Loads

The following types of loading are available in the Nonlinear Structural Analysis workbench:

Creating Pressure Loads: Applies a pressure load to a geometry selection.

Creating Point Loads: Applies a point load to a geometry selection.

Creating Distributed Loads: Applies a distributed load to a geometry selection.

Creating Load Densities: Applies a load density to a geometry selection.

Creating Gravity Loads: Applies a gravity load to a geometry selection.

Creating Rotational Body Force Loads: Applies a rotational body force load to a geometry selection.

Importing Loads: Imports a load definition from GPS into an analysis.

You apply environmental actions, such as loads, to supports (geometrical features) on your model. The supports that are available include points/vertices, curves/edges, surfaces/faces, or volumes/parts. In addition, point, line, or surface groups are also valid supports. You can either select the support and then set the load specifications or set the load specifications and then select the support. Table 9–2 summarizes the supports to which each type of load can be applied.

Table 9–2 Supports for loads.

Load	Point, Vertex, or Point Group	Curve, Edge, or Line Group	Surface, Face, or Surface Group	Volume or Part	Other Supports
Pressure					GPS Pressure
Point					Rigid Body Constraint, GPS Virtual Part, and rigid or smooth couplings
Distributed
Load Density
Gravity					Mesh Parts
Rotational Body Force					Mesh Parts

Creating Pressure Loads

Pressure loads represent uniform scalar pressure fields applied to surface geometries. The force direction for a pressure load is always normal to the surface and remains normal even as the surface rotates, provided that geometric nonlinearity is considered in the step.

Pressure loads can be applied only in mechanical steps.

The magnitude of a pressure load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes).

You can prescribe the time variation of the magnitude of a pressure load in a user subroutine, which is sometimes preferable when the time history of the magnitude is complex. You can also apply knowledgeware techniques to control the value of a pressure load (for more information, see Applying Knowledgeware).

Pressure loads can be applied to surface or face supports or to a surface group. When you select the support, you can also select an existing pressure load that was created from a different analysis case that was created in the Generative Structural Analysis workbench. The new pressure load has the same magnitude and is applied to the same region as the pressure load created in the Generative Structural Analysis workbench. You can modify the magnitude or the region only by modifying the original pressure feature in the Generative Structural Analysis workbench. The original pressure feature in the Generative Structural Analysis workbench can include Data Mapping using values imported from a Microsoft Excel spreadsheet (.xls*) or a text file (.txt). The imported pressure data must satisfy the following criteria:

The data must be arranged in four columns in the following order: X-coordinate, Y-coordinate, Z-coordinate, and pressure value.
The data must include a header row in which the dimensional data are provided in parentheses. Pressure data can be provided without dimensions. The following sample header row provides one example of proper header row syntax:

X(mm) Y(mm) Z(mm) Pressure()

The actual pressure values created from imported data will be the product of the dimensionless pressure values multiplied by the value you provide for the Magnitude of the pressure. For example, if your imported data specify a dimensionless value of 10 at the location (0, 0, 0) and you specify a value of 20N_m2 for the pressure history object, the pressure at that location will be 200N/m² for the analysis.

This task shows you how to create a pressure load on geometry.

Click the Pressure Load icon .

The Pressure dialog box appears, and a Pressure object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select the geometry support (a surface or a pressure load that you created in the Generative Structural Analysis workbench). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select a surface group.

The Supports field is updated to reflect your selection. A temporary symbol will appear at the supports to indicate zero values until you apply a nonzero load.
Enter a value for the pressure magnitude.
Right-click on the Magnitude field to add knowledgeware controls (for more information, see Applying Knowledgeware).
To import and incorporate a pressure history into the pressure load, perform the following steps:
1. Toggle on Data mapping, then click the ... button.
  
  The Data Mapping dialog box appears.
2. Click Browse, then select the spreadsheet or text file from which you want to import temperature data.
  
