mirror of
https://develop.openfoam.com/Development/openfoam.git
synced 2025-11-28 03:28:01 +00:00
5f556ffb4a
- helps reduce clutter in the topoSetDict files.
Caveats when using this.
The older specification styles using "name" will conflict with the
set name. Eg,
{
name f0
type faceSet;
action add;
source patchToFace;
sourceInfo
{
name inlet;
}
}
would flattened to the following
{
name f0
type faceSet;
action add;
source patchToFace;
name inlet;
}
which overwrites the "name" used for the faceSet.
The solution is to use the updated syntax:
{
name f0
type faceSet;
action add;
source patchToFace;
patch inlet;
}
oscillatingInletACMI2D
This tutorial case gives an example of the Arbitrarily Coupled Mesh Interface
(ACMI) usage. The mesh is composed of two mesh regions: an inlet channel which
oscillates in the +/- Y-direction, and a fixed mesh region.
Each ACMI patch requires the specification of a 'non-overlapping' patch. In
this example, the non-overlapping patches are described as walls, e.g. taken
from the constant/polyMesh/boundary file:
1. First ACMI patch pair applied to the inlet channel outlet
ACMI1_couple
{
type cyclicACMI;
nFaces 40;
startFace 43720;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
}
ACMI1_blockage
{
type wall;
nFaces 40;
startFace 43680;
}
1. Second ACMI patch pair applied to the fixed mesh region inlet
ACMI2_couple
{
type cyclicACMI;
nFaces 96;
startFace 43856;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI1_couple;
nonOverlapPatch ACMI2_blockage;
}
ACMI2_blockage
{
type wall;
nFaces 96;
startFace 43760;
}
In the above, the ACMI1_blockage and ACMI1_couple patches occupy the same space,
with duplicate points, edges and faces. The ACMI2_blockage and ACMI2_couple
patches are created similarly.
The duplicate patches are initially created using the createBaffles utility.
Firstly, the original (non-duplicated) patch faces are collected into zones
using the topoSet utility.
Note: when specifying the ACMI patch-pairs, the coupled patch must be specified
before its associated non-overlapping patch.
Each ACMI/non-overlapping patch pair is specified using a master-slave approach.
However, since we are generating boundary patches (which are always master
patches) the slave patches are simply defined using 'dummy' entries, e.g.:
type faceZone;
zoneName couple1Faces;
patches
{
// create cyclic ACMI patch
master
{
//- Master side patch
name ACMI1_couple;
type cyclicACMI;
matchTolerance 0.0001;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
transform noOrdering;
}
slave // dummy entries only
{
//- Slave side patch
name ACMI1_couple;
type patch;
}
// create blockage patch
master2
{
//- Master side patch
name ACMI1_blockage;
type wall;
}
slave12 // dummy entries only
{
//- Slave side patch
name ACMI1_blockage;
type wall;
}
}
Boundary conditions must then be applied to all geometric patches in the usual,
manner, and the cases can be executed in parallel (as shown when running the
Allrun-parallel script) without any speacial treatment, i.e. the case set-up is
the same as when operating in serial mode.
checkMesh
---------
checkMesh will see the 'duplicate' boundary faces but does not know about
the area factors so will complain:
***Boundary openness (-0.0103092 2.3845e-17 3.80774e-17) possible hole in boundary description.
***Open cells found, max cell openness: 0.333333, number of open cells 136
<<Writing 136 non closed cells to set nonClosedCells
As long as these non-closed cells are on the ACMI they can be ignored.
paraFoam
--------
- display: it will not display the outside of the ACMI, there will be a hole.
- cuttingPlanes: they leave out the duplicate faces (i.e. the cells on
the ACMI patches)
- interpolation: the interpolation does not take into account the
area-weights on the ACMI.
pointFields
-----------
Same as paraFoam: the interpolation does not take into account the
area-weights on the ACMI.