FEM Neutral Format File
This document describes how to use FEM Neutral Format files, with which you can exchange data between Creo Simulate and FEA programs. To learn about FME Neutral Format files, see the following:
About the FEM Neutral Format
Use the FEM Neutral Format to create concise model descriptions by using the hierarchical file structure and references to data that is already defined.
A FEM Neutral Format file contains information about an entire Finite Element Model, including the following data:
• Definitions of element types and their topology
• Description of FEM topology (that is, nodes and elements)
• Properties
• Applied loads and constraints
• Calculated results
Currently, Creo Parametric outputs a FEM Neutral Format file containing information only about the model's mesh and loads/constraints. After you run a solver on the model, you must convert the solution results into FEM Neutral Format before the model is retrieved in Creo Simulate.
|
|
 Creo Parametric uses FEM Neutral Format revision 3. |
Consider the following conventions when you create your FEM Neutral Format file:
• FEM Neutral Format files have the extension .fnf.
• A FEM Neutral Format file has the following characteristics:
◦ It is an ASCII file consisting of lines.
◦ Each line contains 80 characters or less.
◦ You can continue longer lines by using sub-lines.
◦ End each sub-line with a backslash character (\), except for the last one.
• The FEM Neutral Format is case-insensitive.
• Lines starting with a pound sign (#) as well as empty lines are treated as comments and are skipped (except for the first line).
Information in a FEM Neutral Format file is organized into sections. Each section describes its own class of objects. The order of sections in the FEM Neutral Format file is critical because information from the earlier-defined sections may be required in the sections that follow. You can skip some of the sections that are not relevant to the model description.
|
|
The FEM Neutral Format is backward-compatible.
|
A FEM Neutral Format file must start with an identification line used to recognize the FEM Neutral Format. The identification line format follows.
#PTC_FEM_NEUT n <flags>
where:
n revision number of the FEM Neutral Format file (corresponds to the revision number of the specification). The default is 3.
flags reserved for future use.
An identification line can appear as follows:
#PTC_FEM_NEUT 1
Include the creation date as a comment:
#DATE Wed Mar 22 13:56:07 EET 2000
Defining an Object
Define each object in a FEM Neutral Format file with "instructions." An instruction line starts with a percent sign (%). It consists of fields separated by spaces and/or tabulations.
An instruction line includes the following components:
• instruction keyword indicating an instruction, for example, statistics
• obj_id integer handle of the object (this ID is not necessarily consecutive)
• key string definition used for a general definition of an object or another string specifying a feature of the object
• data object description (for example, placement, node ID, or element type)
The format of an instruction is as follows:
%instruction <obj_id key> [: data ...]
Follow these general guidelines for writing instructions:
• Standard abbreviations may be used instead of full names of keywords. You can also define and use your own aliases.
• There may be cases when you need to skip a fieldfor example, when a particular field in an instruction is not applicable, or you want to use the system default for this field. To skip a field, enter an asterisk (*) in place of the data to be skipped. In this document, descriptions of the fields that can be replaced with an asterisk (*) are enclosed within angle brackets (< >), and the fields that can be omitted are enclosed in square brackets ([ ])
• You can skip the final fields in an instruction by simply omitting them.
• Non-empty lines that begin with anything other than an asterisk (*) or a percent sign (%) are illegal and will generate an error.
You can define an object using one instruction or a group of instructions. If you use a group of instructions, follow these guidelines:
• If the object contains more than one instruction, you must combine the objects together as a group.
• You must assign the same instruction keyword obj_id to all instructions in the group.
• You must assign the key definition (DEF) to the first instruction in the group.
To learn about the instructions and items you will work with in defining a FEM Neutral Format file, see the following:
List of Available Sections
Sections in a FEM Neutral Format file must appear in the following order:
• HEADER General information about the file and FEM model.
• ELEM_TYPES Definition of element types.
• COORD_SYSTEMS Definition of coordinate systems.
• MATERIALS Definition of materials used in the model.
• PROPERTIES Definition of element properties used in the model.
• MESH Definition of the model's nodes and elements.
• MESH_TOPOLOGY Definition of the model's surfaces and edges.
• LOADS Description of applied load/constraint sets.
• ANALYSIS Definition of analysis types.
• RESULTS Description of solution results of the model.
List of Available Instructions
The following table lists supported instructions, their standard abbreviations, and sections in which they may appear.
|
Instruction Name
|
Abbreviation
|
Section Name
|
|
START_SECT
|
STS
|
|
|
END_SECT
|
ENS
|
|
|
END
|
END
|
outside a section
|
|
ALIAS
|
ALS
|
before using an alias
|
|
TITLE
|
TTL
|
HEADER
|
|
STATISTICS
|
STT
|
HEADER
|
|
ELEM_TYPE
|
ETP
|
ELEM_TYPE
|
|
COORD_SYS
|
CS
|
COORD_SYSTEMS
|
|
MATERIAL
|
MAT
|
MATERIALS
|
|
ELEM_PROP
|
EP
|
PROPERTIES
|
|
ELEM_END_PROP
|
EEP
|
PROPERTIES
|
|
NODE
|
ND
|
MESH
|
|
ELEM
|
EL
|
MESH
|
|
EDGE
|
EDG
|
MESH_TOPOLOGY
|
|
SURFACE
|
SRF
|
MESH_TOPOLOGY
|
|
LOAD_TYPE
|
LTP
|
LOADS
|
|
CON_CASE
|
CC
|
LOADS
|
|
LOAD
|
LD
|
LOADS
|
|
SOLUTION
|
SLU
|
ANALYSIS
|
|
RESULT_TYPE
|
RTP
|
RESULTS
|
|
RESULT
|
RES
|
RESULTS
|
In this document, abbreviations are shown in parentheses. For example: RESULT_TYPE (RES).