  Once you select a file, you can display the imported data in tabular form in the Imported Table dialog box by clicking Show.
3. If desired, toggle on Display Bounding Box to display a three-dimensional box incorporating the minimum and maximum values from the imported table. The bounding box enables you to confirm that the support you select lies completely within the space dictated by the imported data; if a portion of the support is outside this box, an error will be returned during the analysis.
4. Click OK to close the Data Mapping dialog box.
Click More to access additional pressure load options.
1. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the pressure load.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
2. Toggle on Apply user subroutine to define a nonuniform variation of the pressure load magnitude throughout the step in user subroutine DLOAD (in a Nonlinear Structural case). For more information, see Using User Subroutines..
Click OK in the Pressure dialog box.

Symbols representing the applied pressure are displayed on the geometry.

Creating Point Loads

Point loads represent point forces and moments applied to selected degrees of freedom. Point loads can be applied only in mechanical steps.

The magnitude of a point load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). You can also apply knowledgeware techniques to control the value of a point load (for more information, see Applying Knowledgeware).

By default, the components of a concentrated force and moment applied at a point are associated with the global, rectangular Cartesian axis system. You can specify a local coordinate system for the definition of point loads, and you can define the local system as a Cartesian, cylindrical, or spherical axis system. Local coordinate systems are defined in the CATIA Part Design workbench.

Point loads can be applied to point or vertex supports, virtual parts, a point group, or a rigid coupling feature or smooth coupling feature.

This task shows you how to create a point load on geometry.

Click the Point Load icon .

The Point Load dialog box appears, and a Point Load object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select the geometry support (a point). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select a point group.

The Supports field is updated to reflect your selection. A temporary symbol will appear at each support to indicate zero values until you apply a nonzero load.
Enter values for the force components Force 1, Force 2, and Force 3.

Tip: You can drag the compass onto the model to align the directions used for specifying the force with the local model directions. For more information, see Axis System Type in the “Creating Distributed Forces” procedure in the CATIA V5 Generative Structural Analysis User's Guide.

The Force Norm field is updated to show the total resultant force that will be applied to each point.
Enter values for the moment components Moment 1, Moment 2, and Moment 3.

The Moment Norm field is updated to show the total resultant moment that will be applied to each point.
Right-click on a force or moment field to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).
Click More to access additional point load options.
1. Toggle on Follow nodal rotation to make the direction of the force rotate with the rotation of the support point during the analysis. The force can rotate only if the underlying elements have rotational degrees of freedom and the current step accounts for nonlinear geometric effects (see Accounting for Nonlinear Geometric Effects).
2. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the point load.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
3. Toggle on Selected local system, and select a coordinate system to define local directions.
4. If desired, change the local orientation from Cartesian to Cylindrical or Spherical. See Using Local Coordinate Systems for more information.
Click OK in the Point Load dialog box.

Symbols representing the applied force and moment are displayed on the geometry.

Creating Distributed Loads

Distributed loads represent point forces and moments applied to selected degrees of freedom. Distributed loads apply a resultant load to a handler point or to the center of gravity; the load distribution is nonuniform over the supports, with an effect similar to the use of a smooth coupling. Distributed loads can be applied only in mechanical steps.

The magnitude of a distributed load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). You can also apply knowledgeware techniques to control the value of a distributed load (for more information, see Applying Knowledgeware).

By default, the components of a distributed force and moment are associated with the global, rectangular Cartesian axis system. You can specify a local coordinate system for the definition of distributed loads, and you can define the local system as a Cartesian, cylindrical, or spherical axis system. Local coordinate systems are defined in the CATIA Part Design workbench.

Distributed loads can be applied to vertices, edges, faces, or groups containing one or more of these support types.

This task shows you how to create a distributed load on geometry.

Click the Distributed Load icon .

The Distributed Load dialog box appears, and a Distributed Load object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select geometry supports (vertices, edges, or faces). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select groups containing vertices, edges, or faces, or use groups to select a combination of these geometry types.

