MESHING TYPES Part [El_type] [El_variant] [BASE bpart_name or bpart_index]

            

The MESHING TYPES command is used to define the type of element that will be created on existing parts of the geometry when a mesh is generated, it does not set a default type for future geometry creation.

Selection of the specific element types required by a particular FEM package is achieved by using either the generic element type and an element variant or by using a specific FE package element name.

Part El_type

ALL Any-type or NONE

POINTS P-EL or NONE

STRAIGHT 1D-type or NONE

ARC 1D-type or NONE

SPLINE 1D-type or NONE

3SIDES 2D-type or NONE

4SIDES 2D-type or NONE

REGION 2D-type or NONE

4SURFS 3D-type or NONE

5SURFS 3D-type or NONE

6SURFS 3D-type or NONE

PRISM 3D-type or NONE

GBODY 3D-type or NONE

point_name P-EL or NONE

Line_name 1D-type or NONE

Surface_name 2D-type or NONE + BASE

Body_name 3D-type or NONE + BASE

Set_name Any type or NONE

Return Level: MESHING TYPES except for Part ALL which returns to the top level.

Notes:

1.

FEMGEN generic element types
Full details of the generic element types available in FEMGEN are given in Appendix C of the User Manual Appendices.

2.

Element types for `ALL' and `Set_name'
In these two cases, only parts with appropriate geometry will be assigned an element type and variant.

3.

Default Element types
When lines are created the default situation is that as long as no surfaces exist in the model, all lines are given the element type `BE2'. When the first surface is defined these element types are cleared and a `QU4' element type is given to surfaces as they are created (unless another suitable element type is given in the surface definition). A similar change is made to the surface element definitions when the first body is defined.

4.

Element type selection

The operation of this commmand depends on whether an analysis specific environment has been selected.

FEMGEN Neutral environment

When the FEMGEN neutral environment is active (as shown by `Analysis: NEUTRAL' in the monitor) then element types are selected with the generic element type and, optionally, a variant number.

FEM Specific analysis environment

When a specific FEM analysis environment is active (as shown by `Analysis: FEM package name, then element types can be selected in three ways:

(a)

From the menu select a generic element type followed by the required element name from the list shown.

(b)

Use the command line to give the required finite element name for `El_type'

(c)

Use a generic `El_name' and a variant number.

A specific FEM analysis environment can be selected with the PROPERTY FE Program_name command or by using the environment variable `FG_PRE_INT=fem package'. Please refer to the Workstation User Guide for more information on environment variables.

See also Note 6 below.

5.

The El_variant control
The El_variant parameter is an integer selecting one of the possible element variants in the desired FEM-program; the default 1.

It is possible to select different defaults for the element variants by use of the Resource Manager file. (Please refer to the Installation and Customisation Guide for more details).

For each supported FEM-program and each FEMGEN geometric element type, there are a number of element variants. The element types that are supported and their variant numbers can be listed with the command UTILITY TABULATE FE [Program_Name] [El_type].

6.

Point elements
A point element P-EL may be specified for a point. Only a single element type is available although variants may be specified. At no stage are points given a default element type.

7.

Element types for regions
Only TR3, TR6, TR9 or TR15 elements may be specified for surfaces created with the GEOMETRY SURFACE REGION command and with meshing algorithm set to DELAUNAY.

Only QU4, QU9, QU9 or QU12 elements may be specified for surfaces created with the GEOMETRY SURFACE REGION command and with meshing algorithm set to PAVING.

8.

Element types for tetrahedral bodies
Only TE4, TE10 and TE16 elements may be generated in tetrahedral (four surface bodies).

9.

Element types for prisms
Only PE6, PE15 or PE24 elements may be specified for bodies (prisms) created by sweeping surfaces created with the GEOMETRY SURFACE REGION command and with meshing algorithm set to DELAUNAY.

Only HE8, HE20, HE27 or HE32 elements may be specified for bodies (prisms) created by sweeping surfaces created with the GEOMETRY SURFACE REGION command and with meshing algorithm set to PAVING.

10.

