COMSOL 6.4 - Uniaxial Stretching of a Rectangular Sheet

Uniaxial Stretching of a Rectangular Sheet

Wrinkling is a commonly occurring phenomenon in thin sheets, caused by either loading or manufacturing defects. The numerical treatment of wrinkles in thin structures can be approached using the following two theories:

•

Membrane theory along with tension field theory — Membrane theory models wrinkles as a mean surface and gives a correct stress distribution in the wrinkled region. This is computationally inexpensive compared to shell theory, but the wrinkle amplitudes and wavelengths cannot be obtained. An example of modeling wrinkling in a rectangular sheet using the Membrane interface can be found in the Structural Mechanics Module Application Library model Uniaxial Stretching of a Rectangular Membrane.

•

Shell theory — As wrinkling is a local buckling phenomenon, nonlinear postbuckling analysis is needed to find the amplitudes and wavelengths of the wrinkles. This modeling approach is nontrivial and computationally expensive.

In this example, wrinkling in a thin rectangular sheet is modeled using a shell theory. First, a static analysis is performed to determine the region of negative principal stresses without assuming wrinkles. The negative principal stress is a prerequisite for the occurrence of wrinkles. Next, a prestressed buckling analysis is carried out to find out the potential linearized buckling modes. Finally, a nonlinear postbuckling analysis is carried out to investigate the evolution of wrinkles. The example is taken from Ref. 1, with which the results obtained here are compared.

Model Definition

A rectangular sheet 25 cm in length, 10 cm in width, and 0.1 mm thick is stretched in the longitudinal direction.

One of the short edges is fixed, while a prescribed displacement is applied on the opposite edge. The long edges are unconstrained.

The sheet is made of an incompressible neo-Hookean hyperelastic material with a Lame parameter of 6 MPa.

Results and Discussions

The example is based on Ref. 1 and Ref. 2 with some modifications. The authors (see Ref. 2) used 100,000 quadrilateral mesh elements, whereas we use 12,500 elements to save computation time. The nominal strain at which wrinkling starts in the postbuckling analysis depends on the mesh distribution, as reported in Ref. 2 (although the variation is small). Also the buckling modes and the critical factor depend on the mesh distribution. The authors in Ref. 1 reported that the numerical results of the postbuckling analysis depends on the number of modes used as geometric imperfection, as well as on their amplitudes. They have considered four buckling modes and an amplitude equal to 0.1% of the sheet thickness. In this example, four buckling modes are also used but the amplitude varies for each mode. A lower factor is assigned to the higher modes to reduce their influence.

Figure 1 shows the regions of negative transverse stress, called wrinkled regions, for different values of the nominal strain. A static analysis is carried out without any assumption of wrinkles. The occurrence of negative transverse stress shows the possibility of wrinkling. The size of the wrinkled region is reduced with increasing nominal strain. Figure 2 and Figure 3 show the variation of the transverse stress along a central longitudinal and a transverse line, respectively, for different nominal strains. The results are similar to those presented in Ref. 1.

Figure 4 through Figure 7 show the different wrinkling or buckling modes computed in the prestressed buckling analysis. The modes are computed using a nominal strain of 1%, which is the same as in Ref. 1.

Figure 8 shows the wrinkles produced in the postbuckling analysis with different nominal strains. It can be seen that the wrinkle amplitude increases initially and then decreases, which is consistent with results presented in Ref. 1. This behavior becomes clearer in Figure 9, where the wrinkle amplitude is plotted along the transverse line for different nominal strains. The results are consistent with those in the corresponding figure in Ref. 1. The wrinkle amplitude is at a maximum at the center due to the symmetries of the model. At the nominal strain 30%, the wrinkled amplitude becomes very small. As in Ref. 1, when the wrinkle amplitude is plotted against the nominal strain (see Figure 10), a bell-shaped curve is observed. The amplitude values are close to those of Ref. 1. Some small differences are observed due to the modeling differences discussed above.

Figure 1: Wrinkled region in the static analysis.

Figure 2: Transverse stress along the longitudinal line in the static analysis.

Figure 3: Transverse stress along the transverse line in the static analysis.

Figure 4: First mode shape in the prestressed buckling analysis.

Figure 5: Second mode shape in the prestressed buckling analysis.

Figure 6: Third mode shape in the prestressed buckling analysis.

Figure 7: Fourth mode shape in the prestressed buckling analysis.

Figure 8: Out of plane displacement in the postbuckling analysis.

Figure 9: Wrinkle amplitude in the postbuckling analysis.

Figure 10: Wrinkle amplitude versus nominal strain in the postbuckling analysis.

