CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Boundary conditions for a sail boat on FLUENT (http://www.cfd-online.com/Forums/fluent/44399-boundary-conditions-sail-boat-fluent.html)

Gaylor April 10, 2007 02:41

Boundary conditions for a sail boat on FLUENT
 
Hi everybody!

As we explained in a previous message, we are trying to modelize a sailboat on Fluent.

We insist on the fact that our problem deals with FLUENT and not GAMBIT. We already have modelized the geometry of the boat on Gambit.

But now, we have a big problem with the boundary conditions on FLUENT. We are using the VOF model (air/water), free surface. Our parameters (segregated, unsteady, k-epsylon, 2 inlets, 2 outflows)

Shall we use the Open Channel and how can we do that? We want to use velocity inlet but some people told us to use pressure inlet!! Somebody could explain why and the way of doing this???

Thank you very much.

Charles April 10, 2007 03:36

Re: Boundary conditions for a sail boat on FLUENT
 
When using the Open Channel BC you don't need separate air and water inlets and outlets. The reason for selecting pressure inlet is that it allows you to select the Open Channel BC (this is in Fluent 6.2.16 onwards, older versions are more difficult).

Razvan April 10, 2007 03:48

Re: Boundary conditions for a sail boat on FLUENT
 
First of all, you need Fluent 6.2 or 6.3 to be able to use Open Channel. In both versions, only after activating VOF model, "open channel" will become available in the "Boundary conditions" panel.

If you would read the documentation, you will see that "open channel" needs a "Pressure-inlet - Pressure-outlet" or "Mass-flow-inlet - Pressure-outlet" boundary conditions combination to work. The first is easier to setup, because it only requires the velocity of the air+water flow and the level of the free surface + the level of the bottom (both relative to the reference coordinate system of the grid). It has only a slight disadvantage: it needs a dense enough grid on the boundaries to keep the mass imbalance low.

Also, "open channel" does not require separate inlets or outlets for the two phases. It needs only one inlet boundary (pressure-inlet) and one outlet boundary (pressure-outlet).

And you do not necessarily have to use unsteady formulation, "open channel" works well in steady mode also, the only care you have to take is to seriously underrelax the solution (all underrelaxation factors must be 0.5 or less, momentum 0.2-0.3, volume fraction 0.2) and to use "Body Force Weighted" discretisation method for pressure. It wil take maybe 1500-2000 iterations with first order and about 5000 more with second order to obtain a converged solution.

All the best,

Razvan


Gaylor April 10, 2007 08:51

Re: Boundary conditions for a sail boat on FLUENT
 
ok thank you very much for your help.

we have done that but we don't manage to patch water. we only have air or only water. Do you have a solution? shall we patch water to 0,5 instead of 1?

our problem is that we manage to do it for the inlet face but we don't manage to expand it to the volume!

thanks regards

Razvan April 10, 2007 09:19

Re: Boundary conditions for a sail boat on FLUENT
 
To patch the water in the flow volume you need to create a register first. For that you have to go to "Adapt/Region" panel, and "Mark" all cells inside a rectangular region which expands from the free surface position downward. Then type "(rpsetvar 'patch/vof? #t)" in the TUI (without "", of course). This will ensure a smoother initial free surface. Then go to "solve/Initialise/Patch" panel and select "hexahedron-xx" and patch a volume fraction of 1 in it. That's it!

Razvan

flow_CH June 6, 2013 12:10

Quote:

Originally Posted by Razvan
;140766
To patch the water in the flow volume you need to create a register first. For that you have to go to "Adapt/Region" panel, and "Mark" all cells inside a rectangular region which expands from the free surface position downward. Then type "(rpsetvar 'patch/vof? #t)" in the TUI (without "", of course). This will ensure a smoother initial free surface. Then go to "solve/Initialise/Patch" panel and select "hexahedron-xx" and patch a volume fraction of 1 in it. That's it!

Razvan

i want to model a open channel too.
where is "all cells inside a rectangular region which expands from the free surface position downward"? i marked inside the inlet of model for patch, but no cells marked and when i outside the inlet, fluent marked all cells of my model. I think when we define boundary condition of open channel in BC panel, we do not need to patch volume fraction in inlet BC. Am i right?
And i have exactly the "Gayor" problem(we only have air or only water after solve)
i am confused.


All times are GMT -4. The time now is 05:49.