COMSOL 6.4 - Powder Compaction of a Rotational Flanged Component

Powder Compaction of a Rotational Flanged Component

The powder compaction process is common in the manufacturing industry, thanks to its potential to produce components of complex shape and high strength. Because the mechanical properties of the produced component depend on the final density, uniform densification is important. Large variations in density can make a part weak, which affects the overall quality of the component. Finite element analysis with a properly chosen constitutive material model is a handy tool that can provide detailed information about densification, punch forces, friction phenomena, plastic deformation, and internal stresses, in order to better understand the process and to improve the quality of the manufacturing process.

The constitutive material models that are relevant for this type of simulations can broadly be classified in two types:

Porous material models — These can be used for the compaction of medium to low porosity powder. Two examples are the Shima–Oyane and Gurson material models.

Granular material models — These can be used for the compaction of high porosity powder. Examples of this class of material models include the Capped Drucker–Prager and Capped Mohr–Coulomb models.

This example studies the compaction of a rotational flanged component made of iron powder. As the porosity of the powder is large before compaction, a granular material model like the Capped Drucker–Prager (DPC) model is best suited as argued in Ref. 1 and Ref. 2. The elastic regime is represented by a linear elastic material, while a multiplicative plastic strain formulation together with a DPC yield function is used for the plastic regime. Additionally, friction between the powder and the die is taken into account. Simultaneous movement of the top and bottom punches is applied to avoid mesh distortion and other numerical problems. The simulation is performed using a 2D structured mesh with a linear displacement field as reported in Ref. 2.

Model Definition

The geometry of the workpiece (metal powder) and the die is shown in Figure 1. The punch that compacts 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 the die.

Material Properties

For the iron metal powder, an elastoplastic material model with a constitutive relation given by a combination of the linear elastic material model and the Capped Drucker–Prager (DPC) model is used. The material parameters are listed below.


Material parameter	Value
Young’s modulus	2000 MPa
Poisson’s ratio	0.37
Yield function parameter a1	1.3
Initial yield stress σys0	43.5 MPa
Initial void volume fraction	0.4
Hardening modulus	100 MPa
Maximum plastic volumetric strain	0.65
Initial ellipse centroid	1.25 MPa]
Initial pressure limit	10 MPa

The material of the die is assumed to be rigid. Therefore, it does no require any physics nor material properties.

Boundary Conditions

A prescribed displacement boundary condition is used for the upper and lower faces of the metal powder. The displacement in the z direction is controlled by an interpolation function.

Contact

•

Contact pairs are defined with boundaries on the die selected as source, and boundaries on the workpiece selected as destination.

•

Contact with Coulomb friction is considered using the Augmented Lagrangian method. The coefficient of friction is chosen as 0.08.

The mesh on the source only needs to resolve the geometry of the contact surface. Hence no mesh is needed for the domain, but in order to show the die domains in the postprocessing plots the die domains are coarsely meshed.

Results and Discussion

Figure 2 shows the volumetric plastic strain at the end of the compaction process. At the middle corner, the compressive volumetric plastic strain is at its minimum, while it at the top corner is at its maximum.

The compaction process reduces the porosity of the iron 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, nonuniform changes in porosity are expected. Contours of the current relative density at the middle and at the end of the compaction are shown in Figure 3 and Figure 4, respectively. 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 corners, the metal powder is less compacted due to the friction effects

Lastly, the von Mises stress along in the workpiece at the end of compaction is shown in Figure 5 in a 3D representation of the model.

Figure 2: Volumetric plastic strain at the end of compaction.

Figure 3: Current relative density in the middle of compaction.

Figure 4: Current relative density at the end of compaction.

Figure 5: Distribution of the von Mises stress in the workpiece at the end of the compaction process.

Notes About the COMSOL Implementation

The density distribution in the compaction process is affected by the contact pressure and the friction forces, so the accuracy of the contact algorithm is important in the powder compaction process. In this example, the method with a solver is used.

