Home
Verification Problems
This manual presents solved verification models including NAFEMS problems.
NAFEMS Linear Elastic
OS-V: 0010 Elliptic Membrane
Test No. LE1 The model is a thin plate of thickness 0.1m subjected to a uniform pressure for linear static analysis. OptiStruct examines the direct stress $σ_{y y}$ at the point on inside the ellipse on the x-axis.

Welcome
What's New
View new features for OptiStruct 2024.1.
Overview
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.
Tutorials
Discover OptiStruct functionality with interactive tutorials.
User Guide
This manual provides detailed information regarding the features, functionality, and simulation methods available in OptiStruct.
Reference Guide
This manual provides a detailed list and usage information regarding input entries, output entries, and parameters available in OptiStruct.
Example Guide
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.
Verification Problems
This manual presents solved verification models including NAFEMS problems.
- NAFEMS Linear Elastic
  - OS-V: 0010 Elliptic Membrane
    Test No. LE1 The model is a thin plate of thickness 0.1m subjected to a uniform pressure for linear static analysis. OptiStruct examines the direct stress $σ_{y y}$ at the point on inside the ellipse on the x-axis.
  - OS-V: 0020 Cylinder Shell Patch
    Test No. LE2 OptiStruct examines the outer surface tangential stress $θ - θ$ at point E for linear static analysis.
  - OS-V: 0030 Radial Point Load on a Hemisphere
    Test No. LE3 The model is a hemispherical shell subjected to concentrated radial loads at its free edges. It examines the performance of the three-dimensional shell to model local bending behavior under conditions where the deformations are primarily due to bending.
  - OS-V: 0040 Z-Section Cantilever
    Test No. LE5 OptiStruct examines the axial (x-x) stress (compression) at mid-surface, point A for linear static analysis.
  - OS-V: 0050 Skew Plate Normal Pressure
    Test No. LE6 OptiStruct examines the maximum principal stress on the lower surface at the plate center point E for linear static analysis.
  - OS-V: 0060 Thick Plate Pressure
    Test No. LE10 The model is a thick plate subjected to uniform normal pressure of 1 MPa on the upper surface of the plate. OptiStruct examines the direct stress $σ_{y y}$ at the point D for linear static analysis.
  - OS-V: 0070 Solid Cylinder/Taper/Sphere - Temperature
    Test No. LE11 The model is a thick solid cylinder subjected to linear temperature gradient in the radial and axial direction. OptiStruct examines the direct stress $σ_{y y}$ at the point A inside the cylinder on the y axis for linear static analysis.
  - OS-V: 0080 Buckling of Shells and Composites with Offset
    A test of influence of offset on buckling solution for shells, including composite with offset Z0 and element offset ZOFFS.
  - OS-V: 0085 Plane Strain: Analysis of Pressure Vessel
    This problem examines the expansion of a pressure vessel due to an internal pressure.
- NAFEMS Thermo-elastic
- NAFEMS Heat Transfer
- NAFEMS Nonlinear Static Analysis
- NAFEMS Dynamic Response Analysis
- NAFEMS Random Response Analysis
- NAFEMS Normal Modes Analysis
- NAFEMS Composites
- Response Spectrum Analysis
- Elements
- Materials
- Fatigue Analysis
- Rotor Dynamics
- Frequency Response Analysis
- Explicit Dynamic Analysis
- Aeroelastic Analysis
Frequently Asked Questions
This section provides quick responses to typical and frequently asked questions regarding OptiStruct.

View All Altair HyperWorks Help

OS-V: 0010 Elliptic Membrane

Test No. LE1 The model is a thin plate of thickness 0.1m subjected to a uniform pressure for linear static analysis. OptiStruct examines the direct stress $σ_{y y}$ at the point on inside the ellipse on the x-axis.

Figure 1. FE Model with Boundary Conditions and Loadcases

Model Files

Before you begin, copy the file(s) used in this problem to your working directory.

LE1.zip

Benchmark Model

Second order Hexahedral, Penta, Tetra, Quad and Tria elements are used to create the coarse and fine mesh. A uniform outward pressure of 10 MPa is applied on the outer face. The pressure is converted to force and is applied to the nodes for Quad8 and Tria6 elements.

The material properties are:

Material Properties: Value
Young's Modulus: 210 x 10³ MPa
Poisson's Ratio: 0.3

Linear Static Analysis Results

All results are normalized with the target value (92.7 MPa).


	Direct Stress $σ_{y y}$ at Point D (MPa)	Normalized with the Target Value
Solid Hexahedral:
Hex8 coarse	63.15	1.467933492
Hex20 coarse	87.46	1.059913103
Hex8 fine	79.8	1.161654135
Hex20 fine	91.01	1.018569388
Solid Wedges:
Penta6 coarse	48.68	1.904272802
Penta15 coarse	95.21	0.973637223
Penta6 fine	67.3	1.377414562
Penta15 fine	94.28	0.983241409
Solid Tetrahedral:
Tetra4 coarse	53.34	1.737907762
Tetra10 coarse	95.96	0.966027511
Tetra4 fine	66.56	1.392728365
Tetra10 fine	95.28	0.972921914
Quad Shells:
Quad4 coarse	61.83	1.499272198
Quad8 coarse	86.67	1.069574247
Quad4 fine	79.7	1.163111669
Quad8 fine	91.48	1.013336248
Triangular Shells:
Tria3 coarse	54.06	1.714761376
Tria6 coarse	97.07	0.954980942
Tria3 fine	74.21	1.249157795
Tria6 fine	96.64	0.959230132

Reference

NAFEMS R0015 - Selected benchmarks for natural frequency analysis