Translating RADIOSS Input Files to Partial Abaqus Input Files

Using the Translator

The translator requires an input file in block format created by RADIOSS Version 4.4 or 5.1. The input file can have any name and an optional extension.

The RADIOSS data entries that are translated are listed in the tables below. Other RADIOSS keywords and data are skipped over and noted in the log file.

The translator creates a partial Abaqus input file that contains only the model data and time history output data. You can provide additional output data to complete the input.

Element Numbering and Grouping

All elements in the generated Abaqus input file will have unique element numbers. New element numbers will be assigned automatically to elements with non-unique element numbers in the RADIOSS input. Elements that are assigned the same PART identification number are grouped together in an element set.

Elements that have different material or properties must be given different PART identification numbers; that is, the same material and properties must be applicable to all elements grouped in the same element set.

If elements that result from the translation of SPRING have different element properties (such as skew systems used to define local directions) and are assigned the same PART identification number, the translator automatically separates them into different element sets.

Material Models

The translator supports only the material models shown in Table 1. All unsupported material models are translated as linear elastic if a stress-strain law definition is required. In these cases the translator provides nominal values for the material properties.

Summary of RADIOSS Entities Translated

Table 1. Material data.
RADIOSS keyword	Abaqus equivalent
MAT / LAW01 (ELAST)	ELASTIC
MAT / LAW02 (PLAS_JOHN)	PLASTIC, HARDENING=JOHNSON COOK
MAT / LAW03 (HYDPLA)	EOS, TENSILE FAILURE, DAMAGE INITIATION, and DAMAGE EVOLUTION
MAT / LAW19 (FABRI)	USER MATERIAL
MAT / LAW22 (DAMA)	PLASTIC, HARDENING=JOHNSON COOK; RATE DEPENDENT, TYPE=JOHNSON COOK; DAMAGE INITIATION; and DAMAGE EVOLUTION
MAT / LAW35 (FOAM_VISC)	HYPERFOAM and VISCOELASTIC
MAT / LAW36 (PLAS_TAB)	PLASTIC, HARDENING=ISOTROPIC

Table 2. Property data.
RADIOSS keyword	Abaqus equivalent
PROP / TRUS	Truss element properties and grouping data
PROP / BEAM	Beam element properties and grouping data
PROP / SPRING	Connector behavior and grouping data
PROP / SPR_BEAM	Connector behavior and grouping data
PROP / SPR_GENE	Connector behavior and grouping data
PROP / SOLID	Solid element properties and grouping data
PROP / SOL_ORTH	Solid element properties and grouping data
PROP / SHELL	Shell element properties and grouping data
PROP / SH_ORTH	Shell element properties and grouping data

Table 3. Nodal data.
RADIOSS keyword	Abaqus equivalent
NODE	NODE
ADMAS	MASS and ROTARY INERTIA
BCS	BOUNDARY
IMPDISP	BOUNDARY and AMPLITUDE
IMPVEL	BOUNDARY and AMPLITUDE
INIVEL	INITIAL CONDITIONS, TYPE=VELOCITY or ROTATING VELOCITY
CLOAD	CLOAD and AMPLITUDE
GRAV	DLOAD and AMPLITUDE
SKEW	ORIENTATION and TRANSFORM
FRAME	ORIENTATION and TRANSFORM

Table 4. Element data.
RADIOSS keyword	Abaqus equivalent
BRICK	C3D4/C3D6/C3D8R and SOLID SECTION
SHELL¹	S3RS/S4RS and SHELL SECTION; or M3D3/M3D4/M3D4R and MEMBRANE SECTION
SH3N¹	S3RS and SHELL SECTION; or M3D3 and MEMBRANE SECTION
BEAM	B31 and BEAM SECTION, SECTION=CIRC
TRUSS	T3D2 and SOLID SECTION
SPRING	CONN3D2 and CONNECTOR SECTION
¹Shell elements with one integration point through the thickness are translated as membrane elements.

