doc:user:geometry:mesh:3d

Metafor possesses a simple transfinite mesher, which is able to mesh hexahedra (object with 6 sides, such as a cube). For more complex geometries, it is necessary to divide it into hexaedra or use external meshers (Samcef, TetGen, …) and import the mesh in Metafor (see Reading SAMCEF files).

*Preliminary note:* To mesh a `Volume`

, all its `Sides`

and `Curves`

must be meshed first !

Auto-detection is possible if the `Skin`

has 12 edges, each of which possesses only one line.

TransfiniteMesher3D(volumeset(number)).execute(type)

`number` | number of the `Volume to mesh` |

`type` | = `True` if mesh elements must be generated (`CELL_HEXA` )= `False` if only nodes must be generated (useful to debug only) |

In this case, the `Skin`

must be defined with the orientation shown below:

which means that

skin = add(Skin(1)); for i in [1,2,3,4,5,6]: skin.push(sideset(i))

where the number used in the `push`

function are the number of the `Sides`

included in the `Skin`

.

This case is the most general, and can be applied to any `Skin`

with the shape of a hexaedron. The definition of the skin must no longer be as the above figure shows, which means the sides can be “pushed” in the skin in any order.

The mesher needs a set of 12 sets of `Curves`

, where each of these sets defines an edge of the hexaedron.

mat = ((mat11, ..., mat1nbmax), ..., (mat121, ..., mat12nbmax)) TransfiniteMesher3D(volumeset(number)).execute2(mat, type)

where `number`

is the number of the hexahedral `Volume`

to mesh, and `mat`

is a Python tuple with 12 components. Each component is a tuple which contains the number of the curves which constitute each edge. Each of these 12 edges can be made of a different number of curves.

These 12 tuples must be ordered as shown below:

*Example:*

The hexahedral domain above can be meshed with the command:

TransfiniteMesher3D(volumeset(1)).execute2( ((103,101,102),2,3,4,5,6,7,8,10,11,12,13) )

or

TransfiniteMesher3D(volumeset(1)).execute2( (5,11,(103,101,102),10,7,12,3,13,8,6,2,4) )

or

TransfiniteMesher3D(volumeset(1)).execute2( (6,12,2,11,8,13,4,10,5,7,3,(101,102,103)) )

or

...

leading to:

This is done with the commands:

MesherTFI3D =TransfiniteMesher3D(volumeset(number)) MesherTFI3D.setEnableDistribution() MesherTFI3D.execute(type, tri) ou MesherTFI3D.execute2(mat, type)

when one if the edges is already discretized using a mesh elements distribution.

*Note* : By default, the parameter `setEnableDistribution`

is set to `True`

.

This method can be used, but could be improved upon: density non-constant along the extrusion direction, improvement of meshing speed, giving the extruded nodes as groups (internal ones, external surface, …). For now on, a `Side`

, a `Skin`

or a `Group`

can be extruded along any direction, with any number of elements.

The geometry associated to the extrusion can also be created (only for a `Side`

). For a `Skin`

or a `Group`

, we can create the `Points`

and `Curves`

associated by extrusion to the `Points`

and `Curves`

of the object.

Extrusion of a circle pierced by a square (see `apps.qs.extruMesher3d`

and `apps.qs.extruMesher3dTx`

or `apps.qs.extruMesher3dTorsion`

`apps.qs.extruMesher3dDist03`

for modified extrusions).

The definition and meshing of the circle can be seen in the the file. To extrude the result (`Side`

#1):

mesher = ExtrusionMesher3D(sideset(1), groupset(1)) mesher.setFillGroup(True) mesher.setDirection(0.0,0.0,1.0) mesher.setLength(length) mesher.setNbOfLayers(nLayers, dist = 1.0) mesher.setAnglefct(fctAngle) mesher.setXfct(fctX) mesher.setYfct(fctY) mesher.execute() grpNo = mesher.getLastLayer(no)

