Features Supported for Import from Abaqus

When you import a finite element model representation from an Abaqus input file (.inp), the import process replicates the nodes and elements from the Abaqus data in the 3DEXPERIENCE platform, along with a subset of the other features present in the data, such as couplings and connectors. Some Abaqus components are supported by the import process but do not appear in the user interface. The contributions of these components are included when you perform your analysis, but you cannot change them directly in the app.

This page discusses:

Sections

Beam Sections

Abaqus Usage 3DEXPERIENCE Usage
*BEAM SECTION Beam Section
ELSET Element nodes created as node groups under the imported mesh part. Node groups are used as supports.
MATERIAL Material
POISSON Poisson's ratio
LUMPED=YES or NO Use consistent mass matrix formulation clear or selected
SECTION=(TYPE) Shape
Data lines:
  1. Beam profile attributes
  2. Orientation
  1. Parameter values defining the measurements of the beam cross-section
  2. Orientation set to Rotate about beam axis
Note: If the orientation is set to the default (0, 0, -1) or not set and constant orientation is specified in *NORMAL, this constant orientation is set to Rotate about beam axis and Define cross section axis is set to 2-axis.
*TRANSVERSE SHEAR STIFFNESS Transverse shear stiffness: K13 and K23 values

Beam General Sections

Abaqus Usage 3DEXPERIENCE Usage
*BEAM GENERAL SECTION Beam Section with the Integrate section before analysis option selected
ELSET Element nodes created as node groups under the imported mesh part. Node groups are used as supports.
POISSON Poisson's ratio
LUMPED=YES or NO Use consistent mass matrix formulation clear or selected
SECTION=(TYPE) Shape
Data lines:
  1. Beam profile attributes
  2. Orientation
  3. Material
  1. Parameter values defining the measurements of the beam cross-section
  2. Orientation set to Rotate about beam axis
  3. Material
Note: If the orientation is set to the default (0, 0, -1) or not set and constant orientation is specified in *NORMAL, this constant orientation is set to Rotate about beam axis and Define cross section axis is set to 2-axis.
*TRANSVERSE SHEAR STIFFNESS Transverse shear stiffness: K13 and K23 values

Fluid Sections

Abaqus Usage 3DEXPERIENCE Usage
*FLUID SECTION Fluid Section
ELSET Group under imported mesh part
MATERIAL Material

Membrane Sections

Abaqus Usage 3DEXPERIENCE Usage
*MEMBRANE SECTION Membrane Section
ELSET Group under imported mesh part
MATERIAL Material
ORIENTATION Specify orientation
POISSON Poisson's ratio
First parameter at the first data line Thickness

Distributed thickness (nodal or element) import is not supported.

Shell Sections

Abaqus Usage 3DEXPERIENCE Usage
*SHELL SECTION Shell Section
ELSET Group under imported mesh part
MATERIAL Material
OFFSET (SNEG/SPOS) Offset definition
ORIENTATION Specify orientation
POISSON Poisson definition
SECTION INTEGRATION=SIMPSON or GAUSS Integration scheme: Simpson's rule or Gauss quadrature
Number of integration points specified on the second data line. Integration points
*TRANSVERSE SHEAR STIFFNESS Transverse shear stiffness: K11, K12, K22 values
First parameter at the first data line Thickness

Distributed thickness (nodal or element) import is not supported.

Shell General Sections

Abaqus Usage 3DEXPERIENCE Usage
*SHELL GENERAL SECTION Shell Section with the Integrate section before analysis option selected
ELSET Group under imported mesh part
MATERIAL Material
OFFSET (SNEG/SPOS) Offset definition
ORIENTATION Specify orientation
POISSON Poisson definition
*TRANSVERSE SHEAR STIFFNESS Transverse shear stiffness: K11, K12, K22 values
First parameter at the first data line Thickness

Distributed thickness (nodal or element) import is not supported.