Special Instructions
FEM Neutral Format files include special instructions. To learn about these special instructions, see the following topics:
Start and End of a Section
Each section starts with the instruction START_SECT (STS) and ends with the instruction END_SECT (ENS).
A section will appear as follows:
%START_SECT : section_name
......
%END_SECT
END Instruction
The END instruction appears as follows:
%END
The END instruction is optional. In a FEM Neutral Format file, all lines appearing after END are skipped.
Defining Aliases
The ALIAS (ALS) instruction is used to define aliases.
You can define an alias for any keyword (instruction or key) and use it instead of the full name or abbreviation.
|
|
Do not create an alias with the name reserved for keywords and standard abbreviations: this results in an error.
|
If several aliases are defined for a keyword, only the last one is considered valid. You can use only alphanumeric aliases.
An alias is defined as follows:
%ALIAS : keyword alias
where:
keyword = full name or its abbreviation.
alias = user-defined alias.
A Typical Alias
%ALIAS : CON_CASE C
%ALIAS : EL FEM_ELEMENT
Definitions of Some Fields Used in Instructions
FEM Neutral Format instructions can include any of several fields, depending on the instruction. To learn about some of these fields, see the following topics:
Referencing IDs
Use the following format to reference IDs of various geometry objects:
• elem_id ID of an element in the model (any positive number).
• node_id ID of a node in the model (any positive number).
• node_in_el_id ID of a node in an element (in the range from 1 to num_nodes, where num_nodes is the number of element nodes). The order of nodes in the element is defined in the ELEM_TYPE instruction.
• edge_in_el_id ID of an edge in an element (in the range from 1 to num_edges, where num_edges is the number of element edges). The order of edges in the element is defined in the ELEM_TYPE instruction.
• face_in_el_id ID of a face in an element (in the range from 1 to num_faces, where num_faces is the number of element faces). The order of faces in the element is defined in the ELEM_TYPE instruction.
Value Types
Value_type appears in instructions describing applied loads/constraints and obtained results. Typically, the format is as follows:
data_type <MASKABLE>
where:
data_type is one of the following:
• SCALAR (SCL)
• VECTOR_2 (VEC2) a vector with two components
• VECTOR (VEC) a vector with three components
• VECTOR_6 (VEC6) a vector with 6 components
• TENSOR (TNS)
MASKABLE indicates that the instruction may have skipped (not defined) components. MASKABLE can be defined for VECTOR_6 only.
For TENSOR, defined in the XYZ coordinates, the order of the components is the following:
TX, TY, TZ, TXY, TYZ, TXZ
and the tensor is defined as:
T(X,Y,Z) = TX*X*X + TY*Y*Y + TZ*Z*Z + 2*TXY*X*Y + 2*TYZ*Y*Z + 2*TXZ*X*Z
The statement "Value corresponds to the given Value_type" means that the value is one of the following:
• 1 scalar if data_type in Value_type is SCALAR
• 2 scalars if data_type in Value_type is VECTOR_2
• 3 scalars if data_type in Value_type is VECTOR
• 6 scalars if data_type in Value_type is VECTOR_6 or TENSOR
Sections of a FEM Neutral Format File
For the list of sections in a FEM Neutral Format file, refer to
List of Available Sections.
Currently, Creo Parametric outputs a FEM Neutral format file containing all sections except RESULTS.
A solver should create a file that contains all the information from the input file "model.fnf," and append to this information the ANALYSIS and RESULTS sections. You then end up with a file that contains all the information originally defined in the input file, as well as the ANALYSIS and RESULTS data.
The solution results are expected to be in exact correspondence with model definitions.
To learn about these sections and the instructions they can contain, see the following topics:
HEADER Section
The HEADER section can contain the TITLE (TTL) and STATISTICS (STT) instructions.
TITLE (TTL) Instruction
This instruction appears as follows:
%TITLE : Model_name
where:
Model_name is the name of the described model.
A Typical Title
%TITLE : bracket
STATISTICS (STT) Instruction
The STATISTICS (STT) instruction provides information about the number of element types, coordinate systems, materials, element properties, nodes, and elements in the model.
This instruction has the following format:
%STATISTICS : num_elem_types num_coord_systems num_materials\
num_properties num_nodes num_elements
where:
num_elem_types number of element types.
num_coord_systems number of coordinate systems.
num_materials number of materials used in the model.
num_properties number of defined properties.
num_nodes number of nodes in the model.
num_elements number of elements in the model.
