Creating Surface Force Densities

This task shows you how to create a Surface Force Density applied to a surface geometry.

Surface Force Densities are intensive loads representing surface traction fields of uniform magnitude applied to surface geometries.
Surface Force Density objects belong to Loads objects sets.

The user specifies three components for the direction of the field, along with a magnitude information. Upon modification of any of these four values, the surface traction vector components and magnitude are updated based on the last data entry. The surface traction vector remains constant independently of the geometry selection. 

Units are surface traction units (typically N/m² in SI).

Surface Force Density can be applied to the following types of supports:

To know more, refer to Authorized Supports.

Open the sample00.CATAnalysis document from the samples directory.

• Go to View > Render Style > Customize View and make sure the Shading, Outlines and Materials options are active in the Custom View Modes dialog box.

1. Click Surface Force Density in the Loads toolbar.

   The Surface Force Density dialog box appears.

2. You can change the identifier of the Surface Force Density by editing the Name field.

3. Set the Axis system. 

   The Axis System Type combo box allows you to choose between Global, Implicit and User Axis systems for entering components of the traction field vector: Global: if you select the Global Axis system, the components of the surface traction field will be interpreted as relative to the fixed global coordinate system.    Implicit: if you select the Implicit Axis system, the components of the surface traction field will be interpreted as relative to a local variable coordinate system whose type depends on the support geometry.  User:  if you select a User Axis system, the components of the surface traction field will be relative to the specified Axis system. Their interpretation will further depend on your Axis Type choice. To select a User Axis system, you must activate an existing Axis by clicking it in the specification tree. Its name will then be automatically displayed in the Current Axis field. If you choose the User axis system, the Local orientation combo box further allows you to choose between Cartesian, Cylindrical and Spherical local axis orientations.  Cartesian: the components of the surface traction field are interpreted as relative to a fixed rectangular coordinate system aligned with the cartesian coordinate directions of the User-defined Axis. Cylindrical: the components of the surface traction field are interpreted as relative to a local variable rectangular coordinate system aligned with the cylindrical coordinate directions of each point relative to the User-defined Axis. Spherical: the components of the surface traction field are interpreted as relative to a a local variable rectangular coordinate system aligned with the spherical coordinate directions of each point relative to the User-defined Axis.

   You can define the surface traction direction by using the compass.  You can modify the compass orientation either with the mouse or by editing the compass.   By applying the compass to any part geometry, you can align the compass directions with the implicit axis directions of that geometry: drag the compass by handling the red square and drop it on the appropriate surface. The normal direction to this surface defines the new direction. Then, click on the Compass Direction button to take this new direction into account. You can now invert the direction if desired, editing the values of the three components. Even if a User axis system has been referenced, the coordinates of the data mapping stay in the Global axis system. Only the User axis system directions are taken into account with data mapping.

4. Select the geometry support (a face) on which the surface traction is to be applied.

   Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports in sequence, to apply the Surface Force Density to all supports simultaneously. Symbols representing the Surface Force Density are displayed on the support geometry to visualize the traction field. As soon as the support is selected, the Select Mesh Part button is available. To know more about the Select Mesh Part button, refer to Selecting Mesh Parts.

5. Enter a new value for any one of the four fields.

   For example, enter values for the X, Y, Z components of the surface traction field as shown below The corresponding Norm value is automatically computed and displayed. The remaining three fields are automatically computed and displayed. The visualized symbols orientation is also updated to reflect the modification.
   	You can re-use data (Data Mapping) that are external from this version (experimental data or data coming from in-house codes or procedures). For more details, refer to Data Mapping (only available with the ELFINI Structural Analysis product).

6. Click OK in the Surface Force Density dialog box.

   A Surface Force Density object appears in the features tree under the active Loads objects set.

• You can either select the surface and then set the Surface Force Density specifications, or set the Surface Force Density specifications and then select the surface. 
• If you select other surfaces, you can create as many Surface Force Density loads as desired with the same dialog box. A series of Surface Force Densities can therefore be created quickly.
• Loads are required for Stress Analysis computations. 
• If several Analysis Cases have been defined in the Finite Element Model, you must activate a Loads objects set in the features tree before creating a Surface Force Density object (only available if you installed the ELFINI Structural Analysis product).
• Surface Force Density objects can be edited by a double click on the corresponding object or icon in the specification tree.

The ELFINI Structural Analysis product offers the following additional functionalities:

• Contextual menu on the load object:
  • Distributed Force Visualization on Mesh: the translation of your Distributed Force object specifications into solver specifications can be visualized symbolically at the impacted mesh nodes, provided the mesh has been previously generated using a mesh only computation.
    To know more, refer to Visualizing Loads on Mesh.
• Contextual menus on the loads set:
  • Generate Image: generates an image of the computed load objects (along with translating all user-defined Loads specs into explicit solver commands on mesh entities), by generating symbols for the elementary loads imposed by the Loads objects set. The image can be edited to include part or all of the options available.
    To know more, refer to Generating Images.
  • Report: the partial status and results of intermediate pre-processor computations are reported in HTML format. It represents a subset of the global report capability and generates a partial report of the loads objects set Computation.
    To know more, refer to Generating Reports.
• Self-balancing: refer to Creating Pressures.