The Abaqus Configuration File

The Abaqus component configuration file allows you to determine which parameters will be extracted from the ASCII Abaqus input (.inp) file and data (.dat) file when using the Abaqus component. Specifically, it controls parsing of the Abaqus input file and the Abaqus data file.

Using the configuration file, you can define which Abaqus keywords the Abaqus component will support. You can also define the numerical values associated with each keyword that will be parameterized. The file provides the ability to customize the parameter naming patterns. On the output side, it controls the extraction of results tables from the data (.dat) file. Abaqus component parsing of the output database (.odb) file is controlled separately and not by this configuration file.

By default, the Abaqus component configuration file is located in the following directory:

<Isight_install_directory>\<operating_system>\reffiles\SMAFIPconfig

Important: The Abaqus component configuration file requires an exact keyword match between input file and configuration file. For example, *Elastic does not equal *Elas. Therefore, it is important to use full keyword names in the Abaqus input file or to declare both full and partial names in the configuration file.

To define an Abaqus keyword to be parsed, the keyword is added to the configuration file followed by one or more lines that name the parameters to be extracted. For example, consider the following Abaqus input file lines that define the shell thickness and ply angles for a composite laminate:

*SHELL SECTION, ELSET=P1, ORIENTATION=O1, COMPOSITE
0.25, , M1, 0.
0.25, , M1, 45.
0.25, , M1, -45.
0.25, , M1, 90.
0.15, , M1, 90.
0.15, , M1, -45.
0.15, , M1, 45.
0.15, , M1, 0.

The following lines in the configuration file declare that composite shell sections should be supported and that Thickness and Orientation parameters should be created from each of the data lines associated with the keyword:

# Specify a shell cross section
*SHELL SECTION, COMPOSITE
Thickness, , , Orientation

The configuration file supports control over parameter names by tagging a field with a << … > >  identifier. For example, consider the following Abaqus input file lines that define a fluid pressure initial condition:

*INITIAL CONDITIONS, TYPE=FLUID PRESSURE
30001, 6.

The following lines in the configuration file declare that this keyword should be supported and that NodeId should be included in the parameter name for all parameters on that line (in this case FluidPressure):

# Specify initial conditions for the model
*INITIAL CONDITIONS, TYPE=FLUID PRESSURE
<<NodeId>>, FluidPressure

The configuration file supports keyword blocks through the ::BLOCK identifier on the keyword definition line. This identifier is used to associate one keyword with another keyword for parameter naming purposes. For example, consider the following material properties.

*MATERIAL, NAME=RUBBER
*DENSITY
1.E-4, 
*HYPERELASTIC, N=1
100., 25., 1.E-4

The following lines in the configuration file declare density and hyperelastic material properties as supported keywords and associate them both with the *MATERIAL keyword. The material name (RUBBER) is then prepended to the density and hyperelastic material property names.

# Specify material mass density
*DENSITY ::BLOCK=*MATERIAL
MassDensity, Temp

# Specify elastic properties for approximately incompressible 
elastomers
*HYPERELASTIC ::BLOCK=*MATERIAL
mu1, alpha1, D1

To parse output tables from the data (.dat) file, tables must be defined in the configuration file after the OUTPUT EXTRACTIONS line. For example, consider the following output table:

NODE FOOT-   RF1         RF2         RF3
NOTE
3241       872.9       765.2      -936.5     
3243     -1.0792E+04  -139.6      -2692.     
3245       2544.       29.24      -636.7     
3247      -3471.       248.1      -879.4     
3249     -0.1244      -366.6      9.4686E-02 
3251       3473.       247.2       879.7

The following lines in the configuration file will instruct the Abaqus component to create output parameters for each of the values in this table:

HEADER: NODE
NODE FOOT-   RF1         RF2         RF3     
NOTE
NAMING: <<ID>>,,RF1,RF2,RF3
FORMAT: i,s4,r,r,r

The HEADER line denotes the primary parameter name, the NAMING line provides specific name identifiers for each number being extracted, the FORMAT line declares each element of the table as a real (r), integer (i), or string (s).

If minimum and maximum values are provided with a table, they can also be extracted by using the MINIMUM and MAXIMUM lines. To extract just the minimum and maximum values from a given output table, the MINMAXTOTALSONLY line is used. For example, the following table definition creates only minimum and maximum nodal displacements from this table type:

HEADER: NODE
NODE FOOT-   U1          U2          U3       
NOTE
NAMING: <<ID>>,,U1,U2,U3
MINMAXTOTALSONLY
MAXIMUM: ,,U1,U2,U3
MINIMUM: ,,U1,U2,U3
FORMAT: i12,s4,r,r,r

You may experience performance issues if you are working with a very large Abaqus input file. For information about using large files with Isight, search the Dassault Systèmes DSX.ClientCare Knowledge Base at http://www.3ds.com/support/knowledge-base.