PDF
Die Forming
Introduction
Die forming is a widespread manufacture process for sheet-metal forming. The workpiece, usually a metal sheet, is permanently reshaped around a die through plastic deformation by forming and drawing processes.
Simulations can be carried out in order to avoid cracks, tears, wrinkles, and too much thinning and stretching. They are also useful to estimate and overcome the springback phenomenon: once the forming process is done and the forming tools are removed, the workpiece attempts to partially recover its initial shape through relaxation of the elastic stresses. The springback can cause the formed blank to get an unexpected state of warping. To cope with this effect, it is possible to over-bend the sheet. The die, the punch, and the blank-holder must be manufactured to incorporate this effect.
In this model, a flat metal sheet made of aluminum is pressed onto a curved die by a similarly shaped punch. Both the forming and the springback phenomena are modeled. From a simulation point of view, the problem is severely nonlinear due to contact, geometric nonlinearity, and large plastic strains. Figure 1shows the shape after forming.
Figure 1: Deformed shape after the forming process.
Model Definition
The model geometry is shown in Figure 2. Due to the axial symmetry, a 2D axisymmetric formulation can be used. The die and the blank-holder together clamp the blank to be reshaped, while the punch performs the drawing, stretching, and bending.
Figure 2: Forming tools setup.
The analysis is carried out in two steps. First, the punch is pushed toward the sheet through a displacement of 40 mm. This step aims to simulate the forming and drawing processes. A second step is used to perform the springback analysis. The punch is released progressively to model the springback phenomenon.
The sheet is made of aluminum. An isotropic elastoplastic material with user-defined isotropic hardening and large plastic strain formulation is used to characterize the plastic deformation.
The die and the punch are made of structural steel, so they are much more rigid than the aluminum sheet. The die and holder are fixed, and the punch deforms the blank with a prescribed vertical displacement, which is ramped linearly.
Results and Discussion
Figure 3 shows the residual stress after the release of the punch, where large stresses are present in the deformed corners of the blank. These are a consequence of the plastic strains that are shown in Figure 4. As expected, large plastic strains occur, and at the most strained location, the plastic strain exceeds 60%.
Figure 5 shows the variation of the thickness of the deformed part obtained from the die forming process. The initial blank thickness is 0.2 mm. The maximum thinning is observed at the center of the part. A comparison of the maximum radial position between the forming and the release stage would give an idea of the springback.
Finally, the reaction force that is necessary to apply to the punch during the process is shown in Figure 6.
Figure 3: Residual stress after release of the punch.
.
Figure 4: Plastic strains after release of the punch.
Figure 5: Thickness of the part after the die forming process.
Figure 6: Force applied to the punch during the die forming.
Notes About the COMSOL Implementation
The strong nonlinearity of the problem due to contact, plasticity, and geometric nonlinearity may cause some convergence issues. Some useful tips for improving the convergence are given below.
•
Choose the source and destination in contact pairs carefully. Based on stiffness of the metal parts, the sheet should be the destination. The blank/sheet is meshed finely compared to the source. The curved boundaries of the source are also finely meshed compared to the flat boundaries.
•
The parametric sweep must use steps that are small enough to avoid divergence of the solution. If the parametric step chosen by the solver is too large, the initial guess of a solution based on previous computed solution could be too far from the solution in the current step. Use Tuning of step size to manually adjust the parametric steps.
•
To compute the thickness of the deformed shape, a nonlocal projection coupling is used to define the variable th. Such a coupling can integrate any expression across a domain in the spatial frame. Here, integrating ‘1’ across the blank returns its deformed thickness.
Contact is in the model described using the augmented Lagrangian method with a coupled solution method. This method is chosen over the default penalty method to improve the accuracy of the contact condition, that is, to avoid large overclosure between the parts.
Application Library path: Nonlinear_Structural_Materials_Module/Plasticity/die_forming
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  2D Axisymmetric.
2
In the Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
3
Click Add.
4
In the Added physics interfaces tree, select Solid Mechanics (solid).
5
Click  Study.
6
In the Select Study tree, select General Studies > Stationary.
7
Click  Done.