Group 1 | all the mesh element refer to this group (the `FieldApplicator` is applied to this group) |

setFillGroup() | fills Group 1 with the nodes of the mesh |

setDirection | direction of the extrusion (by default = `z` ) |

setLength | length of the extrusion |

setNbOfLayers | nLayers : number of extruded elements |

dist : ratio between the length of the last and first element (default : dist = 1.0) | |

setAnglefct(fctAngle) | Application of a rotation of slices around extrusion vector (direction 'z' but starting from origin!!!) |

fctAngle | One parameter defining rotation of slices function in degrees (t) - t=[0,1] ATTENTION : fctAngle(0) = 0 |

setXfct(fctX) | Application of a modification of the generatrice direction in X Direction |

setYfct(fctY) | Application of a modification of the generatrice direction in Y Direction |

fctX/fctY | One parameter defining modification of generatrice : fct(t) - ATTENTION t=[0,Length] and fctX/fctY(0) = 0 |

execute | execute the extrusion |

getLastLayer(no) | returns the group grpNo (number `no` ) which contains the nodes of the last layer |

When meshing in 2D, the wires must be defined “area to the left”

In a same way, a planar face meshed with triangles can be extruded in 3D to be meshed with prisms (see `apps.monosMeca.monoTrac3dPenta`

).

After the extrusion of a `Side`

, a `Skin`

or a `Group`

, the geometry can also be extruded from a `Side`

with the function:

mesher.createGeometryOn(Side, NoGObject, geometry)

Geometrical objects are created and numbered starting from NoGObject.

The function `createLineAbove`

can create only one `Line`

corresponding to the extrusion of a `Point`

:

line = createLineAbove(pt1, NumLine, NumPtOnTop, geometry)

To create a geometry after the extrusion of a `Side`

, this function is used:

mesher.createGeometry(NoGObject, geometry)

To use this function, the target to extrude must be of type `Side`

Geometrical objects are created and numbered starting from NoGObject.

The retrieval of the created geometrical objetcs is done with the functions:

Vol1 = mesher.getVolumeOnTop(side1) side = mesher.getSideOnTop(curveOrSide) curve = mesher.getCurveOnTop(pointOrCurve) point = mesher.getPointOnTop(ptref)

Vol1 | |

side | `Side` created from the object `curveOrSide` (which corresponds to a `Curve` or a `Side` of the extruded object). If : `curveOrSide` = `Curve` → the returned `Side` is tangent to the extrusion direction. If: `curveOrSide` = `Side` → the extrusion direction is a vector which is normal to the returned `Side` |

curve | `Curve` created from `pointOrCurve` (which corresponds to a `Point` or a `Curve` of the extruded object) If : `pointOrCurve` = `Point` → the returned `Curve` is tangent to the extrusion direction. If: `pointOrCurve` = `Curve` → the extrusion direction is a vector which is normal to the returned `Curve` |

point | `Point` created from `ptref` (`Point` of the extruded object) |

The geometry is created in the test cases `apps.welding.welding`

and `aspCrushing.tests.threeD.smoothStripRoughTool`

.

<important note>
CAREFUL, after creating the geometry, the `Volume`

, returned by the function `mesher.getVolumeOnTop(side)`

must be added with the `push`

command to the `FieldApplicator`

in place of the group (groupset(1) of the constructor of the object `ExtrusionMesher3D`

). In the case where only one layer of elements is found in the extrusion direction, the group (groupset(1) of the constructor of the object `ExtrusionMesher3D`

) must be added with the `push`

command in the `FieldApplicator`

, whichever the extruded entity (`Side`

, `Skin`

or `Group`

).
</note>

Axisymmetric extrusion of a meshed side. The extrusion can be open ($0 < \mbox{angle} < 360^\circ$) or close ($\mbox{angle} = 360^\circ$).

To this day, no reconstruction of the extruded geometry exists. `Groups`

should be used to set boundary conditions.

mesher = RevolutionExtrusionMesher3D(gobject, group, axe, angle=180.0) setAngle(angle) mesher.setNbOfLayers(10) mesher.execute()

gobject | Meshed 2D geometrical entity |

group | Group father of the 3D mesh elements |

axe | Line which defines the revolution axis |

setAngle | Angle of the extrusion (in degrees 0.0 < angle ⇐ 360.0 - default = 180.0) |

setNbOfLayers | number of extruded elements |

setFillGroup | fill the reference group with all nodes (base & generated) |

execute | executes the extrusion |

getLastLayer | return the group of the last layer (if not closed extrusion) |

doc/user/geometry/mesh/3d.txt · Last modified: 2021/11/19 14:52 by papeleux