A Typical Statistic
%STATISTICS : 2 1 2 5 21 33
ELEM_TYPES Section
The ELEM_TYPES section contains the ELEM_TYPE (ETP) instruction.
ELEM_TYPE (ETP) Instruction
An element type description defines a topological scheme of an element. It consists of lines containing data about:
• an element as an entity a line with the key DEF
• each edge lines with the key EDGE
• each face lines with the key FACE
ELEM_TYPE Instruction with the DEF Key
The ELEM_TYPE instruction with the key DEF has the following format:
%ELEM_TYPE id DEF : Class Type <Sub_type Num_corner_nodes \
um_edges Num_faces
where:
Class is one of the following:
• SOLID (SOL) for tetrahedral elements
• SHELL (SHL) for triangle or quad elements
• BAR for elements with 2 nodes (for example, BEAM elements)
• POINT (PNT) for elements with 1 node (MASS or To Ground SPRING elements)
Type is defined as shown in the following table of supported element types.
|
Class
|
Supported Types
|
|
SOLID
|
TETRA (TET)
|
|
SHELL
|
TRIANGLE (TRI),
QUAD (QUA)
|
|
BAR
|
SPAR,
BEAM,
GAP,
ADV_BEAM (ADB),
SPRING (SPR),
ADV_SPRING (ADS)
LINK
|
|
POINT
|
MASS, TO GROUND SPRINGS
|
Sub_type can be LINEAR (LIN) or PARABOLIC (PAR). The default is LINEAR. This field must be skipped if Class is BAR or POINT.
Typical ELEM_TYPE Instructions
%ELEM_TYPE 1 DEF : SOLID TETRA PARABOLIC 4 6 4
%ELEM_TYPE 3 DEF : SHELL QUAD LINEAR 4 4 2
%ELEM_TYPE 4 DEF : SHELL TRIANGLE PARABOLIC 3 3 2
%ELEM_TYPE 7 DEF : BAR GAP * 2 1 0
%ELEM_TYPE 8 DEF : POINT MASS * 1 0 0
ELEM_TYPE Instruction with the EDGE Key
|
|
The number of ELEM_TYPE instructions is equal to Num_edges given in the ELEM_TYPE instruction with the key DEF.
|
The format of the ELEM_TYPE instruction with the key EDGE is as follows:
%ELEM_TYPE id EDGE : edge_id Edge_placement
where:
id same as in the DEF line.
Edge_placement lists the ID's of the element's end nodes and the ID of the mid-node (for PARABOLIC sub_type only) in the following format:
node_in_el_id_1 node_in_el_id_2 <midnode_in_el_id>
ELEM_TYPE Instruction with the FACE Key
|
|
The number of these instructions is equal to Num_faces, given in the ELEM_TYPE instruction with the key DEF.
|
The format is the following:
%ELEM_TYPE id FACE :face_id Face_placement
where:
id same as in the DEF line.
Face_placement consists of the ID's of the element's face edges in the counterclockwise direction, if looked at from the end of the positive normal to the face. The format is the following:
edge_in_el_id_1 edge_in_el_id_2 ...
Example of the ELEM_TYPE Instruction
%ELEM_TYPE 2 DEF : SHELL TRIANGLE PARABOLIC 3 3 2
%ELEM_TYPE 2 EDGE : 1 1 2 4
%ELEM_TYPE 2 EDGE : 2 2 3 5
%ELEM_TYPE 2 EDGE : 3 3 1 6
%ELEM_TYPE 2 FACE : 1 1 2 3 %ELEM_TYPE 2 FACE : 2 1 3 2
COORD_SYSTEMS Section
The COORD_SYSTEMS section contains the COORD_SYS (CS) instructions.
COORD_SYS (CS) Instruction
A description of a coordinate system includes five lines with the following keys: DEF, X_VECTOR, Y_VECTOR, Z_VECTOR, ORIGIN.
COORD_SYS Instruction with the DEF Key
This instruction has the following format:
%COORD_SYS cs_id DEF [: <name <type ]
where:
cs_id ID of the coordinate system (starting with 1).
name (optional) name of the coordinate system.
type is one of the following:
• CARTESIAN (CAR)default
• CYLINDRICAL (CYL)
• SPHERICAL (SPH)
COORD_SYS Instruction with the X_VECTOR Key
This instruction has the following format:
%COORD_SYS cs_id X_VECTOR : X_vect0 X_vect1 X_vect2
where:
cs_id ID of the coordinate system (starting with 1).
X_vect0, X_vect1, and X_vect2 global coordinates of the X-vector of the described coordinate system.
The abbreviated form for X_VECTOR is X.
COORD_SYS Instruction with the Y_VECTOR Key
This instruction has the following format:
%COORD_SYS cs_id Y_VECTOR : Y_vect0 Y_vect1 Y_vect2
where:
cs_id ID of the coordinate system (starting with 1).
Y_vect0, Y_vect1, and Y_vect2 global coordinates of the Y-vector of the described coordinate system.
The abbreviated form for Y_VECTOR is Y.