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
sigma_y0
124[MPa]
1.24E8 Pa
Initial yield stress
U_p
40[mm]
0.04 m
Punch displacement
R0
0.69
0.69
Lankford's coefficient r0
R45
0.69
0.69
Lankford's coefficient r45
R90
0.69
0.69
Lankford's coefficient 90
F
R0/(R90*(R0+1))/sigma_y0^2
3.8483E-17 m²·s4/kg²
Hill's coefficient
G
1/(R0+1)/sigma_y0^2
3.8483E-17 m²·s4/kg²
Hill's coefficient
H
R0/(R0+1)/sigma_y0^2
2.6553E-17 m²·s4/kg²
Hill's coefficient
L
0
0
Hill's coefficient
M
0
0
Hill's coefficient
N
0
0
Hill's coefficient
p
0
0
Loading parameter
Geometry 1
Set the unit of geometry to millimeters (mm).
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Polygon 1 (pol1)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Object Type section.
3
From the Type list, choose Open curve.
4
Locate the Coordinates section. In the table, enter the following settings:
r (mm)
z (mm)
0
42
88.5
42
88.5
2
257.5
2
257.5
40
Fillet 1 (fil1)
1
In the Geometry toolbar, click  Fillet.
2
On the object pol1, select Point 2 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 16.
Fillet 2 (fil2)
1
In the Geometry toolbar, click  Fillet.
2
On the object fil1, select Points 3 and 5 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 18.
Thicken 1 (thi1)
1
In the Geometry toolbar, click  Conversions and choose Thicken.
2
Select the object fil2 only.
3
In the Settings window for Thicken, locate the Options section.
4
From the Offset list, choose Asymmetric.
5
In the Upside thickness text field, type 4.
Fillet 1 (fil1), Fillet 2 (fil2), Polygon 1 (pol1), Thicken 1 (thi1)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1, Ctrl-click to select Polygon 1 (pol1), Fillet 1 (fil1), Fillet 2 (fil2), and Thicken 1 (thi1).
2
Right-click and choose Group.
Punch
1
In the Settings window for Group, type Punch in the Label text field.
2
Click  Build Selected.
Polygon 2 (pol2)
1
In the Geometry toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Object Type section.
3
From the Type list, choose Open curve.
4
Locate the Coordinates section. In the table, enter the following settings:
r (mm)
z (mm)
0
0
86
0
86
-40
260
-40
260
0
386
0
Fillet 3 (fil3)
1
In the Geometry toolbar, click  Fillet.
2
In the Settings window for Fillet, locate the Points section.
3
Click to select the  Activate Selection toggle button for Vertices to fillet.
4
On the object pol2, select Points 3 and 5 only.
5
Locate the Radius section. In the Radius text field, type 16.
Fillet 4 (fil4)
1
In the Geometry toolbar, click  Fillet.
2
On the object fil3, select Points 3 and 5 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 16.
Thicken 2 (thi2)
1
In the Geometry toolbar, click  Conversions and choose Thicken.
2
Select the object fil4 only.
3
In the Settings window for Thicken, locate the Options section.
4
From the Offset list, choose Asymmetric.
5
In the Downside thickness text field, type 4.
Fillet 3 (fil3), Fillet 4 (fil4), Polygon 2 (pol2), Thicken 2 (thi2)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1, Ctrl-click to select Polygon 2 (pol2), Fillet 3 (fil3), Fillet 4 (fil4), and Thicken 2 (thi2).
2
Right-click and choose Group.
Die
1
In the Settings window for Group, type Die in the Label text field.
2
Click  Build Selected.
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 80.
4
In the Height text field, type 20.
5
Locate the Position section. In the r text field, type 300.
6
In the z text field, type 2.
7
Click  Build Selected.
Rectangle 2 (r2)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 380.
4
In the Height text field, type 2.
5
Click  Build All Objects.
6
Click  Build Selected.
Rectangle 1 (r1)
In the Model Builder window, under Component 1 (comp1) > Geometry 1 right-click Rectangle 1 (r1) and choose Group.
Holder
In the Settings window for Group, type Holder in the Label text field.
Rectangle 2 (r2)
In the Model Builder window, under Component 1 (comp1) > Geometry 1 right-click Rectangle 2 (r2) and choose Group.
Blank
In the Settings window for Group, type Blank in the Label text field.
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
From the Pair type list, choose Contact pair.
5
In the Geometry toolbar, click  Build All.
Global Definitions
Prescribed Punch Displacement
1
In the Model Builder window, expand the Component 1 (comp1) > Definitions node.
