PDF
Homogenized Model of a Corrugated Sheet
Introduction
Corrugated sheets have wide applications in mechanical and civil engineering, from the simple case of roofing panels to the complex one of aircraft skins. In most applications, the loads are distributed and the global response is sought. In such cases, it is tedious and computer resource consuming to model the actual geometry. Instead, an orthotropic sheet with equivalent stiffness can be considered. Homogenization techniques based on periodic boundary conditions of a unit cell can be employed to compute the equivalent stiffness matrices for corrugated sheets.
This example presents a homogenization-based numerical model for trapezoidal and round corrugated sheets. The numerically obtained equivalent stiffness matrices are compared with the stiffnesses based on various analytical models proposed in Ref. 1–Ref. 3.
As shown in this example, the equivalent stiffnesses for any corrugated sheet can be obtained numerically and subsequently be used directly in a Section Stiffness material model in the Shell interface with a simplified flat geometry.
The method shown here can be applied for homogenization also for other types of shell structures, for example, perforated sheets.
Model Definition
Figure 1 shows a unit cell of a trapezoidal corrugated sheet, which can be described by five geometric parameters:
•
Half wavelength of corrugation, c
•
Amplitude of corrugation, f
•
Angle of corrugation profile, θ
•
Depth of corrugation, d
•
Sheet thickness, t
The geometric dimensions for the trapezoidal sheet taken from Ref. 1 are c = 0.0508 m, f = 0.0127 m, θ = 45°, d = 0.1016 m, and t = 0.00635 m.
Figure 2 shows a unit cell of a round corrugated sheet. This sheet is described by three geometric parameters:
•
Radius of corrugation, R
•
Depth of corrugation, d
•
Sheet thickness, t
The values of these parameters are chosen so that the size of the geometry is similar to that of the trapezoidal sheet: R = 0.0254 m, d = 0.1016 m, and t = 0.00635 m.
Figure 1: Geometry of a unit cell of a trapezoidal corrugated sheet.
Figure 2: Geometry of a unit cell of a round corrugated sheet.
Material
The material properties for both sheets are taken from Ref. 1: Young’s modulus E = 21 GPa and Poisson’s ratio ν = 0.3.
Analytical Models
This section provides a short theoretical background of the analytical homogenization models proposed in Ref. 1 and Ref. 2. The main objective of this exercise is to obtain an equivalent thick sheet of uniform thickness te from the corrugated sheet shown in the Figure 1. Using Mindlin plate theory, the constitutive equation for the symmetric corrugated sheet in a curvilinear coordinate system is written as
,
where , , and are the force, moment, and transverse shear resultants, respectively. Moreover, , , and are the membrane, bending, and transverse shear strains, respectively.
The constitutive equations for the equivalent flat sheet are written as
,
The equivalent stiffness matrices , , and can be deduced from the stiffness matrices of the corrugated sheet and geometric parameters by subjecting the corrugated sheet to the same boundary conditions as the equivalent sheet and evaluating either internal forces (reactions) or the total strain energy.
The total strain energy for the equivalent sheet is written as
where c is the half wavelength of the corrugation and k is the shear correction factor. The width of the sheet, d, can be chosen arbitrarily.
A specific set of boundary conditions needs to be applied to the corrugated sheet to find the equivalent stiffness matrices. These boundary conditions, when applied to the equivalent sheet, should satisfy the condition
where U is the total strain energy of the corrugated sheet. The purpose of the sets of boundary conditions is to impose constant strain states in an average sense.
Extensional and Bending Stiffnesses
The strain states and stiffness components for the equivalent sheet are given in Ref. 1 and summarized in Table 1.
Table 1: Boundary conditions of the equivalent sheet and corresponding stiffnesses.
Load cases: Strain states
Equivalent energy method
Equivalent force method
 Load case 1:
 Load case 2:
 Load case 3:
 Load case 4:
 Load case 5:
 Load case 6:
Note that the equivalent energy method does not directly provide the coupling terms and . It would be possible to deduce them to, but at the expense of adding more load cases.
The authors of Ref. 1 and Ref. 2 use the strain states above to obtain the equivalent stiffnesses for the corrugated sheet. Table 2 shows the analytical formulas presented in these papers for the corrugated sheet.
Table 2: Analytical formulas for corrugated sheet based on Ref. 1 and Ref. 2.
