PDF
Snap Hook
Introduction
This model simulates the insertion of a snap hook in its slot. Fasteners like this are common in the automotive industry, for example, in the control panel of a car. In this case it is important to know the force that must be applied in order to place the hook in the slot, but also the force needed to remove it. From a numerical point of view, this is a highly nonlinear structural analysis, mainly due to the contact interaction between the hook and the slot, but also due to the elastoplastic constitutive law selected for the hook, and finally due to the geometrical nonlinearity originating from the large displacements.
Model Definition
Due to symmetry, you can study only half of the original snap hook geometry, this way reducing the size of the model. Figure 1 shows the modeled geometry.
Figure 1: Geometry of the modeled snap hook and locking mechanism.
Material Properties
For the hook, assume an elastoplastic material model with isotropic hardening and a constant tangent hardening modulus, with material properties according to the following table.
Material parameter
Value
Young’s modulus
10 GPa
Poisson’s number
0.35
Yield stress
120 MPa
Isotropic tangent modulus
1.2 GPa
The lock is assumed to be rigid and therefore do not require any physics nor material properties.
Boundary Conditions
•
The locking mechanism is considered as rigid, and is modeled as a meshed surface without any physics defined.
•
A prescribed displacement boundary condition is applied at the rightmost bottom surface of the hook. The displacement in the x direction is gradually changed by using the parametric solver; the other two displacement components are zero.
•
A symmetry condition is applied on a boundary aligned with the xy-plane
•
All the other boundaries are free boundaries. However, several of them are selected as parts of a contact pair with the destination side being on the hook surface.
•
Contact between the hook and the look is modeled using a penalty formulation. A Coulomb friction model is applied for the tangential behavior.
Results
The maximum von Mises stress levels are found at parameter step 0.66, that is, just before the hook enters the slot, see Figure 2.
The force required for the insertion and removal of the fastener is shown in Figure 3 as function of the displacement. Distinct peaks are clearly visible that coincide with the instances that the hook comes into and looses contact with the look.
The insertion of the hook causes it to become permanently deformed. As you can see in Figure 4, after the hook has been removed there is a region where the plastic strains are greater than zero. This means that the hook has not returned to its original shape
Figure 2: Distribution of von Mises stress in the hook just before it enters the slot.
.
Figure 3: The mounting force as a function of displacement.
.
Figure 4: Equivalent plastic strain in the hook after its removal from the slot.
Application Library path: Nonlinear_Structural_Materials_Module/Plasticity/snap_hook
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>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Geometry 1
Import 1 (imp1)
1
In the Home toolbar, click  Import.
2
In the Settings window for Import, locate the Import section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file snap_hook.mphbin.
5
Click  Import.
Partition Domains 1 (pard1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Partition Domains.
2
On the object imp1(2), select Domain 1 only.
3
In the Settings window for Partition Domains, locate the Partition Domains section.
4
From the Partition with list, choose Extended faces.
5
On the object imp1(2), select Boundary 11 only.
It might be easier to select the correct boundary by using the Selection List window. To open this window, in the Home toolbar click Windows and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
Form Union (fin)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 click Form Union (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
From the Action list, choose Form an assembly.
4
Clear the Create pairs check box.
Mesh Control Domains 1 (mcd1)
1
In the Geometry toolbar, click  Virtual Operations and choose Mesh Control Domains.
2
On the object fin, select Domains 1–3 only.
3
In the Settings window for Mesh Control Domains, click  Build Selected.
4
Click the  Zoom Extents button in the Graphics toolbar.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, locate the Domain Selection section.
3
From the Selection list, choose Manual.
4
Select Domain 1 only.
Before adding the material for the hook, specify the plasticity model. This way, you can see which material parameters are required.
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid) click Linear Elastic Material 1.
Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Plasticity.
2
In the Settings window for Plasticity, locate the Domain Selection section.
3
In the list, select 2 (not applicable).
4
Select Domain 1 only.
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 Geometric Entity Selection section.
3
In the list, select 2.
4
Select Domain 1 only.
