Material properties are a key component of any
analysis. Material properties determine how a model
reacts to the structural or thermal loads applied in each
analysis step.
Once you create a model, you must assign a material in
the CATIA Part Design or Assembly Design workbench. After
you assign a material, you can edit the properties to
include characteristics specific to the current analysis
case. Basic isotropic structural and thermal material
properties include density and the coefficient of thermal
expansion; you can also specify nonlinear material
properties and complex linear properties. Finally, you
can create CATIA V5 user materials with non-isotropic
material properties to vary material behavior within
composite shells.
Nonlinear Structural Analysis and Thermal Analysis
support the following material types:
You can apply orthotropic three-dimensional behavior
along the default axes or you can apply this behavior
along any user-defined coordinate system by specifying an
orientation in the 3D Property dialog box.
The following tasks are discussed in this section:
Assigning Material
Properties
You must assign a material to a part before you can
analyze it. You can assign materials in the CATIA Part
Design or Assembly Design workbench. If you enter the
Nonlinear Structural Analysis or Thermal Analysis
workbench from a .CATPart or
.CATProduct document
containing a part without a material assignment, a
dialog box appears warning you that the material
definition is missing. You must return to the Part
Design or Assembly Design workbench to apply a
material.
Assigning Material
Properties: Assigns material properties
to parts in a .CATPart or
.CATProduct document in the
Part Design or Assembly Design workbench.
This task shows you how to assign a material
to a part and apply material rendering to the
current view.
-
Open a part in the Part Design workbench or a
product in the Assembly Design workbench.
-
To assign a material to a part, do the
following:
-
Select the PartBody feature in the
specification tree.
-
Click the Apply Material icon
.
The Library dialog box
opens. The default .CATMaterial document is
used.
-
Select a material family from the tabs
along the top of the dialog box, then
choose a material from the displayed
images, and click OK.
The material is applied to the part, and
a material object appears under the
PartBody objects set in the specification
tree.
-
To apply a render style to a part that
reflects the material assignment, select
>> from the menu bar, and toggle
on Materials in the
Custom
View Modes dialog box that
appears.

Specifying Material
Properties
You can customize the material assigned to your
model by defining additional material properties. These
properties range from linear elasticity to user-defined
properties that provide you with full control over the
equations used to define the material. You can select
multiple options to define the material properties. Any
properties that are not needed for the current analysis
case are ignored. Nonlinear and thermal material
properties are located in the Properties
dialog box along with other general material properties
used by CATIA V5.
The following nonlinear and thermal material
properties are available in Nonlinear Structural
Analysis and Thermal Analysis:
Elasticity
Specify linear elasticity by entering a Young's
modulus and Poisson's ratio. Linear elasticity is
intended for use with small elastic strains
(normally less than 5%).
Plasticity
Specify plasticity by entering corresponding
stress and strain values. You can choose isotropic
or kinematic hardening. You must provide tabular
data of stresses, strains, and temperatures to
define isotropic or kinematic hardening.
Hyperelasticity
You can define hyperelasticity for isotropic,
nonlinear materials that exhibit an instantaneous
elastic response to large strains. To use
hyperelastic materials in an analysis, you must
include geometric nonlinearity in the analysis
steps. Analysis steps automatically include
geometric nonlinearity when the model uses
hyperelastic materials.
Hyperelasticity is defined by selecting one of
the following strain energy potentials:
-
Arruda-Boyce
-
Mooney-Rivlin
-
Neo Hooke
-
Ogden
-
Polynomial
-
Reduced Polynomial
-
Van der Waals
-
Yeoh
After selecting a strain energy potential, you
enter the coefficient data that the solver uses to
calculate the material response.
Density
Specify the density for use with gravity loads
or when conducting a heat transfer analysis.
Thermal Conductivity
Specify the thermal conductivity for use in a
heat transfer analysis.
Specific Heat
Specify the specific heat for use in a heat
transfer analysis.
Coefficient of Thermal Expansion
Specify the coefficient of thermal expansion if
you intend to run a thermal analysis and use the
results as the basis for a subsequent structural
analysis.
Some material properties can be defined in both
the CATIA V5 and Nonlinear and Thermal material
property definitions. If you specify a property in both
places, the nonlinear and thermal property always
overrides the corresponding CATIA V5 material
property. For example, if you enter density in the
Nonlinear and
Thermal tabbed page, the density in the
Analysis tabbed page
(CATIA V5 properties) will be ignored when you
run the analysis.
This task shows you how to specify Nonlinear
and Thermal material properties.
-
Right-click on the material object in the
specification tree, and select >
from the menu that appears.
The Properties dialog box
appears.
Note: An interim
dialog box will appear the first time that the
material properties are loaded in a Nonlinear
Structural Analysis or Thermal Analysis
session.
-
Use the arrows near the top of the
Properties dialog box to
scroll and reveal additional tabs; click the
Nonlinear and Thermal tab
when it appears.
A warning dialog box will appear the first
time that Nonlinear and Thermal properties are
loaded in a session. Click OK to
dismiss the warning.
-
In the list of Available Options, toggle
on the material options that you would like to
modify or specify.
The options will appear in the list of
Selected Options.
-
From the list of Selected
Options, select the material option
that you would like to modify or specify.
If it is applicable, the data table for that
material option will appear in the dialog box
below the Selected Options list.
-
Enter the required values for the material
option in the data table cells. For example, to
specify the material's plastic properties, enter
values for the stress and strain.
-
To add or delete table rows, click
Add or Delete
below the data table.
-
To import material data from a file, click the
Folder icon
,
and select a text file.
-
To specify temperature-dependent data for a
material option, toggle on Use
temperature-dependent data.
A Temperature column will
appear in the data table in which you can enter
the temperature values.
-
Click OK in the Properties dialog box to
update the material properties.