Stiffness components
Xia and others (Ref. 1)
Park and others (Ref. 2)
The length and inertia variables for the trapezoidal and round sheets are given in Table 3.
Table 3: Length and inertia variables for trapezoidal and round corrugated sheets.
Variable
Trapezoidal sheet
Round sheet
  c
  c
  2R
  l
  πR
  I1
  2πR
  I2
πR3
  I1s
  2πR
However, the authors of Ref. 1 report incorrect expressions for the variable I1 for both the trapezoidal and the round corrugated sheet. The correct expression for I1 for the trapezoidal sheet is given in Ref. 2, while the expression for the round sheet in Ref. 1 is missing a factor 2.
The author of Ref. 3 uses the variational asymptotic method to obtain the equivalent extensional and bending stiffness matrices. The analytical formulas are presented in Table 4 for the corrugated sheet.
Table 4: Analytical formulas for the corrugated sheet based on Ref. 3.
Stiffness components
Ye and others Ref. 3
Here, Iy = 0.04598132c2t for the trapezoidal sheet and Iy = 0.19635c2t for the round sheet.
When the three different analytical formulas presented in the different papers are compared, the important differences are:
•
In Ref. 2, the effect of the transverse shear stiffness is considered when evaluating the equivalent extension stiffness matrix component ; this effect is neglected in the other two papers.
•
The authors of Ref. 3 report the incorrectness of the analytical formula for the equivalent bending stiffness component proposed in Ref. 1 and Ref. 2. They have presented an analytical formula that closely matches the numerical results presented in this example.
Transverse Shear Stiffness
The authors of Ref. 2 proposed equivalent transverse shear stiffnesses and by comparing one half of the unit cell with a solid block of width c, depth d, and thickness 2f, where f is the amplitude of the corrugated sheet. The proposed analytical formulas are
where l' is half the length of the inclined part only. The integrals J0 and J2 are evaluated as
where s is the curvilinear coordinate along the corrugation profile and n is the local coordinate defined by . The function f(x) describes the shape of the corrugation.
In the current example, no load cases for transverse shear stiffness are provided, since there is no load case that can produce a state of pure transverse shear. Therefore, users have to rely on the analytical formula presented in Ref. 2. However, the shear stiffness is usually of less important than the stiffness in tension and bending.
Numerical Model
In the numerical model, the set of boundary conditions that are applied on the round corrugated sheet in order to mimic the boundary conditions of the equivalent sheet are presented in Table 1. The boundary conditions on the corrugated sheet for the different load cases are given in Table 5. Note that the rotation around the shell normal is always constrained by default.
Table 5: Boundary conditions on the round corrugated sheet.
Load case
Edge 1, X=0
Edge 2,X=2c
Edge 3, Y=0
Edge 4,
Y=d
Points,
(X,Y)= (c,0), (X,Y)=(c,d)
1
u=-c, w=0, θx=0
u=c, w=0, θx=0
v=0, θx=0
v=0, θx=0
NA
2
u=0, w=0, θx=0
u=0, w=0, θx=0
v=-0.5d, θx=0
v=0.5d, θx=0
 
 3
v=-0.5c, w=0, θy=0
v=0.5c, w=0, θy=0
u=-0.25d, w=0, θy=0
u=0.25d, w=0, θy=0
 
 4
u=0, θx=0, θy=-c/L
u=0, θx=0, θy=-c/L
v=0, θx=0
v=0, θx=0
w=0
 5
u=0, θy=0
u=0, θy=0
v=0.5*Zd/L, θx=-0.5d/L, θy=0
v=-0.5*Zd/L, θx=-0.5d/L, θy=0
w=0
 6
u=0, v=0, θx=0.5c/L
u=0,v=0, θx=0.5c/L
u=-0.25Zd/L, θy=-0.25d/L
u=0.25Zd/L, θy=-0.25d/L
w=0
The equivalent extensional and bending matrices can be found by either the equivalent force method or by the equivalent energy method, as shown in Table 6. In this example, the reaction forces are used to compute the internal forces.
Table 6: Extensional and bending stiffness matrices by numerical method.
Load case
Equivalent energy method
Equivalent force method
1
2
 3
 4
 5
 6
Here, denotes summation of reaction forces or moments R over the edge ei.
