COMSOL 6.4 - Modeling Stress Dependent Elasticity

PDF

Modeling Stress Dependent Elasticity

In this example, you learn how to implement a material, in which the elastic modulus varies under compressive and tensile stress.

Model Definition

The geometry is a 10 cm by 1 cm cantilever, fixed at the left end. A pure bending moment (−5/3 Nm) is applied at the other end, which results in a linear stress distribution with peak values of 0.1 MPa.

The material model is a linear elastic, where Young’s modulus is a function of the sign of the mean stress (that is, the pressure). Under compression the material has an elastic modulus of 700 MPa, while under tension the elastic modulus drops to 300 MPa. The transition between the two values is assumed to be continuous between compressive and tensile stress, with a transition zone of 103 Pa.

In this example, Poisson’s ratio is assumed to be constant. This actually violates thermodynamic laws, and an accurate implementation would require a variable Poisson’s ratio too.

Results and Discussion

Figure 1 shows the von Mises stress in the cantilever at maximum loading. Note that the stress distribution is not symmetric as it would be with a constant elastic modulus. The von Mises stress is higher in the compression region, where the material has a higher stiffness.

Figure 1: Von Mises stress distribution.

Figure 2 shows the value of Young’s modulus. Note that the compressive region (in red) is thinner than the tensile one (in blue).

Figure 2: Distribution of mean stress dependent Young’s modulus.

Figure 3 shows the stress in the x direction across the section at x = 5 cm. The slope is steeper in the compressive stress region than in the tensile one. The neutral line between tensile and compressive stress regions has shifted from the middle of the cantilever.

Figure 3: Stress in x direction across the cantilever height (x = 5 cm).

Notes About the COMSOL Implementation

A stress dependent elastic modulus introduces a circular dependency as the stress tensor itself is a function of Young’s modulus and the strain tensor. A stress dependent Young’s modulus would lead to Hooke’s law being described as:

To solve the problem with the circular variable dependency, you need to introduce a new variable onto which the stress value is mapped. Use a weak contribution and an auxiliary dependent variable to map the computed pressure value to the new variable p. Finally, define the Young’s modulus as a function of this new variable p.

In this example, an easier solution would have been to reformulate the problem by instead making the Young’s modulus a function of the volumetric strain, so that

Such a reformulation, which is not always possible to find, avoids the circular dependency and a standard nonlinear problem is obtained.

To access the weak contribution feature, you need to activate the .

Structural_Mechanics_Module/Material_Models/stress_dependent_elasticity

Modeling Instructions

From the menu, choose .

In the window, click

.

1

In the window, click

.

2

In the tree, select > .

3

4

5

In the tree, select > .

6

Rectangle 1 (r1)

1

In the toolbar, click

.

2

In the window for , locate the section.

3

In the text field, type 10[cm].

4

In the text field, type 1[cm].

5

Solid Mechanics (solid)

1

In the toolbar, click

and choose .

2

Select Boundary 1 only.

Fixed Constraint 1

1

In the toolbar, click

and choose .

2

Select Point 1 only.

Boundary Load 1

1

In the toolbar, click

and choose .

2

Select Boundary 4 only.

3

In the window for , locate the section.

4

From the list, choose .

5

Specify the M vector as


-(5/3)[N*m]	z

6

button in the toolbar.

7

In the dialog, in the tree, select the checkbox for the node > .

8

Weak Contribution 1

1

In the toolbar, click

and choose .

2

Select Domain 1 only.

3

In the window for , locate the section.

4

In the text field, type test(p)*(p-solid.pm).

Auxiliary Dependent Variable 1

1

In the toolbar, click

and choose .

2

In the window for , locate the section.

3

In the text field, type p.

There is no need to enforce continuity for the mapped pressure, so using a Gauss-point shape function is a good choice.

4

Locate the section. From the list, choose .

5

Find the subsection. From the list, choose .

You will now define the material properties. As the study is stationary, you can assume the density to be zero.

Material 1 (mat1)

1

In the window, under right-click and choose .

2

In the window for , locate the section.

3

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Poisson’s ratio	nu	0.3	1	Young’s modulus and Poisson’s ratio
Density	rho	0	kg/m³	Basic

You will now create a step function. Later you will use this function to define the Young’s modulus with the input argument being the pressure.

4

In the window, expand the > node.

Piecewise 1 (pw1)

1

In the window, expand the node.

2

Right-click > > > and choose > .

3

In the window for , type E0 in the text field.

4

Locate the section. From the list, choose .

5

From the list, choose .

6

In the text field, type 1e3[Pa].

7

Find the subsection. In the table, enter the following settings:


Start	End	Function
-3000[Pa]	0	300[MPa]
0	3000[Pa]	700[MPa]

Material 1 (mat1)

1

In the window, under > > click .

2

In the window for , locate the section.

3

In the table, enter the following settings:


Property	Variable	Expression	Unit	Size
Young’s modulus	E	E0(p)	Pa	1x1

In the toolbar, click

.

1

Right-click and choose .

2

Select Boundary 1 only.

3

In the window for , locate the section.

4

In the text field, type 20.

1

In the window, right-click and choose .

2

Select Boundary 2 only.

3

In the window for , locate the section.

4

In the text field, type 50.

5

Solution 1 (sol1)

1

In the toolbar, click

.

2

In the window, expand the node.

3

In the window, expand the > > > node, then click .

4

In the window for , click to expand the section.

5

From the list, choose .

6

In the toolbar, click

.

1

In the window, expand the node, then click .

2

In the window for , locate the section.

3

From the list, choose .

The default plot shows the von Mises stress distribution, as shown in Figure 1.

Next, add a plot from to visualize the applied moment resulting in a linearly varying traction.

Result Templates

1

In the toolbar, click

to open the window.

2

Go to the window.

3

In the tree, select > > > .

4

Click the button in the window toolbar.

5

In the toolbar, click

to close the window.

Boundary Loads (solid)

Now create a new plot group for the Young’s modulus, to reproduce Figure 2.

Young’s Modulus

1

In the toolbar, click

.

2

In the window for , type Young's Modulus in the text field.

1

In the toolbar, click

.

2

In the window for , click in the upper-right corner of the section. From the menu, choose > > > .

3

Locate the section. From the list, choose .

Change also the quality settings to get a better visualization.

4

Click to expand the section. From the list, choose .

5

From the list, choose .

6

From the list, choose .

1

In the toolbar, click

.

2

Finally, display the stress variation through the thickness of the beam, Figure 3.

1

In the toolbar, click

.

2

In the window for , locate the section.

3

In row , set to 5[cm].

4

In row , set to 5[cm] and to 1[cm].

Stress Through Thickness

1

In the toolbar, click

.

2

In the window for , type Stress Through Thickness in the text field.

3

Locate the section. From the list, choose .

1

Right-click and choose .

2

In the window for , locate the section.

3

In the text field, type solid.sx.

4

From the list, choose .

5

In the toolbar, click

.