Continuum Shell Sections

Abaqus Usage 3DEXPERIENCE Usage
*SHELL SECTION Continuum Shell Section, if the element type is SC6R or SC8R
ELSET Group under imported mesh part
MATERIAL Material
ORIENTATION Specify orientation
POISSON Poisson definition
SECTION INTEGRATION=SIMPSON or GAUSS Integration scheme: Simpson's rule or Gauss quadrature
Number of integration points specified on the second data line. Integration points

Shear Panel Sections

Abaqus Usage 3DEXPERIENCE Usage
*SHELL GENERAL SECTION Shear Panel Section, if the element type is SHEAR4
ELSET Group under imported mesh part
MATERIAL Material
First parameter at the first data line Thickness

Distributed thickness (nodal or element) import is not supported.

1D Link Sections

Abaqus Usage 3DEXPERIENCE Usage
*SOLID SECTION 1D Link Section, if the element type is T3D2 or T3D3
ELSET Group under imported mesh part
MATERIAL Material
First parameter at the first data line Area

Solid Sections

Abaqus Usage 3DEXPERIENCE Usage
*SOLID SECTION Solid Section
ELSET Group under imported mesh part
MATERIAL Material
ORIENTATION Specify orientation

SPH Particles Sections

Abaqus Usage 3DEXPERIENCE Usage
*SOLID SECTION SPH Particles, if the ELEMENT CONVERSION (*SECTION CONTROLS) value is set to BACKGROUND GRID or YES
ELSET Group under imported mesh part
MATERIAL Material
CONTROLS (*SECTION CONTROLS)

  1. ELEMENT CONVERSION:

    BACKGROUND GRID or YES

  2. KERNAL:

    QUADRATIC, CUBIC, or QUINTIC

  3. PARTICLE THICKNESS=UNIFORM or VARIABLE
  4. Data lines (4th line) *SECTION CONTROLS:
    1. First parameter: Spacing of the background grid or number of particles to be generated per isoparametric direction
    2. Second parameter: Threshold value for the conversion criterion

 Density

  1. Particle Generation: On background grid or Per element
  2. Function order: Second, Third, or Fifth
  3. Particle thickness type: Uniform or Variable
    1. Grid spacing, if ELEMENT CONVERSION=BACKGROUND GRID; Particles per isoparametric direction, if ELEMENT CONVERSION=YES
    2. Criterion, if ELEMENT CONVERSION=YES and CONVERSION CRITERION=TIME
ORIENTATION Material orientation

Surface Sections

Abaqus Usage 3DEXPERIENCE Usage
*SURFACE SECTION Surface Section
ELSET Group under imported mesh part
DENSITY Density

Connections

Couplings

Abaqus Usage 3DEXPERIENCE Usage
*COUPLING Coupling
CONSTRAINT NAME Name
REF NODE and SURFACE A group named ELSET under the imported mesh part. This group is selected as the support for the corresponding coupling.
ORIENTATION Axis system specification: Specify.
INFLUENCE RADIUS Imported but not visible in the user interface.
*DISTRIBUTING/*KINEMATIC First support coupling type: Distributing or Kinematic.

Connectors

Abaqus Usage 3DEXPERIENCE Usage
*CONNECTOR SECTION Connector
ELSET Element nodes created as node groups under the imported mesh part, with the node groups as supports. For single node elements, the second support is specified as ground.
BEHAVIOR Name of the connector behavior
ELIMINATION=NO/YES Imported but not exposed in the user interface. (The ELIMINATION=YES setting is not supported.)
<Assembled Connection Type> Type: <Assembled Connection Type>

All types except SLIPRING are supported.
<Basic translational connection type>, <Basic rotational connection type> Type: Specify; Translation: <Basic translational connection type>; Rotation: <Basic rotational connection type>
<Orientation Name 1> Axis system definition for first node of connector element. Only rectangular axis systems are supported.
<Orientation Name 2> Axis system definition for second node of connector element. If only one orientation is specified, use Set Second Axis System As First.
*CONNECTOR BEHAVIOR Available components definition
NAME (The name referred to by *CONNECTOR SECTION)
EXTRAPOLATION, INTEGRATION, REGULARIZE, and RTOL Imported only when the default values are specified.
*CONNECTOR CONSTITUTIVE REFERENCE
First (and only) data line: Length-1, -2, -3; Angle-1, -2, -3 Length associated with Tx, Ty, Tz; Angle associated with Rx, Ry, Rz.

