`***mesh`#

Description#

Under the mesh description command we may specify the formulation used to satisfy the governing equations of the problem, including assumptions of a quasi-geometrical nature such as plane stress or plane strain conditions. The formulations possible in mechanical problems include classical small deformations, Total-Lagrangian, Updated-Lagrangian, or special cases such as the Cosserat continuum. Thermal problems do not have any alternate formulations.

The procedure also allows specifying a geometry file different than prob.geof.

Syntax#

The syntax for this command is summarized below:

***mesh [ element_type ] \(~\,\) **file filename \(~\,\) **elset elset-name [ element_type ] \(~\,~\,\) *section type \(~\,~\,~\,\) … \(~\,\) **local_frame type \(~\,~\,~\,\) … \(~\,\) **import type fname \(~\,\) **predefined type

The argument element_type defines the type of element (its formulation) which will be used throughout the element set in question. The different types possible are described on the following pages. In order to simply apply the element formulation to the whole structure, fill in the element_type on the same line as the ***mesh keyword. In order to define different element types for different regions of the mesh, put the element_type keys after **elset sub-commands.

Note that plane element geometries in 2D require a specification of element formulation in order to distinguish plane stress or plane strain. The default element type only applies to axisymmetric geometries in 2D. Element names with plane_strain will enforce the \(\epsilon_{33}=0\) condition, while elements with plane_stress enforce \(\sigma_{33}=0\) ¹ ¹Plane stress is imposed in Z-set using additional degrees of freedom, and not at the material behavior level, although this exists too with some of the behaviors (notably gen_evp; see page ). For plane stress behaviors, one must choose ironically plane_strain element formulations..

**elset elset-name

sets the element formulation and possibly other characteristics for a given element set name. When used, no element formulation should be given after the ***mesh keyword.

*section type: this elset sub-command assigns section properties to a shell mesh. See the separate pages following which describe the particular sections available (starting at page ).

**file

Indicates that the mesh is in a file named other than problem.geof.

**import

Indicates that the mesh file is in a separate file, and in a format other than native Z-set. It is normally recommended to use the batch mesher to translate the mesh before running the analysis (see page ).

**local_frame

Assigns a local frame to the degrees of freedom attached to an elset (see page following at ).

**predefined type

Predefined elements may be used to quickly perform calculations on certain meshes. These are limited currently to single elements which can be used to quickly test and verify material behaviors. The predefined type type may be chosen from the following elements: cax8, cax8r, c2d8, c2d8r, cax4, cax4r, c2d4, c2d4r, rve1d, rve2d, rve3d, c3d20, and c3d20r. One can use Zrun -H to see the installed predefined elements.

The elements will be defined in the positive quadrant in a rectangle or cube form with its limits at 1. Two dimensional elements have liset and nsets defined as bottom, right, top, and left.

Caution

In each calculation there may exist several different element types, and several different materials. Unfortunately, the dynamic structure of the program limits the ability to do exhaustive compatibility verification. Caution must therefore be given to the consistency of options within a calculation. The verification procedure will be improved in the next version of the code.

Example#

The following is an example of the “simple” use of ***mesh to assign the whole problem to be a plane stress case, with a single predefined mesh as a 8 nodes 2D element.

***mesh plane_stress
   **predefined c2d8

The second example is of a mesh stored in a fully qualified path name file, and two element sets with different element formulations.

