Material Properties

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:



Material Type Solids Shells
Isotropic Material
Orthotropic Material 3D  

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.

  1. Open a part in the Part Design workbench or a product in the Assembly Design workbench.

  2. To assign a material to a part, do the following:

    1. Select the PartBody feature in the specification tree.

    2. Click the Apply Material icon .

      The Library dialog box opens. The default .CATMaterial document is used.

    3. 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.

  3. To apply a render style to a part that reflects the material assignment, select View>Render Style>Customize View 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.

  1. Right-click on the material object in the specification tree, and select Material object>Definition 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.

  2. 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.

  3. 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.

  4. 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.

  5. 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.

  6. To add or delete table rows, click Add or Delete below the data table.

  7. To import material data from a file, click the Folder icon , and select a text file.

  8. 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.

  9. Click OK in the Properties dialog box to update the material properties.