OpenFoam has many gadgets that come with it for your convenience. If you need a partner, you can go to the following for yourself:
hty@ubuntu:~$ util hty@ubuntu:/opt/openfoam4/applications/utilities$ ls mesh parallelProcessing preProcessing thermophysical miscellaneous postProcessing surface hty@ubuntu:/opt/openfoam4/applications/utilities$
The following is a preliminary overview of several commonly used tools, which will be updated later. It would be grateful to have organized little buddies to call me.
1. Co
C o = δ t ∣ U ∣ δ x Co=\frac{\delta t|\mathbf U|}{\delta x} Co=δxδt∣U∣
2. vorticity (curl of velocity field)
3. yPlus
The y+ value is important because it reflects that the grid grid correctly resolves the boundary layer. In general, you can also use the wall function, otherwise you can use y+<5 at the viscous sublayer. yPlus calculates and reports y+wall patches for all near-wall cells for specified times of laminar flow, LES, and RAS. For walls with wall functionality, the wall function provides y+ values, otherwise the velocity gradient from the near wall and effective laminar viscosity are obtained directly.
4. sample
- Sample utilities are used to generate images or extract surfaces.
- In order to use it, a system/simpleDict file is required under the case folder.
- Type sample-help to get an optional flag.
5. foamCalc
Operate on the farm:
foamCalc <calcType> <fieldName1 ... fieldnameN>
CalType includes:
- div: the divergence of the field requires attention to the fvScheme, which specifies the format necessary for calculating the divergence;
- magSqr: square of amplitude
- mag: amplitude
- grad: the gradient of the field
- components: part of the extraction farm
6. probeLocations
- Continuous sampling at fixed locations over time;
- A system/simpleDict file is required under the case folder.
- Sampling fields and points need to be declared;
fields//Declare sampling field ( p ): probeLocations//Declare sample points ( 0.2 0.2 0.2 );
7. topoSet
The grid sequence (points, polygons, grids) is manipulated through a dictionary file;
topoSetDict file is required;
actions
(
{
name c0;
type cellSet;
action new;
source boxTocell;
sourceInfo
{
box (0.3 0.3 0.3) (0.6 0.6 0);
}
}
);
action types:
- Clear: clear
- invert: Reverse, select unselected elements, reset selected elements to unselected
- Remove: remove
- new +source: Create a new setting or source
- add+source: add source
- delete+source: delete source
Source operation type:
- labelToCell: Select a cell from a given label.
- cellToCell: Copy elements from a cell set.
- ZoeToCell: Select the cells in the cell area.
- faceToCell: Select a cell from a face (owner or neighbor)
- boxToCell: Select the cell in the box.
- cylinderToCell: Select the cell whose center is inside the cylinder.
- sphereToCell: Select the cell whose center is inside the sphere.
- nearestToCell: Select the closest cell center to coordinate.
- fieldToCell: Select a cell with a range of field values.
8. setFields
Mainly used for multiphase flow models to redefine field information.
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
defaultFieldValues
(
volScalarFieldValue alpha.air 1
volScalarFieldValue alpha.water 0
);
regions
(
boxToCell
{
box (0 0 0) (0.01 0.05 0.01);//Grid cells with body centers in this range
fieldValues
(
volScalarFieldValue alpha.air 0
volScalarFieldValue alpha.water 0
);
}
);
// ************************************************************************* //
9. checkMesh
For checking grid quality, the output information is as follows:
[stu cavity]$ checkMesh
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.1
Exec : checkMesh
Date : Sep 28 2020
Time : 21:37:29
Host : "node01"
PID : 151764
Case : /home/student2/OpenFOAM/student2-4.1/run/cavity
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 882
internal points: 0
faces: 1640
internal faces: 760
cells: 400
faces per cell: 6
boundary patches: 3
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 400
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
movingWall 20 42 ok (non-closed singly connected)
fixedWalls 60 122 ok (non-closed singly connected)
frontAndBack 800 882 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 0 0) (0.1 0.1 0.01)
Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
Mesh has 2 solution (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (8.47033e-18 -8.47033e-18 -4.51751e-17) OK.
Max cell openness = 1.35525e-16 OK.
Max aspect ratio = 1 OK.//Aspect ratio
Minimum face area = 2.5e-05. Maximum face area = 5e-05. Face area magnitudes OK.
Min volume = 2.5e-07. Max volume = 2.5e-07. Total volume = 0.0001. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0//Number of non-orthogonal grids
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 1.66533e-14 OK.//Grid skew
Coupled point location match (average 0) OK.
Mesh OK.
End
10. transformPoints
Used for grid movement, scale-up, and rotation.
- translate+vector: moves in the direction of a given vector;
- Rotate+ (vector vector vector): rotates a point along the first vector to the second vector;
- scale+vector: Scale up or down the grid cells according to the specified vector.
