CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Boundary condition of velocity and pressure at interface for air water pipe flow

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

Like Tree1Likes
  • 1 Post By Villo

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 10, 2014, 16:44
Default Boundary condition of velocity and pressure at interface for air water pipe flow
  #1
Member
 
Jignesh
Join Date: Aug 2011
Location: India
Posts: 68
Rep Power: 13
jignesh_thaker2007 is on a distinguished road
Send a message via Yahoo to jignesh_thaker2007
How can i define the boundary condition for velocity and pressure at interface of air-water two phase pipe flow in OpenFOAM?
I am trying to solve the problem of two-phase air water mixture in OpenFOAM. Air is coming from the perforated pipe which has number of holes on its periphery and then mix with water. Actually in gambit i gave interface boundary condition at perforated holes. but when i convert in to openFOAM i am finding difficulty to define the proper boundary condition for velocity and pressure at this interface between air and water in 0 directory.
I drew the geometry in Gambit which is attached here for the reference.

Please some one tell me what is the proper boundary condition of velocity and pressure at interface for my problem.
Attached Images
File Type: jpg mixer.jpg (35.2 KB, 172 views)
jignesh_thaker2007 is offline   Reply With Quote

Old   June 18, 2014, 07:38
Default
  #2
New Member
 
Tommy V
Join Date: Nov 2013
Posts: 29
Rep Power: 11
Villo is on a distinguished road
Hi Jignesh.
OpenFoam does not require any boundary conditions between the two phases... or, in other words, does not require to create any additional face/interface with software as Gambit.
I`m actually using multi-phase multi-flow solvers in OpenFoam, running simulations on meshes created on Gambit. Here you some suggestion to avoid any error when you will import your mesh in OpenFoam:
- connect and link all the face and meshes
- convert all the faces from virtual to real (i think that you already did it being that your wireframe is green)
- delete not used faces/interfaces
- specify as boundary conditions just
-- water inlet
-- air inlet
-- water outlet
-- air outlet
-- walls

If you really require an interface (for meshing reason) create an arbitrary mesh interface at the air holes inlet, this will give you any problem in OpenFoam.

Cheers
jignesh_thaker2007 likes this.
Villo is offline   Reply With Quote

Old   June 19, 2014, 04:03
Default
  #3
Member
 
Jignesh
Join Date: Aug 2011
Location: India
Posts: 68
Rep Power: 13
jignesh_thaker2007 is on a distinguished road
Send a message via Yahoo to jignesh_thaker2007
Thank you for showing your interest for my problem.

I found difficulty because i dont know the values of air velocity coming to the small hole. I only know the inlet air velocity. so please tell me how i define boundary condition for pressure, velocity at small holes if i diidnt define than it will take as wall so air will not come in to outer pipe and it will not mix with water.
jignesh_thaker2007 is offline   Reply With Quote

Old   June 19, 2014, 06:58
Default
  #4
New Member
 
Tommy V
Join Date: Nov 2013
Posts: 29
Rep Power: 11
Villo is on a distinguished road
You`re welcome!
You have to specify just air inlet conditions (red area number 1): conditions at the holes will be solved from your solver!
In Gambit you have to delete all the interface that you have between air and water or make it (in OpenFoam) as arbitrary mesh interface (does not require any boundary condition specification). Another way... if the imported mesh in OpenFoam have still interfaces at the small holes you can delete it using the tool createPatch (in addiction to createPatchDict).
Villo is offline   Reply With Quote

Old   June 19, 2014, 08:22
Default
  #5
Member
 
Jignesh
Join Date: Aug 2011
Location: India
Posts: 68
Rep Power: 13
jignesh_thaker2007 is on a distinguished road
Send a message via Yahoo to jignesh_thaker2007
Actually I dont know how to give AMI in openFOAM please try to explain how will i use AMI in my problem?

when i upload the .msh file from gambit than Airinterface and Waterinterface boundary are to be set as patch type so I changed type of the boundary directory for small holes of innerpipe and outerpipe. Is right way to use AMI?

Airinterface
{
type cyclicAMI;
nFaces 16;
startFace 304;
matchTolerance 0.0001;
neighbourPatch Waterinterface;
transform noOrdering;
}

Waterinterface
{
type cyclicAMI;
nFaces 16;
startFace 304;
matchTolerance 0.0001;
neighbourPatch Airinterface;
transform noOrdering;
}

But OpenFOAM give me the error like in 0 directory cant find patchfield entry for Waterinterface and Airinterface.
Please tel me in 0 (alpha, pressure and velocity) directory what shold i define for Airinterface and Waterinterface?
jignesh_thaker2007 is offline   Reply With Quote

Old   June 19, 2014, 08:28
Default
  #6
New Member
 
Tommy V
Join Date: Nov 2013
Posts: 29
Rep Power: 11
Villo is on a distinguished road
can you post at first the constant/polyMesh/boundary file?
Allow me to be more clear in the explanation
Villo is offline   Reply With Quote

Old   June 19, 2014, 09:10
Default
  #7
New Member
 
Tommy V
Join Date: Nov 2013
Posts: 29
Rep Power: 11
Villo is on a distinguished road
in the 0 field you will have to specify
Waterinterface
{
type cyclicAMI;
}

Airinterface
{
type cyclicAMI;
}
If OpenFoam complain because cannot find the patch in the 0 folder is because these patches don`t have the same name.
Furthermore the AMI specification is normally better to do it via the createPatchDict in order to avoid any problem face ordering


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// This application/dictionary controls:
// - optional: create new patches from boundary faces (either given as
// a set of patches or as a faceSet)
// - always: order faces on coupled patches such that they are opposite. This
// is done for all coupled faces, not just for any patches created.
// - optional: synchronise points on coupled patches.
// - always: remove zero-sized (non-coupled) patches (that were not added)

// 1. Create cyclic:
// - specify where the faces should come from
// - specify the type of cyclic. If a rotational specify the rotationAxis
// and centre to make matching easier
// - always create both halves in one invocation with correct 'neighbourPatch'
// setting.
// - optionally pointSync true to guarantee points to line up.

// 2. Correct incorrect cyclic:
// This will usually fail upon loading:
// "face 0 area does not match neighbour 2 by 0.0100005%"
// " -- possible face ordering problem."
// - in polyMesh/boundary file:
// - loosen matchTolerance of all cyclics to get case to load
// - or change patch type from 'cyclic' to 'patch'
// and regenerate cyclic as above
// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
// with transformations (i.e. cyclics).
pointSync false;
// Patches to create.
(
{
// Name of new patch
name Airinterface_AMI;
// Dictionary to construct new patch from
patchInfo
{
type cyclicAMI;
matchTolerance 1E-7;
}
constructFrom patches;
patches (Airinterface);
}
{
name Waterinterface_AMI;
patchInfo
{
type cyclicAMI;
matchTolerance 1E-7;
}
constructFrom patches;
patches (Waterinterface);
}
);
// ************************************************** *********************** //
Villo is offline   Reply With Quote

Old   June 19, 2014, 10:12
Default
  #8
Member
 
Jignesh
Join Date: Aug 2011
Location: India
Posts: 68
Rep Power: 13
jignesh_thaker2007 is on a distinguished road
Send a message via Yahoo to jignesh_thaker2007
Thanks a lot
Actually i didnt define AMI in 0 directory. After updating it is working now.
jignesh_thaker2007 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 14:30.