Die Forming

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, large strain plasticity, and geometric nonlinearity. 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 towards 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 inFigure 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 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.

Nonlinear_Structural_Materials_Module/Plasticity/die_forming

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

In the tree, select .

Click

In the tree, select .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

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).

In the window, under click .

In the window for , locate the section.

From the list, choose .

Polygon 1 (pol1)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Locate the 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)

In the toolbar, click

On the object , select Point 3 only.

In the window for , locate the section.

In the text field, type 16.

Fillet 2 (fil2)

In the toolbar, click

On the object , select Points 3 and 5 only.

In the window for , locate the section.

In the text field, type 18.

Thicken 1 (thi1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

From the list, choose .

In the text field, type 4.

Fillet 1 (fil1), Fillet 2 (fil2), Polygon 1 (pol1), Thicken 1 (thi1)

In the window, under , Ctrl-click to select , , , and .

Right-click and choose .

Punch

In the window for , type Punch in the text field.

Click

Polygon 2 (pol2)

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Locate the 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)

In the toolbar, click

On the object , select Points 3 and 5 only.

In the window for , locate the section.

In the text field, type 16.

Fillet 4 (fil4)

In the toolbar, click

On the object , select Points 3 and 5 only.

In the window for , locate the section.

In the text field, type 16.

Thicken 2 (thi2)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

From the list, choose .

In the text field, type 4.

Fillet 3 (fil3), Fillet 4 (fil4), Polygon 2 (pol2), Thicken 2 (thi2)

In the window, under , Ctrl-click to select , , , and .

Right-click and choose .

Die

In the window for , type Die in the text field.

Click

Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 80.

In the text field, type 20.

Locate the section. In the text field, type 300.

In the text field, type 2.

Click

Rectangle 2 (r2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 380.

In the text field, type 2.

Click

Rectangle 1 (r1)

In the window, under right-click and choose .

Holder

In the window for , type Holder in the text field.

Rectangle 2 (r2)

In the window, under right-click and choose .

Blank

In the window for , type Blank in the text field.

Form Union (fin)

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Global Definitions

Prescribed Punch Displacement

In the window, expand the node.

Right-click and choose .

In the window for , type Prescribed Punch Displacement in the text field.

Locate the section. In the text field, type U_punch.

In the table, enter the following settings:


t	f(t)
0	0
1	-U_p
2	0

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


Argument	Unit
t	1

In the table, enter the following settings:


Function	Unit
U_punch	m

Hardening Function

In the toolbar, click

and choose .

In the window for , type Hardening Function in the text field.

Locate the section. In the text field, type sigma_h.

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

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


Argument	Unit
t	1

In the table, enter the following settings:


Function	Unit
sigma_h	MPa

Definitions

Integration 1 (intop1)

In the toolbar, click

and choose .

Select Domain 3 only.

In the window for , locate the section.

From the list, choose .

Create explicit selections for the contact boundaries and various domains.

contact_punch

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Boundaries 26, 28, 30, 34, 35, 37, and 39 only.

In the text field, type contact_punch.

contact_die

In the toolbar, click

In the window for , type contact_die in the text field.

Locate the section. From the list, choose .

Select Boundaries 3, 5, 7, 8, 11, 14, 16, 18, and 19 only.

contact_holder

In the toolbar, click

In the window for , type contact_holder in the text field.

Locate the section. From the list, choose .

Select Boundary 42 only.

Select the boundary of the blank which is in contact with the punch and the holder.

contact_blank_up

In the toolbar, click

In the window for , type contact_blank_up in the text field.

Locate the section. From the list, choose .

Select Boundary 23 only.

Select the boundary of the blank which is in contact with the die.

contact_blank_down

In the toolbar, click

In the window for , type contact_blank_down in the text field.

Locate the section. From the list, choose .

Select Boundary 22 only.

die

In the toolbar, click

Select Domain 1 only.

In the window for , type die in the text field.

punch

In the toolbar, click

Select Domain 3 only.

In the window for , type punch in the text field.

holder

In the toolbar, click

In the window for , type holder in the text field.

Select Domain 4 only.

blank

In the toolbar, click

Select Domain 2 only.

In the window for , type blank in the text field.

Create a variable to evaluate the blank thickness after of the release of the punch.

General Projection 1 (genproj1)

In the toolbar, click

and choose .

Select Domain 2 only.

In the window for , locate the section.

In the text field, type R.

In the text field, type Z.

Locate the section. In the text field, type R.

Variables 1

In the window, right-click and choose .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
th	genproj1(1)	m	Thickness

Locate the section. From the list, choose .

Select Domain 2 only.

die_and_holder

In the toolbar, click

In the window for , type die_and_holder in the text field.

Locate the section. Under , click

In the dialog box, in the list, choose and .

Click .

die_blank

Modify the contact pairs by activating option. Make sure that the blank is destination in all contact pairs.

In the window, under click .

In the window for , locate the section.

Select the check box.

Locate the section. From the list, choose .

In the text field, type die_blank.

punch_blank

In the window, click .

In the window for , locate the section.

Select the check box.

Locate the section. From the list, choose .

In the text field, type punch_blank.

holder_blank

In the window, click .

In the window for , locate the section.

Select the check box.

Locate the section. From the list, choose .

In the text field, type holder_blank.

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Materials

Aluminum (mat2)

In the window for , locate the section.

From the list, choose .

Solid Mechanics (solid)

Linear Elastic Material 1

Set the blank domain with an elastoplatic material model.

In the window, under click .

Plasticity 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

From the list, choose .

Find the subsection. From the list, choose .

Contact 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Locate the section. From the list, choose .

In the fp text field, type 1e-4.

Increase the integration order of the contact equation to improve the numerical accuracy

Click the

button in the toolbar.

In the dialog box, in the tree, select the check box for the node .

Click .

In the window for , click to expand the section.

Clear the check box.

In the text field, type 6.

Fix the die and the holder.

Fixed Constraint 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Set prescribed displacements for the punch.

Prescribed Displacement 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Select the check box.

Select the check box.

In the u 0 z text field, type U_punch(p).

Materials

Aluminum (mat2)

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
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	70e9[Pa]	Pa	Young’s modulus and Poisson’s ratio
Poisson’s ratio	nu	0.33	1	Young’s modulus and Poisson’s ratio
Relative permeability	mur_iso ; murii = mur_iso, murij = 0	1	1	Basic
Heat capacity at constant pressure	Cp	900[J/(kg*K)]	J/(kg·K)	Basic
Thermal conductivity	k_iso ; kii = k_iso, kij = 0	238[W/(m*K)]	W/(m·K)	Basic
Electrical conductivity	sigma_iso ; sigmaii = sigma_iso, sigmaij = 0	3.774e7[S/m]	S/m	Basic
Relative permittivity	epsilonr_iso ; epsilonrii = epsilonr_iso, epsilonrij = 0	1	1	Basic
Coefficient of thermal expansion	alpha_iso ; alphaii = alpha_iso, alphaij = 0	23e-6[1/K]	1/K	Basic
Murnaghan third-order elastic moduli	l	-2.5e11[Pa]	N/m²	Murnaghan
Murnaghan third-order elastic moduli	m	-3.3e11[Pa]	N/m²	Murnaghan
Murnaghan third-order elastic moduli	n	-3.5e11[Pa]	N/m²	Murnaghan
Lamé parameter λ	lambLame	5.1e10[Pa]	N/m²	Lamé parameters
Lamé parameter μ	muLame	2.6e10[Pa]	N/m²	Lamé parameters