not enabled there is no liquid mass going into the film and (since it was initialized to zero) you have no film at all.

Have a go at it and let us know.

Cheers,
Michujo.

P.S: The other options account for different mass and momentum exchange mechanisms between the film and the outer flow.

Marbau July 11, 2013 03:43

1 Attachment(s)
Hi, there is no "Phase accretion" option. I use Fluent 14.0.

michujo July 11, 2013 04:15

Oh, I see. As far as I know this option was recently implemented in the 14.5 version.

For V.14 the EWF coupling with an eulerian disperse phase is done through the use of UDF's. Also, there's a tutorial around about how to enable the EWF model with the eulerian-eulerian approach. Ask your Ansys supplier for the UDF's and the tutorial.

The other option is to upgrade your Fluent version to the latest release (14.5.7 I think), where this option is already built-in.

Cheers,
Michujo.

Marbau July 11, 2013 04:18

OK, thank you very much for your help!!

Cheers
Martin

Marbau July 11, 2013 05:46

Just to be on the safe side, I'm mainly interested in the spatial distribution of the impacting particles, the film itself isn't that important. Is there another possibility to investigate that using the Euler-Euler-approach?

michujo July 11, 2013 06:22

Hi. As far as I know you need to enable the wall film in order to obtain the droplet collection efficiency so I'm afraid there's no way around. Again, in that tutorial I mentioned before it is explained how to obtain the collection efficiency on the surface of your body by combining the UDF's and some commands on the text user interface. Contact Ansys support for help.

Cheers,
Michujo.

sfotovati August 28, 2013 20:48

Hi all,

I just want to have the film due to the DPM.

How should I set the initial and boundary conditions for the film over the wall boundary? Do I have to define the flux? Or it will be automatically calculated as particles hit the wall?

Also, do I have to define the initial film thickness?

Thanks for our replies.

Shawn

michujo August 29, 2013 04:00

Hi, I think that for DPM you have to set the "trap" boundary condition on the solid walls.
Yes, the initial film thickness must be defined.

Follow the tutorials online, they are pretty well explained.

Cheers,
Michujo.

sfotovati August 29, 2013 15:20

The simulation crashes immediately. I have no idea why!

I set the wall DPM BC as a trap, but in the EWF setup menu, the DPM control is still disable. I also defined the initial wall film height on the wall, but no flux, as I hope the particles act as a film flux, when they hit the wall. I initialized the EWF, and let the simulations to run, but it crashes right after I hit the run...

Besides the EWF menu, and the wall menu, is there any other places that I have to fix the setups?

michujo August 29, 2013 15:41

Hi, I do not know about your particular case.

I suggest you get yourself a copy of the tutorial of the EWF model, set up the case and run it to check what you might be doing wrong.

Did you run the EWF and DPM models right from the initial solution or did you start from a converged solution of the flow?

If the problem persists I suggest you contact Ansys support if you have access to it.

Cheers,
Michujo.


All times are GMT -4. The time now is 12:55.