Results and Discussion
Figure 3 shows the displacement of the trapezoidal corrugated sheet for the translational load cases, while Figure 4 shows the total rotations of the trapezoidal corrugated sheet for the rotational load cases. The displacements in the translational load cases and the rotations in the rotational load cases for the round corrugated sheet are shown in Figure 5 and Figure 6.
Figure 3: Displacement of the trapezoidal sheet for the translational load cases.
Figure 4: Total rotation of the trapezoidal sheet for the rotational load cases.
Figure 5: Displacement of the round sheet for the rotational load cases.
Figure 6: Total rotation of the round sheet for the rotational load cases.
The equivalent extensional and bending stiffness matrices based on the analytical models are shown in Table 7 for the trapezoidal corrugated sheet and in Table 8 for the round corrugated sheet. In the same table, the values of the equivalent stiffness components obtained by numerical models are shown. The stiffnesses obtained numerically based on reaction forces exactly match those obtained based on energy, indicating the correctness of the applied boundary conditions. The conclusion for each stiffness component is:
•
The analytical values of the extensional stiffness matrix component varies somewhat when compared to each other. The numerical values match more closely with the values presented in Ref. 2 as the authors considered the effect of transverse shear stiffness on the longitudinal extension, an effect the authors of the other two papers have ignored.
•
The analytical values of the extensional stiffness matrix component varies somewhat when compared to each other. For the trapezoidal sheet, the numerical value matches more closely with the values presented in Ref. 2 as the authors considered the effect of the transverse shear stiffness, an effect the authors of the other two papers ignored. However, surprisingly, the round sheet numerical value is twice the analytical value based on Ref. 2.
•
The numerical values of the equivalent extensional stiffness matrix components and closely match the analytical values.
•
The numerical value of the equivalent bending stiffness matrix component closely matches the analytical values.
•
The numerical value of the equivalent bending stiffness matrix component closely matches the analytical values for the trapezoidal sheet (although there is a small mismatch between the numerically obtained and components). For the round sheet, the numerical value of the equivalent bending stiffness matrix component is zero although the analytical value is nonzero.
•
The numerical value of the equivalent bending stiffness matrix component closely matches the analytical value based on the formula presented in Ref. 3, but deviates from the analytical values computed based on the formula presented in Ref. 1 and Ref. 2. The reason is explained by the authors of Ref. 3, who point out errors in the formula presented by the authors of Ref. 1 and Ref. 2.
•
The numerical value of the equivalent bending stiffness matrix component is in the same range as the analytical values for the trapezoidal sheet. For the round sheet, the numerical value of the equivalent bending stiffness matrix component closely matches the analytical value.
Table 7: Stiffness matrices based on analytical and numerical models for trapezoidal sheet.
Stiffness component
Xia and others Ref. 1
Park and others Ref. 2
Ye and others Ref. 3
Numerical: Based on reactions
Numerical: Based on energy
(N/m)
4.0517E6
3.9203E6
4.1496E6
3.9203E6
3.9203E6
(N/m)
1.2155E6
1.1761E6
1.2449E6
1.1761E6
NA
(N/m)
1.6133E8
1.6132E8
1.6097E8
1.6132E8
1.6132E8
(N/m)
4.2489E7
4.2489E7
4.2489E7
4.2489E7
4.2489E7
(Nm)
407.92
407.92
407.92
407.92
407.92
(Nm)
122.38
122.38
122.38
120.859
NA
(Nm)
17809
17809
15823
16237
16243
(Nm)
208.03
208.03
208.03
180.63
180.42
Table 8: Stiffness matrices based on analytical and numerical models for round sheet.
Stiffness component
Xia and others Ref. 1
Park and others Ref. 2
Ye and others Ref. 3
Numerical: Based on reactions
Numerical: Based on energy
(N/m)
9.6175E5
9.2891E5
9.7176E5
9.3558E5
9.3558E5
(N/m)
2.8852E5
2.7867E5
2.9153E5
5.6134E5
NA
(N/m)
2.0955E8
2.0955E8
2.0947E8
2.0980E8
2.0980E8
(N/m)
3.2651E7
3.2651E7
3.2651E7
3.2651E7
3.2651E7
(Nm)
313.47
313.47
313.47
311.85
311.85
(Nm)
94.041
94.041
94.041
0
NA
(Nm)
75026
75026
67570
67921
67921
(Nm)
270.71
270.71
270.71
268.43
268.43
Notes About the COMSOL Implementation
In order to run different constraint cases (called load cases), the Define load cases checkbox and the associated section under it in the Study Extensions section of the Stationary study step can be used. However, the fallout of this design is in some cases (the current example falls in this category) that the reaction forces in one or more load cases are not stored. In this example, we rely on reaction forces for computation of equivalent stiffness matrices; hence, instead of using six load cases on one stationary study step, six different studies are used.