***mesh
  **file  /home/user/meshes/big_mesh.geof
  **elset rubber_part total_lagrangian
  **elset stiff       small_deformation

Mechanical calculations#

The following are brief descriptions of the mechanical element formulations available:

spr: Spring (or pinned truss) elements for one or 2 node geometries (l2d1 l2d2 l3d1 l3d2). This element requires that a valid spring material behavior be assigned to all such elements. The two node element realigns with the line between those two nodes, and is therefore non-linear.
linear_spring: A linearized version of the spring element, so no non-linearities are introduced.
small_deformation, plane_strain, small_deformation_plane_strain: Mechanical elements in small deformation formulations. The integration volume is that of the initial structure, and significant rotations may cause erroneous calculation of the strain. The default 2D geometry is axisymmetric. Choosing the plane_strain option will enforce the \(\epsilon_{33}=0\) condition.
plane_stress: Plane stress 2D element formulations. In order to be compatible with all material behaviors, this element adds degrees of freedom to each Gauss integration point which represent the strain \(\epsilon_{33}\). These DOFs are used to enforce zero surface pressure and therefore \(\sigma_{33}=0\). Relationships may however be defined using the MPC command in order to specify generalized plane strain conditions. Setting the EZ (\(\epsilon_{33}\)) DOF variable to be uniform over an elset yields zero overall applied pressure, but allows variation in the \(\sigma_{33}=0\) field. The \(3\)-direction strain will of course be uniform.
small_deformation_updated, plane_strain_updated, _plane_stress_updated: Identical to the non _updated formulations but using the geometry at the end of an increment as the integration volume. This produces non-linear structural behavior even with linear behavior models.
small_deformation_select_int, small_deformation_select_int_updated: Special version of small deformation elements for linear interpolation to solve the problem of strong local variations or oscillations in the stress fields (esp. pressure terms).
cb_shell, cb_shell_updated_lagrangian: Shell elements formulated using the so-called “continuum based shell” assumption: the mechanical response of the shell element is computed using an underlying 3D volumic element whose geometrical configuration is dynamically constructed at runtime by the mother shell element. See for instance the corresponding chapter in the book: {em Nonlinear Finite Elements for Continua and Structures}, T. Belytschko, W.-K. Liu and B. Moran, Wiley. This element type uses 5 degrees of freedom per node: three displacements U1, U2, U3, and two rotations W1 and W2. Thus the rotation is assumed to be continuous along the shell. Note that you must also give the initial thickness of the shell for this elset, using the following syntax:

**elset shell_part cb_shell
  *thickness 0.1

total_lagrangian, total_lagrangian_plane_strain

Elements formulated for large displacement using Total-Lagrangian assumptions. These elements do not have any straining under rigid body motions.

total_lagrangian_mixte_u_p, total_lagrangian_plane_strain_mixte_u_p

Incompressible elements in large displacements. The formulation is a mixed pressure-displacement Total-Lagrangian method with degrees of freedom for the pressure at certain nodes.

total_lagrangian_mixte_u_ps, total_lagrangian_plane_strain_mixte_u_ps

Incompressible elements in large displacements. The formulation is a mixed pressure-displacement Total-Lagrangian method with a single pressure degree of freedom per element.

updated_lagrangian, updated_lagrangian_plane_strain, updated_lagrangian_plane_stress

Updated Lagrangian element formulation for finite strain calculations. Must be used in the finite strain case for materials with internal variables such as metal plasticity or porous plastic materials. This element type slt/must/ be used in conjunction with behaviors modified for updated Lagrangian methods (see the command ***behavior).

periodic, periodic_plane_strain

periodic elements in axisymmetric, 3D, or plane strain. These elements allow one to impose the mean stress values for a periodic cell. Note that the displacement field that is saved by default is the {em total} displacement field and {em not} only its the periodic part. You can override this choice and save only the periodic part by appending after the periodic keyword: periodic_info **periodic_displacement_field.

smallw, smallw_updated

Continuous mechanical element small displacement, small rotation - 3D only. This element combined with an appropriate behavior such as a smallw crystal can be used to model texture evolution in a crystal for moderate deformations.

