ABAQUS version 6.14 is supported.
After installing ABAQUS, you must configure the
ANSYS_INSTALL_DIR
\v242\aisol\WBAddins\AbaqusAddin\config.xml
file in order to postprocess results. Edit the config.xml file
with a text editor, and specify the version of ABAQUS you have installed:
<AbaqusVersion version="6.14-3">
If more than one version of ABAQUS is installed on your machine, the paths to the version configured for use with Workbench must appear first in your PATH environment variable.
Assuming ABAQUS is installed at C:\SIMULIA\Abaqus, for ABAQUS 6.14-3, the PATH environment variable must contain:
C:\SIMULIA\Abaqus\Commands
C:\SIMULIA\Abaqus\6.14-3\code\bin
C:\SIMULIA\Abaqus\6.14-3\tools\SMApy\python2.7\Lib
If the ABAQUS version installed does not match the version specified in the config.xml file, Mechanical returns an error when trying to postprocess the ODB result file.
The exact results stored by the ABAQUS solver can be controlled using an XML
configuration file. This file uses ABAQUS Program Controlled codes to define
which results to write to the results file. Results are classified by result
type and category. The configuration file is located at
ANSYS_INSTALL_DIR
\v242\aisol\WBAddins\AbaqusAddin\AbaqusArchiveSettings.xml.
The configuration file is read when Mechanical is launched. If changes are made to the file while Mechanical is running, Mechanical must be restarted to reflect the changes.
The XML root element in this file is <AbaqusArchiveSettings
version="1">
. The child nodes of this root element represent
analysis types. The only valid child node is
<Analysis>
, and this child node has the
following attribute:
name
(type string)The analysis type:
struct
eigen
thermal
The <Analysis>
node can have a child node of
<Output>
, which has the following
attribute:
type
(type string)The option type, used to order codes in the solver input file:
nodal
elemental
contact
energy
radiation
The <Output>
node has child nodes of
<Codes>
which have the following
attributes:
value
(type string)List of ABAQUS codes separated by spaces. Usually a list of integers, positive or negative.
position
(type string)For elemental results, if a result exists with a matching position, it is used. Otherwise results without position are used.
category
(type string)Optional, used for options enable or disabled by the user.
stress
strain
thermal
contact
When a solve is executed and the solver input file is created, Mechanical finds
the correct <Analysis>
node in the configuration
file to determine the SAI codes to write to the input file. This check is
performed by finding the analysis type and whether the analysis is linear or
nonlinear. The following table describes the mapping:
Workbench Analysis Type | <Analysis> Node Used |
---|---|
Static Structural (ABAQUS) | struct |
Transient Structural (ABAQUS) | struct |
Modal (ABAQUS) | eigen |
Steady-State Thermal (ABAQUS) | thermal |
Transient Thermal (ABAQUS) | thermal |
In order to postprocess all results from the ABAQUS solver in the Workbench
interface, an XML file is used to map the results between ABAQUS and Workbench.
The XML file defines all of the Workbench result codes with associated data, and
lists the corresponding Samcef codes. The configuration file is located at
ANSYS_INSTALL_DIR
\v242\aisol\WBAddins\AbaqusAddin\VkiAbaqusResultCodes.xml.
The configuration file is read when Mechanical starts postprocessing ABAQUS data. If changes are made to the file while Mechanical is running, Mechanical must be restarted to reflect the changes.
The following is an example result as expressed in the XML configuration:
<Result result_name="U" result_id="101" data_type="nodal" out_unit="length" style="vector" num_comp="5" comp_labels="XYZLABELS" description="Deformations(XYZs)"> <Solver name="Abaqus"> <Code name="U" /> </Solver> <vki vki_root_name="D" /> </Result>
The listing provides the following information:
The Workbench code "U" identified by Mechanical by the ID 101 is a nodal result and is interpreted as a length.
The result is represented in the vector style, has 5 components and is part of the XYZLABELS group.
The result corresponds to vki result "D", which comes from ABAQUS code "U".
