OptiStruct for Linear Analysis (2) Linear Static Analysis

 

1. Elements, Materials, Loads, and Boundary Conditions

In this lesson we will learn about element types and material models in OptiStruct.  We will also look into loads and boundary conditions and how they are applied in OptiStruct.  Watch the video below to learn more.

Elements Classifications

In OptiStruct, there are a selection of element types available to the user. They are usually categorized as 1D, 2D & 3D types.

• 1D or Line

• 2D or Area

• 3D or Volume

• Special

Files:

• I-Beam-Bending-Validation_v1.pdf

 

Material Classification

• Material Definitions

• MAT1

• MAT4

• Element & Material Compatibility

HyperWorks Solver Browser

The HyperWorks Solver Browser provides a solver-centric view of the model structure in a flat, listed tree structure.  You can access it through the  View menu > Solver Browser.

You can use the Solver Browser to create and edit loads and constraints as well as review the model setup. Loads are created using the context menu and selecting Create > Loads.

The Entity Editor provides an easy way to review definitions.  By default, loads are created on node or element sets and realized in solver representation (set/node) during  solver file export.

Loads

• DOF

• Force Load

• Surface Load

• Body Load

• Additional Techniques

2. Exercise - Analysis Setup

In this exercise, we start by loading a model into HyperWorks and then we will organize the model and assign materials and properties to complete the model definition.  Next, we will create constraints & loads in the model and define a loadstep before running the analysis in OptiStruct.  Finally, we will post-process the results using the HyperWorks Post ribbon and HyperView client.

Watch the video below to view a demonstration of the exercise.  Then download the PDF and model files to do the exercise yourself!

Files:

• ex1a.pdf
• 1A.zip

3. Linear Static Analysis & Model Definition

In this lesson we will cover what Linear Static Analysis is and learn about the input file structure.  Watch the video below to learn more.

What is a Static Analysis?

In mechanics we can define a static state as the state of a system that is in equilibrium under an action of balanced forces and moments so that they remain at rest (no velocity).  A static analysis is independent of time. The inertial forces are either ignored or neglected.  In a static analysis, forces are constant, velocity is zero, and acceleration is zero.  The system is subjected to loads and boundary conditions like Forces, Moments, Temperature, and SPCs (Single point constraints) / MPCs (Multi point constraints).

A linear static analysis has some assumptions such as deformations are in the elastic range and stresses are assumed to be linear functions of the strains.  Linear Static solvers produce solutions from the basic equation:

K x = f

where

K = global stiffness matrix

x = displacement vector response to be determined

f = external forces vector applied to the structure

Watch the video below to view an example!

 

 

Model Definition Structure

OptiStruct used a Nastran-style ASCII Input as seen in the image below.

Bulk Data Section

• PARAM

• CORD2R

• GRID

• Elements

• Properties

• Materials

• Loads & Boundary Conditions

• SPC

Consistent Units

Remember that all internal calculations in OptiStruct are unit-less.  It is the responsibility of the user to create the model using a consistent set of units.  Some of the equations that governs consistent units are:

• Force = Mass × Acceleration
• Mass = Density × Volume
• Acceleration = Length / Time^2

As an illustration, you can see below a set of consistent units. To avoid errors, it is essential to be aware of the set units when working with a model.

4. Output File & Run Options

In this lesson we will cover output file types as well as what the run options are.   We will also cover the general workflow for setting up a linear static analysis in HyperWorks for OptiStruct.  Watch the video below to learn more.

Output Files Types

Access the documentation to review the available output file types available in OptiStruct.

Output Result Types

Run Options for OptiStruct

-analysis   Submit an analysis run. The job will be terminated if errors exist in the analysis or optimization data.

-optskip   Submit an analysis run without checking optimization data (skip reading all optimization related cards). 

-check     Submit a check job through the command line.

-nt X   Number of threads/cores (X) to be used for SMP solution.

-np X   Number of processors (X) to be used for SPMD analysis.

-len X   Preferred upper bound on dynamic memory allocation (with X in RAM MBytes)

-maxlen X   Hard upper limit on dynamic memory allocation (in RAM MBytes). OptiStruct will not exceed this limit. 

-core X   The solver assigns the appropriate memory required.  If there is not enough memory available, OptiStruct will error out.

-out     Echoes the output file to the screen.

For more details, refer to the Altair HyperWorks Online Help.

Linear Static Analysis General Workflow and Tools

5. Stress Evaluation, Averaging, & Convergence Studies

In this lesson, we will cover stress evaluation (including extrapolation to nodes) and stress averaging.   We will also take a look at a convergence study.  Watch the video below to learn more.

Stress Evaluation Extrapolation to Nodes

Stresses are always numerically calculated at the (Gauss) Integration Points (IP).  In OptiStruct, by default, element stresses for shell and solid elements are output at the element centroid only.  

Stress output at nodes is an extrapolation: the simplest option to achieve this is bilinear extrapolation. This is equivalent to using shape functions of 1st-order shells.  This can be requested with: 

STRESS(H3D,CORNER)=YES  or STRESS(H3D,BILIN)=YES

• Extrapolation to Nodes - Shells

• Extrapolation to Nodes - Solids

Stress Averaging at Nodes in HyperView

• Simple - Averaging of the stress invariants. Advanced should provide more accurate results
• Advanced - Averaging the stress tensor and calculate invariants from this
• Difference - Max-min nodal value. Good to find areas with large with stress discontinuous → remeshing?
• Maximum/Minimum - Max/min value

Convergence Study

On one hand, a finer mesh results typically in a more accurate solution, but on the other hand it increases the computation time. In order to get an idea of a finite element model that is good enough to predict an accurate solution for a problem with a reasonable model size, a convergence study can be performed:

• Create a mesh using low, but reasonable number of elements and do an analysis
• Refine the mesh, do a reanalysis and compare the results for the first mesh.
• Keep refining the mesh and reanalyzing until the results like max. stress and max. displacement converge.

Example: Solid Bracket

6. Exercise - Static Analysis of a Solid Bracket

In this exercise we will start by loading a torsion link in HyperWorks.  We will then organize the model and assign materials and properties to complete the model definition. Next, we will create constraints & loads in the model and define a loadstep before running the analysis in OptiStruct through the Compute Console.  Finally, we will post-process the results using HyperWorks Post ribbon and HyperView client.

Watch the video below to view a demonstration of the exercise.  Then download the PDF and model files to do the exercise yourself!

Files:

• ex1b.pdf
• 1B.zip

 

Next: OptiStruct for Linear Analysis (3) Inertia Relief Analysis