COORD_SYS Instruction with the Z_VECTOR Key
This instruction has the following format:
%COORD_SYS cs_id Z_VECTOR :Z_vect0 Z_vect1 Z_vect2
where:
cs_id ID of the coordinate system (starting with 1).
Z_vect0, Z_vect1, and Z_vect2 global coordinates of the Z-vector of the described coordinate system.
The abbreviated form for Z_VECTOR is Z.
COORD_SYS Instruction with the ORIGIN Key
This instruction has the following format:
%COORD_SYS cs_id ORIGIN : Orig0 Orig1 Orig2
where:
cs_id ID of the coordinate system (starting with 1).
Orig0, Orig1, and Orig2 global coordinates of the origin of the described coordinate system. The abbreviated form for ORIGIN is ORG.
MATERIALS Section
The MATERIALS section contains the MATERIAL (MAT) instruction.
MATERIAL (MAT) Instruction
The instruction MATERIAL with the key DEF specifies the material name and type. Each additional MATERIAL instruction contains a key indicating the name of the material property to be defined in this instruction.
The following material properties are supported:
• YOUNG_MODULUS (YNG)
• POISSON_RATIO (PSN)
• SHEAR_MODULUS (SHR)
• MASS_DENSITY (DNS)
• THERMAL_EXPANSION_COEFFICIENT (TEC)
• THERM_EXPANSION_REF_TEMPERATURE (TER)
• STRUCTURAL_DAMPING_COEFFICIENT (SDP)
• STRESS_LIMIT_FOR_TENSION (SLT)
• STRESS_LIMIT_FOR_COMPRESSION (SLC)
• STRESS_LIMIT_FOR_SHEAR (SLS)
• THERMAL_CONDUCTIVITY (THC)
• EMISSIVITY (EMS)
• SPECIFIC_HEAT (SHT)
MATERIAL Instruction with the DEF key
This instruction has the following format:
%MATERIAL id DEF: mat_name <mat_type
where:
id material ID (starting with 1).
mat_name name of the material (up to 32 characters).
mat_type type of material. Currently, the system supports only one type: ISOTROPIC (default).
MATERIAL Instruction with the MAT_PROP Key
This instruction has the following format:
%MATERIAL id MAT_PROP : data
where:
id material ID (same as in the DEF line).
Mat_prop one of the names of material properties (refer to
MATERIAL (MAT) Instruction).
data depends on Mat_prop. For all currently supported properties, there is one scalar value.
|
|
Material properties that are not defined are assumed to be zeros.
|
Typical Material Instructions
%MATERIAL 1 DEF : ALUM ISOTROPIC
MATERIAL 1 YOUNG_MODULUS : 1.900000E+07
MATERIAL 1 POISSON_RATIO : 2.100000E-01
%MATERIAL 1 SHEAR_MODULUS : 7.850000E+06
%MATERIAL 1 MASS_DENSITY : 2.830000E-01
%MATERIAL 1 THERMAL_EXPANSION_COEFFICIENT : 6.780000E+00
%MATERIAL 1 THERMAL_CONDUCTIVITY : 1.000000E-02
PROPERTIES Section
The PROPERTIES section may contain the following instructions:
• ELEM_PROP (EP)
• ELEM_END_PROP (EEP)
ELEM_PROP (EP) Instruction:
The ELEM_PROP instruction defines element properties. The key (except when DEF) is the name of the property.
For beam elements with additional end properties, the key REF can be used to reference instructions, defining the appropriate end properties (that is, ELEM_END_PROP).
The supported element properties (keys of the ELEM_PROP instruction) are listed in the following table.
|
Property Name
|
Abbreviation
|
Used for
|
|
THICKNESS
|
THI
|
SHELL elements
|
|
CROSS_SECTION_AREA
|
XSA
|
BEAM and ADV_BEAMelements
|
|
MASS_VALUE
|
MAS
|
MASS elements
|
|
MOMENT_OF_INERTIA
|
INE
|
Moment of inertia in an elemental coordinate system for BEAM and MASS elements
|
|
GAP_VALUE
|
GV
|
GAP elements
|
|
NORMAL_STIFFNESS
|
NST
|
GAP elements
|
|
SLIDE_STIFFNESS
|
SST
|
GAP elements
|
|
EXTENSIONAL_STIFFNESS
|
EST
|
SPRING elements
|
|
TORSIONAL_STIFFNESS
|
TST
|
SPRING elements
|
|
VECTOR_STIFFNESS
|
VST
|
ADV_SPRING elements
|
|
DAMPING
|
DMP
|
ADV_SPRING elements
|
|
STRESS_RECOVERED
|
SRV
|
For ADV_BEAM elements, it may be one of: YES or NO.
|
|
SHEAR_STIFF_FACTOR_IN_XZ_PLANE
|
SSZ
|
ADV_BEAM elements
|
|
SHEAR_STIFF_FACTOR_IN_XY_PLANE
|
SSY
|
ADV_BEAM elements
|
|
SHEAR_RELIEF_COEFF_IN_XZ_PLANE
|
SRZ
|
ADV_BEAM elements
|
|
SHEAR_RELIEF_COEFF_IN_XY_PLANE
|
SRY
|
ADV_BEAM elements
|
The element type Link does not have any property associated with it.