The Supports field is updated to reflect your selection. A temporary symbol will appear at each support to indicate zero values until you apply a nonzero load.
Enter values for the force components Force 1, Force 2, and Force 3.

You can drag the compass onto the model to align the directions used for specifying the force with the local model directions. For more information, see Axis System Type in the “Creating Distributed Forces” procedure in the CATIA V5 Generative Structural Analysis User's Guide.

The Force Norm field is updated to show the total resultant force that will be applied to the model.
Enter values for the moment components Moment 1, Moment 2, and Moment 3.

The Moment Norm field is updated to show the total resultant moment.
Right-click on a force or moment field to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).
Click More to access additional distributed load options.
1. Toggle on Follow nodal rotation to make the direction of the force rotate with the rotation of the support point during the analysis. The force can rotate only if the underlying elements have rotational degrees of freedom and the current step accounts for nonlinear geometric effects (see Accounting for Nonlinear Geometric Effects).
2. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the distributed load.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
3. Toggle on Selected local system, and select a coordinate system to define local directions.
4. If desired, change the local orientation from Cartesian to Cylindrical or Spherical. See Using Local Coordinate Systems for more information.
Select a Handler Point.

The handler point is optional if all supports are of the same type, since the load will be applied evenly to each support. If you used groups to select a combination of geometry types, you must select a handler point so the load can be distributed correctly.
Click OK in the Distributed Load dialog box.

Symbols representing the applied force and moment are displayed on the geometry.

Distributed loads cannot be modified when they are propagated into other analysis steps. They can be edited only in the step in which they were created. For more information on propagation, see Propagation.

Creating Load Densities

Load densities apply force per unit of length or area to each line or element face in the selected support. Load densities can be applied only in mechanical steps.

The magnitude of a load density can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). You can also apply knowledgeware techniques to control the value of a load density (for more information, see Applying Knowledgeware).

By default, the components of a load density are associated with the global, rectangular Cartesian axis system. You can specify a local coordinate system for the definition of load densities, and you can define the local system as a Cartesian, cylindrical, or spherical axis system. Local coordinate systems are defined in the CATIA Part Design workbench.

Load densities can be applied to lines, faces, or groups; however, if load densities are applied to groups, the groups can contain supports of only one type.

This task shows you how to create a load density on geometry.

Click the Load Density icon .

The Load Density dialog box appears, and a Load Density object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select geometry supports (lines or faces). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select groups containing lines or faces.

The Supports field is updated to reflect your selection. A temporary symbol will appear at the supports to indicate zero values until you apply a nonzero load.
Enter values for the force components Force 1, Force 2, and Force 3.

You can drag the compass onto the model to align the directions used for specifying the force with the local model directions. For more information, see Axis System Type in the “Creating Distributed Forces” procedure in the CATIA V5 Generative Structural Analysis User's Guide.

The Force Norm field is updated to show the total resultant force that will be applied to the model.

Moments are not used with load densities.
Right-click on a force field to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).
Click More to access additional load density options.
1. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the load density.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
2. Toggle on Selected local system, and select a coordinate system to define local directions.
3. If desired, change the local orientation from Cartesian to Cylindrical or Spherical. See Using Local Coordinate Systems for more information.
Click OK in the Load Density dialog box.

Symbols representing the applied force are displayed on the geometry.

Load densities cannot be modified when they are propagated into other analysis steps. They can be edited only in the step in which they were created. For more information on propagation, see Propagation.

Creating Gravity Loads

Gravity loads represent uniform accelerations applied to selected degrees of freedom in a fixed direction.

Gravity loads can be applied only in mechanical steps.

The magnitude of a gravity load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). You can also apply knowledgeware techniques to control the value of a gravity load (for more information, see Applying Knowledgeware).

By default, gravity load components are associated with the global, rectangular Cartesian axis system. You can specify a local coordinate system for the definition of gravity loads. Local coordinate systems are defined in the CATIA Part Design workbench.