2_5D, 2_5D_updated

two and one half dimension elements. These use a 3D material law with a 2D geometry. There are six degrees of freedom per Gauss point (element DOFs) \([ t_1~t_2~t_3 ]\) and \([ w_1~w_2~w_3 ]\). The structures displacement field is:

(93)#\[\vect u\left( x,y,z\right) =\vect u_0\left( x,y,z\right) + \vect u_1\left( x,y\right)\]

(94)#\[\begin{split}\begin{aligned} u^x &=&u_1^x+zt_1-w_3\left( y-Y_0\right) z \\ u^y &=&u_1^y+zt_2+w_3\left( x-X_0\right) z \\ u^z &=&u_1^z+zt_3+w_1\left( y-Y_0\right) z-w_2\left( x-X_0\right) z \end{aligned}\end{split}\]

With this element, one can use full 3D material behaviors, and fix out of plane degrees of freedom. The values of \(X_0\) and \(Y_0\) are modified through the ***specials command.

2_5D periodic

It is a small deformation periodic 2_5D element. These use a 3D material law with a periodic 2D geometry The displacement field is searched for in the form

(95)#\[\vect u(x,y,z) = \ten E \cdot \vect x + z\vect t +z\vect w \wedge (\vect x-\vect x_0) + \vect U(x,y)\]

with \(\vect x_0(x_0,y_0,0)\) and \(E_{11}, E_{22}, E_{12}\) are the only non-vanishing components of \(\ten E\). The nodal dof are \(U_1, U_2\). The element dof are \(E_{11}, E_{22}, E_{12},t_1,t_2,t_3,w_1,w_2,w_3\). The previous equation is now written in components:

(96)#\[\begin{split}\begin{aligned} u_1 &=& E_{11}x + E_{12}y + zt_1 - w_3z(y-y_0) + U_1(x,y) \nonumber \\ u_2 &=& E_{12}x + E_{22}y + zt_2 + w_3z(x-x_0) + U_2(x,y) \nonumber \\ u_3 &=& z t_3 - w_2z(x-x_0)+w_1z(y-y_0) \nonumber \end{aligned}\end{split}\]

The gradient of the displacement field is:

(97)#\[\begin{split}\begin{aligned} \left[ \begin{array}{ccc} u_{1,1} & u_{1,2} & u_{1,3} \\ u_{2,1} & u_{2,2} & u_{2,3} \\ u_{3,1} & u_{3,2} & u_{3,3} \end{array} \right] = \left[ \begin{array}{ccc} E_{11}+U_{1,1} & E_{12}+U_{1,2}-w_3 z & t_1-w_3(y-y_0) \\ E_{12}+U_{2,1}+w_3z & E_{22}+U_{2,2} & t_2+w_3(x-x_0) \\ -w_2z & w_1z & t_3+w_1(y-y_0)-w_2(x-x_0) \end{array} \right] \nonumber \end{aligned}\end{split}\]

The associated strain field is:

(98)#\[\begin{split}\begin{aligned} \left[ \begin{array}{ccc} \varepsilon_{11} & \varepsilon_{12} & \varepsilon_{31} \\ - & \varepsilon_{22} & \varepsilon_{23} \\ - & - & \varepsilon_{33} \end{array} \right] = \left[ \begin{array}{ccc} E_{11}+U_{1,1} & E_{12}+(U_{1,2}+U_{2,1})/2 & (t_1-w_3(y-y_0)-w_2 z)/2 \\ - & E_{22}+U_{2,2} & (t_2+w_3(x-x_0)+w_1z)/2 \\ - & - & t_3+w_1(y-y_0)-w_2(x-x_0) \end{array} \right] \nonumber \end{aligned}\end{split}\]

pressure

Fluid interface mesh pressure elements.

cosserat, cosserat_plane_strain, cosserat_plane_stress

Mechanical elements modified for the Cosserat continuum. This method adds DOFs at each node for an independent micro-polar rotation named W3. This method allows limitation of localization under shear deformation in strain-softening materials. The method uses a characteristic material length which must be input in the material definition, and the behavior must be modified for the Cosserat formulation (see the ***behavior command).

Thermal calculations#

For thermal calculations, the type of element is completely defined by the geometry given in the .geof file. The ***mesh command should thus only be used if an alternate geometry file name is to be used.

***mesh

On this page

***mesh#