Nodal thicknesses | ||
| ||
ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE
Defining nodal thicknesses
You can specify the thickness of a shell, membrane, or rigid element at a particular node or node set.
Input File Usage
NODAL THICKNESS node_number or node_set_name, thickness
Abaqus/CAE Usage
Use the following option for a conventional shell composite layup:
Property module: composite layup editor: Shell Parameters: Nodal distribution: select an analytical field or a node-based discrete field
Use the following option for a homogeneous shell section:
Property module: shell section editor: Basic: Nodal distribution: select an analytical field or a node-based discrete field
Use the following option for a composite shell section:
Property module: shell section editor: Advanced: Nodal distribution: select an analytical field or a node-based discrete field
Reading nodal thicknesses from an alternate file
The nodal thickness data can be stored in a separate file and read from there at the start of the analysis. For details on the syntax of such file names, see Input Syntax Rules.
Input File Usage
NODAL THICKNESS, INPUT=file_name
Abaqus/CAE Usage
Reading nodal thicknesses from an alternate file is not supported in Abaqus/CAE.
Generating continuously varying thicknesses between two nodes or node sets
Abaqus can linearly interpolate the thickness between two bounding nodes or node sets. The thicknesses at the bounding nodes must first be defined.
Input File Usage
Use the following options:
NODAL THICKNESS first bounding node or node set, thickness second bounding node or node set, thickness NODAL THICKNESS, GENERATE first bounding node or node set, second bounding node or node set, number of intervals, increment in node numbers
Abaqus/CAE Usage
Generating thicknesses between bounding nodes or node sets is not supported in Abaqus/CAE.
Specifying a continuously varying thickness for shell, membrane, and rigid elements
You must specify that a shell or membrane element is going to have a continuously varying thickness rather than a homogeneous thickness when you define the element section. See Membrane elements, Using a shell section integrated during the analysis to define the section behavior, and Using a general shell section to define the section behavior for details.
In Abaqus/Explicit you must specify that a rigid element is going to have a continuously varying thickness when you define the rigid body to which the element belongs; see Rigid elements. In Abaqus/Standard rigid elements cannot have a continuously varying thickness.
Every node that is part of a shell, membrane, or rigid element using a continuously varying thickness must have a nodal thickness defined. Abaqus will issue an error message if there is a node with no nodal thickness in an element that is using a continuously varying thickness.
Specifying a continuously varying thickness for a composite shell
When a composite shell structure has a continuously varying thickness, the total thickness of the shell at any node is defined by the nodal thickness value. The total thickness at an integration point is interpolated from the nodal thicknesses. The layer thicknesses given in the shell section definition are used as relative thicknesses and are scaled proportionally such that the sum of the layer thicknesses equals the total thickness at the integration point.
Example
For example, if a composite shell section were defined with the following input:
SHELL SECTION, COMPOSITE, NODAL THICKNESS, ELSET=name 1.5, 3, STEEL 2.5, 3, FOAM 1.0, 3, STEEL
and the total thickness at a point was only 1.0, the thicknesses of the individual layers at the point would be 0.3 for the first steel layer, 0.5 for the foam layer, and 0.2 for the second steel layer.
Creating a discontinuity in the shell, membrane, or rigid element thicknesses
You can specify only a single thickness at each node. Therefore, use separate nodes along the interface on shell, membrane, or rigid elements where there is a discontinuity in the thickness and assign the appropriate thickness to each group of nodes. For elements that are not part of a rigid body, multi-point constraints must be used to make the displacements (and rotations, for shells) the same at corresponding nodes.