Creating or Editing Finite Element Models

You must create a finite element model for use with most simulations.

In a product containing 3D shapes and FEM representations, you must create or activate one particular FEM to work in this representation and to access the commands in the model creation apps.

This task shows you how to:

Create New Finite Element Model Representations

  1. There are two ways to open the Finite Element Model dialog box:
    • From the Simulation Initialization dialog box, click .

    • From the Setup section of the action bar in a scenario creation app, click Finite Element Model .

    The Finite Element Model dialog box appears.
  2. Choose which geometries will be initialized as supports of the mesh:
    OptionDescription
    Main bodies Initializes the main bodies only (the PartBody). If the PartBody is empty, the app initializes another solid body. If all solid bodies are empty, the app initializes any ordered geometric set until there is a single 3D result.
    All geometries Initializes all geometries of the part or assembly.
    Selected geometries Enables you to select which geometries of the part or assembly to initialize for meshing.

    If you choose Selected geometries, you can view a list of imported geometries eligible for initialization by clicking Show advanced tree selection. When you click this option, the Body selection dialog box opens, from which you can filter and select your geometries.

    Note: In the case of ordered geometric sets, the app initializes all 2D and 3D geometries as supports. For more information, see Structural Model Creation: Ordered Geometric Sets.

  3. Choose an initialization method for the finite element model:
    OptionDescription
    None Creates a finite element model representation without creating a mesh. Instead, you define the mesh parameters during the creation process. This approach ensures that the created mesh is suitable for your simulation.
    Automatic Creates an initial mesh automatically according to the default mesh settings. For 2D geometries, the app creates a surface quad mesh. For 3D geometries, the app creates a tetrahedron mesh.
    Manual Creates an initial mesh based on your specifications for mesh type, element order, size, and sag ratio.
    Rule-based Creates an initial mesh based on a set of parameters in a meshing rules document that you select.

    For more information about meshing rules, see Creating and Modifying Meshing Rules.

    Procedure-based Creates an initial mesh based on a set of initialization instructions in a Visual Basic script. When you choose procedure-based initialization, you must also define the inputs for the initialization script using a meshing rules document. For more information about procedures, see About User Procedures in the Model Assembly Design Guide. The status icon next to Define inputs changes from red to green once you define all the required inputs for the procedure.
  4. If you selected the Manual initialization method, you must specify the following parameters:
    1. Select the Mesh type.
    2. Select the Element order: linear or quadratic.
    3. Specify the element Size.

      The mesher might vary the element size to improve quality, conformance to geometry, or other parameters.

    4. If you selected Sweep 3D Mesh for solid geometries, specify the Number of layers.
    5. If you selected any other mesh type, specify the Sag ratio.

      The sag ratio controls the degree of conformance between the mesh and curved geometry. It is the ratio of the maximum distance between an element edge and the geometry to the length of the element edge.

    6. If your model includes surface geometries without a defined thickness, specify the Thickness of the shell section.
    7. Select Create knowledge parameters to create Knowledgeware parameters.
  5. Optional: To choose new mesh quality criteria, activate the Select specific quality criteria option and open a saved quality criteria file.

    By default, the criteria specified in the Simulation > Quality options (Me > Preferences) are used.

  6. Click OK.
    The Finite element model / Representation dialog box appears. The dialog box contains only the Finite element model tab because the product is already created.
  7. Optional: Enter a descriptive Name.

The contents of the finite element model representation depend on the product type and the initialization mode. FEM representations for all 1D or 2D geometries, and for 3D geometries with the None initialization mode, contain the Nodes and Elements and Properties containers.

FEM representations for 3D geometries with Automatic or Manual initialization modes populate the containers as follows:

  • If the product contains one 3D shape, the finite element model representation is linked to the 3D shape and a default mesh and default 3D property are created.
  • If the product is an assembly, meshes and 3D properties are created for each PartBody.
All the meshes are created with the same mesh size (ratio of the global bounding sphere), the same sag (ratio of the mesh size), and the same element type (linear) using knowledge parameters and relations.

Edit Existing Finite Element Model Representations

Double-click an element of the FEM representation in the tree to activate a FEM representation.

Tip: The app indicates a product or representation is active by highlighting the feature in the tree in blue.