If blank, the default values are initialized from the geometry.
*CONNECTOR ELASTICITY Elasticity
NONLINEAR Translational/Rotational Stiffness Type: Nonlinear

If this value is not included, linear translational stiffness is used.
COMPONENT=1, 2, 3, 4, 5, 6 Fx, Fy, Fz, Mx, My, Mz
EXTRAPOLATION, FREQUENCY DEPENDENCE, INDEPENDENT COMPONENTS, REGULARIZE, and RTOL Imported only when the default values are specified.
<Value1>,<Value2> Stiffness Value: <Value1> (for Linear Translational/Rotational stiffness)

Force/Moment: <Value1> (for Nonlinear Translational/Rotational stiffness)

Displacement/Rotation: <Value2> (for Nonlinear Translational/Rotational stiffness)
*CONNECTOR DAMPING Damping
NONLINEAR Translation/Rotation Damping Type: Nonlinear

If this value is not included, linear translational/rotational damping is used.

TYPE=VISCOUS By default; other damping types not supported
COMPONENT=1, 2, 3, 4, 5, or 6 Fx, Fy, Fz, Mx, My, or Mz
EXTRAPOLATION, FREQUENCY DEPENDENCE, INDEPENDENT COMPONENTS, REGULARIZE, and RTOL Imported only when the default values are specified.
<Value1>,<Value2> Damping Value: <Value1> (for linear translational/rotational damping type)
Force/Moment=<Value1>; Velocity/Angular Velocity=<Value2> (for nonlinear translational/rotational damping type)

Springs

Abaqus Usage 3DEXPERIENCE Usage
*SPRING Spring
ELSET Element nodes created as node groups under imported mesh part, with the node groups as supports. For single node elements, the second support is specified as ground.
ELEMENT=SPRINGA Spring type: Linear Axial
ELEMENT=SPRING1 or SPRING2 Spring type: Linear General (For SPRING1 the second support is Ground.)
NONLINEAR Nonlinear elasticity (Axial or General)

Only force and relative displacement are supported.
ORIENTATION Axis system definition: Specify (only Cartesian systems supported)

Dashpots

Abaqus Usage 3DEXPERIENCE Usage
*DASHPOT Connector
ELSET Element nodes created as node groups under imported mesh part, with the node groups as supports. For single node elements, the second support is specified as ground.
ELEMENT=DASHPOTA Connector type: Axial
ELEMENT=DASHPOT1 or DASHPOT2 Connector type: General (For DASHPOT1 the second support is ground.)
NONLINEAR Nonlinear damping (only force and velocity supported)
ORIENTATION Axis system definition: Specify (only Cartesian systems supported)

Abstractions

Nonstructural Masses

Abaqus Usage 3DEXPERIENCE Usage
*NONSTRUCTURAL MASS Mass Per Unit Volume, Mass Per Unit Area, or Mass Per Unit Length
ELSET Group under imported mesh part
UNITS=MASS PER VOLUME, MASS PER AREA, MASS PER LENGTH, or TOTAL MASS Type of Mass: Mass Per Unit Volume/Area/Length or Total Mass
DISTRIBUTION=MASS PROPORTIONAL or VOLUME PROPORTIONAL Mass Distribution: Mass Proportional or Volume Proportional
Magnitude value on the data line Magnitude

Point Masses and Inertia

Abaqus Usage 3DEXPERIENCE Usage
*MASS, *ROTARY INERTIA Point Inertia
ELSET Group under imported mesh part
TYPE=ISOTROPIC Imported but not exposed in the user interface. Anisotropic point inertia are not supported.
Magnitude value on the data line Magnitude
ALPHA=0.0 Imported but not exposed in the user interface. Import of any values other than 0.0 is not supported.
ORIENTATION Axis system definition: Specify (only Cartesian systems supported)

Rigid Bodies

Abaqus Usage 3DEXPERIENCE Usage
*RIGID BODY Rigid Body
REF NODE Group under the mesh part containing a reference node
ELSET Group under imported mesh part
TIE NSET Group under the mesh part containing Tie nodes
PIN NSET Group under the mesh part containing Pin nodes
POSITION Reference point, if one is defined, or the CENTER OF MASS