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
1e10[Pa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.35
1
Young’s modulus and Poisson’s ratio
Density
rho
7850[kg/m^3]
kg/m³
Basic
Definitions
Increase the initial yield stress near the contact surface to avoid spurious plastic deformations that might occur due to the computational errors during iterations in the contact force calculations. To implement this, first define a step function that smoothly drops from 1000 to 1 near the hook tip. Then use the step function as a multiplier for the yield stress.
Step 1 (step1)
1
In the Home toolbar, click  Functions and choose Local>Step.
2
In the Settings window for Step, locate the Parameters section.
3
In the Location text field, type 1.5[mm].
4
In the From text field, type 1e3.
5
Click to expand the Smoothing section. In the Size of transition zone text field, type 1e-3.
Set the yield stress of the material definition and multiply it with the step function. Use negative X material coordinate as an argument since it increases along the length of the hook.
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
Initial yield stress
sigmags
1.2e8[Pa]*step1(-X)
Pa
Elastoplastic material model
Isotropic tangent modulus
Et
1.2e9[Pa]
Pa
Elastoplastic material model
Definitions
contact_src
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type contact_src in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select the Group by continuous tangent check box.
5
Select Boundaries 22 and 26–29 only.
contact_dst
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type contact_dst in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 14–16, 18, and 19 only.
Contact Pair 1 (p1)
1
In the Definitions toolbar, click  Pairs and choose Contact Pair.
2
In the Settings window for Pair, locate the Source Boundaries section.
3
From the Selection list, choose contact_src.
4
Locate the Destination Boundaries section. Click to select the  Activate Selection toggle button.
5
From the Selection list, choose contact_dst.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
para
0
0
Continuation parameter
Definitions
Displacement
1
In the Definitions toolbar, click  Interpolation.
2
In the Settings window for Interpolation, type Displacement in the Label text field.
3
Locate the Definition section. From the Data source list, choose File.
4
Click  Browse.
5
Browse to the model’s Application Libraries folder and double-click the file snap_hook_disp.txt.
6
Click  Import.
7
In the Function name text field, type disp.
8
Locate the Interpolation and Extrapolation section. From the Interpolation list, choose Piecewise cubic.
9
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
1
10
In the Function table, enter the following settings:
Function
Unit
disp
mm
Solid Mechanics (solid)
Prescribed Displacement 1
1
In the Physics toolbar, click  Boundaries and choose Prescribed Displacement.
2
Select Boundary 2 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
Select the Prescribed in x direction check box.
5
Select the Prescribed in y direction check box.
6
Select the Prescribed in z direction check box.
7
In the u 0 x text field, type disp(para).
Contact 1
In the Model Builder window, click Contact 1.
Friction 1
1
In the Physics toolbar, click  Attributes and choose Friction.
2
In the Settings window for Friction, locate the Friction Parameters section.
3
In the μ text field, type 0.1.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundary 4 only.
Now create the mesh, start by defining a refined mesh in the contact region and where plastic strains are expected.
Mesh 1
Edge 1
1
In the Mesh toolbar, click  Boundary and choose Edge.
2
Select Edges 24, 33, 36, 39, 45, and 50 only.
Size 1
1
Right-click Edge 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section.
5
Select the Maximum element size check box. In the associated text field, type 4e-5.
6
Select the Minimum element size check box. In the associated text field, type 1E-5.
7
Select the Curvature factor check box. In the associated text field, type 0.2.
Size
1
In the Model Builder window, under Component 1 (comp1)>Mesh 1 click Size.
2
In the Settings window for Size, locate the Element Size section.
3
Click the Custom button.
4
Locate the Element Size Parameters section. In the Maximum element size text field, type 3E-4.
5
In the Minimum element size text field, type 1e-4.
6
In the Maximum element growth rate text field, type 3.
7
In the Curvature factor text field, type 0.3.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1, 3, and 4 only.
Mapped 1
Add a surface mesh for the lock. Notice that no mesh is needed for the domain.
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
In the Settings window for Mapped, locate the Boundary Selection section.
3
From the Selection list, choose contact_src.
Size 1
1
Right-click Mapped 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely coarse.
Distribution 1
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Edges 65 and 71 only.
3
In the Settings window for Distribution, click  Build All.
4
Click the  Zoom Extents button in the Graphics toolbar.
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 check box.
Set up an auxiliary continuation sweep for the para parameter.