2
Right-click Global Definitions and choose Functions > Interpolation.
3
In the Settings window for Interpolation, type Prescribed Punch Displacement in the Label text field.
4
Locate the Definition section. In the Function name text field, type U_punch.
5
In the table, enter the following settings:
t
f(t)
0
0
1
-U_p
2
0
6
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
1
7
In the Function table, enter the following settings:
Function
Unit
U_punch
m
Hardening Function
1
In the Home toolbar, click  Functions and choose Global > Interpolation.
2
In the Settings window for Interpolation, type Hardening Function in the Label text field.
3
Locate the Definition section. In the Function name text field, type sigma_h.
4
In the table, enter the following settings:
t
f(t)
0
0
0.02
43
0.05
76
0.1
103
0.15
115
0.2
127
0.3
129
0.4
129.3
0.5
129.4
5
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
1
6
In the Function table, enter the following settings:
Function
Unit
sigma_h
MPa
Definitions
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
Select Domain 3 only.
3
In the Settings window for Integration, locate the Advanced section.
4
From the Method list, choose Summation over nodes.
Create explicit selections for the contact boundaries and various domains.
Punch, Contact
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, locate the Input Entities section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundaries 26, 28, 30, 34, 35, 37, and 39 only.
5
In the Label text field, type Punch, Contact.
Die, Contact
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Die, Contact in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 3, 5, 7, 8, 11, 14, 16, 18, and 19 only.
Holder, Contact
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Holder, Contact in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 42 only.
Select the boundary of the blank which is in contact with the punch and the holder.
Blank, Contact Up
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Blank, Contact Up in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 23 only.
Select the boundary of the blank which is in contact with the die.
Blank, Contact Down
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Blank, Contact Down in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundary 22 only.
Die
1
In the Definitions toolbar, click  Explicit.
2
Select Domain 1 only.
3
In the Settings window for Explicit, type Die in the Label text field.
Punch
1
In the Definitions toolbar, click  Explicit.
2
Select Domain 3 only.
3
In the Settings window for Explicit, type Punch in the Label text field.
Holder
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Holder in the Label text field.
3
Select Domain 4 only.
Blank
1
In the Definitions toolbar, click  Explicit.
2
Select Domain 2 only.
3
In the Settings window for Explicit, type Blank in the Label text field.
Create a variable to evaluate the blank thickness after of the release of the punch.
General Projection 1 (genproj1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose General Projection.
2
Select Domain 2 only.
3
In the Settings window for General Projection, locate the Source Map section.
4
In the r-expression text field, type R.
5
In the z-expression text field, type Z.
6
Locate the Destination Map section. In the r-expression text field, type R.
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
th
genproj1(1)
m
Thickness
4
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Domain.
5
Select Domain 2 only.
Die and Holder
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Die and Holder in the Label text field.
3
Locate the Input Entities section. Under Selections to add, click  Add.
4
In the Add dialog, in the Selections to add list, choose Die and Holder.
5
Click OK.
Die to Blank
Modify the contact pairs by activating Manual control of selection option. Make sure that the blank is destination in all contact pairs.
1
In the Model Builder window, under Component 1 (comp1) > Definitions click Contact Pair 1 (ap1).
2
In the Settings window for Pair, locate the Pair Type section.
3
Select the Manual control of selections and pair type checkbox.
4
Locate the Source Boundaries section. From the Selection list, choose Die, Contact.
5
Locate the Destination Boundaries section. From the Selection list, choose Blank, Contact Down.
6
In the Label text field, type Die to Blank.
Punch to Blank
1
In the Model Builder window, click Contact Pair 2 (ap2).
2
In the Settings window for Pair, locate the Pair Type section.
3
Select the Manual control of selections and pair type checkbox.
4
Locate the Source Boundaries section. From the Selection list, choose Punch, Contact.
5
Locate the Destination Boundaries section. From the Selection list, choose Blank, Contact Up.
6
In the Label text field, type Punch to Blank.
Holder to Blank
1
In the Model Builder window, click Contact Pair 3 (ap3).
2
In the Settings window for Pair, locate the Pair Type section.
3
Select the Manual control of selections and pair type checkbox.
4
Locate the Source Boundaries section. From the Selection list, choose Holder, Contact.
