3.2.34 Translating RADIOSS input files to partial Abaqus input files
Product: Abaqus/Explicit
Overview
The translator from RADIOSS to Abaqus converts certain keywords in a RADIOSS input file into their equivalent in Abaqus/Explicit.
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 3.2.34–1. 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
| 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 |
| 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 |
| 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 |
| 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 3.2.34–5 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 |
| 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 3.2.34–7 Monitored volume and seat belt data.
| RADIOSS keyword | Abaqus equivalent |
|---|---|
| MONVOL / GAS MONVOL / 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 3.2.34–8 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 line options
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.
This option is used to specify the name of the file containing the RADIOSS data. The file extension is optional.
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.
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.
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.
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.
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.