9.3.3. Input File Format (ANSYS & NASTRAN)
The FFlex body of RecurDyn at the minimum requires the definition of nodes and element and their connections. If the property and material data do not exist, RecurDyn/FFlex automatically generates the default properties and materials based on the connection information
How to make an input file
The NASTRAN input is a file that contains FE information to analyze the system. RecurDyn extracts the necessary information from this file.
The ANSYS input file is an exported file from ANSYS using the CDWRITE command and the input file has an extension cdb.
CDWRITE Command Form (CDWRITE, Option, Fname, Ext, -- , Fnamei, Exti, Fmat )
Option: Selects the data to write (ALL, COMB, DB, SOLID….).
Fname: File name and directory path. An unspecified directory path defaults to the working directory.
Ext: File name extension. If Fname is blank, the extension defaults to ‘*. cdb'.
--: Unused field
Fnamei: The name of IGES file which contains parts or assemblies is supported by the mechanical application and its directory path.
Exti: File name extension. The extension defaults to IGES.
Fmat: Format of the output file (It defaults to BLOCKED)
BLOCKED: The Output is read faster more in this format.
UNBLOCKED
Caution
RecurDyn/FFlex recommends the user does not use additional command parameters.
When you use the CDWRITE command with additional command parameters, Fmat of additional command parameters must be BLOCKED to import the *.cdb file.
For more information about the CDWRITE command, refer to the ANSYS manual.
Supported Nastran Command
Nastran input file (*.dat / *.bdf) can be imported to RecurDyn. However, RecurDyn does not support parts of all command. Table 9.2 shows supported commands.
Type |
Commands |
|
---|---|---|
Node |
GRID |
|
Element |
BEAM |
CBEAM |
SHELL |
CTRIA3 CTRIA6 CQUAD4 CQUAD8 |
|
SOLID |
CTETRA CPENTA CHEXA CPYRAM |
|
MASS |
CONM2 |
|
RIGID |
RBE2, RBE3 |
|
Property |
PBEAM PBEAML PSHELL PSOLID |
|
Material |
MAT1 MAT2 MAT8 |
|
Coordinate |
CORD1C CORD1R CORD1S CORD2C CORD2R CORD2S |
|
B.C. |
SPC SPC1 |
|
Set |
SET |
Note
If the SET is used, Grid ID and Element ID must have unique ID.
RecurDyn does not support stress output option field and related fields.
RecurDyn only supports interpolation element type of ‘Rotation & Translation’. So, REFC field of RBE3 is converted to ‘123456’. User cannot control this value in GUI.
RecurDyn only supports ‘1’ as weighting factor. So, WTi field of RBE3 is converted to ‘1’. User cannot control this value in GUI.
RecurDyn only supports translation degree of freedom in the case of independent nodes. So, Ci field of RBE3 is converted to ‘123’. User cannot control this value in GUI.
Supported Elements
Some kinds of structural elements are imported. Refer to Table 9.3.
Type |
RecurDyn/FFlex |
NASTRAN |
ANSYS |
---|---|---|---|
1D Element |
Beam 2 |
CBEAM |
Beam 4 Beam 188 |
2D Element |
Shell 3 |
CTRIA 3 CTRIA 6 |
Shell 63 Shell 93 Shell 181 |
Shell 4 |
QUAD 4 |
Shell 63 Shell 181 |
|
Shell 9 |
QUAD 8 |
Shell 93 |
|
3D Element |
Solid 4 |
CTETRA |
Solid45 Solid185 |
Solid 5 |
CPYRAM |
Solid95 Solid185 Solid186 |
|
Solid 6 |
CPENTA |
Solid45 Solid95 Solid185 Solid186 |
|
Solid 8 |
CHEXA |
Solid 45 Solid 185 |
|
Solid 10 |
CTETRA |
Solid 92 Solid95 Solid186 Solid187 |
|
Solid 26 |
CHEXA |
Solid 95 Solid 186 |
|
Rigid Element |
Rigid Element |
RBE2, RBE3 |
Rigid Region |
Mass Element |
Mass Element |
CONM2 |
Mass 21 |
Supported Materials and Properties
Type |
RecurDyn/FFlex |
NASTRAN |
ANSYS |
---|---|---|---|
1D Element |
PBEAM |
PBEAM PBEAML |
Real Constant SECTYPE, SECDATA |
2D Element |
PSHELL |
PSHELL |
Real Constant SECTYPE, SECDATA |
3D Element |
PSOLID |
PSOLID |
NONE |
Material |
Isotropic Orthotropic2D Anistropic2D Plastic |
MAT1 MAT2 MAT8 |
Material |
Supported Boundary/Set Type
Type |
RecurDyn /FFlex |
NASTRAN |
ANSYS |
---|---|---|---|
Boundary |
BC |
SPC |
Displacement Constraint |
SPC1 |
|||
Set |
SET |
SET |
Component |
Caution
In the 2D element, the parabolic triangular type that has 6 nodes are converted to linear element
In the 3D element, the parabolic pentagonal type that has 6 nodes are converted to a linear element.
In ANSYS, the constraint equation is converted to a rigid element where the base node is treated as a primary node.
The Pyramid type elements are divided into two tetrahedral elements.
During the SET data converting, corresponding patch sets that include some or partial entities are automatically generated.