Forces

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

• Force loads can be applied to nodes, edges, or surfaces.
• Force loads can be applied in any direction, as specified by a vector. Additionally, a surface force can be applied normal to the surface. Depending upon the type of model (CAD-based or hand-built), Force loads may or may not be available. Depending upon the specific type of force load (nodal, edge, or surface), local coordinate systems may or may not be supported. See the following bullets for details.
  • Nodal forces are supported for all CAD-based and hand-built models. Local coordinate systems are supported for nodal force objects.
  • Edge forces apply nodal forces to each node along the edge. The magnitudes of the nodal forces are calculated so that the force is evenly distributed along the edge. Edge forces are applicable only to CAD-based solid or surface models and 2D Mesh Generation models. Local coordinate systems are supported for edge forces.
  • Surface forces are only applicable to CAD-based solid or surface models. A surface force applies an equivalent pressure to the selected surface, so the distribution of force is uniform even if the nodes are unevenly spaced. Local coordinate systems are NOT supported for surface forces. The load direction must either be normal or specified using the global axis directions (radio buttons or vector components).

    As an alternative to applying the specified force magnitude to each of several selected surfaces, you can choose to distribute a specified force magnitude over two or more surfaces. If this option is activated, the total force is distributed based on the relative area of each surface selected. See the Apply Forces section below for more details.

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 magnitude in the X direction, you have just applied 100 lbs (10 objects * 10 lbs per object) to your model. The same is true if you apply the force to 10 surfaces or 10 edges. The exception to this rule is for surface forces applied to two or more surfaces when the Distribute magnitude across all surfaces option is enabled. See the Apply Forces section below for more details.

Analysis-Specific Parameters:

1. 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.
2. 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. 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. Alternatively, specify the total force to be distributed over multiple surfaces in the Magnitude field.
• Specify the direction of the load in the Direction section.
• Click the Flip Direction button () to invert the sign of the applied load, reversing its direction.
• If two or more surfaces are selected, the Distribute magnitude across all surfaces option will be available. When this option is activated, the specified magnitude is distributed on a pro rata basis depending upon the area of each selected surface. The example in the following table explains how the load is distributed:

  Example:

  Assume that a total force of 2,500 N is distributed over three surfaces (a, b, and c) with areas of 100, 300, and 600 mm², respectively.

  Surface	Area (mm2)	Force (N)
  a	100	250 (= 100/1,000 * 2,500)
  b	300	750 (= 300/1,000 * 2,500)
  c	600	1,500 (= 600/1,000 * 2,500)
  	Total Area = 1,000	Total Force = 2,500

  Caution: Be careful when running a Parametric Study on models with a distributed surface force applied. The forces applied to individual surfaces of a distributed force group are not updated when the model geometry changes. If any of the parameters you are manipulating affect the area of a surface to which a distributed force is applied, the force distribution will no longer be correct.

The arrows used to indicate applied forces point in the specified load vector direction, including the Normal direction for forces applied normal to surfaces. However, the lengths of the force arrows are not scaled to indicate the relative magnitude of the applied forces.

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

Import Reaction Forces From an Electrostatic Analysis

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. To activate the output of the reaction forces, see the Calculating the Forces and Charge Caused by the Electrostatic Field section on the Analysis Parameters: Electrostatic Field Strength and Voltage page. (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:

1. With nothing selected, right-click in the display area of the FEA Editor. Select the Loads from File command.
2. Press the Browse button in the Results File column. A dialog box appears. Use the Files of type: pull-down to select the Electrostatic Reaction Forces (*.efr) type of file to read for the loads.
3. Select the file and click Open.
4. 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.
5. 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.
6. 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.
7. 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 dialog box.
• 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 Temperatures page.
• Loads from a text file can be imported to the structural analysis. See the Loads from File page.