ELEM_PROP Instruction with the DEF key
This instruction has the following format:
%ELEM_PROP id DEF: elem_type_id <name
where:
id ID of the set of properties.
elem_type_id ID of ELEM_TYPE for which the properties are defined.
name name of this set of properties (if it is named).
ELEM_PROP Instruction with the PROP_NAME Key
This instruction has the following format:
%ELEM_PROP id PROP_NAME : data
where:
id ID of the set of properties being defined.
PROP_NAME one of the property names (refer to ELEM_PROP (EP) Instruction). The property name has to be valid for a given ELEM_TYPE, referenced in the line DEF.
data depends on the PROP_NAME:
• For MASS_VALUE, GAP_VALUE, NORMAL_STIFFNESS, SLIDE_STIFFNESS, EXTENSIONAL_STIFFNESS, TORSIONAL_STIFFNESS, and CROSS_SECTION_AREA, data is one scalar value.
• For THICKNESS, data is num_nodes scalar values, one per element node; values are in the order of node ID's within the element (num_nodes is the number of corner nodes for ELEM_TYPE, referenced in the line DEF).
• For MOMENT_OF_INERTIA, data is a one-vector (three scalars) value.
• For VECTOR_STIFFNESS and DAMPING, data is a one-vector (three scalars) value, defined in the coordinate system, referenced in the description of the element.
Typical ELEM_PROP Instructions
%ELEM_TYPE 2 DEF : SHELL TRIANGLE LINEAR 3 3 2
...
%ELEM_TYPE 3 DEF : BAR SPAR * 2 1 0
...
%ELEM_PROP 1 DEF : 2
%ELEM_PROP 1 THICKNESS : 0.5 0.6 1.0
...
%ELEM_PROP 2 DEF : 3
%ELEM_PROP 2 CROSS_SECTION_AREA : 0.01
ELEM_PROP Instruction with the REF Key
This instruction has the following format:
%ELEM_PROP id REF: node_in_el_id end_prop_id
where:
node_in_el_id is the node ID number inside the element.
end_prop_idrefers to the corresponding ELEM_END_PROP instruction.
ELEM_END_PROP (EEP) Instruction
|
Property name
|
Abbreviation
|
Used for
|
|
CROSS_SECTION_AREA
|
XSA
|
BEAM and ADV_BEAM elements
|
|
PIN_FLAG
|
PIN
|
ADV_BEAM elements
|
|
MOMENT_OF_INERTIA_ABOUT_Z_AXIS
|
MIZ
|
ADV_BEAM elements
|
|
MOMENT_OF_INERTIA_ABOUT_Y_AXIS
|
MIY
|
ADV_BEAM elements
|
|
AREA_PRODUCT_OF_INERTIA
|
API
|
ADV_BEAM elements
|
|
TORSION_STIFFNESS_PARAMETER
|
TSP
|
ADV_BEAM elements
|
|
NONSTRUCT_MASS_PER_UNIT_LENGTH
|
NML
|
ADV_BEAM elements
|
|
Y_COORD_OF_POINT_C
|
YCC
|
ADV_BEAM elements
|
|
Z_COORD_OF_POINT_C
|
ZCC
|
ADV_BEAM elements
|
|
Y_COORD_OF_POINT_D
|
YCD
|
ADV_BEAM elements
|
|
Z_COORD_OF_POINT_D
|
ZCD
|
ADV_BEAM elements
|
|
Y_COORD_OF_POINT_E
|
YCE
|
ADV_BEAM elements
|
|
Z_COORD_OF_POINT_E
|
ZCE
|
ADV_BEAM elements
|
|
Y_COORD_OF_POINT_F
|
YCF
|
ADV_BEAM elements
|
|
Z_COORD_OF_POINT_F
|
ZCF
|
ADV_BEAM elements
|
|
NONSTR_MASS_MOMENT_PER_UNIT_LEN
|
NMU
|
ADV_BEAM elements
|
|
WARPING_COEFFICIENT
|
WRC
|
ADV_BEAM elements
|
|
Y_COORD_OF_GRAVITY_CENTER
|
YGC
|
ADV_BEAM elements
|
|
Z_COORD_OF_GRAVITY_CENTER
|
ZGC
|
ADV_BEAM elements
|
|
Y_COORD_OF_NEUTRAL_AXIS
|
YNA
|
ADV_BEAM elements
|
|
Z_COORD_OF_NEUTRAL_AXIS
|
ZNA
|
ADV_BEAM elements
|
All of the end properties listed above are scalars.
ELEM_END_PROP Instruction with the DEF Key
This instruction has the following format:
%ELEM_END_PROP id DEF: elem_type_id <name
where:
id ID of the set of properties.
elem_type_id ID of the ELEM_TYPE for which this set is defined.
name name of this set of properties (if it is named).
ELEM_END_PROP Instruction with the PROP_NAME
This instruction has the following format:
%ELEM_END_PROP id PROP_NAME : data
where:
id is the ID of the set of properties being defined.