References

1. A. Perez-Foguet, A. Rodriguez-Ferran, and A. Huerta, “Consistent tangent matrices for density-dependent finite plasticity models,” Int. J. Numer. Anal. Meth. Geomech., vol. 25, pp. 1045–1075, 2001.

2. A.R. Khoei, A. Shamloo, and A.R. Azami, “Extended finite element method in plasticity forming of powder compaction with contact friction,” Int.J. Solids Struct., vol. 43, pp. 5421–5448, 2006..

Nonlinear_Structural_Materials_Module/Porous_Plasticity/compaction_of_a_rotational_flange

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
t	0[s]	0 s	Time parameter

Definitions

Top Punch Displacement

In the toolbar, click

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

Locate the section. In the text field, type disp1.

In the table, enter the following settings:


t	f(t)
0	0
10	-6.06

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


Argument	Unit
t	s

In the table, enter the following settings:


Function	Unit
disp1	mm

Bottom Punch Displacement

Right-click and choose .

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

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


t	f(t)
10	7.7

Geometry 1

Rectangle 1 (r1)

In the toolbar, click

In the window, click .

In the window for , locate the section.

From the list, choose .

In the window, click .

In the window for , locate the section.

In the text field, type 6.3.

In the text field, type 25.4.

Click

Rectangle 2 (r2)

Right-click and choose .

In the window for , locate the section.

In the text field, type 4.6.

In the text field, type 13.7.

Locate the section. In the text field, type 6.3.

Click

Rectangle 3 (r3)

Right-click and choose .

In the window for , locate the section.

In the text field, type 20.2.

In the text field, type 11.7.

Locate the section. In the text field, type 13.7.

Click

Union 1 (uni1)

In the toolbar, click

and choose .

Select the objects and only.

In the window for , click

Rectangle 4 (r4)

In the window, under > right-click and choose .

In the window for , locate the section.

In the text field, type 15.6.

In the text field, type 13.7.

Locate the section. In the text field, type 10.9.

In the text field, type 0.

Click

Click the

button in the toolbar.

Rectangle 5 (r5)

Right-click and choose .

In the window for , locate the section.

In the text field, type 6.3.

In the text field, type 25.4.

Locate the section. In the text field, type 26.5.

Click

Union 2 (uni2)

In the toolbar, click

and choose .

Click the

button in the toolbar.

Select the objects and only.

In the window for , locate the section.

Clear the checkbox.

Click

Rectangle 1 (r1)

In the window, under > right-click and choose .

Internal Die

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

Rectangle 2 (r2), Rectangle 3 (r3), Union 1 (uni1)

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

Right-click and choose .

Compact

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

Rectangle 4 (r4), Rectangle 5 (r5), Union 2 (uni2)

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

Right-click and choose .

External Die

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

Form Union (fin)

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Click

Add the interior edge in the workpiece geometry to in order to generate a structured mesh.

Mesh Control Edges 1 (mce1)

In the toolbar, click

and choose .

On the object , select Boundary 8 only.

In the window for , click

In subsequent steps, the side domain will be not be part of the physics. Hence use the toggle button in to switch the boundaries, so that the workpiece boundaries are chosen as destination boundaries.

Definitions

Contact Pair 2 (ap2)

In the window, under > click .

In the window for , click the

button.

Locate the section. Click to select the

toggle button.

Locate the section. Click to select the

toggle button.

Domains 1 and 3 (die) are considered as rigid and fixed, hence there is no need to consider them in physics, only a mesh is required.

Change the discretization to .

Solid Mechanics (solid)

In the window, under click .

In the window for , locate the section.

Click

Select Domain 2 only.

Click to expand the section. From the list, choose .

For the elastoplastic analysis of the workpiece, choose a – model by adding a subnode to the . Set the formulation to to force large strains to be used.

Linear Elastic Material 1

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Porous 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 .