The XML Result
object can have the following
attributes:
result_name
(type string)The Workbench name of the result. Standard Mechanical names are reserved.
result_id
(type integer)The Workbench ID of the result. Standard Mechanical IDs are reserved; you should start numbering solver-specific results at 100000. You should not choose a number larger than 1000000 because those numbers are internally reserved.
data_type
(type string enumerate)The result type:
nodal
elem_nodal
elemental
out_unit
(type string enumerate)The unit type of the result:
no_units
acceleration
angle
angular_velocity
area
capacitance
charge
charge_density
conductivity
current
current_density
density
displacement
electric_conductivity
electric_field
electric_flux_density
electric_resistivity
energy
film_coeff
force
force_intensity
frequency
heat_flux
heat_generation
heat_rate
inductance
inverse_stress
length
magnetic_field_intensity
magnetic_flux
magnetic_flux_density
mass
moment
moment_inertia
permeability
permittivity
poisson
power
pressure
relative_permeability
relative_permittivity
section_modulus
specific_heat
specific_weight
shear_strain
stiffness
strain
stress
strength
thermal_expansion
temperature
time
velocity
voltage
volume
gasket_stiffness
moment_inertia_mass
psd_acceleration
psd_acceleration_grav
psd_displacement
psd_velocity
rotational_damping
rotational_stiffness
translational_damping
angular_acceleration
seedbeck_coefficient
decay_constant
fracture_energy
shock_velocity
energy_density_mass
electric_conductance_per_unit_area
psd_stress
psd_strain
psd_force
psd_moment
psd_pressure
force_per_angular_unit
impulse
impulse_per_angular_unit
temperature_difference
material_impedance
rs_acceleration
rs_acceleration_grav
rs_displacement
rs_velocity
warping_factor
thermal_conductance
inverse_length
inverse_angle
thermal_capacitance
normalized_value
mass_flow_rate
unitless
stress_intensity_factor
sqrt_length
energy_per_volume
thermal_gradient
style
(type string enumerate)The style of the value:
scalar
vector
tensor
tensor_strain
euler_angles
coordinate
shear_moment_diagram
num_comp
(type integer)Number of components, between 1 and the length of
comp_labels
.comp_labels
(type string enumerate)The component labels:
XYZLABELS
STRESSLABELS
CONTACTLABELS
BEAMLABELS
GASKETLABELS
NLLABELS
MISCLABELS
SENGLABELS
SPRINGLABELS
BEAM188LABELS
RADIOSITYLABELS
EULERLABELS
BEAMRXLABELS
THERMALMASSLABELS
SHELLMBPLABELS
SLASHPNUMLABELS
CINTLABELS
PRIN_S_LABELS
PDMG_LABELS
PFC_LABELS
CDM_LABELS
CONTDEBONDLABELS
BEARINGLABELS
BLANKLABELS
is_membrane
(type boolean)If this attribute is present and marked true, the result is only added if the model has a membrane.
is_six_dof
(type boolean)Optional, applies for only "R" and "M" type Mechanical results.
description
(type string)Free text.
The <Solver>
node references the solver used by
the attribute name
. All child
<Code>
nodes are the codes associated to the
Workbench result for this solver. A code is an alphanumerical string referred by
attribute name
. It is possible to define several codes
for the same solver.
The <vki>
node is another way to match the solver
result. This node has the following attributes:
vki_root_name
(type string)The vki root name as described in the documentation/API.
vki_aux_name
(type string)Only required if
vki_root_name
is set to UNKNOWN. Matches the vki result in case of unknown vki type.
Note: If solver-specific data and vki data are fulfilled for a specific result, Mechanical will first try to match the vki code. If it is not found, it will try to match the solver-specific code. For example, when reading a result file, the vki dataset E_ELAST is found, with solver-specific data EE. Mechanical looks for a Workbench result having vki root name E_ELAST. If not found, it looks for a Workbench result having Abaqus code EE.
Limitations
If the XML of the configuration file is missing or not well-formed, no results are available.
If a result has invalid syntax (missing XML components, invalid attributes), it is not available.
Mechanical must be restarted if any changes are made to the result configuration file during operation.
The following results don't appear in the XML file, as they have behavior which is not compatible:
SERR - not associated to VKI or ABAQUS, is available if S and SVOLU are also available.
NDIR, EDIR - not associated to VKI or ABAQUS, is available if the model contains shells.