OptiStruct is a proven, modern structural solver with comprehensive, accurate and scalable solutions for linear and nonlinear
analyses across statics and dynamics, vibrations, acoustics, fatigue, heat transfer, and multiphysics disciplines.
The OptiStruct Example Guide is a collection of solved examples for various solution sequences and optimization types and provides
you with examples of the real-world applications and capabilities of OptiStruct.
This section presents nonlinear small displacement analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents nonlinear large displacement analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents nonlinear transient analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
Demonstrate a Transfer Path Analysis (TPA) on a simplified vehicle model using OptiStruct. TPA is used to calculate and rank the noise or vibration contributions for a given Response Point, through the different
structural transmission paths in a system.
Demonstrates how to identify sensitive design parameters within a full vehicle NVH model, both as a way to understand
the dynamics of the system and what design changes can be made to improve a vehicle response, using OptiStruct and NVH post-processing in HyperView.
Demonstrate Infinite Elements, which is effectively modeled to measure the sound pressure of the 2.1 Home Theater
System in OptiStruct with effective modeling practice.
Explicit Analysis of the impacting plates to extract the contact forces and performing Frequency Response Analysis
using these forces as input to study the sound radiation by the plates.
This section presents normal modes analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents complex eigenvalue analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents thermal and heat transfer analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents analysis technique examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents shape optimization example problems, solved using OptiStruct. Each example uses a problem description, execution procedures and results to demonstrate how OptiStruct is used in shape optimization.
The examples in this section demonstrate how topography optimization generates both bead reinforcements in stamped
plate structures and rib reinforcements for solid structures.
The examples in this section demonstrate how the Equivalent Static Load Method (ESLM) can be used for the optimization
of flexible bodies in multibody systems.
This section presents multiphysic examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents response spectrum examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
This section presents nonlinear explicit analysis examples generated using OptiStruct. Each example uses a problem description, execution procedures, and results to demonstrate how OptiStruct is used.
The OptiStruct Example Guide is a collection of solved examples for various solution sequences and optimization types and provides
you with examples of the real-world applications and capabilities of OptiStruct.
The operational loading involves three steps (or subcases).
In the first subcase a pre-tensioning force of 3.5E3 Newton’s is applied on 3 bolts that
are connected to the flange. In the second subcase a Clamping pressure of 1E4 MPA is applied
on the flange and 1MPA is applied on the folding blades. In the third subcase a tip load is
applied on the flat surface of the blade.
Case 1
Nonlinear Static Analysis
Bolt Pretension
Case 2
Nonlinear Static Analysis
Pressure Load with CNTNLSUB and
STATSUB(PRETENS)
Case 3
Modal Frequency Response Analysis
With STATSUB (PRELOAD)
In Modal Frequency Response Analysis, the modal solution is performed using
AMSES.
FE Model
Bolts
CBEAM
CHEXA
Flange and Blade
CTETRA
The linear material properties are:
MAT1
Young’s Modulus
2.1E5
Poisson's Ratio
0.3
Initial Density
7.8E-9
Results
The displacement results on the bolts for subcase 1 and read the .PRET
file and review the results. In Figure 2, observe the
displacement results snapshot from all the 3 subcases.
In subcase 3, the preloading is captured by a geometric stiffness matrix which is based on the stresses of the preloading nonlinear
static subcase 2. In prestressed analysis, this geometric stiffness matrix is augmented with
the original stiffness matrix of the (unloaded) structure.
In this model since there is contact, the contact status can be carried over from the
preloading subcase 2 to the preloaded subcase 3.
For comparison study, when this example model is run with and without STATSUB
(Pre-Load) in subcase 3, notice the different in the frequencies of the
eigenvector in the .out files. In the Modal Frequency Response Analysis
without Preload you have rigid body modes as the contact between the bolts and the flange
has not been established.
Also, when you plot the MFREQ results at frequency 300Hz, notice the
difference between the mode shape.