For better accuracy, select the with a solution method.

Contact 1

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Friction 1

In the toolbar, click

and choose .

In the window for , locate the section.

In the μ text field, type 0.08.

Prescribed Displacement 1

In the toolbar, click

and choose .

Select Boundary 7 only.

In the window for , locate the section.

From the list, choose .

In the u 0 z text field, type disp1(t).

Prescribed Displacement 2

In the toolbar, click

and choose .

Select Boundary 6 only.

In the window for , locate the section.

From the list, choose .

In the u 0 z text field, type disp2(t).

Materials

Iron Powder

In the window, under right-click and choose .

In the window for , type Iron Powder 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	2[GPa]	Pa	Young’s modulus and Poisson’s ratio
Poisson’s ratio	nu	0.37	1	Young’s modulus and Poisson’s ratio
Density	rho	7540	kg/m³	Basic
Initial yield stress	sigmags	43.5[MPa]	Pa	Poroplastic material model
Initial void volume fraction	f0	0.6	1	Poroplastic material model
Yield function parameter	a1yield	1.3	1	Pressure-dependent plasticity
Initial pressure limit	pc0	10[MPa]	Pa	Cap and cutoff
Initial ellipse centroid	pcc0	1.25[MPa]	Pa	Cap and cutoff
Hardening modulus	Kc	100[MPa]	Pa	Cap and cutoff
Maximum volumetric plastic strain	epvolmax	0.65	1	Cap and cutoff

Mesh 1

Mapped 1

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Domain 2 only.

Click to expand the section. From the list, choose .

Click to expand the section. Select the checkbox.

Distribution 1

Right-click and choose .

Select Boundaries 6 and 19 only.

In the window for , locate the section.

In the text field, type 4.

Distribution 2

In the window, right-click and choose .

Select Boundary 5 only.

In the window for , locate the section.

In the text field, type 20.

Mapped 2

In the toolbar, click

In the window for , locate the section.

From the list, choose .

Select Domain 4 only.

Locate the section. From the list, choose .

Locate the section. Select the checkbox.

Distribution 1

Right-click and choose .

Select Boundaries 7 and 18 only.

In the window for , locate the section.

In the text field, type 20.

Distribution 2

In the window, right-click and choose .

Select Boundary 13 only.

In the window for , locate the section.

In the text field, type 16.

Size

In the window, under > click .

In the window for , locate the section.

From the list, choose .

Free Quad 1

In the toolbar, click

In the window for , click

contact in addition to the material and geometric nonlinearity in the model demands special solver settings to achieve smooth convergence.

Study 1

Step 1: Stationary

Set up an auxiliary continuation sweep for the t parameter.

In the window, under click .

In the window for , click to expand the section.

Select the checkbox.

Click

In the table, enter the following settings:


Parameter name	Parameter value list	Parameter unit
t (Time parameter)	range(0,0.2,10)	s

Solution 1 (sol1)

In the toolbar, click

In the window, expand the node.

Set up the solver 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 checkbox.

In the text field, type 0.0005.

In the text field, type 0.2.

From the list, choose .

In the window, under > > > click .

In the window for , click to expand the section.

From the list, choose .

In the toolbar, click

Result Templates

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > > and > > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Results

Study 1/Solution 1 (sol1)

In the window, expand the > node, then click .

Selection

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Select Domain 2 only.

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

Study 1/Solution 1 (2) (sol1)

Right-click and choose .

Selection

In the window, expand the node, then click .

In the window for , locate the section.

Click

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 .

In order to visualize the undeformed dies, set up node in the next 3D plot with a zero expression. Select the dataset, and add a node for the visualization.

Stress, 3D (solid)

In the window, expand the > node, then click .

In the window for , locate the section.

Clear the checkbox.

Surface 2

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. In the text field, type 0.

Click to expand the section. From the list, choose .

Material Appearance 1

Right-click and choose .