Abaqus Interface

Overview of the Abaqus Interface.

Supported Abaqus Profiles

Standard.2d: Generates a deck for two-dimensional models containing planar or axisymmetric elements for use with Abaqus Standard.
Standard.3d: Generates a deck for three-dimensional models containing bar, shell, and solid elements for use with Abaqus Standard.
Explicit: Generates a deck for use with Abaqus Explicit.

Import and Export

HyperMesh places all elements into separate components, based on sectional property. Each component is written out from HyperMesh as an element set in the Abaqus input deck.
Although HyperMesh supports 160 characters in entity names, Abaqus output files are truncated at 80 characters to match the Abaqus name support level.
Loads and constraints are organized under load collectors in HyperMesh and added to a load step for the *STEP card in the Abaqus history definition. If loads are applied to node or element sets, you can resolve these sets to individual nodes or elements by enabling the Expand loads on sets option in the Import panel under Import options.
Output options are organized under output blocks in HyperMesh. These output blocks also need to be added to load steps.
Resolve sets into nodes or elements, which are defined using the GENERATE parameter, using the Solver options in the Import Browser. This is useful when nodes/elements are renumbered due to ID conflicts during import.

Syntax

HyperMesh supports some abbreviated key words and parameters.
All Abaqus keywords and parameters supported in HyperMesh are not case insensitive.
HyperMesh ignores spaces in keyword lines.
HyperMesh supports quotation marks around component (ELSET with sectional properties) names, which is especially useful for names that begin with a number.

HyperMesh Operations

Warnings and error messages are written to a file named abaqus.msg. Unrecognized lines are written to a *.hmx file. These files are created in the same directory from where HyperMesh is launched.
Step time calculations can differ between HyperMesh and Abaqus (Explicit analyses), therefore you may find differences between reported values in the Abaqus status (.sta) file and the Time subpanel of the Check Elems panel. The values reported by HyperMesh are close estimates of the step time; refer to the Abaqus documentation to learn about the factors that Abaqus/Explicit uses to reach the final result.

Degenerated Brick Element

Elements that are defined in one configuration can be degenerated or collapsed to create other configurations, while still preserving the number of nodes and element type in the original configuration.

For example, the HyperMesh Qaud4 element can degenerate into a Tria3 element, but when exported, the four nodes and quadrilateral element information is written in the solver deck.

Degenerated brick elements are either Hex8 or Hex20 elements, collapsed into a wedge element (Penta6 or Pet15). Penta6 (Element configuration 206) is a 3D, 1st order, triangular prism shape element with a 6 noded order as shown inFigure 1. Hex8 (Element configuration 208) is a 3D, 1st order, brick shape element with a 8 noded order as shown in Figure 2. The Degenerated Brick (Element configuration 206) option is a 3D, 1st order, triangular prism shape element with a 8 noded order as shown in Figure 3.

Standard node order for a 1st order, penta6 element will be 1, 2, 3, 4, 5, 6. In cases of degenerated brick elements, the node order will be 1, 2, 2, 4, 5, 6, 6, 8, with nodes 2 and 6 being repeated during export. The same node repetition method is used for a 2nd order, degenerated brick element, but nodes 2 and 6 will be repeated twice and node 18 will be repeated once (1, 2, 2, 4, 5, 6, 6, 8, 9, 10, 2, 12, 6, 14, 15, 16, 17, 18, 18, 20).

Since the 8-noded, hexa element is degenerated into a 8-noded penta element, the 1st order brick element option is added under the 6-noded penta (Element configuration 206) and the 2nd order brick element option is added under the 15-noded penta (Element configuration 215).