5
Locate the Destination Boundaries section. From the Selection list, choose Blank, Contact Up.
6
In the Label text field, type Holder to Blank.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Structural steel.
4
Click the Add to Component button in the window toolbar.
5
In the tree, select Built-in > Aluminum.
6
Click the Add to Component button in the window toolbar.
7
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Aluminum (mat2)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Selection list, choose Blank.
Solid Mechanics (solid)
Linear Elastic Material 1
Set the blank domain with an elastoplastic material model.
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
From the Selection list, choose Blank.
4
Locate the Plasticity Model section. From the σe list, choose Hill orthotropic.
5
From the Specify list, choose Hill’s coefficients.
6
From the σys0 list, choose Reciprocal average.
7
From the εpe list, choose von Mises.
8
Find the Isotropic hardening model subsection. From the list, choose Hardening function.
Contact 1
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Contact 1.
2
In the Settings window for Contact, locate the Contact Method section.
3
From the list, choose Augmented Lagrangian.
4
From the Solution method list, choose Fully coupled.
5
Locate the Contact Pressure Penalty Factor section. From the Penalty factor control list, choose Manual tuning.
6
In the fp text field, type 5e-4.
Increase the integration order of the contact equation to improve the numerical accuracy.
7
Click the  Show More Options button in the Model Builder toolbar.
8
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Advanced Physics Options.
9
Click OK.
10
In the Settings window for Contact, click to expand the Quadrature Settings section.
11
Clear the Use automatic quadrature settings checkbox.
12
In the Integration order text field, type 6.
Fix the die and the holder.
Fixed Constraint 1
1
In the Physics toolbar, click  Domains and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, locate the Domain Selection section.
3
From the Selection list, choose Die and Holder.
Set prescribed displacements for the punch.
Prescribed Displacement 1
1
In the Physics toolbar, click  Domains and choose Prescribed Displacement.
2
In the Settings window for Prescribed Displacement, locate the Domain Selection section.
3
From the Selection list, choose Punch.
4
Locate the Prescribed Displacement section. From the Displacement in r direction list, choose Prescribed.
5
From the Displacement in z direction list, choose Prescribed.
6
In the u 0 z text field, type U_punch(p).
Materials
Aluminum (mat2)
1
In the Model Builder window, under Component 1 (comp1) > Materials click Aluminum (mat2).
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
Hill’s coefficients
{Hillcoefficients1, Hillcoefficients2, Hillcoefficients3, Hillcoefficients4, Hillcoefficients5, Hillcoefficients6}
{F, G, H, L, M, N}
m²·s4/kg²
Elastoplastic material model
Hardening function
sigmagh
sigma_h(solid.epe)
Pa
Elastoplastic material model
Density
rho
2700[kg/m^3]
kg/m³
Basic
Young’s modulus
E
70[GPa]
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.33
1
Young’s modulus and Poisson’s ratio
Mesh 1
Mesh the curved boundaries more densely compared to the flat boundaries. Use a fine mesh for the blank as it is destination in all contact pairs.
Mapped 1
1
In the Mesh toolbar, click  Mapped.
2
In the Settings window for Mapped, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Blank.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundary 21 only.
3
Click the  Zoom Extents button in the Graphics toolbar.
4
In the Settings window for Distribution, locate the Distribution section.
5
In the Number of elements text field, type 3.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
Select Boundary 23 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 400.
Edge 1
1
In the Mesh toolbar, click  More Generators and choose Edge.
Zoom in and out to select the following boundaries.
2
Select Boundaries 14, 16, 18, 19, 35, 37, and 39 only.
Size 1
1
Right-click Edge 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
4
Click the Custom button.
5
Locate the Element Size Parameters section.
6
Select the Maximum element size checkbox. In the associated text field, type 1.
7
Select the Minimum element size checkbox. In the associated text field, type 0.001.
Mapped 2
1
In the Mesh toolbar, click  Mapped.
2
In the Settings window for Mapped, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 4 only.
Distribution 1
1
Right-click Mapped 2 and choose Distribution.
2
Select Boundaries 41 and 43 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 1.
Free Triangular 1
In the Mesh toolbar, click  Free Triangular.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Coarse.
4
Click  Build All.
Study 1
1
In the Model Builder window, click Study 1.
2
Click Show Default Solver to customize the solver settings. Use a Constant (Newton) method as the nonlinear method in the Fully Coupled node and a Linear predictor in the Parametric node.