Gravity loads can be applied to volume or part supports, point masses (distributed masses applied to one or more points), a body group, or a mesh part. If a gravity load is applied to geometry that is the support for a distributed mass object other than a point mass, the gravity load is also applied to the distributed mass. (See Creating Distributed Masses for more information.)

This task shows you how to create a gravity load on geometry.

Click the Gravity Load icon .

The Gravity dialog box appears, and a Gravity object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select the geometry support (a volume, part, distributed mass object, or mesh part). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select a body group.

The Supports field is updated to reflect your selection. A temporary symbol will appear at the supports to indicate zero values until you apply a nonzero load.
Enter values for the load components Component 1, Component 2, and Component 3.
Right-click on a component field to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).
Click More to access additional gravity load options.
1. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the gravity load.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
2. Toggle on Selected local system, and select a coordinate system to define local directions.
Click OK in the Gravity dialog box.

Symbols representing the applied force are displayed on the geometry.

Creating Rotational Body Force Loads

Rotational body force loads represent acceleration fields induced by rotational motion applied to parts. You specify a rotation axis and values for the angular velocity and/or angular acceleration magnitudes. The rotational body force load applied to the part is a combination of the centrifugal load and the rotary acceleration load. The magnitude of the centrifugal load is proportional to the angular velocity squared. The magnitude of the rotary acceleration load is directly proportional to the angular acceleration.

The magnitude of a rotational body force load can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). The value of the rotational body force is determined by multiplying the centrifugal load and the rotary acceleration load by the value of the amplitude. You can also apply knowledgeware techniques to control the value of a rotational body force load (for more information, see Applying Knowledgeware).

Rotational body force loads can be applied only in mechanical steps.

Rotational body force loads can be applied to volume or part supports, to body groups, or to mesh parts.

This task shows you how to create a rotational body force load on geometry.

Click the Rotational Body Force icon .

The Rotational Body Force dialog box appears, and a Rotational Body Force object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the load by editing the Name field.
Select the geometry support (a volume, part, or mesh part). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the load to all supports simultaneously. You can also select a body group.

The Supports field is updated to reflect your selection. A temporary symbol will appear at the supports to indicate zero values until you apply a nonzero load.
Select an existing line or a construction axis to specify the rotation axis. Any selectable geometry is highlighted when you pass the cursor over it.

The Axis of rotation field is updated to reflect your selection.
Enter a value for the Rotational velocity.
Enter a value for the Rotational acceleration.
Right-click on the velocity or acceleration field to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).
Click More to access additional rotational body force load options.
1. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the rotational body force load.
  
  If you do not specify an amplitude in a Nonlinear Structural case, the solver applies the reference magnitude based on the Default load variation with time option that you selected when you created the step. The solver either applies the reference magnitude linearly over the step (Ramp) or applies it immediately at the beginning of the step and subsequently holds it constant (Instantaneous).
Click OK in the Rotational Body Force dialog box.

Symbols representing the applied force are displayed on the geometry.

Importing Loads

Imported loads enable you to incorporate a load definition or an entire load set from GPS into your analysis. Imported loads can be oriented using rectangular coordinate systems only, and the following load types are available for import:

Pressure
Distributed force
Moment
Bearing load
Imported force
Imported moment
Acceleration
Rotational force
Line force density
Surface force density
Volume force density
Force density

This task shows you how to import a load definition into your analysis.

Click the Imported Load icon .

The Imported Load dialog box appears, and an Imported Load object appears in the specification tree under the Loads objects set for the current step.
You can change the identifier of the imported load or load set by editing the Name field. By default, Nonlinear Structural Analysis uses the same name that the load or load set was assigned in GPS.
Select the load or load set that you want to import. Any selectable load is highlighted when you pass the cursor over it.

The Supports field is updated to reflect your selection.
Click More to view the propagation status of the imported load. The propagation status shows the following:
- Whether the imported load was Created in this step or Propagated into this step.
- Whether the imported load is Active or Inactive.
Click OK in the Imported Load dialog box.

Symbols representing the applied force are displayed on the geometry.