Reference
The authors acknowledge that naming conventions and input style formats for numgeo are based on those used by Abaqus1, a proprietary, general purpose finite element code.
The numgeo input file basically consists of two sections: a model definition Section describing the geometry and boundary conditions of the problem and one or more steps defining the loads:
** This has no effect on the output
** and only serves for identification
* End Input
All input is preceded by keywords, which all start with an asterisk (*), indicating the kind of data which follows. Detailed information on every keyword is given in the subsequent sections. In the following, a brief description of the structure model and step definition sections is given.
Upper vs lower case
The numgeo input file is case-insensitive - use upper and lower cases as you wish.
Blanks and tab stops
Blanks are ignored in the numgeo input file - use them to clarify your input file as you wish. Caution: tab stops are not automatically translated to blanks and should always be avoided.
Comments
Use comments and blank lines to clarify your input file - both will be ignored by numgeo. Comments start with ** and can be placed at the beginning of a line or somewhere within a line:
-
Example 1:
** This is a line comment. The entire line will be ignored.
-
Example 2:
*Amplitude, name=name1, type=tabular ** This is an inline comment after a valid keyword
Model definition
The model definition Section starts at the beginning of the file and ends at the occurrence of the first *step statement.
The first statement of the model definition is the *node statement (see Node), followed by the node definitions.
Next, the elements are defined using the element keyword (see input_element) and listing for each element its type, which nodes belong to the element and in what order. Multiple node and *element statements are possible.
Nodes and elements can be grouped into sets using the keywords nset (see input_nset) and elset (see input_elset) respectively.
Next, a material and other properties are assigned to an element set by means of the keyword card solid section (input_solid_section). Subsequent, the assigned properties have to be defined, in this example, a material is defined using the material keyword. Other properties such as soil-water-retention curves etc. may follow. See the "Property:" sections (input_material ff) for more details.
The Amplitude and Initial conditions keywords are not mandatory. More details are given in input_amplitude and input_initial.
The definition of boundary conditions (*Boundary, see input_boundary) in the model definition Section may be skipped, but has then to be given during the first step definition.
n1, x1, y1, z1
n2, x2, y2, z2
…
*Element, type = ...
e1, n1, n2, n3, ...
…
*Nset, name = ...
…
*Elset, name = ...
…
*Solid Section, ...
…
*Material, name = ...
…
[Other property definitions]
…
*Amplitude, name = ...
…
*Initial conditions, ...
…
*Boundary
Model definitions using parts and instances
*Node
n1, x1, y1, z1
n2, x2, y2, z2
⋮
*Element, type = ...
e1, n1, n2, n3, ...
⋮
*Nset, name = ...
⋮
*Elset, name = ...
⋮
*Solid section, ...
⋮
*End part
**
** - - - - Add a second part - - - -
**
*Assembly, name = ...
*Instance, name = ..., part = ...
x1, y1, z1
x1, y1, z1, x2, y2, z2, θ
⋮
*End Instance
**
** - - - - Add a second instance - - - -
**
*End Assembly
For models with different geometrical instances, a subdivision into parts is often beneficial.
A part definition is started using the *Part statement. Each part is assigned a name. Within the part definition section, nodes, elements, sets and solid sections can be defined. The part definition is closed using the *End part statement. The number of defined parts is not restricted.
Once parts have been defined, an assembly is defined using *Assembly. Again, the assembly is given a name. Within the assembly, instances are defined. Instances refer to the previously defined parts Part = .... The nodes of an instance can be moved by definition of a vector x1, y1, z1 in the line following the instance definition. They can also be rotated around the vector which is formed by the line connecting x1, y1, z1 and x2, y2, z2 by the angle θ. Each defined part has to be defined as an instance in the assembly.
The assembly is finished using the *End assembly statement.
Sets that have been defined in the part section can be used in the step definition if the name of the instance is added with a point before the set name, e.g. instance-1.set-1.
Note that no 'internal' set definition exists. Thus, every set defined in the assembly can be used in the step environment. Note in addition that it is prohibited to have the same set name twice even if they are defined in different parts.
-
For more information visit: https://www.3ds.com/de/produkte-und-services/simulia/produkte/abaqus/ ↩