4
Click to expand the Study Extensions section. Select the Auxiliary sweep check box.
5
Click  Add.
6
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Continuation parameter)
range(0,2e-2,2)
 
7
In the Home toolbar, click  Compute.
Results
Stress (solid)
1
In the Settings window for 3D Plot Group, locate the Data section.
2
From the Parameter value (para) list, choose 0.66.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Stress (solid)
Add surface plot of the lock. You can write an arbitrary value in the expression field since a uniform color is used.
Surface 1
1
In the Model Builder window, right-click Stress (solid) and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type 1.
4
Click to expand the Title section. From the Title type list, choose None.
5
Click to collapse the Title section. Locate the Coloring and Style section. From the Coloring list, choose Uniform.
6
From the Color list, choose Gray.
Selection 1
1
Right-click Surface 1 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose contact_src.
Stress (solid)
Create a new view to plot the stress in the XY-plane.
1
In the Model Builder window, under Results click Stress (solid).
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 Stress (solid) toolbar, click  Plot.
5
Click the  Go to XY View button in the Graphics toolbar.
View 3D 2
1
In the Model Builder window, expand the Results>Views node, then click View 3D 2.
2
In the Settings window for View 3D, locate the View section.
3
Clear the Show grid check box.
4
Select the Lock camera check box.
This helps to ensure that the view is not accidentally changed.
Camera
1
In the Model Builder window, expand the View 3D 2 node, then click Camera.
2
In the Settings window for Camera, locate the Camera section.
3
From the Projection list, choose Orthographic.
Add a predefined plot showing the equivalent plastic strain.
4
In the Home toolbar, click  Add Predefined Plot.
Add Predefined Plot
1
Go to the Add Predefined Plot window.
2
In the tree, select Study 1/Solution 1 (sol1)>Solid Mechanics>Equivalent Plastic Strain (solid).
3
Click Add Plot in the window toolbar.
4
In the Home toolbar, click  Add Predefined Plot.
5
Click  Add Predefined Plot.
Results
Deformation 1
1
In the Model Builder window, expand the Results>Equivalent Plastic Strain (solid) node.
2
Right-click Surface 1 and choose Deformation.
3
In the Settings window for Deformation, locate the Scale section.
4
Select the Scale factor check box. In the associated text field, type 1.
Equivalent Plastic Strain (solid)
Add surface plot of the lock. You can write an arbitrary value in the expression field since a uniform color is used.
Surface 2
1
In the Model Builder window, right-click Equivalent Plastic Strain (solid) and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type 1.
4
Click to expand the Title section. From the Title type list, choose None.
5
Click to collapse the Title section. Locate the Coloring and Style section. From the Coloring list, choose Uniform.
6
From the Color list, choose Gray.
Selection 1
1
Right-click Surface 2 and choose Selection.
2
In the Settings window for Selection, locate the Selection section.
3
From the Selection list, choose contact_src.
4
In the Equivalent Plastic Strain (solid) toolbar, click  Plot.
5
Click the  Go to Default View button in the Graphics toolbar to return to the model’s default view.
Plot the reaction force needed to position the hook as function of the displacement.
Reaction force
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Reaction force in the Label text field.
3
Locate the Legend section. Clear the Show legends check box.
Global 1
1
Right-click Reaction force and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
2*solid.RFtotalx
N
Reaction force
The factor of two is included to give the total force needed to position the hook. The computed reaction forces correspond to a half of the real structure, since you make use of the symmetry.
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type disp(para).
6
From the Unit list, choose mm.
7
Click to expand the Coloring and Style section. From the Width list, choose 2.
8
Find the Line markers subsection. From the Marker list, choose Point.
Add a color expression to distinguish the insertion and removal paths.
Color Expression 1
1
Right-click Global 1 and choose Color Expression.
2
In the Settings window for Color Expression, locate the Expression section.
3
In the Expression text field, type para>1.
4
Click to expand the Title section. From the Title type list, choose Manual.
5
In the Title text area, type Insertion (green) and removal (red).
6
Locate the Coloring and Style section. Click  Change Color Table.
7
In the Color Table dialog box, select Traffic>TrafficLight in the tree.
8
Click OK.
9
In the Reaction force toolbar, click  Plot.