Notes About the COMSOL Implementation

The sheet will easily buckle under compressive loads, so modes with a small negative critical load factors are not the desired ones. To find the actual wrinkling modes using the study, the settings in the node must be tuned. The results in Ref. 1 and Ref. 2 show that wrinkles appear in the sheet at nominal strains around 1% to 5%. The sheet has a prestretch of 1%, which means that the critical load factor is around 1 for the wrinkling modes. Hence, in the node, enter 1 in the text field . Also, set the to .

The settings for the postbuckling analysis are made easier by the node. It contains a section that allows choosing the buckling solution and modes that will define the prescribed displacements. The button generates one node for each structural mechanics physics interface involved, and sets the prescribed deformations with the variables defined by the node. The prescribed deformations are those computed in the linear buckling study multiplied by the scale factor. Low values of the scale factor make the buckling effect sharper, at the expense of the convergence properties.

References

1. V. Nayyar, K. Ravi-Chandar, and R Huang, “Stretch-induced stress patterns and wrinkles in hyperelastic thin sheets,” Int. J. Solids Struct., vol. 48, pp. 3471–3483, 2011.

2. V. Nayyar, “Stretch-induced compressive stress and wrinkling in elastic thin sheets,” Master’s Thesis, The University of Texas at Austin, Austin, TX, 2010.

Nonlinear_Structural_Materials_Module/Hyperelasticity/sheet_uniaxial_stretching

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

Geometric Parameters

In the window, under click .

In the window for , type Geometric Parameters in the text field.

Locate the section. In the table, enter the following settings:


Name	Expression	Value	Description
mu	6[MPa]	6E6 Pa	Lame parameter
W	10[cm]	0.1 m	Width of sheet
alpha	2.5	2.5	Aspect ratio of sheet
L	alpha*W	0.25 m	Length of sheet
th	W/1000	1E-4 m	Thickness of sheet
numX	L/1[mm]	250	Number of mesh elements in X direction
numY	W/2[mm]	50	Number of mesh elements in Y direction
nominalStrain	1[%]	0.01	Nominal strain
geomImpFactor	1E4	10000	Geometric imperfection factor

Geometry 1

Work Plane 1 (wp1)

In the toolbar, click

Work Plane 1 (wp1) > Plane Geometry

In the window, click .

Work Plane 1 (wp1) > Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type L.

In the text field, type W.

Click

Add longitudinal and transverse central lines for result evaluation.

Work Plane 1 (wp1) > Line Segment 1 (ls1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the text field, type 0.5*W.

Locate the section. From the list, choose .

In the text field, type L.

In the text field, type 0.5*W.

Work Plane 1 (wp1) > Line Segment 2 (ls2)

Right-click > > > > and choose .

In the window for , locate the section.

In the text field, type 0.5*L.

In the text field, type 0.

Locate the section. In the text field, type 0.5*L.

In the text field, type W.

Click

Definitions

Maximum 1 (maxop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Minimum 1 (minop1)

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Shell (shell)

Hyperelastic Material, Layered 1

In the toolbar, click

and choose .

Select Boundary 1 only.

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

Fixed Constraint 1

In the toolbar, click

and choose .

Select Edges 1 and 3 only.

Prescribed Displacement/Rotation 1

In the toolbar, click

and choose .

Select Edges 11 and 12 only.

In the window for , locate the section.

From the list, choose .

In the u 0 x text field, type nominalStrain*L.

From the list, choose .

Materials

Material 1 (mat1)

In the window, under right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Lamé parameter μ	muLame	mu	N/m²	Lamé parameters
Density	rho	500	kg/m³	Basic
Thickness	lth	th	m	Shell
Mesh elements	lne	1	1	Shell

Mesh 1

Mapped 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Distribution 1

Right-click and choose .

Select Edges 1 and 3 only.

In the window for , locate the section.

In the text field, type numY/2.

Distribution 2

In the window, right-click and choose .

Select Edges 2 and 7 only.

In the window for , locate the section.

In the text field, type numX/2.

Click

Study: Static Analysis

In the window, click .

In the window for , locate the section.

Clear the checkbox.

In the text field, type Study: Static Analysis.

Step 1: Stationary

In the window, under click .

In the window for , click to expand the section.

Select the checkbox.

Click

In the table, enter the following settings:


Parameter name	Parameter value list	Parameter unit
nominalStrain (Nominal strain)	range(0,2.5,30)	%

In the toolbar, click

Results

Layered Material 1

In the window, expand the node.

Right-click > and choose > .

Wrinkled Region, Comparison (Static Analysis)

In the toolbar, click

In the window for , type Wrinkled Region, Comparison (Static Analysis) in the text field.

