CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Boundary conditions for a sail boat on FLUENT

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 10, 2007, 02:41
Default Boundary conditions for a sail boat on FLUENT
  #1
Gaylor
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   April 10, 2007, 03:36
Default Re: Boundary conditions for a sail boat on FLUENT
  #2
Charles
Guest
 
Posts: n/a
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).
  Reply With Quote

Old   April 10, 2007, 03:48
Default Re: Boundary conditions for a sail boat on FLUENT
  #3
Razvan
Guest
 
Posts: n/a
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

  Reply With Quote

Old   April 10, 2007, 08:51
Default Re: Boundary conditions for a sail boat on FLUENT
  #4
Gaylor
Guest
 
Posts: n/a
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
  Reply With Quote

Old   April 10, 2007, 09:19
Default Re: Boundary conditions for a sail boat on FLUENT
  #5
Razvan
Guest
 
Posts: n/a
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
  Reply With Quote

Old   June 6, 2013, 12:10
Default
  #6
Senior Member
 
Saeed
Join Date: Jan 2013
Posts: 177
Rep Power: 4
flow_CH is on a distinguished road
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.

Last edited by flow_CH; June 27, 2013 at 08:38.
flow_CH is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
non reflective boundary conditions for incompresible flow Pascal_doran OpenFOAM Programming & Development 15 August 7, 2014 05:55
Boundary Conditions for aircraft engine in Fluent 6.3 Tareen FLUENT 0 July 20, 2011 00:05
Exporting Fluent boundary conditions for Ansys FEA Cav FLUENT 0 February 22, 2010 12:14
How to set the wind tunnel Boundary conditions in Fluent??? Saima FLUENT 1 April 14, 2009 00:12
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 16:21.