Tutorial: Inertia Relief Analysis

Define a force using components and run an analysis with inertia relief.

In this lesson you will:
  • Apply forces and moments using component force mode
  • Run an analysis with inertia relief

Overview

Inertia relief is a numerical method used for analyzing unconstrained structures. A typical example is an aircraft in steady flight where the lift, drag, and thrust loads are balanced by gravity acting on the mass of the total aircraft. This acceleration due to gravity is equal and opposite to the acceleration that would result for the unconstrained structure.

At a component level, with inertia relief it is possible to analyze a part in isolation if the loads at the interface points are known or can be measured/calculated and the part can be considered to be in static equilibrium.

This tutorial examines a motorcycle rear swing arm where the attaching structures—shock absorber, frame, and axle—are unknown but the loads at the interface points have been provided. It comprises two main sections:
  • load setup
  • running inertia relief
The following table provides the loads that will be used in this exercise. They are also shown throughout the exercise as required.
Location Shock Pivot Axle
Force Fx N -2352 980 1372
Fy N 3211 -3700 489
Fz N -635 645 0
Moment Mx N*mm 0 -104867 -278
My N*mm 0 -188238 779
Mz N*mm 0 0 -7998

Apply a Component Force to the Shock Mount

  1. Press F7 to open the Demo Browser.
  2. Double-click the 0.0_swingarm_IR_FEA.x_b file to load it in the modeling window.
    This is a solid model of a single part motorcycle swing arm.


  3. Make sure the display units in the Unit System Selector are set to MMKS (mm kg N s).
  4. Select the Apply Force tool on the Structure ribbon.


    Tip: To find and open a tool, press Ctrl+F. For more information, see Find and Search for Tools.
  5. Click to apply the force to the hole center of the shock mount.


  6. Switch to Component Force Mode on the microdialog, and click the chevron to expand it.


  7. Enter the following values:
    • Fx: -2352 N
    • Fy: 3211 N
    • Fz: -635 N


  8. Right-click and mouse through the check mark to exit, or double-right-click.

Apply a Component Force and Moment to the Swing Arm Pivot

  1. Zoom in on the swing arm pivot.
  2. Select the Connectors tool.


  3. Create a connector at the center of the hole by selecting the two faces as shown:


  4. Select the Apply Force tool and apply a force to the center point of the connector.


  5. Switch to Component Force Mode on the microdialog, and click the chevron to expand it.


  6. Enter the following values:
    • Fx: 980 N
    • Fy: -3700 N
    • Fz: 645 N


  7. Select the Apply Torque tool and apply a torque to the center point of the connector.


  8. Switch to Component Torque Mode on the microdialog, and click the chevron to expand it.


  9. Enter the following values:
    • Tx: -104867 N*mm
    • Ty: -188238 N*mm
    • Tz: 0 N*mm


  10. Right-click and mouse through the check mark to exit, or double-right-click.

Apply a Component Force and Moment to the Center of the Axle

  1. Zoom in on the center of the axle.


  2. Select the Apply Force tool and apply a force to the hole center of the axle.


  3. Switch to Component Force Mode on the microdialog, and click the chevron to expand it.


  4. Enter the following values:
    • Fx: 1372 N
    • Fy: 489 N
    • Fz: 0 N


  5. Select the Apply Torque tool and apply a torque to the hole center of the axle.


  6. Switch to Component Torque Mode on the microdialog, and click the chevron to expand it.


  7. Enter the following values:
    • Tx: -278 N*mm
    • Ty: 779 N*mm
    • Tz: -7998 N*mm


  8. Right-click and mouse through the check mark to exit, or double-right-click.

Run an Analysis with Inertia Relief

  1. Click Run Analysis on the Analyze icon to open the Run Analysis window.


  2. Use the following settings:


  3. Change the Element size to 2 mm.
  4. Make sure that Speed/Accuracy is set to Faster.
  5. Click Load Cases and select Use Inertia Relief.
  6. Click Run to perform the analysis.
  7. When the analysis is complete, double-click on the name of the run to view the results.
  8. Select von Mises Stress for the Result Type.
  9. Change the Max value to 200 MPa.
    Note: Even without supports, the analysis runs as any imbalance in the loads is reacted by the inertia forces.