PROP_NAME is one of the keys listed above. The property name must be valid for a given ELEM_TYPE, referenced in the line DEF.
data depends on the PROP_NAME.
Typical ELEM_END_PROP Instructions
%ELEM_TYPE 3 DEF : BAR BEAM * 2 1 0 ...
%ELEM_PROP 2 DEF : 3
%ELEM_PROP 2 REF : 1 5
%ELEM_PROP 2 REF : 1 7
%ELEM_PROP 2 MOMENT_OF_INERTIA : 0. 0. 0.
...
%ELEM_END_PROP 5 DEF : 3
%ELEM_END_PROP 5 CROSS_SECTION_AREA : 0.1
...
%ELEM_END_PROP 7 DEF : 3
%ELEM_END_PROP 7 CROSS_SECTION_AREA : 0.21
...
MESH Section
The MESH section may contain the following instructions:
• NODE (ND)
• ELEM (EL)
NODE (ND) Instruction
This instruction has the following format:
%NODE node_id DEF : placement <cs_id
where:
node_id node ID in the model (starting with 1).
placement vector of the node coordinates.
cs_id ID of the coordinate system used for constraints applied to this point. If skipped, the default coordinate system is used.
Typical Node Instructions
%NODE 1 DEF : 0.8 -0.88 9. 2
%NODE 2 DEF : 0. 1. 2.
ELEM (EL) Instruction
This instruction has the following format:
%ELEM elem_id DEF : elem_type_id <material_id <prop_id placement
where:
elem_id is the ID of the element in the model (starting with 1).
elem_type_id refers to the ELEM_TYPE description.
material_id refers to the MATERIAL description (not required for MASS, SPRING, and ADVANCED SPRING elements).
prop_id refers to the ELEM_PROP description (may not be defined for some elements).
placement describes element placement, depends on the ELEM_TYPE.
Element Placement
This instruction has the following format:
node1_id node2_id ... [cs_id] [offsets]
For SOLID and SHELL elements, placement is a list of node_id's for all element nodes. Corner nodes should be listed first in the order referenced in ELEM_TYPE; then mid-nodesin the order of element edges. The format is as follows:
node1_id ... nodeN_id
where:
N num_nodes for linear elements from the corresponding ELEM_TYPE definition, or (num_nodes + num_edges) for parabolic elements.
For MASS and To Ground SPRING elements, placement is defined as follows:
node_id <cs_id
where:
node_id ID of the element node.
cs_id ID of the elemental coordinate system. For MASS elements, cs_id is required only if inertia is defined for the element; that is, Prop_id is defined, and it references a set of properties with the MOMENT_OF_INERTIA line.
For SPAR, GAP, SPRING elements, placement is:
node1_id node2_id
where:
node1_id, node2_id IDs of its end nodes.
For BEAM, ADV_BEAM elements, placement is defined as follows:
node1_id node2_id cs_id <offset1 offset2>
where:
node1_id, node2_id IDs of its end nodes.
cs_id ID of the elemental coordinate system.
offset1 vector representing the offset of the first bar end from node1 in the elemental coordinate system.
offset2 vector representing the offset of the second bar end from node2 in the elemental coordinate system.
The default for offset1 and offset2 is a zero vector.
For ADV_SPRING element, placement is:
node1_id node2_id cs_id
where:
node1_id,
node2_id
IDs of its end nodes.
cs_id ID of the elemental coordinate system.
Refer to the following example:
%ELEM_TYPE 5 DEF : BAR BEAM * 2 1 0
...
...
%COORD_SYS 3 DEF : * CARTESIAN
%COORD_SYS 3 X_VECTOR : 0. 1. 0.
%COORD_SYS 3 Y_VECTOR : 1. 0. 0.
%COORD_SYS 3 Z_VECTOR : 0. 0. -1.
%COORD_SYS 3 ORIGIN : 0.88 -99. -1.5
...
...
%ELEM_PROP 2 DEF : 5
%ELEM_PROP 2 CROSS_SECTION_AREA : 0.01 0.021
%ELEM_PROP 2 MOMENT_OF_INERTIA : 0. 0. 0.
...
...
%MATERIAL 1 DEF : ALUM ISOTROPIC
%MATERIAL 1 YOUNG_MODULUS : 1.900000E+07
%MATERIAL 1 POISSON_RATIO : 2.100000E-01
...
...
...
%NODE 7 DEF : 0.88 -99. -1.5 .88 -99. -1.5
%NODE 8 DEF : 0.88 0. -1.5 .88 0. -1.5
%ELEM 10 DEF : 5 1 2 7 8 3 0.1 0. 0. 0. 0. 0.
MESH_TOPOLOGY Section
The MESH_TOPOLOGY section may contain the following instructions:
• EDGE (EDG)
• SURFACE(SRF)
EDGE (EDG) instruction with the DEF Key
This instruction has the following format:
%EDGE edge_id DEF: <num_nodes>
where:
edge_id ID of the edge.
num_nodes number of nodes on the edge.
EDGE (EDG) instruction with the NODES Key
This instruction has the following format:
%EDGE edge_id NODES: <corner_node_id>
where:
corner_node_id list of corner node IDs along the edge. The length of the list is num_nodes.