The Parametric switch option in the Parametric Sweep under study is used to switch between the trapezoidal and the round sheet.
References
1. Y. Xia, M.I. Friswell, and E.I. Saavedra Flores,  “Equivalent models of corrugated panels,” Int. J. Solids and Structures, vol. 49, pp. 1453–1462, 2012.
2. K.J. Park, K. Jung, and Y.W. Kim, “Evaluation of homogenized effective properties for corrugated composite panels,” Composite Structures, vol. 140, pp. 644–654, 2016.
3. Z. Ye, V.L. Berdichevsky, and W. Yu, “An equivalent classical plate model of corrugated structures,” Int. J. Solids and Structures, vol. 51, pp. 2073–2083, 2014.
Application Library path: Structural_Mechanics_Module/Material_Models/corrugated_sheet
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 > Shell (shell).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Geometry 1
First, add parameters unique to a trapezoidal and a round corrugated sheet. Then, add a Parameter Case for common parameters between trapezoidal and round corrugated sheets in order to be used in a parametric switch.
Global Definitions
Geometric Properties
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, type Geometric Properties in the Label text field.
3
Locate the Parameters section. In the table, enter the following settings:
Name
Expression
Value
Description
theta
45[deg]
0.7854 rad
Angle of corrugation profile for trapezoidal corrugated sheet
R
0.0254[m]
0.0254 m
Radius of corrugation for round corrugated sheet
Common Geometric and Material Properties
1
In the Home toolbar, click  Parameters and choose Add > Parameters.
2
In the Settings window for Parameters, type Common Geometric and Material Properties 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 corrugated_sheet_parameters_trapezoidal.txt.
5
In the Home toolbar, click  Parameter Case.
6
In the Settings window for Case, type Trapezoidal Corrugation in the Label text field.
7
In the Home toolbar, click  Parameter Case.
8
In the Settings window for Case, type Round Corrugation in the Label text field.
9
Locate the Parameters section. Click  Load from File.
10
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_parameters_round.txt.
Next, create unit cells for trapezoidal and round corrugated sheets. These unit cells, like many others, can be found in the built-in Part Libraries.
11
In the Model Builder window, right-click Global Definitions and choose Geometry Parts > Part Libraries.
Part Libraries
In the Part Libraries window, select COMSOL Multiphysics > Unit Cells and RVEs > Corrugated Sheets > trapezoidal_corrugation in the tree.
Trapezoidal Corrugation
Right-click Global Definitions and choose Add to Model.
Geometry Parts
In the Model Builder window, under Global Definitions right-click Geometry Parts and choose Part Libraries.
Part Libraries
1
In the Part Libraries window, select COMSOL Multiphysics > Unit Cells and RVEs > Corrugated Sheets > round_corrugation in the tree.
2
Click  Add to Model.
Round Corrugation
Right-click Geometry Parts and choose Add to Model.
Geometry 1
If 1 (if1)
1
In the Geometry toolbar, click  Programming and choose If + End If.
2
In the Settings window for If, locate the If section.
3
In the Condition text field, type case==1.
Trapezoidal Corrugation 1 (pi1)
1
In the Geometry toolbar, click  Part Instance and choose Trapezoidal Corrugation.
2
In the Settings window for Part Instance, locate the Input Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
c
c
0.0508 m
Half wavelength of corrugation
f
f
0.0127 m
Amplitude of corrugation
theta
theta
45 °
Angle of corrugation profile
d
d
0.1016 m
Depth
If 2 (if2)
In the Geometry toolbar, click  Programming and choose If + End If.
End If 2 (endif2), If 2 (if2)
In the Model Builder window, under Component 1 (comp1) > Geometry 1, Ctrl-click to select If 2 (if2) and End If 2 (endif2).
