3.2.21 Execution procedure for translating PAM-CRASH input files to partial ABAQUS input files

Product: ABAQUS/Explicit  

Reference

Overview

The translator from PAM-CRASH to ABAQUS converts certain keywords in a PAM-CRASH input file into their equivalent in ABAQUS/Explicit.

Using the translator

The translator requires an input file created by PAM-CRASH 2003. The input file can have any name and extension.

The PAM-CRASH data entries that are translated are listed in the tables below. Other PAM-CRASH 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. You must provide history data (including output data) to complete the input.

Element numbering and grouping

All elements must have unique element numbers. Elements that are assigned the same PART identification number are grouped together in an element set.

Except for connector elements that result from the translation of SPRING and KJOIN, section properties need to be entered in the PART section rather than individually in the element section. Elements that have different material or section properties should be given different PART identification numbers; that is, the same material and section properties must be applicable to all elements grouped in the same element set.

For connector elements that result from the translation of SPRING and KJOIN, if elements that have different element data (such as frame numbers used to define local directions) 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 3.2.21–3. All unsupported material models between Types 1 and 99 are translated as bilinear elastic-plastic, and all other material types 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.

History section data

The translator creates a history section based partially on keywords (except TITLE) from the control section of the PAM-CRASH file as shown in Table 3.2.21–1. Other control data are unsupported.

Summary of PAM-CRASH entities translated

Table 3.2.21–1 Control section data.

PAM-CRASH keywordABAQUS equivalent
TITLE*HEADING
RUNEND*DYNAMIC, EXPLICIT time period
TCTRL / DYNA_MASS_SCALE*VARIABLE MASS SCALING

Table 3.2.21–2 Part section data.

PAM-CRASH keywordABAQUS equivalent
PART / BARTruss element properties and grouping data
PART / BEAMBeam element properties and grouping data
PART / SPRINGConnector behavior and grouping data
PART / KJOINConnector type, behavior, and grouping data
PART / SOLIDSolid element properties and grouping data
PART / SHELLShell element properties and grouping data
PART / MEMBRMembrane element properties and grouping data
PART / TIEDMesh tie constraint data and parameters
PART / PLINKMesh-independent fastener data and parameters

Table 3.2.21–3 Material section data.

PAM-CRASH keywordABAQUS equivalent
MATER / Types 1, 99C3D4/C3D6/C3D8R; solid material model data
MATER / Types 100, 101, 102, 103S3RS/S4RS; shell material model data
MATER / Types 150, 151 M3D3/M3D4/M3D4R and *USER MATERIAL
MATER / Types 200, 201, 202T3D2/B31; beam and truss material model data
MATER / Types 203, 204, 205, 230CONN3D2; connector behavior data
MATER / Types 212, 213B31; beam material model data

Table 3.2.21–4 Node section data.

PAM-CRASH keywordABAQUS equivalent
FRAME*ORIENTATION and *TRANSFORM
NODE*NODE
MASS*MASS and *ROTARY INERTIA
NSMAS*NONSTRUCTURAL MASS
INVEL*INITIAL CONDITIONS, TYPE=VELOCITY or ROTATING VELOCITY
BOUNC*BOUNDARY
DIS3D*BOUNDARY and *AMPLITUDE
VEL3D*BOUNDARY and *AMPLITUDE
DAMP*DLOAD and *AMPLITUDE
TRSFM*NODE with transformed coordinates

Table 3.2.21–5 Element section data.

PAM-CRASH keywordABAQUS equivalent
SOLIDC3D4/C3D6/C3D8R and *SOLID SECTION
TETR4C3D4 and *SOLID SECTION
SHELLS3RS/S4RS and *SHELL SECTION
MEMBRM3D3/M3D4R and *MEMBRANE SECTION
BEAMB31 and *BEAM SECTION, SECTION=CIRC
BARFor MATER / Types 203 and 204: CONN3D2 and *CONNECTOR SECTION [AXIAL]For all other MATER / Types: T3D2 and *SOLID SECTION
SPRINGCONN3D2 and *CONNECTOR SECTION [CARTESIAN + CARDAN]
KJOINCONN3D2 and *CONNECTOR SECTION
PLINK*FASTENER and *FASTENER PROPERTY; CONN3D2 and *CONNECTOR SECTION

Table 3.2.21–6 Constraint section data.

