<!-- source-page: 141 -->

the results in the Visualization module of Abaqus/CAE to view the vector components in the transformed systems.

Output database output of history vector-valued quantities at transformed nodes can be in the local or global system (see “Output to the output database,” Section 4.1.3). By default, the values are written in the global system (since this is more convenient for postprocessing).

<!-- source-page: 142 -->

<!-- source-page: 143 -->

# 2.1.6 ADJUSTING NODAL COORDINATES

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• \*ADJUST   
• “Defining adjust points constraints,” Section 15.15.5 of the Abaqus/CAE User’s Guide

# Overview

Nodal adjustment is used for:

• adjusting user-specified nodal coordinates so that the nodes lie on a given surface; and   
• specifying the direction along which the nodes are moved.

# Adjusting nodal coordinates

In general, user-specified nodal coordinates are not modified during input file processing. However, there are some situations where mesh coordinates are known only in a generic way and it is inconvenient to determine their coordinates for their actual usage. For example, when using fasteners the specified reference node should be positioned at its projection point on the associated surface. Since that location may be known only approximately, you can use nodal adjustment to move the reference node to that location automatically. For typical usage of the nodal adjustment feature, refer to “About assembled fasteners,” Section 29.1.3 of the Abaqus/CAE User’s Guide.

When using this feature, the nodes are adjusted to lie on the specified surface without regard for shell thickness or shell offsets. Therefore, it is not advisable to use this feature as a way of correcting initial overclosures for contact or for tie constraints. In addition, care should be taken when choosing the nodes to be adjusted because the feature does not respect any constraints relating the relative position of the adjusted node with other nodes (e.g., rigid body definitions).

Input File Usage: Use the following option to identify the nodes to be moved and the surface onto which the nodes are to be moved:

\*ADJUST, NODE SET=name, SURFACE=name

Abaqus/CAE Usage: Use the following option to move the control point of a coupling constraint onto the coupling surface:

Interaction module: Constraint→Create: Coupling; Adjust control point to lie on surface

Use the following option to move any point or points onto any surface:

Interaction module: Constraint→Create: Adjust points

<!-- source-page: 144 -->

# Specifying the nodal adjustment direction

A node can be moved to the surface using a normal adjustment or a directed adjustment. By default, the node is adjusted to the closest point on the specified surface along the normal to the surface. You can specify an orientation to move the node to the surface along a given direction rather than along the normal to the surface. The vector along the local Z-direction from the orientation definition is used to move the node to the surface (see “Orientations,” Section 2.2.5). If no projection can be found, the nodal coordinates are left unmodified.

Input File Usage: \*ADJUST, ORIENTATION=name

Abaqus/CAE Usage: The orientation projection option is not supported in Abaqus/CAE.

<!-- source-page: 145 -->

# 2.2 Element definition

• “Element definition,” Section 2.2.1   
• “Element foundations,” Section 2.2.2   
• “Defining reinforcement,” Section 2.2.3   
• “Defining rebar as an element property,” Section 2.2.4   
• “Orientations,” Section 2.2.5

<!-- source-page: 146 -->

<!-- source-page: 147 -->

# 2.2.1 ELEMENT DEFINITION

Products: Abaqus/Standard Abaqus/Explicit

# References

• \*ELCOPY   
• \*ELEMENT   
• \*ELGEN   
• \*ELSET

# Overview

This section describes the methods for defining elements in an Abaqus input file. In a preprocessor such as Abaqus/CAE, you define the model geometry rather than the nodes and elements; when you mesh the geometry, the preprocessor automatically creates the nodes and elements needed for analysis. Although the concepts discussed in this section apply in general to the element definitions in the input file that is created by Abaqus/CAE, the methods and techniques described here apply only if you are creating the input file manually.

Element definition consists of:

• assigning an element number to the element;   
• defining individual elements by specifying their nodes;   
• grouping elements into element sets; and   
• creating elements from existing elements by generating them incrementally or by copying existing elements.

If any element is specified more than once, the last specification given is used.

# Assigning an element number to the element

Each individual element must have a numeric label called the element number, which is assigned when the element is defined. The element number must be a positive integer, and the maximum element number allowed is 999999999 (for information on integer input, see “Input syntax rules,” Section 1.2.1). The elements do not need to be numbered continuously.

An Abaqus model can be defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1). In such a model almost all elements must belong to a part or part instance. The only exceptions are mass, rotary inertia, capacitance, connector, spring, and dashpot elements, which can belong to a part or to the assembly. Element numbers must be unique within a part, part instance, or the assembly; but they can be repeated in different parts or part instances.

<!-- source-page: 148 -->

You can define individual elements by specifying the element number and the nodes that define the element. In addition, you must specify the element type. The element must be chosen from one of the element types specified in Part VI, “Elements”; or, in Abaqus/Standard, it can be a user-defined element (“User-defined elements,” Section 32.17.1) or a substructure (“Using substructures,” Section 10.1.1).

Input File Usage: \*ELEMENT, TYPE=name

For example, the following lines create element number 11, which is of type C3D8R, by defining its nodes (2, 3, 9, 7, 5, 8, 12, 16):

\*ELEMENT, TYPE=C3D8R

11, 2, 3, 9, 7, 5, 8, 12, 16

# Using large node numbers with elements that use many nodes

The following rules apply when defining elements:

• The connectivity for each element is considered a logical record, and any number of input lines can be used to specify it. Abaqus will read the first line for an element and consider the next line a continuation line if a comma ends the line and the element definition is not complete.   
• Any number of continuation lines can be used.   
• For elements such as C3D27 with a variable number of nodes (see “Solid (continuum) elements,” Section 28.1.1), the last line should not end with a comma or Abaqus will interpret the next element definition as a continuation of the current element.