Table 5. Constraint data.
RADIOSS keyword	Abaqus equivalent
RWALL	RIGID BODY and CONTACT
RBODY	RIGID BODY and/or MPC (type BEAM) To define an element as a rigid body, enter all the element node numbers in the node group associated with the rigid body.
INTER / Type 2	TIE and FASTENER
INTER / Types 7, 10, 11	CONTACT, CONTACT CONTROLS ASSIGNMENT, CONTACT FORMULATION, CONTACT INCLUSIONS, CONTACT EXCLUSIONS, CONTACT PROPERTY ASSIGNMENT, SURFACE INTERACTION, and SURFACE PROPERTY ASSIGNMENT
CYL_JOINT	CONN3D2 and CONNECTOR SECTION

Table 6. Group data.
RADIOSS keyword	Abaqus equivalent
SUBSET	ELSET; data for elements to be grouped in a set using ELSET
PART	ELSET; data for elements to be grouped in a set using ELSET
MAT	ELSET; data for elements to be grouped in a set using ELSET
PROP	ELSET; data for elements to be grouped in a set using ELSET
NODE	NSET; data for elements to be grouped in a set using NSET
SH3N	ELSET; data for elements to be grouped in a set using ELSET
SHEL	ELSET; data for elements to be grouped in a set using ELSET
GRNOD	NSET; data for elements to be grouped in a set using NSET
GRSH3N	ELSET; data for elements to be grouped in a set using ELSET
GRSHEL	ELSET; data for elements to be grouped in a set using ELSET
GRSPRI	ELSET; data for elements to be grouped in a set using ELSET
GENE	NSET; data for elements to be grouped in a set using NSET
SEG	ELSET; data for elements to be grouped in a set using ELSET
SURF	ELSET and NSET

Table 7. Monitored volume and seat belt data.
RADIOSS keyword	Abaqus equivalent
MONVOL / GASMONVOL / AIRBAG	FLUID BEHAVIOR, FLUID CAVITY, FLUID EXCHANGE, FLUID EXCHANGE ACTIVATION, FLUID EXCHANGE PROPERTY, FLUID INFLATOR, FLUID INFLATOR ACTIVATION, FLUID INFLATOR MIXTURE, FLUID INFLATOR PROPERTY, MOLECULAR WEIGHT, CAPACITY, and PHYSICAL CONSTANTS
SPRING with property SPR_PUL	ELEMENT, TYPE=CONN3D2; CONNECTOR SECTION; and BOUNDARY

Table 8. Miscellaneous data.
RADIOSS keyword	Abaqus equivalent
TITLE	HEADING
ACCEL	CONN3D2 and connector type ACCELEROMETER
FUNCT	Data for material properties and time-dependent parameters, such as AMPLITUDE, CONNECTOR ELASTICITY, PLASTIC, and FLUID EXCHANGE PROPERTY
SECT	INTEGRATED OUTPUT SECTION
SENSOR / Type 0	Use activation time in AMPLITUDE
TH	Data for time history output, such as OUTPUT, HISTORY; NODE OUTPUT; ELEMENT OUTPUT; and ENERGY OUTPUT

Command Summary

abaqus fromradiossjobjob-nameinputinput-filesplitAirbagElements{OFFON}readAbaqusDatdata-fileuserDefaultMassreal-numberuserDefaultInertiareal-numberuserHistoryTimereal-number

Command Line Options

job: This option is used to specify the name of the Abaqus input file to be output by the translator. The name of the Abaqus input file must be given without the .inp extension. Diagnostics created by the translator are written to a file named job-name_fromradioss.log.
input: This option is used to specify the name of the file containing the RADIOSS data. The file extension is optional.
splitAirbagElements: This option is used to specify the splitting of 4-node airbag membrane elements into two 3-node airbag membrane elements. The default value is ON. Airbag membrane elements result from the translation of SHELL or SH3N with one integration point through the thickness. This option is valid only if the keyword MONVOL/AIRBAG is specified in the RADIOSS input file.
readAbaqusDat: This option enables the use of an Abaqus data (.dat) file from a previous Abaqus analysis to reformulate spot weld definitions. The data file should identify spot welds that could not be formed. Using this option, the attachment points for the identified spot welds are translated using distributed coupling constraints.
userDefaultMass: This option is used to specify the nodal mass that is assigned to additional nodes generated during the translation that require nonzero mass. This value should be small (typically 10⁻⁶ times the mass for the entire model). If this option is omitted, the default mass is set to 10⁻⁴.
userDefaultInertia: This option is used to specify the rotary inertia that is assigned to additional nodes generated during the translation that require nonzero rotary inertia. This value should be small (typically 10⁻⁶ times the inertia for the entire model). If this option is omitted, the default rotary inertia is set to 10⁻³.
userHistoryTime: This option is used to specify the time interval used for time history output. If this option is omitted, the time history interval is set to 10⁻⁵.