Utilities

Prepared by Ivan Batistić, with additions by Philip Cardiff

Section Aims

This document describes the solids4foam utilities located in applications/utilities;
Utilities are executables that provide various pre and post-processing functionalities;
These solids4foam utilities provide functionalities not available in the standard OpenFOAM utilities (OpenFOAM-wiki).

`abaqusMeshToFoam`

Utility purpose Mesh converter: converts Abaqus mesh (in *.inp format) into the FOAM mesh format.
Currently, this utility only supports 3-D hexahedral cells/elements. Note that each distribution of OpenFOAM comes with a set of mesh converters (but not for Abaqus), see the available one here.
Arguments
- <mesh.inp> name of the Abaqus mesh file.
Options/parameters

None
Example of usage
```
abaqusMeshToFoam mesh.inp
```
Note
- Only the following Abaqus element types are supported: C3D8 and C3D8R.
- Only the first PART is used and the rest are ignored.
- Node sets, element sets and surfaces are not converted.

`addTinyPatch`

Utility purpose For a chosen patch, find the closest face to the specified location and separate it into a new patch.
The utility can be used, for example, to create patches for specifying point loads.
Arguments
- <currentPatchName> chosen patch name;
- <newTinyPatchName> name of the one-face patch to be created;
- "(x y z)" location vector.
Options/parameters

None
Example of usage
```
addTinyPatch Top TopNew "(30 30 0)"
```

addTinyPatch: top patch before and after adding one-face patch addTinyPatch: top patch before and after adding one-face patch

Note

When using addTinyPatch the original mesh is overwritten!

`foamMeshToAbaqus`

Utility purpose Mesh converter: converts FOAM mesh into Abaqus mesh (*.inp format). Currently, this utility only supports 3-D hexahedral cells/elements.
Arguments

None
Options/parameters

None
Example of usage
```
foamMeshToAbaqus
```
Converted mesh is written to theabaqusMesh.inp file.
Creates a node set and and element set and a surface for each boundary patch.
Also creates a element set for each material in the materials file (if it is exists).
Note
- Only works for hexahedral cells as yet.
- Created for Abaqus-6.9-2, but should work for new versions too.

`perturbMeshPoints`

Utility purpose
Add a random perturbation to each mesh points. The perturbation of a point is calculated as a scale factor times the local minimum edge length.

By default, boundary points are slide along the patch. Patches which should not move can be defined via the fixedPatches entry.

In OpenFOAM.com, points on feature edges are not moved, where feature edges are defined by the minimum cosine angle (minCos). This feature is not currently implemented with OpenFOAM.org and foam-extend.

The inputs are defined in $FOAM_CASE/system/perturbMeshPointsDict, and consist of a seed (for the random number generator) and a scaling factor to scale the perturbations relative to the local minimum edge length. The scaling factor is a vector to allow different scalings in different directions; for example, for 2-D, the Z component should be set to 0.0.

This utility is useful for creating distorted grids for testing discretisations.
Arguments
None
Options/parameters

None

Dictionary
Inputs are defined in dictionary named perturbMeshPointsDict and located in system directory:

// Perturn by 30% of the local minimum edge length in the X, Y and Z directions
scaleFactor (0.3 0.3 0.3);

// Gaussian or uniform random distribution
Gaussian    no;

// Seed for random number generator
seed        1;

// Minimum cosine to find feature edges
// Points on feature edges are not moved
minCos      0.7;

// Names of patches which should not be perturbed
fixedPatches
(
    // Add patch names here
);
  

The Gaussian distribution can only be used in combination with OpenFOAM.com.

Example of usage
```
perturbMeshPoints
```
The figure below shows mesh before and after using perturbMeshPoints utility.

perturbMeshPoints: mesh before and after point perturbation perturbMeshPoints: mesh before and after point perturbation

Note

Perturbed mesh (polyMesh) is stored in the 0 directory and needs to be movedto constant before running the simulation!

`splitPatch`

Utility purpose Splits a patch into two patches by putting faces in the given bounding box in a new patch.
Arguments None
Options/parameters

-overwrite overwrite the original mesh when storing mesh after patch splitting.
Dictionary
```
patchToSplitName    Top;

newPatchName        TopNew;

boundBoxes
(
    (0 0 0.01) (1 1 1)
);
```
- patchToSplitName is a name of the patch to be split;
- newPatchNameis the name of the splitted patch part;
- boundBoxes is list of bounding boxes; each defined with two vectors: (xmin ymin zmin) and (xmax ymax zmax). Boundary patch faces inside this bounding box will be put in a new patch.
  Note: The face's centre point is tested to see if it is inside the bounding boxes!
Example of usage
```
splitPatch
```

splitPatch: top patch before and after split

Note

The mesh with the new patch is stored in a new time-step directory (1 for example) and should be moved to the constant before running the simulation. Alternatively, the -overwrite option can be used to overwrite the original mesh.