Numerical Ventilation (NV)
 

Hi every body,


In Star-ccm+ i have a problem for my DFBI simulation of high speed planing craft (2DOF with and without overset mesh) and that is air ventilation under the hull.


For this i had already tried mesh refinement and the time step to resolve the issue but the problem is still there.


I read in several articles that negative source (Sink) should be used to solve this problem.


Can any one help me that how to use negative source's?


Thanks in advance!

Can any one please give me some reply.? I did not find any thread also which discusses about negative sorces under the hull. So please advice if you know the answer.
regards
Arman

Please help me friends, because it's a matter of necessity for my project.

Hi
 

Hi,

I am sorry but I don't understand the problem you are facing.

Are you not able to model the ventilation? or the simulation is crashing?

Can you explain a little more based on a figure showing the ventilation in it?

May be I can help you.

Hi dear HARIHARAN K

Thank you for your attention to my problem.


I tried to simulate the 2-DOF motion of a planing hull at different speeds up to fully planing.
It was observed that air propagated down the hull in the near wall cells in areas.
Beacuse of the low air density relative to water, the drag force decreases.
This phenomenon induces also wrong trim and sinkage value.


So i am looking for a solution to prevent this.

Hi Arman

I have faced the same problem.. There are some useful thesis and papers that can help us.

One of them is Mancini's PhD Thesis.. The other is Viola, Flay and Ponzini's paper. There is also another, Bohm's PhD thesis.

There are some methods to achieve this problem. I am also still trying to understand and implement these methods.

may be we can help each other.

Yes, it is a common issue in planing hull simulation.

Try to reduce the aspect ratio of the cells near the intersection between the fluid and hull, say near the stagnation area.

Negative source is an alternative.

Turn the option from:
Go to Region -> Overset (or whatever the region name is) -> Physics Condition -> Volume Fraction Source Option

Then set the values at:
Go to Region -> Overset (or whatever the region name is) -> Physics Condition -> Volume Fraction Sources. (A possible option is method: composite and then you specify the source for air)

However, you might need to use field function to specify
1. Where will the source going to be activated (say only close to the wetted hull)
2. The value of the source (where this one you might do some trial error)

Dear Emre Ka


Yes, I've read them too


But the problem is that they have written only briefly:(

This is important for my project, so I'm happy to work with you to find the solution:)


Ragards.

Hi KBH

First of all,thanks for your description.


According to your recommendations, I have done the following steps:


I went to: Region->Overset-> Physics Condition-> Volume Fraction Source option->Phase source term (is Activated)

Then:
Physics values-> Volume Fraction Sources->Method->Composite-> Method for Air->Field function-> Scalar function->-----


To continue this, what field function do I define? (more details)


Best Regards

I will give you a rough idea, the details you need to work it out.
You need to create Field Function (FF) that will do what you want.

Say you want to create the negative (air) source near the hull. You will need to
1. Determine the location where you will turn the source on
2. How big the strength of the source

For 1:
Say if you want to apply source only close to the hull, you can use WallDistance FF. So you can make a new FF say 'source_zone' with definition:
($WallDistance < 1e-2) ? 1 : 0
Which means that the function will give you 1 when the distance to the wall is less than 0.01 and 0 if the distance is bigger than that.

For 2:
You can say make a FF say 'source_strength' with definition:
$source_zone*some_negative_constant
So the constant will be applied only to those area where you have defined in (1)

Of course those two FF can be combined, but say if you want to have a more complicated definition on where the source being applied (ex: only the bottom part of the hull as it does not make sense applying negative source on the superstructure), it will be easier to decouple them.

Thank's a lot

I get it and have a try...

There is a feature called "Replacing VOF Phases" just for this purpose.

Replacing VOF phases may solve this problem however it has to be used one or two steps after your solution has reached the steady regime. If you use this feature in all analyses, your reults are breaking bad.

Hi:)
If i want to define FF 'source_zone' for Part of my geometry;for example near to the stagination point.How can to do this?

Hi all,


For a brief step by step precise solution you can refer to "Avci&Barlas" approach which uses phase replacement model.



http://jmst.ntou.edu.tw/marine/26-5/617-628.pdf

Further Explaination
 

Hello everybody,

I am having the same issues at the moment with plaining hulls. I did not quite understand the field function definition. Is there somebody who could go over it please?

Regards,

Filippo

You may try the steps as mentioned in the paper given above.

Initially you may try

${VolumeFractionair} < .50

If the amount of air that is intaked under the hull is more than 50% you can just change .50 to new value. Ex. 0.6 0.75 or whatever. If the amount is less than .50 again you may try what you seen from the volume fraction scene. Ex. 0.25 0.30 You can visualise the amount via volume fraction scene. On page 622 it is explained.

Trouble with overset region
 

Hi

I did the steps outlined in the paper but am getting this error.

Unable to compute field function User Field Function 1 on "Boat Overset". Please check that function is defined here.

what do I do to define the region in the field function

Thanks

I think you should rearrange volumefraction of air in the overset region, than apply the procedure. I didnt use overset mesh in the mentioned case

maybe too late but here it is the solution by siemens