You are here: metafor.ltas.ulg.ac.be » doc » Documentation » elements » General Points » Volume element

doc:user:elements:volumes:volumeelement

In this section, Metafor volume element are described. A `FieldApplicator`

interaction is associated to them.

`Volume2DElement`

and `Volume3DElement`

are basic elements in Metafor. `Volume2DElement`

is a quadrangle with 4 nodes in 2D, while `Volume3DElement`

is a hexaedron with 8 nodes in 3D. Each element has respectively 8 and 24 degrees of freedom.

By default, if $n$ is the degree of mechanical interpolation and $d$ the element dimension, the number of integration points in the deviatoric part of the stress field is $(n+1)^{d}$, unless stated otherwise with the definition of `NIPDKSI`

, `NIPDETA`

or `NIPDZETA`

(see Parameters).

For example, the interpolation of `Volume2DElement`

is of the first degree ($n=1$), and it is a 2D element ($d=2$), leading to 4 integration points.

The number of integration points in the volume part of the stress field (pressure) depend on the chosen method to integrate stresses and cannot be modified.

- The angular velocity
`OMEGA`

is used when loading comes from centrifugal forces (whatever the integration scheme). - Both start and end points of the rotation axis can be moved (see fixation and loading).

- When
`MDE_IQSI=1`

and`MDE_NDYN=2`

, centrifugal forces are computed during a quasi-static equilibrium phase. Then, they are replaced by the real structural rotation. - If
`MDE_IQSI=2`

and`MDE_NDYN=2`

: The quasi-static equilibrium phase is applied, but the frame of the blade is still used.

* `MDE_IQSI=0`

:

ti.setUseInitialRotationBalancing(False)

* `MDE_IQSI=1`

:

ti.setUseInitialRotationBalancing(True) ti.setShiftToFixedFrame(True)

* `MDE_IQSI=2`

:

ti.setUseInitialRotationBalancing(True) ti.setShiftToFixedFrame(False)

* `MDR_DTMR`

:

ti.setInitialRotationFactorIncrement(_initialRotationFactorIncrement)

ti is a reference towards the current dynamic time integration scheme.

- In axisymmetric modeling, Selective Reduced Integration with Pressure Report
`VES_CMVIM_SRIPR`

must be used. - EAS Formulation is not valid in axisymmetric modeling, some EAS modes are missing along $\theta$.

Thermomechanical formulation of `Volume[2][3]DElement`

.

For the mechanical part, linear elements are still used, so a 4-nodes quadrangle in 2D and a 8-nodes hexaedron in 3D, leading to 8 and 24 degrees of freedom.

For the thermal part, first (`TmVolume[2|3]DElement`

) or second (`Tm2Volume[2|3]DElement`

) order thermal nodes are added.

`TmVolume[2|3]DElement`

has therefore 4/8 degrees of fredom in 2/3D, when `Tm2Volume[2|3]DElement`

has 8/20 dofs.

By default, the number of integration points in the deviatoric and volume part of the stress field is equal to those of `Volume[2|3]DElement`

.

Likewise, the default number of integration points is given by $(m+1)^d$, where $m$ is the thermal degree of interpolation (different from the mechanical one for `Tm2Volume[2|3]DElement`

). This number can be changed by the definition of `NIPTKSI`

, `NIPTETA`

or `NIPTZETA`

.

Volume mechanical element with the shape of a pentahedron (a triangular prism to be more accurate). This pentahedron has 6 nodes, so 18 dofs.

By default, stresses are integrate over 2 integration points in the deviatoric part, unless stated otherwise by the definition of `NIPDKSI`

, `NIPDETA`

or `NIPDZETA`

. The number of integration points in the volume part of the stress field (pressure) depends on the chosen method to integrate stresses are cannot be modified.

3-nodes triangular element in 2D, 6 dofs.

By default, stresses are integrate over 1 integration points in the deviatoric part.

4-nodes tetrahedron in 3D, 12 dofs.

By default, stresses are integrate over 1 integration points in the deviatoric part.

`QuadVolume2DElement`

and `QuadVolume3DElement`

are quadratic elements. `QuadVolume2DElement`

is a 8-nodes quadratic quadrangle, `QuadVolume2DElement`

a 20 quadratic hexaedron. They are purely mechanical, with respectively 16 and 60 dofs.

By default, stresses are integrate over 4/27 integration points in the deviatoric part in 2/3D, with the formula already stated for `Volume[2|3]DElement`

. The standard formulation must be used (`CAUCHYMECHVOLINTMETH = VES_CMVIM_STD`

), which is not the default one.

*Remark*: To use these higher order elements, the mesh must be also defined as second or third degree.

Quadratic, 6-nodes triangular element in 2D, 12 dofs. The standard formulation must be used (`CAUCHYMECHVOLINTMETH = VES_CMVIM_STD`

).

By default, stresses are integrated over 3 integration points in the deviatoric part.

*Remark*: To use these higher order elements, the mesh must be also defined as second or third degree.

Quadratic, 10-nodes tetrahedron in 3D, 30 dofs. As with quadratic elements in 2D, the standard formulation must be used (`CAUCHYMECHVOLINTMETH = VES_CMVIM_STD`

).