SURFACE (SRF) instruction with the DEF Key
This instruction has the following format:
%SURFACE surface_id DEF: <num_faces>
where:
surface_id ID of the surface.
num_faces number of faces lying on the surface.
SURFACE (SRF) instruction with the FACES Key
This instruction has the following format:
%SURFACE surface_id FACES: <elem_id face_id>
where:
elem_id face_id list of element and face ID pairs. The length of the list is num_faces.
LOADS Section
The LOADS section may contain the following instructions:
• LOAD_TYPE (LTP)
• CON_CASE (CC)
LOAD_TYPE (LTP) Instruction
This instruction has the following format:
%LOAD_TYPE id DEF: Name Placement_type Value_type
where:
Name is the name of the load/constraint. It can be one of the following:
• PRESSURE (COEFF)
• FORCE (FOR)
• MOMENT (MOM)
• DISPLACEMENT (DSP)
• TEMPERATURE (TEM)
• ACCELERATION (ACC)
• ANG_VELOCITY (AVE)
• CONVECTION (CNV)
• HEAT_FLUX (HFL)
• HEAT_SOURCE (HSR)
• FREQ_RANGE (FRQ)
• NUM_MODES (MNU)
• INIT_GUESS (ING)
Placement_type can be one of the following: BODY, ELEM, ELEM_FACE, ELEM_EDGE, NODE.
Typical LOAD_TYPE Instructions
%LOAD_TYPE 1 DEF : DISPLACEMENT NODE VECTOR_6 MASKABLE
%LOAD_TYPE 3 DEF : FORCE NODE VECTOR
%LOAD_TYPE 5 DEF : ACCELERATION BODY VECTOR
%LOAD_TYPE 7 DEF : TEMPERATURE NODE SCALAR
CON_CASE (CC) Instruction
This instruction has the following format:
%CON_CASE id DEF : name <num_steps
where:
name name of the analysis.
num_steps number of steps for time-dependent analyses (reserved for future use). The system default is 1.
A Typical CON_CASE Instruction
%CON_CASE 1 DEF : Case1
Instruction LOAD (LD)
This instruction has the following format:
%LOAD id DEF : load_type_id con_case_id <step \
<cs_type> <cs_id <mask
%LOAD id VAL : <placement value
where:
load_type_id refers to LOAD_TYPE.
con_case_id refers to CON_CASE containing this load/constraint. If this analysis is time-dependent and the load/constraint is included in one step, specify the case number starting with 1.
cs_type indicates whether the value is defined in the global coordinate system (GCS), local nodal coordinate system (NCS), or local elemental coordinate system (ECS). For SCALAR values, cs_type should be skipped. The default is GCS.
cs_id refers to the definition of coordinate system.
mask string of 0's or 1's, used to define mask for MASKABLE values (refer to
LOAD_TYPE (LTP) Instruction).
placement depends on the corresponding LOAD_TYPE.
value corresponds to the Value_type, defined in LOAD_TYPE. For MASKABLE loads, it contains only values for components with 1's.
Placement
If Placement_type in LOAD_TYPE is:
• BODY then placement is absent.
• ELEM then placement is elem_id.
• ELEM_FACE then placement is elem_id face_in_el_id.
• ELEM_EDGE then placement is elem_id edge_in_el_id.
• NODE then placement is node_id.
Refer to the following example:
%NODE 5 DEF : 0.88 -99. -1.5
...
%NODE 15 DEF : 11. -11. 0.11
...
%LOAD_TYPE 3 DEF : DISPLACEMENT NODE VECTOR_6 MASKABLE
...
%LOAD 1 DEF : 3 1 * GCS * 111000
%LOAD 1 VAL : 5 0. 0. 0.
%LOAD 1 VAL : 15 3. 4. 5.
ANALYSIS Section
The ANALYSIS section may contain the SOLUTION (SLU) instruction.
SOLUTION Instruction with the Key DEF
This instruction has the following format:
%SOLUTION id DEF : type <sub_type
where:
type type of analysis. It can be either STRUCTURAL, THERMAL, or MODAL.
sub_type either STATIC (default for the type STRUCTURAL) or STEADY_STATE (default for the type THERMAL).
SOLUTION Instruction with the Key CON_CASES
This instruction has the following format:
%SOLUTION id CON_CASES : con_case_ids
where:
con_case_ids IDs of analyses (refer to the CON_CASE instructions) to be solved in this run of the solver.
Typical SOLUTION Instructions
%SOLUTION 1 DEF : STRUCTURAL STATIC
%SOLUTION 1 CON_CASES : 1 3 4 7
RESULTS Section
The RESULTS section may contain the following instructions:
• RESULT_TYPE (RTP)
• RESULT (RES)
RESULT_TYPE (RTP) Instruction
This instruction has the following format:
%RESULT_TYPE id DEF : Name Placement_type Value_type
where:
Name is the name of the result. It can be one of the following:
• DISPLACEMENT (DSP)
• STRESS (STR)
• STRAIN (STN)
• REACTION_FORCE (RF)
• ERROR_ESTIMATE (ERR)
• THERMAL_STRAIN (THS)
• TEMPERATURE (TEM)
• HEAT_FLUX (HFL)
• HEAT_GRADIENT (HGR)
• MODE_FREQUENCY (FRQ)
Placement_type one of the following types:
• ELEM is the elemental result (currently it may be only ERROR_ESTIMATE).
