Import ANSYS File: Elements

Description

ANSYS uses E or EN to define elements by element numbering and node connectivity. E is a Batch format specific command.

ANSYS uses EMORE to define additional nodes for node connectivity of the last defined element using the E or EN commands. EMORE is a Batch format specific command.

ANSYS uses ERRANG to specify the range of elements to be read from the node file defined by EREAD. ERRANG is a Batch format specific command.

ANSYS uses EREAD to read elements defined by element numbering and connectivity from a text file. EREAD is a Batch format specific command.

ANSYS uses EBLOCK to define elements by element numbering and node connectivity. EBLOCK is a CDB format specific command.

Creating Elements and Element Properties

Straus7 creates new elements and associated element properties according to the material reference number, active element type, real set and section ID.

Element Numbering

New Straus7elements are numbered sequentially (starting at 1), whereas elements in the ANSYS file can be arbitrarily numbered (as long as all element numbers are unique). In general, new Straus7 element numbers won't be the same as their corresponding ANSYS element numbers. The ANSYS element numbers are assigned to the Straus7 elements as ID attributes.

Element Properties

Straus7 creates new element properties according to the unique combination of material reference number, element type, real set and section ID. Element property names are specified according to the material reference number (MAT), element type (TYPE), real set (REAL) and section ID (SECNUM), and adopt the following convention:

"MAT N_MAT/ TYPE N_TYPE/ REAL N_REAL/ SECNUM N_SECNUM"

Material reference numbers, real sets and section IDs are only specified if required by the element type. For example, if a new element property is a combination of material reference number 7, element type 5 and section ID 8, the property name will be:

"MAT 7/ TYPE 5/SECNUM 8"

If a material reference number is specified, the material name is defined according to the material reference number as follows:

"MAT N_MAT"

Element material properties and attributes specified by the material reference number, active element type, real set, section ID and active element coordinate system are assigned according to the specified element type:

ANSYS Element Type	Straus7 Element Type	Description
MASS21, MASS166	Translational Mass, Rotational Mass	The translational and rotational mass components of MASS21 are interpreted according to the nodal coordinate system. Straus7 accumulates the translational and rotational mass components from MASS21 and MASS166 at each node and assigns node translational mass and node rotational mass attributes.
MPC184	Pinned Link, Rigid Link	Straus7 creates a pinned link or rigid link in accordance with the element option keys.
COMBIN14, COMBIN40	Spring-Damper	Straus7 creates a linear spring-damper element. If specified at the nodes, the mass of COMBIN40 is assigned as a node non-structural mass attribute.
COMBIN39	Spring-Damper	Straus7 creates a nonlinear elastic or elastic-plastic spring damper element and assigns the nonlinear table as an Axial Force vs Displacement (Force vs Displacement) table or Torque vs Twist (Moment vs Rotation) table in accordance with the element option keys.
LINK10	Cable, Cutoff Bar	Straus7 creates a cable element (tension only) or cutoff bar element (compression only) in accordance with the selected element option keys. The initial strain value for the cable element is assigned as a cable free length attribute.
LINK1, LINK8	Truss	Straus7 creates a truss element and assigns the initial strain value as a beam pre strain attribute.
LINK180	Truss	Straus7 creates a truss element and assigns the mass value as a uniformly distributed beam non-structural mass. An initial stress value applied using ISTRESS is assigned as a beam pre-tension attribute.
CONTAC12, CONTAC52, CONTA178	Normal Point Contact, Zero Gap Point Contact	Straus7 creates a normal or zero gap point contact element in accordance with the selected element option keys. The stiffness and friction values are assigned as initial stiffness and friction values C1 and C2.
BEAM3, BEAM4, BEAM54	Beam	Straus7 creates a beam element and assigns the initial strain value as a beam pre-strain attribute. For BEAM3 and BEAM54 the mass value is assigned as a uniformly distributed beam non-structural mass.
BEAM24	Beam	Straus7 creates a beam element. The thin walled beam section geometry is not supported.
BEAM44	Beam	Straus7 creates a beam element and assigns the translational and rotational end releases as beam translational end release and beam rotational end release attributes.
BEAM188, BEAM189	Beam	Straus7 creates a beam element. The third node of BEAM189 is omitted. An initial stress value applied using ISTRESS is assigned as a beam pre tension attribute.
MATRIX27	User-defined Beam	Straus7 creates a user-defined beam element. The global Cartesian coordinate system is assumed for the stiffness matrix.
PIPE16, PIPE18, PIPE20, PIPE60	Pipe	Straus7 creates a pipe element. For PIPE18 and PIPE60 the pipe radius is assigned as a pipe radius attribute.
PLANE2	2D Plane Stress, 2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane stress, 2D plane strain or axisymmetric element according to the selected option keys. An isotropic or orthotropic material is specified.
PLANE13	2D Plane Stress, 2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane stress, 2D plane strain or axisymmetric element according to the selected option keys. An isotropic, orthotropic or anisotropic material is specified. The anisotropic material is defined using the TB data table type ANEL.
PLANE42, PLANE82	2D Plane Stress, 2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane stress, 2D plane strain or axisymmetric element according to the selected option keys. An isotropic or orthotropic material is specified. A Drucker-Prager yield criterion is defined using the TB data table type DP.
PLANE182, PLANE183	2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane strain or axisymmetric element according to the selected option keys. An isotropic, orthotropic, anisotropic or rubber material may be defined. The anisotropic material is defined using the TB data table type ANEL. The rubber material is defined using the TB data table type HYPER.
PLANE35, PLANE55, PLANE77	2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane strain or axisymmetric element according to the selected option keys. An isotropic or orthotropic material may be defined.
HYPER56, HYPER74, HYPER84	2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane strain or axisymmetric element according to the selected option keys. A rubber material is specified using the TB data table type MOONEY.
FLUID79	2D Plane Strain, Axisymmetric	Straus7 creates a 2D plane strain or axisymmetric element according to the selected option keys. A fluid material is defined.
FLUID81	Axisymmetric	Straus7 creates an axisymmetric element of fluid material.
SHELL57	Plate/Shell	Straus7 creates a plate/shell element of isotropic or orthotropic material. A Drucker-Prager yield criterion is defined using the TB data table type DP. An element coordinate system may be defined using ESYS.
SHELL91, SHELL99	Plate/Shell	Straus7 creates a plate/shell element of isotropic, orthotropic, laminate or user-defined material. A Drucker-Prager yield criterion is defined using the TB data table type DP. Laminate failure criteria is defined using the TB data table type FAIL. The mass per unit area value is assigned as a plate face non-structural mass. An element coordinate system may be defined using ESYS.
SHELL131, SHELL132	Plate/Shell	Straus7 creates a plate/shell element of isotropic, orthotropic or laminate material. A laminate material is defined and referenced according to the specified section ID (SECNUM).
SHELL181, SHELL281	Plate/Shell	Straus7 creates a plate/shell element of isotropic, orthotropic, laminate, user-defined or rubber material. A laminate material is defined and referenced according to the specified section ID (SECNUM). A user-defined material is defined using the TB data table ANEL. A rubber material is specified using the TB data table type HYPER. The mass per unit area value is assigned as a plate face non-structural mass. Reduced integration may be specified. An element coordinate system may be defined using ESYS.
SHELL28	Shear Panel	Straus7 creates a shear panel element of isotropic material. The mass per unit area value is assigned as a plate face non-structural mass.
SHELL41, SHELL63	Plate/Shell, 3D Membrane	Straus7 creates a plate/shell or 3D membrane element in accordance with the selected option keys. An isotropic or orthotropic material is specified. The mass per unit area value is assigned as a plate face non-structural mass.
SOLID45, SOLID62, SOLID92, SOLID95	Brick	Straus7 creates a brick element of isotropic or orthotropic material. A Drucker-Prager yield criterion is defined using the TB data table type DP. The 2×2×2 order reduced integration option for SOLID95 is applied to the Gauss points.
SOLID5, SOLID64, SOLID98	Brick	Straus7 creates a brick element of isotropic, orthotropic or anisotropic material. The anisotropic material is defined using the TB data table ANEL.
SOLID185, SOLID186, SOLID187	Brick	Straus7 creates a brick element of isotropic, orthotropic, anisotropic or rubber material. The anisotropic material is defined using the TB data table ANEL. A rubber material is specified using the TB data table type HYPER. An element coordinate system may be defined using ESYS.
SOLID164	Brick	Straus7 creates a brick element of isotropic, orthotropic, anisotropic or rubber material. The anisotropic material is defined using the TB data table ANEL. A rubber material is specified using the TB data table type MOONEY.
SOLID70, SOLID87, SOLID90	Brick	Straus7 creates a brick element of isotropic or anisotropic material.
HYPER58, HYPER86, HYPER158	Brick	Straus7 creates a brick element of rubber material. The rubber material is specified using the TB data table type MOONEY.
VISCO107	Brick	Straus7 creates a brick element of isotropic material.
FLUID80	Brick	Straus7 creates a brick element of fluid material.

Translational and Rotational Mass Attributes

Straus7 assigns the translational mass attributes in the global Cartesian coordinate system. For rotational mass attributes, Straus7 creates user-defined coordinate systems aligned with the principal axes and posts these coordinate systems with the default title "ANSYS Rotational Mass UCS: Node N".

Non-Structural Mass Attributes

Distributed masses specified for elements are not load case dependent in ANSYS. Straus7 assigns the node non-structural mass, beam non-structural mass and plate face non-structural mass attributes to all imported load cases.

Beam Principal Axis Angles

Straus7 applies the beam principal axis angle attribute to beam elements when a local axis angle is specified, or when a beam without a reference node is defined. The default ANSYS beam local axis system differs from the Straus7 convention for a beam without a reference node and requires a principal axis rotation of 90 degrees for consistency. Beam principal axis angles specified by a local axis angle are defined such that the principal 1 axis is rotated relative to the default ANSYS local axis system.

Plate Local Axis Angles

Straus7 applies the plate local axis angle attribute to plate elements when a local axis angle or element coordinate system is specified, or when the default ANSYS local axis system differs from the Straus7 convention. Plate local axis angles specified by a local axis angle are defined such that the local x-axis is rotated relative to the default ANSYS local axis system.