If 2 (if2)
1
Drag and drop below End If 1 (endif1).
2
In the Settings window for If, locate the If section.
3
In the Condition text field, type case==2.
Round Corrugation 1 (pi2)
1
In the Geometry toolbar, click  Part Instance and choose Round Corrugation.
2
In the Settings window for Part Instance, locate the Input Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
R
R
0.0254 m
Radius of corrugation
d
d
0.1016 m
Depth
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
Global Definitions
Common Geometric and Material Properties
Add different selections in order to simplify the application of boundary condition.
Geometry 1
Pair 1, Source
1
In the Geometry toolbar, click  Selections and choose Union Selection.
2
In the Settings window for Union Selection, type Pair 1, Source in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Input Entities section. Click  Add.
5
In the Add dialog, in the Selections to add list, choose Pair 1, Source (Trapezoidal Corrugation 1) and Pair 1, Source (Round Corrugation 1).
6
Click OK.
Pair 1, Destination
1
In the Geometry toolbar, click  Selections and choose Union Selection.
2
In the Settings window for Union Selection, type Pair 1, Destination in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Input Entities section. Click  Add.
5
In the Add dialog, in the Selections to add list, choose Pair 1, Destination (Trapezoidal Corrugation 1) and Pair 1, Destination (Round Corrugation 1).
6
Click OK.
Pair 2, Source
1
In the Geometry toolbar, click  Selections and choose Union Selection.
2
In the Settings window for Union Selection, type Pair 2, Source in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Input Entities section. Click  Add.
5
In the Add dialog, in the Selections to add list, choose Pair 2, Source (Trapezoidal Corrugation 1) and Pair 2, Source (Round Corrugation 1).
6
Click OK.
Pair 2, Destination
1
In the Geometry toolbar, click  Selections and choose Union Selection.
2
In the Settings window for Union Selection, type Pair 2, Destination in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Edge.
4
Locate the Input Entities section. Click  Add.
5
In the Add dialog, in the Selections to add list, choose Pair 2, Destination (Trapezoidal Corrugation 1) and Pair 2, Destination (Round Corrugation 1).
6
Click OK.
Ball Selection 1 (ballsel1)
1
In the Geometry toolbar, click  Selections and choose Ball Selection.
2
In the Settings window for Ball Selection, locate the Geometric Entity Level section.
3
From the Level list, choose Point.
4
Locate the Ball Center section. In the x text field, type c.
5
Locate the Ball Radius section. In the Radius text field, type 1e-5*c.
Ball Selection 2 (ballsel2)
1
In the Geometry toolbar, click  Selections and choose Ball Selection.
2
In the Settings window for Ball Selection, locate the Geometric Entity Level section.
3
From the Level list, choose Point.
4
Locate the Ball Center section. In the x text field, type c.
5
In the y text field, type d.
6
Locate the Ball Radius section. In the Radius text field, type 1e-5*c.
Union Selection 5 (unisel5)
1
In the Geometry toolbar, click  Selections and choose Union Selection.
2
In the Settings window for Union Selection, locate the Geometric Entity Level section.
3
From the Level list, choose Point.
4
Locate the Input Entities section. Click  Add.
5
In the Add dialog, in the Selections to add list, choose Ball Selection 1 and Ball Selection 2.
6
Click OK.
7
In the Settings window for Union Selection, click  Build Selected.
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 Geometric entity level list, choose Edge.
4
From the Selection list, choose Pair 1, Source.
5
Locate the Advanced section. From the Method list, choose Summation over nodes.
Integration 2 (intop2)
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 Geometric entity level list, choose Edge.
4
From the Selection list, choose Pair 2, Source.
5
Locate the Advanced section. From the Method list, choose Summation over nodes.
Integration 3 (intop3)
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 Geometric entity level list, choose Point.
4
From the Selection list, choose Ball Selection 1.
5
Locate the Advanced section. From the Method list, choose Summation over nodes.
Next, add analytical and numerical formulas for equivalent stiffness from text files.
Analytical Stiffness Components by Xia et al.
1
In the Model Builder window, right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Analytical Stiffness Components by Xia et al. in the Label text field.
3
Locate the Variables section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_variables_Xia.txt.
Analytical Stiffness Components by Park et al.
1
Right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Analytical Stiffness Components by Park et al. in the Label text field.
