CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Other] Adaptive mesh does not work at the axisymmetric boundary

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 4, 2020, 06:13
Default Adaptive mesh does not work at the axisymmetric boundary
  #1
New Member
 
Golden
Join Date: Sep 2019
Posts: 4
Rep Power: 6
CloudBird is on a distinguished road
Hello,everyone! Recently, I am working on a jet simulation based on interFoam and I used adaptive mesh to refine the region near the interface. My geometry is an axisymmetric configuration with wedge boundary condition(see Fig1). During the simulation process, I found that the mesh near the symmetry axis whose boundary condition is empty didn't get refined(see Fig2). Fig 3 is the cellLevel field generated by the adaptive mesh code and you can see that the region near the symmetry axis is not in the refined area.

Fig.1 the geometry of my cases

Fig.2 the refined mesh near the interface

Fig.3 the cellLevel near the interface

This is my dynamicMeshDict:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  8
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh   dynamicRefineFvMesh;

// How often to refine
refineInterval  1;

// Field to be refinement on
field           alpha.liquid;

// Refine field in between lower..upper
lowerRefineLevel 0.01;
upperRefineLevel 0.99;

// If value < unrefineLevel unrefine
unrefineLevel   10;

// Have slower than 2:1 refinement
nBufferLayers   1;

// Refine cells only up to maxRefinement levels
maxRefinement   2;

// Stop refinement if maxCells reached
maxCells        200000;

// Flux field and corresponding velocity field. Fluxes on changed
// faces get recalculated by interpolating the velocity. Use 'none'
// on surfaceScalarFields that do not need to be reinterpolated.
correctFluxes
(
  (phi none)
  (nHatf none)
  (rhoPhi none)
  (alphaPhi0.liquid none)
  (ghf none)
);

// Write the refinement level as a volScalarField
dumpLevel       true;


// ************************************************************************* //
In my opinion, this error may related to the empty boundary condition which I apply to the axis. But I don't have any idea how to fix it.

I hope someone can help me out and any suggestion is welcome. Thanks in advance!

Kind regards,
CloudBird
Attached Images
File Type: png 03.png (7.4 KB, 142 views)
File Type: png 04.png (125.4 KB, 144 views)
File Type: png 05.png (6.6 KB, 140 views)
CloudBird is offline   Reply With Quote

Old   October 4, 2020, 16:05
Default
  #2
Member
 
Rodrigo
Join Date: Mar 2010
Posts: 98
Rep Power: 16
guin is on a distinguished road
I wouldn't expect it to refine there. Adaptive mesh refinement in OF relies on the assumption of hexahedral elements. Wedges are not hexahedra, thus they are left unchanged...
guin is offline   Reply With Quote

Old   October 5, 2020, 03:40
Default
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,904
Rep Power: 33
hjasak will become famous soon enough
First, you can get rid of the pole patch either by removing it by hand if there are no faces or by collapsing the points first.

Second foam-extend actually provides adaptivity on polyhedral cells so the problem goes away.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   October 5, 2020, 05:42
Default
  #4
New Member
 
Golden
Join Date: Sep 2019
Posts: 4
Rep Power: 6
CloudBird is on a distinguished road
Quote:
Originally Posted by guin View Post
I wouldn't expect it to refine there. Adaptive mesh refinement in OF relies on the assumption of hexahedral elements. Wedges are not hexahedra, thus they are left unchanged...
Thank you~ I will try to give a tiny thickness in the axis and have a try (^-^)
CloudBird is offline   Reply With Quote

Old   October 5, 2020, 05:46
Default
  #5
New Member
 
Golden
Join Date: Sep 2019
Posts: 4
Rep Power: 6
CloudBird is on a distinguished road
Quote:
Originally Posted by hjasak View Post
First, you can get rid of the pole patch either by removing it by hand if there are no faces or by collapsing the points first.

Second foam-extend actually provides adaptivity on polyhedral cells so the problem goes away.

Hrv
Thank you, sir. I will try for the extend version
CloudBird is offline   Reply With Quote

Reply

Tags
adaptive mesh refinement, axisymmetric, openfoam

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
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 08:38
My radial inflow turbine Abo Anas CFX 27 May 11, 2018 02:44
CFD analaysis of Pelton turbine amodpanthee CFX 31 April 19, 2018 19:02
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 22:11
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Meshing & Mesh Conversion 2 July 15, 2005 05:15


All times are GMT -4. The time now is 15:44.