Powder Compaction of a Cup

In this example, the fabrication of a cup through powder compaction is simulated. The powder compaction process is becoming common in the manufacturing industry, thanks to its potential to produce components of complex shape and high strength.

Combining the Fleck-Kuhn-McMeeking (FKM) model with the Gurson-Tvergaard-Needleman (GTN) model for porous plasticity makes it possible to cover a wide range of porosity values. Friction between the metal powder and the die is taken in to account. From a simulation point of view, this is a highly nonlinear structural analysis because of the contact interaction between the moving parts, the elastoplastic constitutive law selected for the metal powder, and the geometrical nonlinearity caused by the large displacements.

Model Definition

The geometry of workpiece (metal powder) and die are shown in Figure 1. The punch to compact the workpiece is not modeled. Instead, a prescribed displacement in the normal direction is used to compact the powder. Due to the axial symmetry, the size of model can be reduced.

Figure 1: Geometry of the workpiece (metal powder) and die.

Material Properties

For the aluminum metal powder, an elastoplastic material model with a constitutive relation given by a combination of the Fleck–Kuhn–McMeeking (FKM) model and the Gurson–Tvergaard–Needleman (GTN) is used. The parameters for the FKM-GTN model are given below.


Material parameter	Value
Young’s modulus	70 GPa
Poisson’s ratio	0.33
Initial yield stress	200 MPa
Tvergaard correction coefficient q1	1.5
Tvergaard correction coefficient q2	1
Tvergaard correction coefficient q3	2.25
Initial void volume fraction	0.28
Maximum void volume fraction	0.36

The material of the die is irrelevant, since it is assumed to be rigid. Hence, the rigid domain material model is selected for the die.

Boundary Conditions

The applied boundary conditions are:

•

The inner and outer dies are fixed.

•

A prescribed displacement boundary condition for the upper and lower face of the metal powder. The displacement in the z direction is controlled by a parameter called para.

Results

Figure 2 shows the volumetric plastic strain at the end of compaction process. At the middle of the fillet, the volumetric plastic strain is at its minimum. At ends of the fillet, the volumetric plastic strain is high. The volumetric plastic strain at the corner points of the workpiece are about 12%, probably due to the friction.

Figure 2: The volumetric plastic strain at the end of compaction.

The compaction process reduces the porosity of the aluminum powder and increases its density. This process also results in an increase in the strength of the component. Considering the type of geometry and loading, non-uniform changes in porosity are expected. Contours of the current void volume fraction or porosity are shown in Figure 3. The metal powder in the thin lower portion of the workpiece is more compacted than the material in the middle or top portion. At the central region near to the fillet, the metal powder is less compacted due to material sliding on the rounded corner.

Figure 3: Current void volume fraction at the end of compaction.

The von Mises stress along with effective plastic strain in the workpiece at the end of compaction is shown in Figure 4

Figure 4: The von-Mises stress in the workpiece at the end of compaction.

Notes About the COMSOL Implementation

To improve the convergence and speed up the computations a customized mesh is used. The curved boundaries in a contact are well resolved using finer mesh, while the straight edges of the rigid domains are meshed with single elements, see Figure 5. The mesh on rigid parts only serve to describe the geometry accurately.

The parametric steps in the solver settings are tuned according to the used mesh. Changes in the mesh size may cause slower convergence and could thus require a modified step size to obtain the solution efficiently.

Figure 5: Customized mesh.

Nonlinear_Structural_Materials_Module/Porous_Plasticity/powder_compaction_of_a_cup

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

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
para	0[mm]	0 m	Displacement parameter
sigmay0	200[MPa]	2E8 Pa	Initial yield stress
q1	1.5	1.5	Tvergaard correction coefficient
q2	1	1	Tvergaard correction coefficient
q3	2.25	2.25	Tvergaard correction coefficient
F0	0.28	0.28	Initial void volume fraction
Fmax	0.36	0.36	Maximum void volume fraction

Geometry 1

Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 20[mm].

In the text field, type 40[mm].

Rectangle 2 (r2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 10[mm].

In the text field, type 20[mm].

Difference 1 (dif1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Find the subsection. Click to select the

toggle button.

Select the object only.

Click

Fillet 1 (fil1)

In the toolbar, click

On the object , select Point 4 only.

It might be easier to select the correct point by using the window. To open this window, in the toolbar click and choose . (If you are running the cross-platform desktop, you find in the main menu.)

In the window for , locate the section.

In the text field, type 3[mm].

Click

Rectangle 3 (r3)

In the toolbar, click

In the window for , locate the section.

In the text field, type 10[mm].

In the text field, type 25[mm].

Locate the section. In the text field, type -5[mm].