3
Locate the Variables section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_variables_Park.txt.
Analytical Stiffness Components by Ye et al.
1
Right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Analytical Stiffness Components by Ye et al. in the Label text field.
3
Locate the Variables section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_variables_Ye.txt.
Numerical Stiffness Components Based on Reaction Forces
1
Right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Numerical Stiffness Components Based on Reaction Forces in the Label text field.
3
Locate the Variables section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_variables_reaction_forces.txt.
Numerical Stiffness Components Based on Energy Equivalence
1
Right-click Definitions and choose Variables.
2
In the Settings window for Variables, type Numerical Stiffness Components Based on Energy Equivalence in the Label text field.
3
Locate the Variables section. Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file corrugated_sheet_variables_energy_equivalence.txt.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
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
EE
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
Nu
1
Young’s modulus and Poisson’s ratio
Density
rho
1
kg/m³
Basic
Shell (shell)
Thickness and Offset 1
1
In the Model Builder window, under Component 1 (comp1) > Shell (shell) 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.
Set up the boundary conditions corresponding to the six different load cases and group them as per the load case.
Load Case 1: DA11 and DA12
1
In the Model Builder window, right-click Shell (shell) and choose Node Group.
2
In the Settings window for Group, type Load Case 1: DA11 and DA12 in the Label text field.
Prescribed Displacement/Rotation 1
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement/Rotation.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Edge Selection section.
3
From the Selection list, choose Pair 1, Source.
4
Locate the Prescribed Displacement section. From the Displacement in x direction list, choose Prescribed.
5
In the u 0 x text field, type -c.
6
From the Displacement in z direction list, choose Prescribed.
7
Locate the Prescribed Rotation section. From the By list, choose Rotation.
8
Select the Free rotation around t1 direction checkbox.
Prescribed Displacement/Rotation 2
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement/Rotation.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Edge Selection section.
3
From the Selection list, choose Pair 1, Destination.
4
Locate the Prescribed Displacement section. From the Displacement in x direction list, choose Prescribed.
5
In the u 0 x text field, type c.
6
From the Displacement in z direction list, choose Prescribed.
7
Locate the Prescribed Rotation section. From the By list, choose Rotation.
8
Select the Free rotation around t1 direction checkbox.
Prescribed Displacement/Rotation 3
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement/Rotation.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Edge Selection section.
3
From the Selection list, choose Pair 2, Source.
4
Locate the Prescribed Displacement section. From the Displacement in y direction list, choose Prescribed.
5
Locate the Prescribed Rotation section. From the By list, choose Rotation.
6
Select the Free rotation around t2 direction checkbox.
Prescribed Displacement/Rotation 4
1
In the Physics toolbar, click  Edges and choose Prescribed Displacement/Rotation.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Edge Selection section.
3
From the Selection list, choose Pair 2, Destination.
4
Locate the Prescribed Displacement section. From the Displacement in y direction list, choose Prescribed.
5
Locate the Prescribed Rotation section. From the By list, choose Rotation.
6
Select the Free rotation around t2 direction checkbox.
Load Cases 2–6
Create five similar load cases by enforcing the constraints on edges and points as shown in the table below:
Load case
Edge 1
Edge 2
Edge 3
Edge 4
Point 1
Load case 2
u=0, w=0, theta_x=0
u=0, w=0, theta_x=0
v=-0.5d, theta_x=0
v=0.5d, theta_x=0
 
Load case 3
v=-0.5c, w=0, theta_y=0
v=0.5c, w=0, theta_y=0
u=-0.25d, w=0, theta_y=0
u=0.25d, w=0, theta_y=0
 
Load case 4
u=0, theta_x=0, theta_y=-c/L
u=0, theta_x=0, theta_y=-c/L
v=0, theta_x=0
v=0, theta_x=0
w=0
Load case 5
u=0, theta_y=0
u=0, theta_y=0
v=0.5Zd/L, theta_x=-0.5d/L, theta_y=0
v=-0.5Zd/L, theta_x=-0.5d/L, theta_y=0
w=0
Load case 6
u=0, v=0, theta_x=0.5c/L
u=0, v=0, theta_x=0.5c/L
u=-0.25Zd/L, theta_y=-0.25d/L
u=0.25Zd/L, theta_y=-0.25d/L
w=0
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 Geometric entity level list, choose Entire geometry.
