Normal Definitions at Nodes

Normals can be defined at nodes:

  • with a user-specified normal definition;

  • following the nodal coordinates as part of the node definition for beam and shell elements;

  • on rigid main surfaces used in contact pairs in Abaqus/Standard;

  • in beam and shell elements;

  • for line spring elements to give the direction normal to the flaw in the structure;

  • for gasket elements to give the thickness direction of the elements; and

  • for contour integral evaluation.

The normals defined at nodes do not affect the element face normals, which are defined by the element connectivity. They need not be of unit length.

This page discusses:

See Also
In Other Guides
*NORMAL
*NODE

ProductsAbaqus/StandardAbaqus/Explicit

Contact Surfaces in Abaqus/Standard

User-specified surface normals for contact surfaces in Abaqus/Standard are relevant only when the small-sliding contact approach is used or when the finite-sliding contact approach is used with rigid elements that make up the main surface. User-specified surface normals defined on deformable main surfaces in contact pairs are ignored when finite sliding is used.

The small-sliding contact formulation uses the surface normals at each node along the main surface to define a normal vector that varies smoothly from point to point on the surface. For a detailed discussion on how the “main plane” is constructed for each secondary node using the surface normals, see Contact Formulations in Abaqus/Standard.

For main surfaces composed of rigid elements Abaqus/Standard smooths any discontinuous surface normal transitions between the rigid elements. The surface normals at the nodes are used to control the surface normal interpolation. For a detailed discussion on the smoothing of such main surfaces, see Analytical Rigid Surface Definition.

To define the normal, specify the components of the normal in the global coordinate system.

Input File Usage

NORMAL, TYPE=CONTACT SURFACE

Elements

User-specified normals might be necessary for beam and shell elements, line spring elements, gasket elements, or elements involved in contour integral evaluations. In such cases specify the components of the normal in the global coordinate system.

Input File Usage

NORMAL, TYPE=ELEMENT

Beam and Shell Elements

User-specified normals might be needed to define the desired normal directions at shell surface intersections or at beam intersections where the automatically determined normals might be inappropriate for the model (see Beam Element Cross-Section Orientation or Defining the Initial Geometry of Conventional Shell Elements).

The nodal normals can also be defined as part of the node definition. While you can define a single normal for all elements connected to a node as part of the node definition, a user-specified normal definition defines a normal for a particular element at a node, thus allowing you to define separate normals for each element connected to a node. User-specified normal definitions supersede normals defined as part of a node definition.

Input File Usage

NODE
Specify the normals in the fifth, sixth, and seventh positions on the data line.

For example, the following lines define some normals as part of node definitions; the normal to be used at node 7 in element 2 is then redefined using a user-specified normal definition:

NODE
6, 5., 5., , -0.5, .8
7, 10., 8., , -0.5, .8
9, 14., 4., , .6, .6
NORMAL
2, 7, .6, .6

Gasket Elements

For gasket elements user-specified normals can be used to specify the thickness direction of the elements. The nodal thickness directions can also be defined as part of the gasket section definition. Thickness directions defined by user-specified normals supersede thickness directions defined as part of the gasket section definition. See Defining the Gasket Element's Initial Geometry for a description of the definition of the thickness direction for these elements.

Contour Integral Evaluation

For contour integral evaluations (Contour Integral Evaluation) surface normals should be specified at all surface nodes lying within the bounds of the requested contours. These nodes are printed out under the “Contour Integral” information in the data (.dat) file. For accurate contour integral evaluation, it is important that the virtual crack extension direction is in the plane of the surface for the following cases: when a crack front intersects the external surface of a three-dimensional solid, when the crack front intersects a surface of material discontinuity, or when the crack is in a curved shell. If no normals are specified, Abaqus calculates the normals automatically, except for a model with tetrahedral elements. In the latter case, you must always specify the normals to improve the accuracy of contour integral evaluation at the free surface.

The nodal normal data specified as part of a node definition is not activated for solid elements unless a user-specified normal definition is used in the model; it suffices to include a user-specified normal definition for only one node to activate the utilization of the nodal normal data specified as part of a node definition.

The Coordinate System in Which Normals Are Defined

Abaqus models can be defined in terms of an assembly of part instances (see Assembly Definition). Normals at nodes defined within a part (or part instance) are defined relative to the part coordinate system. These normals are rotated according to the positioning data given for each instance of the part. Normals can be defined at reference nodes at the assembly level if necessary. Normals defined at the assembly level are defined in the global coordinate system.

For models that are not defined in terms of an assembly of part instances, normals are defined in the global coordinate system.