PDF
Inflation of a Square Airbag
Introduction
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 due to zero bending stiffness. This undesirable limitation can be overcome 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 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 Wrinkling 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, the Stabilization feature 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 types 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.
Application Library path: Structural_Mechanics_Module/Buckling_and_Wrinkling/membrane_airbag_inflation
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  3D.
2
In the Select Physics tree, select Structural Mechanics > Membrane (mbrn).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Global Definitions
Model Parameters
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, type Model Parameters in the Label text field.
3
Locate the Parameters section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file membrane_airbag_inflation_parameters.txt.
Definitions
Interpolation 1 (int1)
1
In the Definitions toolbar, click  Interpolation.
2
In the Settings window for Interpolation, locate the Definition section.
3
In the Function name text field, type F.
4
In the table, enter the following settings:
t
f(t)
0
100
1
1
5
Locate the Units section. In the Function table, enter the following settings:
Function
Unit
F
N/m
6
In the Argument table, enter the following settings:
Argument
Unit
t
1
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
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 the geometry is constructed.
Geometry 1
Work Plane 1 (wp1)
1
In the Model Builder window, expand the Component 1 (comp1) > Geometry 1 node.
2
Right-click Geometry 1 and choose Work Plane.
Work Plane 1 (wp1) > Square 1 (sq1)
1
In the Work Plane toolbar, click  Square.
2
In the Settings window for Square, locate the Size section.
3
In the Side length text field, type L/2.
4
Locate the Position section. In the xw text field, type L/2.
5
In the Work Plane toolbar, click  Build All.
Materials
Material 1 (mat1)
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
When modeling wrinkling, constant strain triangular (CST) elements are a good choice due to their numerical stability. Use a triangular mesh and change the default Quadratic discretization to Linear.
Membrane (mbrn)
1
In the Settings window for Membrane, click to expand the Discretization section.
2
From the Displacement field list, choose Linear.
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Membrane (mbrn) click Linear Elastic Material 1.
Wrinkling 1
In the Physics toolbar, click  Attributes and choose Wrinkling.
Thickness and Offset 1
1
In the Model Builder window, under Component 1 (comp1) > Membrane (mbrn) click Thickness and Offset 1.
2
In the Settings window for Thickness and Offset, locate the Thickness and Offset section.
3
In the d0 text field, type th.
Symmetry 1
1
In the Physics toolbar, click  Edges and choose Symmetry.
2
Select Edges 1 and 3 only.
Prescribed Displacement 1
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement.
2
Select Edges 2 and 4 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
From the Displacement in z direction list, choose Prescribed.
Face Load 1
1
In the Physics toolbar, click  Boundaries and choose Face Load.
2
Select Boundary 1 only.
3
In the Settings window for Face Load, locate the Force section.
4
From the Load type list, choose Pressure.
5
In the p text field, type -Pmax*para.
Add a parametrically decreasing edge load on the outer edges in the lateral direction as a form of spring support in order to achieve numerical stability for this problem.
Edge Load 1
1
In the Physics toolbar, click  Edges and choose Edge Load.
2
Select Edges 2 and 4 only.
3
In the Settings window for Edge Load, locate the Coordinate System Selection section.
4
From the Coordinate system list, choose Local edge system.
5
Locate the Force section. Specify the fL vector as
0
xl
-F(para)
yl
0
zl
Add a Stabilization feature in order to improve numerical stability.
Stabilization 1
In the Physics toolbar, click  Boundaries and choose Stabilization.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) > Materials click Material 1 (mat1).
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
Ey
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
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  More Generators and choose Mapped.
2
In the Settings window for Mapped, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Edge Selection section.
3
From the Selection list, choose All edges.
4
Locate the Distribution section. In the Number of elements text field, type 10.
Convert 1
1
In the Mesh toolbar, click  Modify and choose Convert.
2
In the Settings window for Convert, locate the Element Split Method section.
3
From the Element split method list, choose Insert centerpoints.
4
Click  Build All.