By default, stresses are integrated over 4 integration points in the deviatoric part.

*Remark*: To use these higher order elements, the mesh must be also defined as second or third degree.

The AEJ element (“Average Elemental Jacobian”) is a first degree triangle/tetrahedron, used to avoid locking which appears with standard formulation in incompressible configurations (Poisson ratio close to 0.5, Von Mises plasticity).

*Careful* : This elements must be used together with the integration scheme CAUCHYMECHVOLINTMETH = VES_CMVIM_AEJ.

The idea is to replace the *kinematic* Jacobian $J_e$ of the element by a new value called $J_{e,aej}$. This modified Jacobian is obtained by:

- defining nodal Jacobians $J_I$, equal to the rate of volume change around this node (which requires a sum over neighboring triangles/tetrahedra).
- averaging the $J_I$ over the element.

This corresponds to setting the incompressibility constraints to the nodes, and no longer to the integration points. The degrees of freedom of the AEJ element are then extended, corresponding to these of the standard triangle/tetrahedron augmented by the dofs of neighboring nodes.

Code Metafor | Description | Dependency |
---|---|---|

`MATERIAL` | Number of the volume material to consider | - |

`STIFFMETHOD` | Method used to compute the stiffness matrix = `STIFF_ANALYTIC` : analytic matrix (default) = `STIFF_NUMERIC` : numerical matrix | - |

`DAMPSTIFF` | Part of the Stiffness matrix used to build damping matrix used by Damped Time Integration scheme usual value : 1.0e-7 - 1.0e-5 | Time (need DMUPERSTEP or DMUPERSTAGE) |

`DAMPMASS` | Part of the Mass matrix used tobuild damping matrix used by Damped Time Integration scheme usual value : 1.0e3 - 1.0e5 | Time (need DMUPERSTEP or DMUPERSTAGE) |

`OMEGA` | Angular speed (°/s) to simulate a rotating frame (calculation of centrifugal and Coriolis forces). If `MDE_IQSI=1` and `MDE_NDYN=2` , centrifugal forces are computed during a quasi-static equilibrium phase. Then, they are replaced by the real structural rotation. If `MDE_IQSI=2` and `MDE_NDYN=2` , centrifugal forces are computed during a quasi-static equilibrium phase. Then, the simulation is carried in the moving frame, so centrifugal and Coriolis forces are taken into account in the model. | time |

`OMEGA_PT1` | Number of the first point which defines the rotation axis | - |

`OMEGA_PT2` | Number of the second point which defines the rotation axis | - |

`CORIOLIS` | Boolean to take into account Coriolis forces in a moving frame, during a dynamic simulation. True (default) / False | - |

`GRAVITY_X` , `GRAVITY_Y` , `GRAVITY_Z` | Gravity | time |

`CAUCHYMECHVOLINTMETH` | Method used to integrate the mechanical part of volume elements (stresses) = `VES_CMVIM_SRI` = `VES_CMVIM_SRIPR` (default) = `VES_CMVIM_STD` = `VES_CMVIM_EAS` | - |

`CONSERVINGMETHOD` | Use of `conservative algorithm` = `VES_WITHOUTCORRECTION` : plastic correction tensors neglected (default) = `VES_WITHCORRECTION` : plastic correction tensors considered | - |

`NIPDKSI` , `NIPDETA` , `NIPDZETA` | Number of deviatoric integration points in each direction | - |

`NIPTKSI` , `NIPTETA` , `NIPTZETA` | Number of thermal integration points in each direction | - |

`EASS` | Number of pure shear modes for the EAS formulation (careful, the default value corresponds to 3D modeling, for 2D set `EASS` to 2)2D : 2 3D : 6 (default) or 12 | - |

`EASV` | Number of volume modes for EAS formulation (careful, the default value corresponds to 3D modeling, for 2D set `EASV` to 2) 2D : 2 or 4 3D : 3 (default) or 9 | - |

`KEAS` | Local stifness matrix for EAS formualtion =0 : local tangent matrix EAS analytic (default) =1 : local tangent matrix EAS numerical | - |

`IEAS` | Maximal number of iterations for the calculation of EAS modes (default : 10) | - |

`TEAS` | Transformation of EAS modes from the isoparametric space =0 : Simo-Armero transformation (default) =1 : Glaser-Armero transformation [do not use, still under development] | - |

`EEAS` | Extrapolation of EAS modes =0 : modes set to 0 for each time step (safe but slow). =1 : classical extrapolation (default) =2 : initialization to the value corresponding to the previous step. =3 : set to 0 for each iteration | - |

`PEAS` | Accuracy of resolution of EAS modes (default: 1.0e-8) unfortunately NOT adimensional!!! ⇒ = 1.0e-8 for “small tests” in mm ⇒ = 1.0e-6 for “real tests” in mm ⇒ = 1.0e-9 for “real tests” in m | - |

`VERBOSE` | (bool) Debug information concerning resolution of EAS (default: false) | - |

doc/user/elements/volumes/volumeelement.txt · Last modified: 2020/12/29 18:27 by tanaka