Once a file is opened in FE Modeler, the first step to create an Initial Geometry is to identify the exterior faces. Exterior faces are defined by the components that contain the surfaces of the elements for brick or tetrahedron meshes, and the elements themselves for a shell mesh. This can be accomplished by creating face components (see Creating Components and Assemblies) or by using the automated Skin Detection Tool. In addition, you can define surfaces from a selection of element faces.
The Skin Detection Tool (SDT) groups exterior element faces into SDT Components. The number of faces generated is based on the Tolerance Angle value contained in the Skin Detection Tool Details.
To create, clear, or add groups of SDT Components:
Create: To create SDT components, select the Skin Detection Tool object in the Outline and click the button.
: To clear SDT components, select the Skin Detection Tool object in the Outline and click the button.
: To add STD components to the Components list, expand Skin Detection Tool, select any component(s) in the Outline, and click the button. (for more on adding SDT components, see Using Iterative Skin Detection.
Note: You can also use a right mouse click on the Skin Detection Tool or a component and select one of the options above to perform one of these actions.
Once created, these skin components are listed under the Skin Detection Tool object, as illustrated below, and each component forms a face during Initial Geometry creation.
Newly Created SDT Components ![]() |
Following SDT Component creation, you need to consider the Details associated with the new SDT Components, specifically the number of the faces that are created (based on the tolerance angle). If this number is too high, you may want to clear the components, modify the Tolerance Angle, and create new components.
It is also important to note that you can simply generate an Initial Geometry without first creating SDT Components: they are automatically created during that process. However, doing so does not allow you to examine and/or modify the Details associated with the newly created faces.
Any face components defined in FE Modeler are also considered when defining an exterior face. For example, you may need to apply a pressure load over a small area of a larger surface. You can create a face component that includes the element faces over which the pressure is applied as detailed in the Creating Components and Assemblies section. The geometry creation algorithm then creates a face from this component. Shell elements and faces of solid elements that are defined by the nodes of the face component will be removed from the SDT skin when it is generated. If you remove a face component from the Components item in the tree, the shell elements and faces of solid elements that are defined by the face component will be added to the SDT skin when it is generated.
The user will be able to retrieve the areas on the geometry where node components exist in the input mesh. These node components will be internally converted into shell element components or facets of solid element components to be used in the generation of the geometry. Some additional edges and vertices will be added to the geometry if applicable.
To use node components in the geometry generation, change the Use
Node Components option in the Details View of Geometry Synthesis
to Yes and generate the geometry. You can also see
the preview results as usual by creating the SDT components.
If Use Node Components is set, you will see the following behavior:
If you add a Node Component to the Components item in the tree, the shell elements and faces of solid elements that are defined by the nodes of the node component will be removed from the SDT skin when it is generated.
If you remove a Component from the Components item in the tree, the shell elements and faces of solid elements that are defined by the nodes of the node component will be added to the SDT skin when it is generated.
Note: If you change Use Node Components to yes after having created the initial geometry, the initial geometry will be invalidated.
The Initial Geometry feature supports 2D shells and 3D solids. All other element types, if present, are ignored during geometry creation.
An example of the SDT Details View content, for the Algorithm Detection by angle, is illustrated below.

Once generated, the Details View for the Skin Detection Tool provides the categorized information as described in the tables shown below. The options of the Algorithm Parameters Category change based upon the selected Algorithm.
Definition Category
| Option/Field | Description | ||
| Execution Type | Automatic: Skin detection is automatically performed using the specified (or default) Tolerance Angle when initial geometry is created. Manual: You manually perform skin detection or define face components. | ||
| Algorithm | |||
| Number of Skin Components | Displays the current number of SDT Components. | ||
Algorithm Parameters Category
If Algorithm is | |
| Option/Field | Description |
| Tolerance Angle | The SDT process computes the angle between the normals of two adjacent elements in the mesh. If this angle is less than or equal to the Tolerance Angle then the two elements are in the same component, otherwise, they are separated. The default Tolerance Angle is . |
| Forbid Close Components | If activated, this special algorithm cuts the closed surfaces into several components. It provides a simple method to avoid problematic faces on closed surfaces. |
| Cut Angle | Only displayed if Forbid Close Components equals . It is the angle used in the above algorithm to separate the elements into components. |
If Algorithm is | |
| Option/Field | Description |
| Sharp Edges Angle | During the SDT process, if the angle between the normals of two adjacent elements is more than or equal to the Sharp Edges Angle, then the edge shared by the two elements is used to compute the component's boundary. |
| Ignore the Secondary Nodes | Select Yes if you wish to drop the secondary nodes. |
| Planes Tolerance Angle | This option allows the user to detect the planes in the mesh. If the angle between the normals of two adjacent elements is less than or equal to the Planes Tolerance Angle then the two elements are in the same component. |
Treeview Display Category
| Option/Field | Description |
| Display all SDT Components' treenodes | If , all SDT component treenodes are displayed in the Outline. |
| Number of SDT Components' treenodes displayed | The maximum number of SDT components treenodes displayed in the Outline. This field can be edited only if the Display all SDT Components' treenodes field's value equals No. |