Click

Fillet 2 (fil2)

In the toolbar, click

On the object , select Point 3 only.

In the window for , locate the section.

In the text field, type 3[mm].

Rectangle 4 (r4)

In the toolbar, click

In the window for , locate the section.

In the text field, type 5[mm].

In the text field, type 50[mm].

Locate the section. In the text field, type 20[mm].

In the text field, type -5[mm].

Click

Form Union (fin)

In the window, under click .

In the window for , locate the section.

From the list, choose .

In the toolbar, click

Click

Definitions

Add a model for domains 1 and 3 (die), and fix the domains. Set the density to zero as it does not affect the analysis.

Solid Mechanics (solid)

Rigid Material 1

In the window, expand the node.

Right-click and choose .

Select Domains 1 and 3 only.

In the window for , locate the section.

From the ρ list, choose .

Fixed Constraint 1

In the toolbar, click

and choose .

For the elastoplastic analysis of the workpiece, choose the porous plasticity model by adding a subnode to the .

Linear Elastic Material 1

In the window, under click .

Porous Plasticity 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Assign aluminum material properties to domain 2 (workpiece).

Materials

Aluminum

In the window, under right-click and choose .

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

Select Domain 2 only.

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


Property	Variable	Value	Unit	Property group
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
Density	rho	2700	kg/m³	Basic
Initial yield stress	sigmags	sigmay0	Pa	Poroplastic material model
Initial void volume fraction	f0	F0	1	Poroplastic material model
Tvergaard correction coefficient q1	q1GTN	q1	1	Poroplastic material model
Tvergaard correction coefficient q2	q2GTN	q2	1	Poroplastic material model
Tvergaard correction coefficient q3	q3GTN	q3	1	Poroplastic material model
Maximum void volume fraction	fmax	Fmax	1	Poroplastic material model

Solid Mechanics (solid)

Contact 1

In the window, under click .

Friction 1

In the toolbar, click

and choose .

In the window for , locate the section.

In the μ text field, type 0.1.

Prescribed Displacement 1

In the toolbar, click

and choose .

Select Boundary 8 only.

In the window for , locate the section.

Select the check box.

In the u 0 z text field, type -para.

Prescribed Displacement 2

In the toolbar, click

and choose .

Select Boundary 10 only.

In the window for , locate the section.

Select the check box.

In the u 0 z text field, type para.

Now create the mesh. Start by defining a refined mesh in the contact region between the inner die and the workpiece, specifically at the fillet. Use a single mesh element on the straight edges of the inner and outer die.

Mesh 1

Mapped 1

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Domain 3 only.

Distribution 1

Right-click and choose .

Select Boundaries 15 and 16 only.

In the window for , locate the section.

In the text field, type 1.

Free Triangular 1

In the toolbar, click

Distribution 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Click

In the dialog box, type 12 in the text field.

Click .

In the window for , locate the section.

In the text field, type 12.

Distribution 2

In the window, right-click and choose .

In the window for , locate the section.

Click

In the dialog box, type 5 in the text field.

Click .

In the window for , locate the section.

In the text field, type 27.

Distribution 3

Right-click and choose .

Select Boundaries 1–4 only.

In the window for , locate the section.

In the text field, type 1.

Free Triangular 1

Right-click and choose .

Study 1

Step 1: Stationary

Set up an auxiliary continuation sweep for the para parameter.

In the window, under click .

In the window for , click to expand the section.

Select the check box.

Click

In the table, enter the following settings:


Parameter name	Parameter value list	Parameter unit
para (Displacement parameter)	range(0,2e-5,2e-3)	m

Solution 1 (sol1)

In the toolbar, click

In the window, expand the node.

The step size is tuned in order to improve the convergence.

In the window, expand the node, then click .

In the window for , click to expand the section.

Select the check box.

In the text field, type 2e-7.

In the text field, type 2e-5.

In the toolbar, click

Add Predefined Plot

Go to the window.

In the tree, select and .

Click in the window toolbar.

In the toolbar, click

In order to visualize the von Mises stress in the deformed workpiece along with undeformed dies, duplicate the dataset, and set the selection to the domains 1 and 3. Set up a new dataset based on .

Results

Study 1/Solution 1 (2) (sol1)

In the window, expand the node.

Right-click and choose .

Selection

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Domains 1 and 3 only.

Revolution 2D 1

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

Stress, 3D (solid)

In the window, expand the node.

Surface 1

The in node set to 2 in order to visualize the compaction.

Deformation

In the window, expand the node, then click .

In the window for , locate the section.

In the text field, type 2.

Stress, 3D (solid)

In order to visualize undeformed dies, set up node by duplicating the node. Select the dataset, and type zero in the expression field. Add a node for the visualization.

Surface 2