• ELEM_NODE is the non-averaged data, defined for every node of an element (for example, STRESS, STRAIN, THERMAL_STRAIN, HEAT_FLUX, HEAT_GRADIENT)
• NODE is the nodal data (for example, DISPLACEMENT, REACTION_FORCE, TEMPERATURE).
• BODY is the whole model result (currently it may be only MODE_FREQUENCY).
The following table lists Solid Element Result Types.
|
Placement_type
|
Result_type
|
|
NODE
|
DISPLACEMENT, REACTION_FORCE, STRESS, STRAIN, TEMPERATURE, HEAT_FLUX, HEAT_GRADIENT
|
|
ELEM
|
ERROR_ESTIMATE
|
|
ELEM_NODE
|
STRESS, STRAIN, THERMAL_STRAIN, HEAT_FLUX, HEAT_GRADIENT
|
|
BODY
|
MODE_FREQUENCY
|
The following table lists Shell Element Result Types.
|
Placement_type
|
Result_type
|
|
NODE
|
DISPLACEMENT, REACTION_FORCE, STRESS, STRAIN, TEMPERATURE, HEAT_FLUX, HEAT_GRADIENT
|
|
ELEM
|
ERROR_ESTIMATE
|
|
ELEM_NODE
|
STRESS, STRAIN, THERMAL_STRAIN, HEAT_FLUX, HEAT_GRADIENT
|
|
BODY
|
MODE_FREQUENCY
|
|
ELEM_FACE
|
ERROR_ESTIMATE (For different values on both sides)
|
|
FACE_NODE
|
STRESS, STRAIN (For different values on both sides)
|
Refer to the following examples:
%RESULT_TYPE 1 DEF : DISPLACEMENT NODE VECTOR_6
%RESULT_TYPE 3 DEF : STRESS ELEM_NODE TENSOR
%RESULT_TYPE 4 DEF : ERROR_ESTIMATE ELEM SCALAR
RESULT (RES) Instruction
This instruction has the following format:
%RESULT id DEF : result_type_id con_case_id <step/mode> <cs_type>
%RESULT id VAL : placement value
where:
result_type_id refers to RESULT_TYPE.
con_case_id refers to the analysis for which the results were obtained. If a analysis has steps, the number of steps must be specified.
step/mode is the time step or mode number for dynamic and modal analyses.
cs_type indicates whether a value is defined in the global coordinate system (GCS), local nodal coordinate system (NCS), or local elemental coordinate system (ECS). For SCALAR values, it should be skipped. The default is GCS.
placement depends on Placement_type, defined in the RESULT_TYPE.
value corresponds to Value_type, defined in RESULT_TYPE.
Placement of Results
The following table lists possible placements depending on Placement_type given in the RESULT_TYPE instruction.
|
Placement_type
|
Placement
|
|
ELEM
|
elem_id
|
|
ELEM_FACE
|
elem_id face_in_el_id
|
|
ELEM_NODE
|
elem_id node_in_el_id
|
|
FACE_NODE
|
elem_id face_in_el_id node_in_el_id
|
|
NODE
|
node_id
|
|
BODY
|
none
|
%ELEM_TYPE 1 DEF : SHELL TRIANGLE LINEAR 3 3 2
%ELEM_TYPE 1 EDGE : 1 1 2
%ELEM_TYPE 1 EDGE : 2 2 3
%ELEM_TYPE 1 EDGE : 3 3 1
%ELEM_TYPE 1 FACE : 1 1 2 3
%ELEM_TYPE 1 FACE : 2 1 3 2
%RESULT_TYPE 1 DEF : DISPLACEMENT NODE VECTOR_6
%RESULT_TYPE 2 DEF : STRESS FACE_NODE TENSOR\ ECS
%RESULT_TYPE 3 DEF : ERROR_ESTIMATE ELEM SCALAR
%ELEM 5 DEF : 1 ....
# Displacement
%RESULT 1 DEF : 1 1
# in node17
%RESULT 1 VAL : 17 1. 2. 3. 0. 0. 0.
# in node 25
%RESULT 1 VAL : 25 11. 22. 33. 0. 0. 0.
...
# Stress
%RESULT 20 DEF : 2 1 * ECS
# in SHELL element #5, face 1 (top), node #1
%RESULT 20 VAL : 5 1 1 0.1 0.2 0.3 0.4 0.5 -0.6
# in SHELL element #5, face 2 (bottom), node #1
%RESULT 20 VAL : 5 2 1 ...
# in SHELL element #5, face 2 (bottom), node #3
%RESULT 20 VAL : 5 2 3 ...
...
# Error Estimate
%RESULT 50 DEF : 3
# on element #5, Face 1 (Top)
%RESULT 50 VAL : 5 1 0.5
# on element #5, Face 2 (Bottom)
%RESULT 50 VAL : 5 2 0.05