Solution 1 (sol1)
In the Study toolbar, click  Show Default Solver.
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
p (Loading parameter)
range(0,0.01,2)
 
Solution 1 (sol1)
1
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Fully Coupled 1.
2
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
3
From the Nonlinear method list, choose Constant (Newton).
4
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 click Parametric.
5
In the Settings window for Parametric, click to expand the Continuation section.
6
Select the Tuning of step size checkbox.
7
In the Initial step size text field, type 1e-5.
8
In the Minimum step size text field, type 1e-5.
9
In the Maximum step size text field, type 0.01.
10
From the Predictor list, choose Linear.
Add a stop condition to prevent computation after full release. The stop condition is controlled by the gap distance between punch and blank.
11
Right-click Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > Parametric and choose Stop Condition.
12
In the Settings window for Stop Condition, locate the Stop Expressions section.
13
Click  Add.
14
In the table, enter the following settings:
Stop expression
Stop if
Active
Description
comp1.solid.gapmin_ap2>1e-4
True (>=1)
√
Stop expression 1
15
Locate the Output at Stop section. From the Add solution list, choose Step after stop.
Click on Get Initial Value in order to generate the default plots, so that they can be modified, and can be used for visualization while solving.
16
In the Study toolbar, click  Get Initial Value.
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
From the Update at list, choose Steps taken by solver.
Now compute the solution.
5
In the Study toolbar, click  Compute.
Results
Residual Stress
The default plot shows the von Mises stress after release of the punch as in Figure 3:
1
In the Settings window for 2D Plot Group, type Residual Stress in the Label text field.
2
In the Residual Stress toolbar, click  Plot.
The following steps create the plot in Figure 1:
Study 1/Solution 1, Blank
1
In the Model Builder window, expand the Results > Datasets node.
2
Right-click Results > Datasets > Study 1/Solution 1 (sol1) and choose Duplicate.
3
In the Settings window for Solution, type Study 1/Solution 1, Blank in the Label text field.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domain 2 only.
Revolution 2D
1
In the Model Builder window, under Results > Datasets click Revolution 2D.
2
In the Settings window for Revolution 2D, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1, Blank (sol1).
4
Click to expand the Revolution Layers section. In the Start angle text field, type 0.
5
In the Revolution angle text field, type 360.
Deformed Shape, 3D
1
In the Model Builder window, under Results click Stress, 3D (solid).
2
In the Settings window for 3D Plot Group, type Deformed Shape, 3D in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Label.
4
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Surface 1
1
In the Model Builder window, expand the Deformed Shape, 3D node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
Select the Description checkbox. In the associated text field, type Deformed shape, 3D.
Material Appearance 1
1
Right-click Surface 1 and choose Material Appearance.
2
In the Settings window for Material Appearance, locate the Appearance section.
3
From the Material list, choose Aluminum (mat2).
4
In the Deformed Shape, 3D toolbar, click  Plot.
The following steps create the plot in Figure 4:
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) > Solid Mechanics > Equivalent Plastic Strain (solid).
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
Equivalent Plastic Strain (solid)
1
In the Settings window for 2D Plot Group, locate the Plot Settings section.
2
Clear the Plot dataset edges checkbox.
Deformation 1
1
In the Model Builder window, expand the 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 checkbox. In the associated text field, type 1.
5
In the Equivalent Plastic Strain (solid) toolbar, click  Plot.
The following steps create the plot in Figure 5:
Blank Thickness
1
In the Results toolbar, click  2D Plot Group.
2
In the Settings window for 2D Plot Group, type Blank Thickness in the Label text field.
3
Locate the Plot Settings section. From the Frame list, choose Spatial  (r, phi, z).
Surface 1
1
Right-click Blank Thickness and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type th.
Deformation 1
1
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 1.
4
In the Blank Thickness toolbar, click  Plot.
The following steps create the plot in Figure 6:
Punch Force
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Punch Force in the Label text field.
Global 1
1
Right-click Punch 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
-intop1(solid.RFz)
kN
Punch force
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type -U_punch(p).
6
Select the Description checkbox. In the associated text field, type Vertical displacement.
7
Click to expand the Legends section. Clear the Show legends checkbox.
8
In the Punch Force toolbar, click  Plot.