Element types for general bodies
Only TE4, TE10, TE16 elements may be specified for general bodies.

11.

Removing element types
The MESHING TYPES Part NONE will prevent elements being generated on the named part.

12.

The BASE control
The BASE keyword is only for use with interface element types. It is used to control the orientation of the elements during mesh generation, ref: MESHING OPTIONS CHECK INTER-ELS. The through-thickness direction of the interface elements is taken as the direction from the base_part to the part, of the same type, that is opposite. The base_part must be a surface if the meshed part is a body and a line if the meshed part is a surface.

For the case in which an interface element type has been specified for a named body, the optional keyword BASE may be used in order to redefine the base surface for that body. The base surface of a body B1 is that which is first output under the command, UTILITY TABULATE GEOMETRY B1. The base surface may be specified by name (and if so must be a constituent surface of the definition of the body to which the command has been applied), or by an integer index from 1 to 6. For 5-surfaced bodies or prisms, the first or second surfaces in the body definition may be used [index 1 or 2], whereas for 6-surfaced bodies, any of the surfaces in the body definition may be used [index 1,2,3,4,5 or 6].

The BASE keyword may only be applied to prisms, and bodies of 5 or 6 surfaces.

For the case in which an interface element type has been specified for a named 4-sided surface, the optional keyword BASE may be used in order to redefine the base line for that surface. The base line of a surface S4 is that which is first output under the command, UTILITY TABULATE GEOMETRY S4. The base line may be specified by name (and if so must be a constituent line of the definition of the surface to which the command has been applied), or by an integer index from 1 to 4.

The BASE keyword may only be applied to 4-sided surfaces.

Rules for Divisions

1.

The number of divisions along a side must be $<$100.

2.

A side with 1 mid-side node must have an even number of divisions.

3.

A side with 2 mid-side nodes must have a number of divisions that is divisible by three.

4.

For TR3 elements there are no restrictions.

5.

For QU4 elements the sum of the divisions around a surface must be an even number.

6.

For QU8 and QU9 elements the sum of the divisions around a surface must be a multiple of 4 (because of rules 2 and 5).

7.

For QU12 elements the sum of the divisions around a surface must be a multiple of 6 (because of rules 3 and 5).

8.

For bodies, the divisions on the second surface (the top) must correspond to the divisions on the first surface (the bottom) and the rules above apply for each surface of the body even if no surface elements are generated.

Also, all sides connecting the top and bottom surfaces must have an equal number of divisions.

Examples:

1.

MESHING TYPES S1 QU8

Elements on surface S1 will be type QU8 and by default will be variant 1.

2.

MESHING TYPES ALL HE20 2

All 3D Elements will be type HE20 variant 2.

3.

MESHING TYPES ALL C3D20

All 3D Elements will be ABAQUS element type C3D20, provided that the ABAQUS analysis environment has been selected.

4.

MESHING TYPES L1 BE2 4

Elements on line L1 will be type BE2. Variant 4 will be used in analysis.

5.

MESHING TYPES 3SIDES TR6 2

All elements on all triangular surfaces will be TR6 variant 3.

6.

MESHING TYPES REGION TR15

All elements on all regions will be type TR15.

7.

MESHING TYPES PRISM SOLID73

All elements of all prisms will be ANSYS element type SOLID73, provided that the ANSYS analysis environment has been selected.

8.

MESHING TYPES B12 IS44 1 BASE S14

The elements on body B12 will be interface element type IS44, variant 1, with B12 redefined with a base surface of S14.

9.

MESHING TYPES B14 IS84 BASE 2

The elements on body B14 will be interface element type IS84, with B14 redefined with base surface to be the second surface referenced in the current definition of B14.

10.

MESHING TYPES S7 IL32 7 BASE 4

The elements on surface S7 will be interface element type IL32 variant 7, with S7 redefined with base line to be the fourth line referenced in the current definition of S7.

See also the following commands

'GEOMETRY BODY'
'GEOMETRY SURFACE'
'GEOMETRY LINE'
'UTILITY TABULATE FE'
'PROPERTY FE'