Home
Verification Problems
This manual presents solved verification models including NAFEMS problems.
NAFEMS Nonlinear Static Analysis
OS-V: 0250 3D Sheet Metal Forming
Contacts Benchmark 3 For quasi-static analysis using elastic plastic material, geometric non-linearity and nonlinear boundary conditions.

Welcome
What's New
View new features for OptiStruct 2024.
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
- NAFEMS Thermo-elastic
- NAFEMS Heat Transfer
- NAFEMS Nonlinear Static Analysis
  - OS-V: 0220 3D Punch (Rounded Edges)
    Contacts Benchmark 2 For quasi-static analysis using linear elastic material, geometric non-linearity and nonlinear boundary conditions.
  - OS-V: 0230 3D Loaded Pin
    Contacts Benchmark 4 For Quasi-static analysis using Linear elastic material, geometric non-linearity and nonlinear boundary conditions. OptiStruct FE results examine the plot of contact pressure, tangential stress and relative tangential slip against angle $θ$ .
  - OS-V: 0240 3D Steel Roller on Rubber
    Contacts Benchmark 5For quasi-static analysis using linear elastic material, geometric non-linearity and nonlinear boundary conditions.
  - OS-V: 0250 3D Sheet Metal Forming
    Contacts Benchmark 3 For quasi-static analysis using elastic plastic material, geometric non-linearity and nonlinear boundary conditions.
  - OS-V: 0260 Shell Bending under a Tip Load
    A beam is analyzed for bending due to tip load. OptiStruct investigates the vertical steady-state displacement at the tip of the beam.
  - OS-V: 0270 Torsional Creep of Circular Shaft
    This benchmark illustrates the structural response of a power law creeping material in a geometrical configuration subjected to pure torsion. OptiStruct examines strain at the edge of the shaft.
  - OS-V: 0280 Axisymmetric Elements - Interference Fit Between Two Cylinders
    The model examines the contact pressure between two cylinders in case of interference fit of 20 mm.
  - OS-V: 0290 Lee's Frame Postbuckling
    Examines the postbuckling behavior of an L-shaped frame (Lee’s frame) loaded by a vertical point load.
  - OS-V: 0291 Hertzian Contact - Elastic Sphere and Rigid Half-space
    Hertzian contact is demonstrated using OptiStruct for an elastic sphere and rigid half-space problem.
  - OS-V: 0292 Hertzian Contact - Rigid Sphere and Elastic Half Space, 2D Axisymmetric, S2S Contact
    Hertzian contact is demonstrated using OptiStruct for rigid sphere and elastic half-space –2D axisymmetric, S2S CONTACT.
  - OS-V: 0293 Hertzian Contact - Rigid Sphere and Elastic Half Space, S2S Contact with Smoothing
    Hertzian contact is demonstrated using OptiStruct for rigid sphere & elastic half space – S2S CONTACT with Smoothing.
- 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: 0250 3D Sheet Metal Forming

Contacts Benchmark 3 For quasi-static analysis using elastic plastic material, geometric non-linearity and nonlinear boundary conditions.

OptiStruct FE results examine the forming angle and angle after the punch is released. OptiStruct also examines the contact features of the rigid and deformable bodies and sliding contact around the circular surfaces.

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.

Benchmark Model

Hexa8 elements are used to create the half model of the sheet and Quad4 elements are used to model the punch and the die. The punch radius is 23.5 mm, the die radius is 25 mm, the die shoulder radius is 4 mm, width of the tool is 50 mm, length of sheet is 120 mm, sheet thickness is 1 mm and the width of the sheet is 30 mm. The punch stroke is 28.5 mm. The bottom surface is fixed. Two different contact properties are used, one with coefficient of friction 0.0 and the second with coefficient of friction 0.1342. For the contacts between the punch and the sheet, punch is considered as main surface and the sheet as secondary and for the contacts between the die and the sheet die is considered as main and sheet as secondary.

The material properties are:

Material Properties: Value
E: 70.5 kN/mm²
$υ$: 0.342
$σ$ ₀ (Initial yield stress): 194 N/mm²
Hollomon hardening: $σ$ =K x $ε$ ⁿ; K = 550.4 N/mm²; n = 0.223

Nonlinear Static Analysis Results

Characteristic angles during process.


Frictional Coefficient=0	NAFEMS	OptiStruct Results	Normalized
Forming angle	21.88	20.50	1.067317
Angle after release	48.38	45.53	1.062596


Frictional Coefficient=0.1348	NAFEMS	OptiStruct Results	Normalized
Forming angle	21.84	22.437	0.973392
Angle after release	54.45	43.22	1.259833

Reference

NAFEMS R0094 - Advanced finite element contact benchmarks, Konter 2006