Inflation of a Square Airbag

The numerical treatment of thin structures with a membrane model is much simpler than with a shell model due to the assumption of zero bending stiffness. However, for some load cases this assumption is disadvantageous. For instance, when a membrane is subjected to compressive stresses, it may trigger wrinkling when these reach a critical level defined by the bending stiffness.This undesirable limitation can be overcame with the incorporation of a wrinkling model that removes these instabilities.

In this example, a squared airbag is inflated using an inner air pressure. The results are compared with the example presented in Ref. 1.

Model Definition

A squared airbag 6 mm in thickness and 1.2 m in diagonal length is inflated using a constant air pressure of 5 kPa. The membrane is modeled with an isotropic linear elastic material. The material properties given in Table 1 are taken from Ref. 1.

Material Properties

Table 1: Material properties.
Property	Variable	Isotropic Model
Young’s modulus	E	588 MPa
Poisson’s ratio	ν	0.4

Only a quarter of the square airbag is analyzed due to the intrinsic symmetry of the model.

Results and Discussions

Figure 1 shows the wrinkled regions in the inflated airbag. Apart from the central region, wrinkles develop everywhere.

The transverse displacement in the inflated airbag is shown in Figure 2. The variation of the principal stresses at the end of the inflation process is shown in the Figure 3 and Figure 4. The minimum value of the second principal stress is almost zero. Both figures show tensile principal stresses after inflation.

Figure 5 shows the displacement at various points versus the inflating pressure, these points are compared to the results given in Ref. 1. At the final pressure, the values match the reference values very well. Similarly, Figure 6 shows the variation of the first principal (tensile) stress at the midpoint versus the inflating pressure. The result also matches the reference value given in Ref. 1.

Figure 1: Wrinkled region in the inflated airbag.

Figure 2: Transverse displacement after inflation.

Figure 3: First principal stress after inflation.

Figure 4: Second principal stress after inflation.

Figure 5: Displacements at different points after inflation.

Figure 6: First principal stress at midpoint.

Notes About the COMSOL Implementation

A wrinkling model based on the modified deformation gradient is incorporated within the membrane theory using the feature, which solves a set of nonlinear equations with the Newton–Raphson method.

Since the unstressed membrane does not have any stiffness in the normal direction, a very small spring support is added in order to stabilize the model. To further improve the numerical stability, a spring support is provided in the form of an edge load which decreases parametrically as the model becomes stable.

Constant strain triangle (CST) elements are numerically stable for wrinkling problems. CST elements give constant strains, which in turn give constant stresses for homogeneous material properties, ensuring that the whole element is either wrinkled, slack, or taut. These type of elements are used for the analysis.

Reference

1. A. Jarasjarungkiat, R. Wuchner, and K.U.Bletzinger, “A wrinkling model based on material modification for isotropic and orthotropic membranes,” Compt. Methods Appl. Mech. Engrg., vol. 197, pp. 773–788, 2008.

Structural_Mechanics_Module/Buckling_and_Wrinkling/membrane_airbag_inflation

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

Model Parameters

In the window, under click .

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

Locate the section. Click

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

Definitions

Interpolation 1 (int1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type F.

In the table, enter the following settings:


t	f(t)
0	100
1	1

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


Function	Unit
F	N/m

In the table, enter the following settings:


Argument	Unit
t	1

Variables 1

In the window, right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
wmax_ref	21.75[cm]	m	Transverse displacement at midpoint, reference
vmax_ref	12.03[cm]	m	Lateral displacement at midpoint on side edge, reference
dispmax_ref	4.94[cm]	m	Total displacement at corner point, reference
sp1max_ref	0.39[kN/cm^2]	N/m²	First principal stress at midpoint, reference

Due to symmetry only a quarter of geometry is constructed.

Geometry 1

Work Plane 1 (wp1)

In the window, expand the node.

Right-click and choose .

Work Plane 1 (wp1)>Square 1 (sq1)

In the toolbar, click

In the window for , locate the section.

In the text field, type L/2.

Locate the section. In the text field, type L/2.

In the toolbar, click

Materials

Material 1 (mat1)

In the window, under right-click and choose .

To model wrinkling, constant strain triangular (CST) elements are numerically stable. Use a triangular mesh and change the default discretization to .

Membrane (mbrn)

In the window for , click to expand the section.

From the list, choose .

Linear Elastic Material 1

In the window, under click .

Wrinkling 1

In the toolbar, click

and choose .

Thickness and Offset 1

In the window, under click .

In the window for , locate the section.

In the d text field, type th.

Symmetry 1

In the toolbar, click

and choose .

Select Edges 1 and 3 only.

Prescribed Displacement 1

In the toolbar, click

and choose .

Select Edges 2 and 4 only.

In the window for , locate the section.

Select the check box.

Face Load 1

In the toolbar, click

and choose .

Select Boundary 1 only.

In the window for , locate the section.

From the list, choose .

In the p text field, type -Pmax*para.

Add a parametrically decreasing edge load on the outer edges in the lateral direction as form of spring support in order to achieve numerical stability for this problem.

Edge Load 1

In the toolbar, click

and choose .

Select Edges 2 and 4 only.

In the window for , locate the section.

From the list, choose .

Locate the section. Specify the FL vector as


0	xl
-F(para)	yl
0	zl

Add a spring support in the thickness direction in order to achieve numerical stability for this problem.

Spring Foundation 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 kA table, enter the following settings:


0	0	0
0	0	0
0	0	1e-3[N/m^3]

Materials

Material 1 (mat1)

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


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