PDF
Pressurized Orthotropic Container
Introduction
A container made of rolled steel is subjected to an internal overpressure. As an effect of the manufacturing method, 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. The model also shows how to define and use curvilinear coordinates aligned with the principal directions of the material, which in this case follow the contours of the container.
Model Definition
The 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.
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.
Figure 1: Schematic description of the container geometry and dimensions.
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 shape of the component, see Figure 2.
Figure 2: Orientation of the local material coordinate system. The second principal direction is oriented in the circumferential direction, perpendicular to the rz-plane.
The Curvilinear Coordinates interface is used to compute an orthogonal system of coordinates that follow the shape of the container.
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 the internal pressure p:
(1)
Following Hill’s criterion, 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 31.4 MPa. For isotropic steel with a yield stress of 381 MPa, the 10% yielded volume is reached when p = 29 MPa. Therefore, with orthotropic steel, the pressure needed to reach 10% yielded volume is about 8% higher than when using isotropic steel. The extent of plastic strains is shown also 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
Hill orthotropic plasticity is available in COMSOL as a built-in option in the Plasticity 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.
A coordinate system that follows the geometrical shape is created by the Curvilinear Coordinates interface. For axisymmetric geometries, the new base vectors, x1 and x3, are computed for the geometry. In a case of geometric nonlinearity, the coordinates R and Z define the positions with respect to the initial configuration (material frame) whereas r and z define the positions with respect to the deformed configuration (spatial frame). Generally, material properties are defined in terms of the initial configuration. To assign the new base vector system to the component, select Curvilinear System from the Coordinate system list in the Settings window for Linear Elastic Material.
Figure 5 visualizes the base vector system defined by the curvilinear system using an arrow surface plot. 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 of the inner surface is oriented to the interior of the container, which enables to directly apply the inner pressure load, see Figure 6,
Figure 5: Orientation of the curvilinear 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.
Application Library path: Nonlinear_Structural_Materials_Module/Plasticity/orthotropic_container
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D Axisymmetric.
2
In the Select Physics tree, select Mathematics > Curvilinear Coordinates (cc).
3
Click Add.
4
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies > Stationary.
8
Click  Done.
Global Definitions
Load the parameters from the appended file.
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file orthotropic_container_parameters.txt.
Definitions
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Selection list, choose All domains.
4
Locate the Advanced section. From the Frame list, choose Material  (R, PHI, Z).
Variables 1
1
In the Model Builder window, right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
y_vol
intop1(solid.epe>0)/intop1(1)
 
Yielded volume fraction
Geometry 1
Circle 1 (c1)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type Rc.
4
In the Sector angle text field, type alpha.
5
Locate the Position section. In the z text field, type sf-(Rc-hi).
6
Locate the Rotation Angle section. In the Rotation text field, type 90-alpha.
Circle 2 (c2)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type Rc+th.
4
In the Sector angle text field, type alpha.
5
Locate the Position section. In the z text field, type sf-(Rc-hi).
6
Locate the Rotation Angle section. In the Rotation text field, type 90-alpha.
Crown
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
In the Settings window for Difference, type Crown in the Label text field.
3
Select the object c2 only.
4
Locate the Difference section. Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object c1 only.
Circle 3 (c3)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type Rk+th.
4
In the Sector angle text field, type 90-alpha.
5
Locate the Position section. In the r text field, type Ri-Rk.
6
In the z text field, type sf.
7
Click  Build Selected.
Circle 4 (c4)
1
In the Geometry toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type Rk.
4
In the Sector angle text field, type 90-alpha.
5
Locate the Position section. In the r text field, type Ri-Rk.
6
In the z text field, type sf.
7
Click  Build Selected.
Knuckle
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object c3 only.
3
In the Settings window for Difference, locate the Difference section.
4
Click to select the  Activate Selection toggle button for Objects to subtract.
5
Select the object c4 only.
6
Click  Build Selected.
7
In the Label text field, type Knuckle.
Flange
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, type Flange in the Label text field.
3
Locate the Size and Shape section. In the Width text field, type th.
4
In the Height text field, type sf.
5
Locate the Position section. In the r text field, type Ri.
6
Click  Build All Objects.
Klöpper Head
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
In the Settings window for Union, type Klöpper Head in the Label text field.
3
Click in the Graphics window and then press Ctrl+A to select all objects.
4
Locate the Union section. Clear the Keep interior boundaries checkbox.
5
Click  Build All Objects.
Cylinder
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, type Cylinder in the Label text field.
3
Locate the Size and Shape section. In the Width text field, type th.
4
In the Height text field, type hcyl.
5
Locate the Position section. In the r text field, type Ri.
6
In the z text field, type -hcyl.
7
Click  Build All Objects.