Customize the study settings in order to achieve a better convergence.
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, click to expand the Study Extensions section.
3
Select the Auxiliary sweep checkbox.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Parameter)
range(0,0.01,1)
 
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Parametric 1.
4
In the Settings window for Parametric, click to expand the Continuation section.
5
Select the Tuning of step size checkbox.
6
In the Maximum step size text field, type 0.01.
7
From the Predictor list, choose Linear.
8
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 click Fully Coupled 1.
9
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
10
From the Nonlinear method list, choose Constant (Newton).
11
From the Stabilization and acceleration list, choose Anderson acceleration.
Before solving the study, add default plots in order to visualize the results while solving.
12
In the Model Builder window, click Study 1.
13
In the Settings window for Study, locate the Study Settings section.
14
Clear the Generate default plots checkbox.
15
In the Study toolbar, click  Show Default Plots.
Results
Mirror 3D 1
1
In the Model Builder window, expand the Results node.
2
Right-click Results > Datasets and choose More 3D Datasets > Mirror 3D.
3
In the Settings window for Mirror 3D, locate the Plane Data section.
4
From the Plane list, choose XZ-planes.
5
In the Y-coordinate text field, type 0.5*L.
Mirror 3D 2
1
Right-click Mirror 3D 1 and choose Duplicate.
2
In the Settings window for Mirror 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 1.
4
Locate the Plane Data section. From the Plane list, choose yz-planes.
5
In the x-coordinate text field, type 0.5*L.
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, type displa in the text field.
5
In the tree, select General > Displacement (m).
6
Click OK.
7
In the Settings window for Preferred Units, locate the Units section.
8
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Displacement
m
cm
9
Click  Apply.
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) > Membrane (mbrn) > Displacement (mbrn).
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
Transverse Displacement
1
In the Settings window for 3D Plot Group, type Transverse Displacement in the Label text field.
2
Locate the Data section. From the Dataset list, choose Mirror 3D 2.
Surface 1
1
In the Model Builder window, expand the Transverse Displacement node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type w.
4
Click to expand the Quality section. From the Smoothing threshold list, choose None.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Transverse Displacement toolbar, click  Plot.
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, click to expand the Results While Solving section.
3
Select the Plot checkbox.
4
In the Study toolbar, click  Compute.
Results
First Principal Stress
1
Right-click Transverse Displacement and choose Duplicate.
2
Drag and drop Transverse Displacement 1 below Transverse Displacement.
3
In the Settings window for 3D Plot Group, type First Principal Stress in the Label text field.
4
Locate the Color Legend section. Select the Show maximum and minimum values checkbox.
Surface 1
1
In the Model Builder window, expand the First Principal Stress node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Membrane > Stress > Principal stresses > mbrn.sp1Gp - First principal stress - N/m².
3
Locate the Expression section. In the Unit field, type kN/cm^2.
4
Locate the Coloring and Style section. From the Color table list, choose Prism.
First Principal Stress
1
In the Model Builder window, click First Principal Stress.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose New view.
4
In the First Principal Stress toolbar, click  Plot.
5
Click the  Go to XY View button in the Graphics toolbar.
6
Click the  Show Grid button in the Graphics toolbar.
Second Principal Stress
1
Right-click First Principal Stress and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Second Principal Stress in the Label text field.
3
Drag and drop below First Principal Stress.
Surface 1
1
In the Model Builder window, expand the Second Principal Stress node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Membrane > Stress > Principal stresses > mbrn.sp2Gp - Second principal stress - N/m².
Second Principal Stress
1
In the Model Builder window, click Second Principal Stress.
2
In the Second Principal Stress toolbar, click  Plot.
Wrinkled Region
1
Right-click Second Principal Stress and choose Duplicate.
2
Drag and drop Second Principal Stress 1 below Second Principal Stress.
3
In the Settings window for 3D Plot Group, type Wrinkled Region in the Label text field.
4
Locate the Color Legend section. Clear the Show maximum and minimum values checkbox.
