VMMECH002

VMMECH002
Rectangular Plate with Circular Hole Subjected to Tensile Loading

Overview

Reference:J. E. Shigley, Mechanical Engineering Design, McGraw-Hill, 1st Edition, 1986, Table A-23, Figure A-23-1, pg. 673
Solver(s)
ANSYS AIM
ANSYS Mechanical
Analysis Type(s):Linear Static Structural Analysis
Element Type(s):Solid

Test Case

A rectangular plate with a circular hole is fixed along one of the end faces and a tensile pressure load is applied on the opposite face. A convergence with an allowable change of 10% is applied to account for the stress concentration near the hole. The Maximum Refinement Loops is set to 2 and the Refinement mesh control is added on the cylindrical surfaces of the hole with Refinement = 1.

Find the Maximum Normal Stress in the x direction on the cylindrical surfaces of the hole.

Material PropertiesGeometric PropertiesLoading
E = 1000 Pa
ν = 0
Length = 15 m
Width = 5 m
Thickness = 1 m
Hole radius = 0.5 m
Pressure = -100 Pa

Analysis Assumptions and Modeling Notes for ANSYS Mechanical

The following figure shows the finite element model in ANSYS Mechanical:

Figure 59:  ANSYS Mechanical Schematic

ANSYS Mechanical Schematic

Results Comparison for ANSYS Mechanical

ResultsTargetMechanicalError (%)
Maximum Normal X Stress (Pa)312.5314.80.736

Analysis Assumptions and Modeling Notes for ANSYS AIM

The following figure shows the finite element model in ANSYS AIM:

Figure 60:  ANSYS AIM Schematic

ANSYS AIM Schematic

Results Comparison for ANSYS AIM

ResultsTargetAIMError (%)
Maximum Normal X Stress (Pa)312.5310.755-0.559

Release 18.2 - © ANSYS, Inc. All rights reserved.