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 Pair 1, Source.
4
Locate the Distribution section. In the Number of elements text field, type 20.
Distribution 2
1
In the Model Builder window, 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 Pair 2, Source.
4
Locate the Distribution section. In the Number of elements text field, type 10.
5
Click  Build Selected.
Add a Parametric Sweep and choose the Parametric switch option in the study settings.
Study: Load Case 1
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study: Load Case 1 in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots checkbox.
Parametric Sweep
1
In the Study toolbar, click  Parametric Sweep.
2
In the Settings window for Parametric Sweep, locate the Study Settings section.
3
From the Sweep type list, choose Parameter switch.
4
Click  Add.
5
In the table, enter the following settings:
Switch
Cases
Case numbers
Common Geometric and Material Properties
All
range(1,1,2)
Step 1: Stationary
1
In the Model Builder window, click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Shell (shell) > Load Case 2: DA21 and DA22, Component 1 (comp1) > Shell (shell) > Load Case 3: DA33, Component 1 (comp1) > Shell (shell) > Load Case 4: DD11 and DD12, Component 1 (comp1) > Shell (shell) > Load Case 5: DD21 and DD22, and Component 1 (comp1) > Shell (shell) > Load Case 6: DD33.
5
Right-click and choose Disable.
6
In the Study toolbar, click  Compute.
Add five Stationary studies, one for each of the remaining load cases. Disable all constraints except those related to the current load case.
Set default units for result presentation.
Results
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 General > Displacement (m) 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
Displacement
m
mm
8
Click  Add Physical Quantity.
9
In the Physical Quantity dialog, select General > Plane angle (rad) in the tree.
10
Click OK.
11
In the Settings window for Preferred Units, locate the Units section.
12
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Plane angle
rad
°
13
Click  Apply.
Displacement for Translational Load Cases
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement for Translational Load Cases in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Load Case 1/Parametric Solutions 1 (sol2).
4
From the Common Geometric and Material Properties list, choose Trapezoidal Corrugation.
5
Locate the Color Legend section. Select the Show units checkbox.
6
Click to expand the Plot Array section. From the Array type list, choose Linear.
Surface 1
Right-click Displacement for Translational Load Cases and choose Surface.
Deformation 1
1
In the Model Builder window, right-click Surface 1 and choose Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor checkbox. In the associated text field, type 0.15.
Surface 2
1
In the Model Builder window, under Results > Displacement for Translational Load Cases right-click Surface 1 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Load Case 2/Parametric Solutions 2 (sol6).
4
From the Common Geometric and Material Properties list, choose Trapezoidal Corrugation.
5
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
6
Click to expand the Title section. From the Title type list, choose None.
Surface 3
1
Right-click Surface 2 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Load Case 3/Parametric Solutions 3 (sol10).
Displacement for Translational Load Cases
In the Model Builder window, click Displacement for Translational Load Cases.
Table Annotation 1
1
In the Displacement for Translational Load Cases toolbar, click  More Plots and choose Table Annotation.
2
In the Settings window for Table Annotation, locate the Data section.
3
From the Source list, choose Local table.
4
In the table, enter the following settings:
x-coordinate
y-coordinate
z-coordinate
Annotation
c
-0.5*d
0
Load case 1
3.5*c
-0.5*d
0
Load case 2
6*c
-0.5*d
0
Load case 3
5
Locate the Coloring and Style section. Clear the Show point checkbox.
6
From the Anchor point list, choose Upper middle.
Displacement for Translational Load Cases
Click the  Zoom Extents button in the Graphics toolbar.
Total Rotations for Rotational Load Cases
1
Right-click Displacement for Translational Load Cases and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Total Rotations for Rotational Load Cases in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Load Case 4/Parametric Solutions 4 (sol14).
Surface 1
1
In the Model Builder window, expand the Total Rotations for Rotational Load Cases node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type shell.totrot.
Deformation 1
1
In the Model Builder window, expand the Surface 1 node, then click Deformation 1.
2
In the Settings window for Deformation, locate the Scale section.
3
In the Scale factor text field, type 10.
Surface 2
1
In the Model Builder window, under Results > Total Rotations for Rotational Load Cases click Surface 2.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Load Case 5/Parametric Solutions 5 (sol18).
4
Locate the Expression section. In the Expression text field, type shell.totrot.
