COMSOL 6.4 - Pressurized Orthotropic Container

Pressurized Orthotropic Container — Shell Version

A container made of rolled steel is subjected to an internal overpressure. As an effect of the manufacturing method of the steel sheet, one of the three material principal directions — the out-of- plane direction — has a higher yield stress than the other two. Hill’s orthotropic plasticity is used to model the differences in yield strength.

This example demonstrates how to perform the analysis of the container using the interface and the model.

Model Definition

The metal container has the shape of a cylinder capped by two torispherical heads (also called Klöpper head). The cylinder has an internal radius of Ri = 24 cm, a height of h = 80 cm, and its thickness is t = 2 cm. The torispherical head is made out of three parts: the crown, the knuckle and the flange. The crown has an internal radius of Rc = 43.2 cm, the knuckle has an internal radius of Rk = 5.2 cm, and the straight flange is s = 7 cm in height, see Figure 1

Figure 1: Schematic description of the container geometry and dimensions.

Because of 2D axial symmetry and reflection symmetry, it is sufficient to model a quarter of the container; see Figure 1. The red lines define the rotation symmetry axis and the reflection symmetry axis.

Material Model

The elastoplastic material is defined by a Young’s modulus, E = 205 GPa and a Poisson’s ratio, ν = 0.28. Hill’s orthotropic plasticity governs the yielding, with the yield stress components given by

There is no hardening, so the material is perfectly plastic. The numbers in the subscripts denote the principal material directions, as indicated in the following section.

Material Orientation

The rolled steel sheet has better mechanical properties in the out-of-plane direction, direction 3. To account for this anisotropy, use a special coordinate system that follows the component shape has to be used; see Figure 2. When using the Shell interface, this coordinate system coincides with the local coordinates of the shell.

Figure 2: Orientation of local material coordinate system. The second principal direction is oriented in the circumferential (out-of-plane) direction, perpendicular to the rz-plane.

Results and Discussion

An approximate analytical solution can be obtained for the cylindrical part of the container. The principal stresses in the center of the container can be estimated from the internal radius Ri, the wall thickness t and internal pressure p:

(1)

Following Hill’s criterion, the yielding occurs when

or replacing by the expressions in Equation 1

The material parameters, F = G = 2.47·10−18 1/Pa2 and H = 4.42·10−18 1/Pa2, give the analytical onset of yielding in the center of the cylinder at p = 37.8 MPa. Given the curvature of the knuckle, the material in the torispherical head undergoes plastic deformation below this onset pressure.

Figure 3 shows the von Mises stress at 10% yielded volume, which happens when the inner pressure reaches 30.4 MPa. For isotropic steel with yield stress of 381 MPa, the 10% yielded volume is reached when p = 28.4 MPa. Therefore, with orthotropic steel, the pressure needed to reach 10% yielded volume is about 7% higher than when using an isotropic steel sheet. The extent of plastic strains is shown in Figure 4.

Figure 3: Distribution of von Mises stress at 10% yielded volume.

Figure 4: Equivalent plastic strain at 10% yielded volume.

Notes About the COMSOL Implementation

The structure is modeled with the interface and the model. This feature enables to model phenomena that are thickness dependent, such as . The user interface is similar to what is available in the interface.

Hill orthotropic plasticity is available in COMSOL as a built-in option under the node, where either Hill’s coefficients or initial yield stresses can be given. The yield strength values can also be specified in the material node.

Figure 5 visualizes the boundary system and the thickness of the shell. The red arrows denote direction 1, while the blue arrows denote direction 3. The out-of-plane direction is used as direction 2 (not plotted). The normal is oriented to the interior of the container, which enables to directly apply the inner pressure load, see Figure 6.

Figure 5: Thickness of the shell and orientation of the boundary system.

Figure 6: Orientation and amplitude of the applied pressure load.

A stop condition is added to the parametric solver, so that the simulation stops when 10% of the material has exceeded the yield limit. Unless you are performing a failure analysis, it is not necessary to compute the whole plastic history, and the stop condition saves much computation time from being spent in the strongly nonlinear regime.

Nonlinear_Structural_Materials_Module/Plasticity/orthotropic_container_shell

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > .

Click .

Click

In the tree, select > .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file orthotropic_container_parameters.txt.

Geometry 1

Crown

In the toolbar, click

and choose .

In the window for , type Crown in the text field.

Locate the section. In the text field, type sf-(Rc-hi).

Locate the section. In the text field, type Rc.

Locate the section. In the text field, type 90-alpha.

Knuckle

In the toolbar, click

and choose .

In the window for , type Knuckle in the text field.

Locate the section. In the text field, type Ri-Rk.

In the text field, type sf.

Locate the section. In the text field, type Rk.

Locate the section. In the text field, type 90-alpha.

Flange

In the toolbar, click

and choose .

In the window for , type Flange in the text field.

Locate the section. From the list, choose .

In the text field, type Ri.

In the text field, type sf.

Locate the section. From the list, choose .

In the text field, type Ri.

Cylinder

In the toolbar, click

and choose .

In the window for , type Cylinder in the text field.

Locate the section. From the list, choose .

In the text field, type Ri.

Locate the section. From the list, choose .

In the text field, type Ri.

In the text field, type -hcyl.

Click

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

Variables 1

In the toolbar, click

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
y_vol	intop1(shell.llem1.xdintopall(shell.epe>0))/intop1(shell.llem1.xdintopall(1))		Yielded volume fraction

The shell.llem1.xdintopall operator integrates the argument quantity across the thickness.

Set the boundary system to have the first tangent vector oriented upward and the normal oriented to the interior as shown on Figure 5. The latter will make it easier to apply the internal pressure.

Boundary System 1 (sys1)

In the window, click .

In the window for , locate the section.

Find the subsection. From the list, choose .

Select the checkbox.

Shell (shell)

Linear Elastic Material, Layered 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Plasticity 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the σe list, choose .

From the σys0 list, choose .

From the εpe list, choose .

Find the subsection. From the list, choose .

Symmetry Plane 1

In the toolbar, click

and choose .

Select Point 3 only.

Face Load 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

In the p text field, type pressure.

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Materials

Steel AISI 4340 (mat1)

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Thickness	lth	th	m	Shell
Initial tensile and shear yield stresses	{ys1, ys2, ys3, ys4, ys5, ys6}	{381[MPa],381[MPa],450[MPa],240[MPa],240[MPa],220[MPa]}	N/m²	Elastoplastic material model
Mesh elements	lne	5	1	Shell