Utilities

Prepared by Ivan Batistić

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. Details regarding the FOAM mesh format can be found, for example, here.
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

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 interior mesh point. Boundary points are not perturbed, except for in-plane motion on empty and wedge patches.
The utility can be used to create a distorted mesh to test the behavior (accuracy, order of accuracy, stability, etc.) of a discretisation procedure.
Arguments
None
Options/parameters

None
Dictionary
Inputs are defined in dictionary named perturbMeshPointsDict and located in system directory:
```
seed        1;
  
scaleFactor (5e-3 5e-3 5e-3);
  
Gaussian    no;
```
- seed is a scalar value used for the random number generator;
- scaleFactor is a scaling vector which scales the point perturbation in each direction separately;
- Gaussian enforces Gaussian distribution when perturbing points, otherwise uniform distribution is expected. Only 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

Note

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

Tip

For 2-D simulations, there is no need to perturb points in the empty direction. For an empty direction, zero scaling should be used, e.g.:
scaleFactor (5e-3 5e-3 0);

`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.