# TR.14.2 Element Mesh Generation

This set of commands is used to generate finite element meshes. The procedure involves the definition of super-elements, which are subsequently divided into smaller elements.

## Description

Tip: It is generally recommend that you use the parametric method of mesh generation (See TR.14.1 Parametric Mesh Models) so you can modify the mesh parameters after creating the mesh.
Note: This method of generating element meshes is a one-type operation. That is, once you have saved the STAAD.Pro input file using these commands, the program will replace these commands with the resulting nodes and elements this command generates.

This is the second method for the generation of element incidences. If you needs to divide a big element into a number of small elements, you may use this facility which generates the joint numbers and joint coordinates, the element numbers and the element incidences automatically. Use of this feature consists of two parts:

1. Definition of the super-element boundary points: A super-element may be defined by either 4 boundary points or 8 boundary points ( see figure below). A boundary point is denoted by a unique alphabet (A-Z in upper case or a-z in lower case) and its corresponding coordinates. Hence, any 4 or 8 of the 52 characters may be used to define the super-element boundary. If 4 points are used to define the super-element, each side of the super-element will be assumed to have a straight edge connecting the 2 points defining that side. If 8 points are used, each side will be a smooth curve connecting the 3 points defining that side.
2. Generation of sub-elements: define the super-element using boundary points (4 or 8 as explained above) and specify the total number of sub-elements required.

## General Format

`DEFINE MESH`
`Ai xi yi zi ( { CYLINDRICAL, RCYLINDICRAL } ( x0, y0, z0 ) )`
`…`
`Aj xj yj zj ( { CYL, RCYL } ( x0, y0, z0 ) )`
`GENERATE ELEMENT { (QUADRILATERAL), TRIANGULAR }`
`MESH Ai Aj … n1 (n2)`
`MESH Am An … n3 (n4)`
`…`

(up to 21 MESH input lines)

Where:

ParameterDescription
Ai, Aj Letters A-Z or letters a-z. The maximum is 52.
xi, yi, zi Coordinates for boundary point Ai.
x0, y0, z0 Optional Cartesian coordinates of the origin for cylindrical coordinates when CYL (cylindrical) or RCYL (reverse cylindrical) options are used. This defaults to the global origin of the model (0,0,0).

The 3 fields (xi, yi, zi) may be replaced by a joint number whose coordinates have been defined in the JOINT COORDINATE command by entering Ai JOINT jn instead.

ParameterDescription
Ai, Aj, Ak A rectangular super-element defined by four or eight boundary points.
n1 Number of elements along the side A i Aj of the super-element. (Must not exceed 28).
n2 Number of elements along the side A j Ak of the super-element. (Must not exceed 28).

If n2 is omitted, that is, only n1 is provided, then n1 will indicate the total number of elements within the super-element. In this case, n1 must be the square of an integer.

## Limits

There is a limit of 21 Mesh commands. Up to 33,000 joints may be generated and up to 67,000 elements. Total number of joints in the model after this command is completed may not exceed 100,000.

## Notes

All coordinates are in current unit system. While using this facility you has to keep the following points in mind:

1. All super-elements must be 4-noded or 8-noded. Generated elements for 4-noded super-elements will retain the straight-line edges of the super-elements, while joints of elements generated from 8-noded super-elements will lie on a curved trajectory.

 A) Mesh generated for a 4-noded super-element B) Mesh generated for an 8-noded super-element

### Mesh generation for super elements

2. Two super-elements, which have a common boundary, must have the same number of elements along their common boundary.
3. Sequence of super-elements - MESH commands define the super-elements. The sequence of this MESH command should be such that once one is defined, the next super-elements should be the ones connected to this. Therefore, for convenience, the first super-element should be the one, which is connected by the largest number of super-elements. In the example shown here for the tank, the bottom super-element is specified first.
4. This command must be used after the MEMBER INCIDENCE and ELEMENT INCIDENCE section and before the MEMBER PROPERTIES and ELEMENT PROPERTIES section. The elements that are created internally are numbered sequentially with an increment of one starting from the last member/element number plus one. Similarly the additional joints created internally are numbered sequentially with an increment of one starting from the last joint number plus one. It is advisable that users keep the joint numbers and member/element numbers in a sequence with an increment of one starting from one.
5. If there are members embracing a super-element which is being meshed, you must take care of the required additions/modifications in the MEMBER INCIDENCE section themselves since a few more new joints might appear on the existing common boundary as a result of meshing the super-element. See the following figure:

### Additional joints on a super element

Note: If a member exists between points A and B, the user must breakup this member into 4 parts. Members will not be meshed automatically.
6. The sub-elements will have the same direction (Clockwise or Anti-clockwise) as the super-elements. For a super-element bounded by four points A, B, C and D, if ABCD, BCDA etc. are in clockwise direction, CBAD or DCBA etc. are in anti-clock wise direction. If the particular super-element is denoted as ABCD, all the sub-elements in it will have a clockwise element incidence in this example.
7. Element incidences of the generated sub-elements may be obtained by providing the command 'PRINT ELEMENT INFORMATION' after the 'MESH...' command in the input file.
8.  If the STAAD input file contains commands for JOINT COORDINATES, MEMBER INCIDENCES, ELEMENT INCIDENCES, and MESH GENERATION, they should be specified in the following order:

```STAAD SPACE
UNIT  …
JOINT COORDINATES
…
MEMBER INCIDENCES
…
ELEMENT INCIDENCES
…
DEFINE MESH
…
GENERATE ELEMENT
… ```
9. Newly created joints will be merged with existing joints if they are within 0.001 inches of each other.

## Example

The following section of input illustrates the use of MESH GENERATION facility, the user may compare this with the geometry inputs for Example Prob. No. 10:

### Mesh generation used in Example Problem 10

```STAAD SPACE TANK STRUCTURE WITH
* MESH GENERATION
UNIT  . . .
DEFINE MESH
A 0 0 0 ; B 0 20 0 ; C 20 20 0
D 20 0 0 ; E 0 0 -20 ; F 0 20 -20
G 20 20 -20 ; H 20. 0. -20
GENERATE ELEMENT
MESH AEHD 16
MESH EABF 16