[stu run]$ ls cavity [stu run]$ cp -r cavity cavityTranslate [stu run]$ touch cavityTranslate/cavityTranslate.OpenFAOM //Create a file that can be opened by a paraview [stu run]$ transformPoints -case cavityTranslate/ -translate "(0.2 0.2 0.2)" //Shift grid cells /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 4.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 4.1 Exec : transformPoints -case cavityTranslate/ -translate (0.2 0.2 0.2) Date : Sep 28 2020 Time : 22:03:41 Host : "node01" PID : 152372 Case : ./cavityTranslate nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Translating points by (0.2 0.2 0.2) Writing points into directory "./cavityTranslate/constant/polyMesh" End [stu run]$ paraview //Open paraview to compare the differences
11. createBaffles
- Converts an internal surface to two boundary surfaces without thickness, or converts multiple boundary surfaces to one boundary surface.
- You can add boundary conditions on this surface.
createBafflesDict
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Sample for creating baffles:
// - usually converting internal faces into two boundary faces
// - or converting boundary faces into a boundary face
// (internalFacesOnly=false)(though should use really createPatch
// to do this)
//
// - selection of faces (and orientation) to 'baffle' through:
// faceZone:
// type faceZone;
// zoneName f0;
// searchableSurface:
// type searchableSurface;
// surface triSurfaceMesh;
// name baffle1D.stl;
//
// - specification of patches for baffle sides in one of two modes:
// - patchPairs : create two patches of same type, same input
// - patches : create patches separately, full control over what
// to create on what side
// (this mode can also create duplicate (overlapping)
// sets of baffles:
// - internalFacesOnly = false
// - have 4 entries in patches:
// - master
// - slave
// - additional master
// - additional slave)
// Whether to convert internal faces only (so leave boundary faces intact).
// This is only relevant if your face selection type can pick up boundary
// faces.
internalFacesOnly true;
// Optionally do not read/convert/write any fields.
//noFields true;
// Baffles to create.
baffles
{
baffle1
{
//- Use surface to select faces and orientation.
type searchableSurface;
surface triSurfaceMesh;
name baffle1D.stl;
//- Optional flip
//flip false;
// Generate patchGroup baffle1 with two patches:
// - baffle1_master
// - baffle1_slave
patchPairs
{
type wall;
//- Optional override of added patchfields. If not specified
// any added patchfields are of type calculated.
patchFields
{
U
{
type fixedValue;
value uniform (0 0 0);
}
}
}
}
cyclicFaces//cyclic: periodic condition
{
//- Select faces and orientation through a searchableSurface
type searchableSurface;
surface searchablePlate;
origin (0.099 -0.006 0.004);
span (0 0.012 0.012);
// Generate patches explicitly
patches
{
master
{
//- Master side patch
name fan_half0;
type cyclic;
neighbourPatch fan_half1;
patchFields
{
p
{
type fan;
patchType cyclic;
jump uniform 0;
value uniform 0;
jumpTable polynomial 1((100 0));
}
}
}
slave
{
//- Slave side patch
name fan_half1;
type cyclic;
neighbourPatch fan_half0;
patchFields
{
p
{
type fan;
patchType cyclic;
value uniform 0;
}
}
}
}
}
}
// ************************************************************************* //
12. refineMesh
Encrypted Grid
- You can use refineMesh directly
refineMesh -overwrite//Overwrite the original grid, rewrite the encryption so that no new folders are generated
- You can also use refineMeshDict:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Cells to refine; name of cell set
set c0;// Involving topoSet
// Type of coordinate system:
// - global : coordinate system same for every cell. Usually aligned with
// x,y,z axis. Specify in globalCoeffs section below.
// - patchLocal : coordinate system different for every cell. Specify in
// patchLocalCoeffs section below.
// - fieldBased : uses the list of field names from the directions list for
// selecting the directions to cut. Meant to be used with geometricCut, but
// can also be used with useHexTopology.
coordinateSystem global;
//coordinateSystem patchLocal;
//coordinateSystem fieldBased;
// .. and its coefficients. x,y in this case. (normal direction is calculated
// as tan1^tan2)
globalCoeffs
{
tan1 (1 0 0);
tan2 (0 1 0);
}
patchLocalCoeffs
{
patch outside; // Normal direction is facenormal of zero'th face of patch
tan1 (1 0 0);
}
// List of directions to refine, if global or patchLocal
directions
(
tan1
tan2
normal
);
// List of directions to refine, if "fieldBased". Keep in mind that these
// fields must be of type "vectorField", not "volVectorField".
//directions
//(
// radialDirectionFieldName
// angularDirectionFieldName
// heightDirectionFieldName
//);
// Whether to use hex topology. This will
// - if patchLocal: all cells on selected patch should be hex
// - split all hexes in 2x2x2 through the middle of edges.
useHexTopology true;
// Cut purely geometric (will cut hexes through vertices) or take topology
// into account. Incompatible with useHexTopology
geometricCut false;
// Write meshes from intermediate steps
writeMesh false;
// ************************************************************************* //