This pdf has brief introduction to the Inertia Relief Analysis with the help of Ansys.

1. By Rahul Shedage
M.Tech. Mechanical Design
Inertia Relief Analysis of a Suspension Shock Linkage
In this tutorial, an existing finite element model of a suspension linkage will be used to demonstrate how to
set up and perform a inertia relief analysis. ANSYS Workbench Mechanical supports Inertia Relief in a static
analysis.
The following exercises are included:
• Introduction
• Setting Project page
• Retrieving the Ansys geometry input file
• Creating mesh model
• Applying Loads and Boundary Conditions to the Model
• Solving the model
• Adding results to solution
• Viewing the results
The following file is needed to perform this tutorial: Inertia_relief.agdb
Exercise:
1. Introduction:
Consider a structure that has mass, and a vertical load that exceeds its weight. Without constraint in the
vertical direction, the global stiffness matrix is singular, and no solution exists.
Inertia Relief during analysis of such a structure requires that mass be properly represented, just enough
constraint be applied to prevent free body translation and rotation, loads be applied, and Inertia Relief be
requested. Other conditions must be met. The IRLF command is employed by ANSYS during Solve.
The following conditions and limitations, taken from the ANSYS Help Viewer, must be considered:
Inertia Relief – Linear Static Structural Analyses Only
Calculates accelerations to counterbalance the applied loads. Displacement constraints on the
structure should only be those necessary to prevent rigidbody motions (6 for a 3D structure). The sum
of the reaction forces at the constraint points will be zero. Accelerations are calculated from the
element mass matrices and the applied forces. Data needed to calculate the mass (such as density)
must be input. Both translational and rotational accelerations may be calculated.
• This option applies only to linear static structural analyses.
• Nonlinearities, elements that operate in the nodal coordinate system, and axisymmetric or
generalized plane strain
• elements are not allowed.

2. By Rahul Shedage
M.Tech. Mechanical Design
• Models with both 2D and 3D element types or with symmetry boundary constraints are not
recommended.
• Loads may be input as usual. Displacements and stresses are calculated as usual.
• Symmetry models are not valid for inertia relief analysis.
2. Setting Project page:
1. Open the Project page.
2. From the Units menu verify:
– Project units are set to “Metric (kg, mm, s, C, mA, mV).
– “Display Values in Project Units” is checked (on).
3. From the Toolbox insert a “Static Structural” system into the Project Schematic.

3. By Rahul Shedage
M.Tech. Mechanical Design
3. Retrieving the Ansys geometry input file
1. From the Geometry cell, RMB and “Import Geometry > Browse”. Import the file “Inertia_relief.agdb”.
(RMB: Right Mouse Button)
2. Double click the “Model” cell to start the Mechanical application
3. Set the working unit system: “Units > Metric (mm, kg, N, s, mV, mA)”.

4. By Rahul Shedage
M.Tech. Mechanical Design
4. Creating Mesh Model:
1. Highlight the mesh branch, “RMB > Insert > Method”.
2. In Geometry lable select the solid body from the working area,
3. Define Mehod > Hex Dominent and Free Face Mesh Type > Quad/Tria

5. By Rahul Shedage
M.Tech. Mechanical Design
4. Mesh > RMB > Show > Mappable Faces
5. Then click on Mesh > RMB > Insert > Mapped Face Meshing and in the faces select the faces that we
have found in step 4.
6. Review the meshed model

6. By Rahul Shedage
M.Tech. Mechanical Design
5. Apply Loads and BCS
1. Create Named Selection sets of nodes for application of loads and support
2. Name first node set as Force 10000 and second set of nodes as a Fixed. Above figure shows the set of
nodes for applying loads i.e. Force 10000
3. Highlight the “Static Structural” branch.
RMB > Insert > Nodal Force”.
4. In named selection select the Force 10000 Node set that we have created earlier.
In Definition > X Component > 10000N (other component forces are set to zero), here only compressive loads
are applied to see deformation and stresses.
5. Highlight the “Static Structural” branch.
RMB > Insert > Nodal Displacement”.
6. In named selection select the Fixed Node set that we have created earlier
7. Give Nodal Displacement as 0 for X, Y, and Z direction as,

7. By Rahul Shedage
M.Tech. Mechanical Design
6. Solve the System:
1. In the Workbench Mechanical interface, if a static analysis is requested, the Analysis Settings
branch offers Inertia Relief in its Details as in Figure below. Using Inertia Relief assumes qualifying
conditions in the model are met:
Set Inertia Relief to “On”.

8. By Rahul Shedage
M.Tech. Mechanical Design
2. Choose solve from the tool bar or RMB Solution branch and choose “Solve”
7. Adding Results to Solution:
1. Highlight the solution branch:
2. From the context menu, choose Stresses > Equivalent (von-Mises) or RMB > Insert > Stress >
Equivalent (von-Mises)
3. Repeat the step above, choose Deformation > “Total Deformation”
4. Solve again.
Note: adding results and resolving the model will not cause a complete solution to take place. Results
are stored in the database and requesting results requires only an update.

9. By Rahul Shedage
M.Tech. Mechanical Design
8. Viewing the Results
.1. Click on Deformation from solution tab,
The maximum deformation is 2.5667 mm
2. Click on Equivalent Stresses from Solution,
The maximum stress in 477.34 MPa
3 To animate the result click on Play,
This is the complete procedure for Inertia Relief Analysis in ANSYS Workbench.