Surface 3
1
In the Model Builder window, click Surface 3.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Load Case 6/Parametric Solutions 6 (sol22).
4
Locate the Expression section. In the Expression text field, type shell.totrot.
Table Annotation 1
1
In the Model Builder window, click Table Annotation 1.
2
In the Settings window for Table Annotation, locate the Data section.
3
In the table, enter the following settings:
x-coordinate
y-coordinate
z-coordinate
Annotation
c
-0.5*d
0
Load case 4
3.5*c
-0.5*d
0
Load case 5
6*c
-0.5*d
0
Load case 6
Analytical Extensional Stiffness Matrix by Xia et al.
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Analytical Extensional Stiffness Matrix by Xia et al. in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Load Case 1/Parametric Solutions 1 (sol2).
4
From the Common Geometric and Material Properties list, choose From list.
5
In the Common Geometric and Material Properties list box, select Trapezoidal Corrugation.
6
Click to expand the Format section. From the Include parameters list, choose Off.
7
Locate the Transformation section. Select the Transpose checkbox.
Global Evaluation 1
1
Right-click Analytical Extensional Stiffness Matrix by Xia et al. and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
DA11_Xia
N/m
Equivalent extensional stiffness matrix, 11-component
DA12_Xia
N/m
Equivalent extensional stiffness matrix, 12-component
DA22_Xia
N/m
Equivalent extensional stiffness matrix, 22-component
DA33_Xia
N/m
Equivalent extensional stiffness matrix, 33-component
4
In the Analytical Extensional Stiffness Matrix by Xia et al. toolbar, click  Evaluate.
Evaluation Group 2-6
For evaluation of the remaining analytical stiffness terms, create five similar evaluation groups by duplicating Evaluation Group 1. Replace the expressions in the global evaluation node in each evaluation group. Rename all evaluation groups appropriately.
Numerical Extensional Stiffness Matrix Based on Reaction Forces
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Numerical Extensional Stiffness Matrix Based on Reaction Forces in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Load Case 1/Parametric Solutions 1 (sol2).
4
From the Common Geometric and Material Properties list, choose From list.
5
In the Common Geometric and Material Properties list box, select Trapezoidal Corrugation.
6
Locate the Format section. From the Include parameters list, choose Off.
7
Locate the Transformation section. Select the Transpose checkbox.
Global Evaluation 1
1
Right-click Numerical Extensional Stiffness Matrix Based on Reaction Forces and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
DA11_R
N/m
Equivalent extensional stiffness matrix, 11-component
DA21_R
N/m
Equivalent extensional stiffness matrix, 21-component
Global Evaluation 2
1
In the Model Builder window, right-click Numerical Extensional Stiffness Matrix Based on Reaction Forces and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Study: Load Case 2/Parametric Solutions 2 (sol6).
4
From the Common Geometric and Material Properties list, choose From list.
5
In the Common Geometric and Material Properties list box, select Trapezoidal Corrugation.
6
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
DA12_R
N/m
Equivalent extensional stiffness matrix, 12-component
DA22_R
N/m
Equivalent extensional stiffness matrix, 22-component
Global Evaluation 3
1
Right-click Numerical Extensional Stiffness Matrix Based on Reaction Forces and choose Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Data section.
3
From the Dataset list, choose Study: Load Case 3/Parametric Solutions 3 (sol10).
4
From the Common Geometric and Material Properties list, choose From list.
5
In the Common Geometric and Material Properties list box, select Trapezoidal Corrugation.
6
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
DA33_R
N/m
Equivalent extensional stiffness matrix, 33-component
7
In the Numerical Extensional Stiffness Matrix Based on Reaction Forces toolbar, click  Evaluate.
Evaluation Group 8-10
For evaluation of the remaining numerical stiffness terms, create three similar evaluation groups by duplicating Evaluation Group 7. Replace the expressions in the global evaluation node in each evaluation groups. Assign the correct dataset and rename all evaluation groups appropriately.
Select all result nodes and group them together.
Trapezoidal Corrugation
1
In the Model Builder window, under Results click Group 7.
2
In the Settings window for Group, type Trapezoidal Corrugation in the Label text field.
Duplicate the Trapezoidal Corrugation result group node. Change the loop levels in the parametric dataset to get the results for round corrugation.