For example,

```txt
* ELEMENT, TYPE=C3D20
100001, 100001, 100002, 100003, 100004, 100005, 100006, 100007, 100008, 100009, 100010, 100011, 100012, 100013, 100014, 100015, 100016, 100017, 100018, 100019, 100020 
```

# Reading element definitions from a file

Element definitions can be read into Abaqus from an alternate file. The syntax of such file names is described in “Input syntax rules,” Section 1.2.1.

Input File Usage: \*ELEMENT, INPUT=file\_name

# Reading substructure definitions from a substructure library

Substructure definitions can be read from the substructure library in which the substructure resides (“Using substructures,” Section 10.1.1).

Input File Usage: \*ELEMENT, FILE=substructure\_library\_name

If the FILE parameter is used without a value, the default substructure library name is used.

<!-- source-page: 149 -->

# Defining axisymmetric elements with asymmetric deformation

You can define a positive offset number that will be used to specify nodes for axisymmetric elements with asymmetric deformation (see “Choosing the element’s dimensionality,” Section 27.1.2; “Axisymmetric solid elements with nonlinear, asymmetric deformation,” Section 28.1.7; and “Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10, for more information on axisymmetric elements with asymmetric deformation; they are available only in Abaqus/Standard). The default offset is 100000.

Input File Usage: \*ELEMENT, OFFSET=number

# Defining gasket elements

There are several methods for defining gasket elements. (See “Gasket elements: overview,” Section 32.6.1; “Including gasket elements in a model,” Section 32.6.3; and “Defining the gasket element’s initial geometry,” Section 32.6.4, for more information on gasket elements; they are available only in Abaqus/Standard.)

In the first method you define individual elements by specifying the element number and the nodes that define the element.

In the second method you specify only the nodes on the bottom surface of the gasket element and a positive offset number that will be used to define the corresponding nodes for the top surface. For the 18-node gasket element you give the first eight nodes followed by the midsurface node; i.e., node 17 in the full element nodal connectivity.

Abaqus/Standard can generate the midface nodes of the 18-node gasket elements automatically if both element faces are part of contact surfaces. To invoke this feature, you enter a blank instead of the actual node numbers in either of the above input methods. Abaqus/Standard will then generate the node numbers and coordinates of the midface nodes automatically.

Input File Usage: Use the following option to specify the element number and the nodes that define the element:

\*ELEMENT, TYPE=name

Use the following option to specify the nodes on the bottom surface of the element and a positive offset number for the top surface:

\*ELEMENT, TYPE=name, OFFSET=offset number

Using solid element connectivity to define gasket elements

The node numbering scheme for gasket elements does not correspond to the node numbering scheme for continuum elements, which can be inconvenient if the mesh generator used does not support gasket elements directly or in thermal-stress analysis where continuum elements are used to model the heat conduction in the gasket. For such cases you can specify that solid element connectivity is used to define the gasket element. By default, it is assumed that the first (S1) face of the solid element coincides with the first (SNEG) face of the gasket element. If the equivalent solid element is oriented differently, specify the face number on the solid element that corresponds to the first face of the gasket element. The

<!-- source-page: 150 -->

solid element must have the same number of nodes on each face as the corresponding gasket element; any nodes between the faces will be ignored. The 18-node gasket element is an exception. If both element faces are part of contact surfaces, the connectivity of a 20-node brick element can be used, and Abaqus/Standard will generate the node numbers and coordinates of the midface nodes automatically.

Abaqus/Standard will transform the solid element connectivity to the normal gasket element connectivity immediately upon reading the data. Hence, all output to the data (.dat), results (.fil), and output database (.odb) files will use the normal gasket element connectivity.

# Input File Usage:

Use the following option to specify solid element connectivity for a gasket element in which the first face of the solid element corresponds to the first face of the gasket element:

\*ELEMENT, TYPE=name, SOLID ELEMENT NUMBERING

Use the following option to specify solid element connectivity for a gasket element and the face of the solid element that corresponds to the first face of the gasket element:

\*ELEMENT, TYPE=name, SOLID ELEMENT NUMBERING=face number

# Examples

The following lines create GK3D12M element number 11 that has node numbers 1, 2, 3, 4, 5, 6, 1001, 1002, 1003, 1004, 1005, and 1006:

```txt
* ELEMENT, TYPE=GK3D12M
11, 1, 2, 3, 4, 5, 6, 1001, 1002, 1003, 1004, 1005, 1006 
```

The same element connectivity is also created by the following lines:

```txt
* ELEMENT, TYPE=GK3D12M, OFFSET=1000
11, 1, 2, 3, 4, 5, 6 
```

The equivalent solid element would be C3D15, with the following input:

```txt
* ELEMENT, TYPE=GK3D12M, SOLID ELEMENT NUMBERING
11, 1, 2, 3, 1001, 1002, 1003, 4, 5, 6, 1004, 1005, 1006, 501, 502, 503 
```

where nodes 501, 502, and 503 would not be used.

# Defining cohesive elements

There are three methods for defining cohesive elements. (See “Cohesive elements: overview,” Section 32.5.1; “Modeling with cohesive elements,” Section 32.5.3; and “Defining the cohesive element’s initial geometry,” Section 32.5.4, for more information on cohesive elements.)

• In the first method you specify the element number and all of the nodes that define the element.
