Forces

Note: The information in this section applies to all linear and nonlinear analyses that support force loads.

A force can be applied to a node, edge or surface.

An edge force applies nodal forces to each node along the edge. The magnitudes of the nodal forces is calculated so that the force is evenly distributed along the edge.
A surface force applies an equivalent pressure to the selected surface.
A force can be applied in any direction specified by a vector. A surface force can also be applied normal to the surface.

What does a force do?

The data entered for the force is applied to each object selected and in the direction you specify. Therefore, if you select 10 nodes and specify a 10 lb force in the X direction, you have just applied 100 lbs (10 objects * 10 lbs) to your model. The same is true if you apply the force to 10 surfaces or 10 edges.

Analysis-Specific Parameters:

For Linear analyses:
- Nodal and edge forces are applied to a load case. The load case is defined in the Load Case/ Load Curve field. If you want a nodal or edge force to be applied in multiple load cases, you can copy it to a new load set and change the value in the Load Case/ Load Curve field.
- For a surface force to be applied to a model a Pressure multiplier must be defined in the Multipliers tab of the Analysis Parameters dialog box.
For Nonlinear analyses:
- All forces will follow a load curve throughout the analysis. Select the loads curve in the Load Case/ Load Curve field.

Apply Forces

If you have nodes, edges or surface selected, you can right-click in the display area and select the Add pull-out menu. Select the Nodal Force, Edge Force or Surface Force command. Edge forces can only be applied to parts that originated from CAD solid models or 2D Mesh Generation. You can also access this command from the ribbon (Setup Loads Force). You can click the ribbon command either before or after selecting the objects to which you wish to apply the force.

Specify the magnitude of the force that is applied to each selected object in the Magnitude field and the direction of the load in the Direction section. When you apply a surface force in the Normal direction, arrows display on the model in the FEA Editor. However, the arrows do not display perpendicular to the surface, but rather normal to a horizontal line . In the Results environment, the arrows accurately depict the direction of the normal surface force.

For linear analyses, if you are applying an edge or nodal force, specify the load case or load curve in which you want the force placed in the Load Case/Load Curve field. Surface forces are controlled by the global load case Pressure multiplier within the Analysis Parameters dialog box. For nonlinear analyses, specify the load curve number within the Load Case/Load Curve field for all surface, edge, and nodal forces.

Note: See the comments under the Application of Loads and Constraints at Duplicate Vertices heading on the Loads and Constraints page for information about how nodal loads are applied at duplicate vertices.

Import Reaction Forces From an Electrostatic Analyses

The structural reactions to the electrostatic force between conductors (usually significant only in MEMS applications) can be calculated. If an electrostatic analysis has been performed in a different model, and if the reaction forces were calculated in the different model, then those reaction forces can be applied to the structural model. See Electrostatic: Analysis Parameters: Electrostatic Field Strength and Voltage: Calculating the Forces and Charge Caused by the Electrostatic Field in this section for activating the output of the reaction forces. (Although the electrostatic forces in the binary results file are in units of voltage × current × time/length, the software automatically converts this to force units when applying the loads to the model.)

Attention: Due to changes in the software, electrostatic forces calculated prior to V23.1 (February 2009) should not be used with software versions V23.1 or newer. If these results are needed in V23.1 or newer, the analysis must be performed again.

The nodes in the stress model need to match the nodes in the electrostatic model where the reaction forces were calculated. But, the electrostatic parts do not need to be included in the stress analysis. For example, the force may be calculated on the surface of a part representing the dielectric material between conductors (such as air). Air between conductors would not be included in the stress analysis.

The method to apply the reaction forces to the stress model is as follows:

With nothing selected, right-click in the display area of the FEA Editor. Select the Loads from File command.
Press the browse button in the Results File column. A dialog box appears. Select the results file. Use the Files of type: pull-down to select the Electrostatic Reaction Forces (*.efr) type of file to read for the loads.

Select the file and click Open.

Since electrostatic analyses can only have a single load case, the Load Case from File column will show zero (0). However, you can import multiple sets of loads into a single model by pressing the Add Row button. The loads assigned to the other rows of the spreadsheet can be from the same file and design scenario, from different files, or from different design scenarios. For example, you may want to apply the same electrostatic forces to more than one load case in the stress analysis. Or, you may want to calculate stresses for electrostatic force results at two different applied voltages, each one being from a different design scenario.

The loads are placed in a specific load case or load curve in the stress analysis; enter the load case/load curve in the Structural Load Case field.

If you want the loads to be multiplied by a constant value before being applied to the model, specify the constant value in the Multiplier column.

Press the OK button.

Note:
The imported loads do not appear in the FEA Editor. They appear in the Results environment after doing a Check Model or performing the analysis.

For linear analyses, don't forget to define the number of load cases as necessary for the imported loads. If the model is set up for 2 load cases and a load imported from an electrostatic analysis is assigned to load case 5, the load on load case 5 does not exist. The model has only two load cases. To create the additional load cases in this example, add three rows on the Multipliers tab of the Analysis Parameters screen.

For nonlinear analyses, don't forget to define the load curves as necessary for the imported loads. If a load imported from an electrostatic analysis is assigned to load curve 5 and this load curve is not defined, the multiplier will be 0!

Tip:
The Loads from File dialog box can also be used for the following:

Load temperatures from another model. See the page Setting Up and Performing the Analysis: General Information (Common to Multiple Analysis Types): Loads and Constraints: Temperatures.

Loads from a text file can be imported to the structural analysis. See the page Setting Up and Performing the Analysis: General Information (Common to Multiple Analysis Types): Loads from File.

Parent topic: Loads and Constraints