Price Free!

Project Overview

In this training, we first perform a finite element analysis of a thick-walled cylinder subjected to internal pressure using the Abaqus software. Then, the numerical results are compared with the Analytical Solution based on Lamé's equations to evaluate the accuracy of the simulation.

The main objective is to investigate the distribution of radial stress and hoop stress across the cylinder wall and compare their values at the inner and outer surfaces.

Thick-walled cylinder model subjected to internal pressure
Thick-walled cylinder model considered in the problem.

Model Description

The model consists of a thick-walled steel cylinder with an inner radius of 50 mm, an outer radius of 100 mm, and a length of 200 mm.

The cylinder is subjected to an internal pressure of 10 MPa, while the external pressure is zero.

The material is assumed to be homogeneous, isotropic, and linearly elastic. The material properties are defined as follows: Young's modulus is 210,000 MPa and Poisson's ratio is 0.3.

Since the wall thickness is large compared to the inner radius, the cylinder is classified as a thick-walled cylinder. Therefore, Lamé's equations are used to calculate the analytical radial and hoop stress distributions.

Geometry and dimensions of the thick-walled cylinder
Geometry and dimensions of the thick-walled cylinder.

Abaqus Simulation

First, the cylinder is modeled in the Abaqus software using a two-dimensional Axisymmetric formulation.

The internal pressure is applied to the inner surface of the cylinder, and a static stress analysis is performed to obtain the stress distribution throughout the cylinder wall.

The model is discretized using CAX4R elements. A mesh size of 1 mm is used to obtain more accurate numerical results.

Radial and Hoop Stress Results

After completing the analysis, the radial and hoop stresses are extracted from the Abaqus results.

The radial stress is compressive at the inner surface due to the applied internal pressure and approaches zero at the outer surface.

The hoop stress is tensile throughout the cylinder wall. Its maximum value occurs at the inner surface and decreases toward the outer surface.

Radial stress distribution in the thick-walled cylinder
Radial stress distribution obtained from Abaqus.
Hoop stress distribution in the thick-walled cylinder
Hoop stress distribution obtained from Abaqus.

Analytical Solution

Next, the radial and hoop stresses are calculated using the Analytical Solution based on Lamé's equations for thick-walled cylinders.

The radial and hoop stress distributions are given by:

σr = A − B / r2

σθ = A + B / r2

The constants A and B are calculated using the following equations:

A = (Pia2 − Pob2) / (b2 − a2)

B = a2b2(Pi − Po) / (b2 − a2)

In these equations, Pi and Po represent the internal and external pressures, respectively. The parameters a and b are the inner and outer radii, and r is the radial coordinate.

For the given cylinder, the calculated constants are:

A = 3.3333 MPa

B = 33,333.3333 MPa·mm²

Therefore, the analytical stress distributions are:

σr = 3.3333 − 33,333.3333 / r2

σθ = 3.3333 + 33,333.3333 / r2

The radial coordinate r is expressed in millimeters, and the resulting stresses are obtained in MPa.

At the inner surface, the analytical radial and hoop stresses are −10 MPa and 16.667 MPa, respectively.

At the outer surface, the corresponding values are 0 MPa and 6.667 MPa.

Analytical calculation of radial and hoop stresses using Lame equations
Analytical solution based on Lamé's equations.

Comparison of Results

Finally, the stress values obtained from the Abaqus simulation are compared with those calculated using the Analytical Solution.

The comparison is performed at the inner and outer surfaces of the cylinder. The numerical results show good agreement with the analytical values.

Stress Component
Abaqus (MPa)
Analytical (MPa)
Difference
Radial Stress – Inner
−9.74
−10.00
2.6%
Radial Stress – Outer
0.03
0.00
-
Hoop Stress – Inner
16.41
16.667
1.54%
Hoop Stress – Outer
6.70
6.667
0.5%

The relative differences between the Abaqus and analytical results are approximately 2.6% for the radial stress at the inner surface, 1.54% for the hoop stress at the inner surface, and 0.5% for the hoop stress at the outer surface.

For the radial stress at the outer surface, the analytical value is zero. Therefore, the absolute difference of 0.03 MPa is reported instead of a percentage.

These results demonstrate good agreement between the finite element simulation and the analytical solution.

What You Will Learn

  • How to model a thick-walled cylinder in Abaqus.
  • How to define material properties in Abaqus.
  • How to apply internal pressure to a cylindrical structure.
  • How to define a axisymmetric model using CAX4R elements.
  • How to perform a static stress analysis.
  • How to obtain radial and hoop stresses from Abaqus results.
  • How to calculate radial and hoop stresses using Lamé's equations.
  • How to determine the stress distribution across the cylinder wall.
  • How to compare numerical results with the Analytical Solution.
  • How to evaluate the accuracy of a finite element model.

Key Features

  • Thick-walled cylinder subjected to internal pressure.
  • Two-dimensional axisymmetric finite element model.
  • Linear elastic material behavior.
  • Radial and hoop stress analysis.
  • Analytical Solution based on Lamé's equations.
  • Numerical simulation using Abaqus.
  • Stress comparison at the inner and outer surfaces.
  • Mesh refinement to improve numerical accuracy.
  • Comparison between Abaqus and Analytical Solution.
Files Included
What you will receive after purchase
File Type
Content
Description
🧩 Abaqus
CAE File
Complete Abaqus model
📄 Abaqus
INP File
Abaqus input file
🎥 Video
Full Video
Step-by-step explanation of the project

Project Information

Important information about this project

🎥
Video Tutorial Available
📦
Project Type Training Project
💻
Abaqus Version Abaqus 2017
🌐
Language English
📥
Access Free

Payment & Support

Need help with this project?

🎓

Project Support

If you need assistance with this project or have questions about the Abaqus model, please contact us.

✉️

Need Help?

For questions and technical support, please contact us by email.

saeedofmoeini@gmail.com

chat_bubble_outlineReviews

There are no reviews yet.

Be the first to review “Radial and Hoop Stress Analysis of a Thick-Walled Cylinder Under Internal Pressure | Abaqus vs. Analytical Solution”

Your email address will not be published. Required fields are marked *