PAM-CRASH keywordABAQUS equivalent
RWALL
(Stationary, segmented finite rigid wall)
Velocity flag=0
Wall description=20
*RIGID BODY and *CONTACT
RBODY
Types 0, 3
*RIGID BODY and/or *MPC (MPC type BEAM)
To define a group of elements as a rigid body, enter the part identification number of that element group as the PART entity1.
To define an element as a rigid body, enter the element number as the ELE entity or enter all the element node numbers as the NOD entity2.
RBODY
Type 1
CONN3D2, *CONNECTOR SECTION [PROJECTION CARTESIAN + PROJECTION FLEXION-TORSION], *CONNECTOR DAMAGE INITIATION, and *CONNECTOR DAMAGE EVOLUTION
CNTAC
Sliding interface types:
33, 34, 36, 37, 46
*CONTACT, *CONTACT INCLUSIONS, *CONTACT EXCLUSIONS, *CONTACT PROPERTY ASSIGNMENT, *CONTACT FORMULATION, *SURFACE INTERACTION, and *SURFACE PROPERTY ASSIGNMENT
TIED*TIE
1 If PART entities are used to define a rigid body, RBODY is translated as *RIGID BODY.
2 If the ELE and NOD entities constitute all elements in a part, RBODY is translated as *RIGID BODY. If the ELE and NOD entities do not constitute all elements in a part (i.e., if the part consists of both rigid and deformable elements), RBODY is translated as *MPC (MPC type BEAM), a beam-type multi-point constraint for the set of nodes that consists of all input NOD entities and nodes extracted from all ELE entities.

Table 3.2.21–7 Nodes/faces/elements entity selection data.

PAM-CRASH keywordABAQUS equivalent
ELE*ELSET; data for elements to be grouped in a set using *ELSET
PARTData for selecting element sets (*ELSET) already defined
NODData for nodes to be grouped in a set using *NSET
ELE>NODSame procedure as ELE
PART>NODSame procedure as PART
DELELE*ELSET and *NSET
DELPART*ELSET and *NSET
DELNOD*ELSET and *NSET
GRPNamed set of entities defined in GROUP

Table 3.2.21–9 Seat belt data.

PAM-CRASH keywordABAQUS equivalent
SLIPR*ELEMENT, TYPECONN3D2; *CONNECTOR SECTION; and *BOUNDARY
RETRA*ELEMENT, TYPECONN3D2; *CONNECTOR SECTION; and *BOUNDARY

Table 3.2.21–10 Miscellaneous data.

PAM-CRASH keywordABAQUS equivalent
GROUPConvert entities to ABAQUS equivalents
METRIC*INITIAL CONDITIONS, TYPE=REF COORDINATE
SENSORType-1: use activation time in *AMPLITUDE
Type-4: use belt feed rate in *CONNECTOR LOCK
FUNCTData for material properties and time-dependent parameters, such as *AMPLITUDE, *CONNECTOR ELASTICITY, *PLASTIC, and *FLUID EXCHANGE PROPERTY
THELEElement sets defined as *ELSET; output quantities are not specified for the element set
THNODNode sets defined as *NSET; output quantities are not specified for the node set

Command summary

abaqus frompamcrash
job=job-name
 
input=input-file
[pLinkConnectors={OFF |  ON}]
[splitAirbagElements={OFF |  ON}]
[autoKJoinStops={OFF | ON}]

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 will be written to a file named job-name_frompam.log.

input

This option is used to specify the name of the file containing the PAM-CRASH data. The name of the file must be given with the file extension.

pLinkConnectors

This option is used to specify the inclusion of connector elements in the PLINK translation. The default value is ON.

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 MEMBR and MATER / Types 150 and 151. This option is valid only if the keyword BAGIN is specified in the PAM-CRASH input file.

autoKJoinStops

This option is used to add connector stops to the behavior of all KJOIN connector elements. If the stiffness interpolated at an endpoint on the force-displacement curve exceeds the stiffness interpolated at an adjacent point by a factor of 10, a connector stop is defined at the point adjacent to the endpoint. The default value is OFF.