Curvilinear Coordinates (cc)
1
In the Model Builder window, under Component 1 (comp1) click Curvilinear Coordinates (cc).
2
In the Settings window for Curvilinear Coordinates, locate the Settings section.
3
Select the Create base vector system checkbox.
Diffusion Method 1
In the Physics toolbar, click  Domains and choose Diffusion Method.
Inlet 1
1
In the Physics toolbar, click  Attributes and choose Inlet.
2
In the Settings window for Inlet, locate the Boundary Selection section.
3
Click  Clear Selection.
4
Select Boundary 1 only.
Diffusion Method 1
In the Model Builder window, click Diffusion Method 1.
Outlet 1
1
In the Physics toolbar, click  Attributes and choose Outlet.
2
In the Settings window for Outlet, locate the Boundary Selection section.
3
Click  Clear Selection.
4
Select Boundary 3 only.
Solid Mechanics (solid)
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
Symmetry Plane 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry Plane.
2
Select Boundary 3 only.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 2, 4, 8, and 10 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Pressure.
5
In the p text field, type pressure.
Linear Elastic Material 1
1
In the Model Builder window, click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Coordinate System Selection section.
3
From the Coordinate system list, choose Curvilinear System (cc) (cc_cs).
Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, locate the Plasticity Model section.
3
From the σe list, choose Hill orthotropic.
4
From the σys0 list, choose Reciprocal average.
5
From the εpe list, choose von Mises.
6
Find the Isotropic hardening model subsection. From the list, choose Perfectly plastic.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Steel AISI 4340.
4
Click the Add to Component button in the window toolbar.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Steel AISI 4340 (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
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 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 1 only.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Boundaries 4, 7, 10, and 11 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 10.
Distribution 3
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 25.
4
Select Boundaries 2, 6, 8, and 9 only.
5
Click  Build All.
6
In the Model Builder window, click Mesh 1.
The mesh should consist of 350 quadrilateral elements, with 5 elements through the thickness. Finer elements are created at the knuckle since stress gradients are expected there.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkbox for Solid Mechanics (solid).
Step 2: Stationary 2
1
In the Study toolbar, click  Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
In the Solve for column of the table, under Component 1 (comp1), clear the checkbox for Curvilinear Coordinates (cc).
Set up an auxiliary continuation sweep for the pressure parameter.
4
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
pressure (Internal pressure)
range(16, 0.2, 36)
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
Introduce a stop condition to stop the solver when a certain amount of material has yielded.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 2 node.
4
Right-click Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 2 > Parametric 1 and choose Stop Condition.
5
In the Settings window for Stop Condition, locate the Stop Expressions section.
6
Click  Add.
7
In the table, enter the following settings:
Stop expression
Stop if
Active
Description
0.1-comp1.y_vol
Negative (<0)
√
Stop expression 1
Specify that the solution is to be stored both before and after the stop condition is reached.
8
Locate the Output at Stop section. From the Add solution list, choose Steps before and after stop.
9
In the Study toolbar, click  Compute.
Results
Streamline 1
1
In the Model Builder window, expand the Results > Vector Field (cc) node, then click Streamline 1.
2
In the Settings window for Streamline, locate the Streamline Positioning section.
3
In the Density level text field, type 10.9.
4
In the Vector Field (cc) toolbar, click  Plot.
Material Principal Direction
1
In the Model Builder window, under Results click Coordinate system (cc).
2
In the Settings window for 2D Plot Group, type Material Principal Direction in the Label text field.
3
Click to expand the Title section. From the Title type list, choose None.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Equivalent Plastic Strain (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Equivalent Plastic Strain (solid)
1
In the Equivalent Plastic Strain (solid) toolbar, click  Plot.
2
In the Model Builder window, under Results click Equivalent Plastic Strain (solid).
The onset of plasticity can be investigated by evaluating the volume of the material which has exceeded the yield stress.
Yielded Volume
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Yielded Volume in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Custom.
4
Find the Type and data subsection. Clear the Type checkbox.
5
Clear the Unit checkbox.
6
Locate the Plot Settings section.
7
Select the x-axis label checkbox. In the associated text field, type Pressure (N/m<sup>2</sup>).
Global 1
1
Right-click Yielded Volume and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
y_vol
1
Yielded volume fraction
4
Click to expand the Legends section. Clear the Show legends checkbox.
5
In the Yielded Volume toolbar, click  Plot.
Set default units for result presentation.
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
8
Select the Apply conversions to expressions with the same dimensions checkbox.
9
Click  Apply.
Stress, 3D (solid)
1
In the Model Builder window, under Results click Stress, 3D (solid).
2
In the Settings window for 3D Plot Group, locate the Color Legend section.
3
Select the Show units checkbox.
4
In the Stress, 3D (solid) toolbar, click  Plot.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Solid Mechanics > Applied Loads (solid).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.