Locate the section. From the list, choose .

From the list, choose .

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

Locate the section. Clear the checkbox.

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

In the text field, type 0.5.

Surface 1

Right-click and choose .

In the window for , locate the section.

In the text field, type shell.syy<=0.

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

From the list, choose .

Solution Array 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

In the list, choose , , , and .

Locate the section. From the list, choose .

Wrinkled Region, Comparison (Static Analysis)

In the window, under click .

Table Annotation 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

In the table, enter the following settings:


x-coordinate	y-coordinate	z-coordinate	Annotation
0.3*L	0	0	Strain = 5%
1.6*L	0	0	Strain = 10%
0.3*L	2.2*W	0	Strain = 20%
1.6*L	2.2*W	0	Strain = 30%

Locate the section. Clear the checkbox.

Wrinkled Region, Comparison (Static Analysis)

Click the

button in the toolbar.

In the window, click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Click the

button in the toolbar.

Click the

button in the toolbar.

Click the

button in the toolbar.

Transverse Stress, Longitudinal Line (Static Analysis)

In the toolbar, click

In the window for , type Transverse Stress, Longitudinal Line (Static Analysis) in the text field.

Locate the section. From the list, choose .

In the text field, type 3,5,9,13.

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

Locate the section. Select the checkbox.

In the text field, type -0.02.

In the text field, type 1.02.

In the text field, type -0.005.

In the text field, type 0.005.

Line Graph 1

Right-click and choose .

Select Edges 4 and 9 only.

In the window for , locate the section.

In the text field, type gpeval(4,shell.atxd1(0,mean(shell.syy)))/shell.Eequ.

Select the checkbox. In the associated text field, type Nondimensional Cauchy stress, yy component.

Locate the section. From the list, choose .

In the text field, type X/L.

Click to expand the section. Select the checkbox.

In the toolbar, click

Transverse Stress, Transverse Line (Static Analysis)

In the toolbar, click

In the window for , type Transverse Stress, Transverse Line (Static Analysis) in the text field.

Locate the section. From the list, choose .

In the text field, type 3,5,9,13.

Locate the section. From the list, choose .

Locate the section. Select the checkbox.

In the text field, type -0.02.

In the text field, type 1.02.

In the text field, type -0.0008.

In the text field, type 0.0005.

Line Graph 1

Right-click and choose .

Select Edges 6 and 8 only.

In the window for , locate the section.

In the text field, type gpeval(4,shell.atxd1(0,mean(shell.syy)))/shell.Eequ.

Select the checkbox. In the associated text field, type Nondimensional Cauchy stress, yy component.

Locate the section. From the list, choose .

In the text field, type Y/W.

Locate the section. Select the checkbox.

In the toolbar, click

Add Study

In the toolbar, click

to open the window.

Go to the window.

Find the subsection. In the tree, select > .

Right-click and choose .

In the toolbar, click

to close the window.

Study: Prestressed Buckling Analysis

In the window for , type Study: Prestressed Buckling Analysis in the text field.

Solution 2 (sol2)

In the toolbar, click

Step 2: Linear Buckling

In the window, under click .

In the window for , locate the section.

In the text field, type 10.

Locate the section. From the list, choose .

From the list, choose .

Solution 2 (sol2)

In the window, expand the > > node.

In the window, under > > click .

In the window for , locate the section.

In the text field, type 1.

From the list, choose .

In the toolbar, click

Results

Mode Shape (Prestressed Buckling Analysis)

In the window for , type Mode Shape (Prestressed Buckling Analysis) in the text field.

In the toolbar, click

Now, prescribe a deformation to the geometry from the calculated buckling modes to perform a postbuckling analysis.

Definitions (comp1)

Buckling Imperfection 1 (bcki1)

In the toolbar, click

and choose .

In the window for , locate the section.

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


Mode	Scale factor
1	geomImpFactor
2	geomImpFactor/5
3	geomImpFactor/10
4	geomImpFactor/20

Click in the upper-right corner of the section. This creates a node with the requested deformation settings. The newly created node is automatically disabled in the existing study steps to enable further computations without changes in the results.

Locate the section. From the list, choose .

From the list, choose .

In the text field, type range(0,0.5,30).

In the text field, type %.

Click in the upper-right corner of the section.

This button creates a new study with stationary step, activates geometric nonlinearities and applies an auxiliary sweep for the postbuckling study.

Study: Postbuckling Analysis

In the window, click .

In the window for , locate the section.

Clear the checkbox.

In the text field, type Study: Postbuckling Analysis.

In the toolbar, click