Surface 1
1
In the Model Builder window, expand the Wrinkled Region node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Membrane > Wrinkling > mbrn.iswrinkled - Is wrinkled - 1.
3
Locate the Coloring and Style section. From the Color table list, choose Rainbow.
4
Locate the Quality section. From the Evaluation settings list, choose Manual.
5
From the Smoothing list, choose None.
6
In the Wrinkled Region toolbar, click  Plot.
Point Displacements
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Point Displacements in the Label text field.
Point Graph 1
1
Right-click Point Displacements and choose Point Graph.
2
Select Point 2 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type w.
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Transverse displacement at midpoint
Point Graph 2
1
Right-click Point Graph 1 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Selection section.
3
Click  Clear Selection.
4
Select Point 1 only.
5
Locate the y-Axis Data section. In the Expression text field, type v.
6
Locate the Legends section. In the table, enter the following settings:
Legends
Lateral displacement at midpoint on side edge
Point Graph 3
1
Right-click Point Graph 2 and choose Duplicate.
2
In the Settings window for Point Graph, locate the Selection section.
3
Click  Clear Selection.
4
Select Point 3 only.
5
Locate the y-Axis Data section. In the Expression text field, type mbrn.disp.
6
Locate the Legends section. In the table, enter the following settings:
Legends
Total displacement at corner point
Global 1
1
In the Model Builder window, right-click Point Displacements and choose Global.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1 (sol1).
4
From the Parameter selection (para) list, choose Last.
5
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
wmax_ref
cm
Transverse displacement at midpoint, reference
6
Click to expand the Coloring and Style section. From the Color list, choose From theme.
7
Find the Line markers subsection. From the Marker list, choose Square.
8
From the Positioning list, choose Interpolated.
9
Set the Number value to 12.
10
Click to expand the Legends section. From the Legends list, choose Manual.
11
In the table, enter the following settings:
Legends
Reference values at last step
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
vmax_ref
cm
Lateral displacement at midpoint on side edge, reference
4
Locate the Legends section. Clear the Show legends checkbox.
Global 3
1
Right-click Global 2 and choose Duplicate.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
dispmax_ref
cm
Total displacement at corner point, reference
Point Displacements
1
In the Model Builder window, click Point Displacements.
2
In the Settings window for 1D Plot Group, click to expand the Title section.
3
From the Title type list, choose Manual.
4
In the Title text area, type Point displacements.
5
Locate the Legend section. From the Layout list, choose Outside graph axis area.
6
From the Position list, choose Bottom.
7
In the Number of rows text field, type 2.
8
In the Point Displacements toolbar, click  Plot.
Point Stress
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Point Stress in the Label text field.
3
Locate the Legend section. From the Position list, choose Upper left.
Point Graph 1
1
Right-click Point Stress and choose Point Graph.
2
Select Point 2 only.
3
In the Settings window for Point Graph, locate the y-Axis Data section.
4
In the Expression text field, type mbrn.sp1.
5
In the Unit field, type kN/cm^2.
6
Locate the Legends section. Select the Show legends checkbox.
7
From the Legends list, choose Manual.
8
In the table, enter the following settings:
Legends
First principal stress at midpoint
Point Stress
1
In the Model Builder window, click Point Stress.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the y-axis label checkbox.
Global 1
1
Right-click Point Stress and choose Global.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1 (sol1).
4
From the Parameter selection (para) list, choose Last.
5
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
sp1max_ref
kN/cm^2
First principal stress at midpoint, reference
6
Click to expand the Title section. From the Title type list, choose None.
7
Locate the Coloring and Style section. From the Color list, choose From theme.
8
Find the Line markers subsection. From the Marker list, choose Square.
9
From the Positioning list, choose Interpolated.
10
Locate the Legends section. From the Legends list, choose Manual.
11
In the table, enter the following settings:
Legends
Reference value at last step
Point Stress
1
In the Model Builder window, click Point Stress.
2
In the Point Stress toolbar, click  Plot.