PDF
Two-Stage Powder Compaction Process
Introduction
Powder compaction is a key process in powder metallurgy that allows the manufacturing of quality products of complex shapes. The density of the powder compact is a fundamental factor that determines the overall quality of sintered products, as regions with lower density can reduce the mechanical strength. Multiple parameters and operating conditions need to be optimized to obtain a uniform density, for example, reducing the friction with the walls and using multistage compaction processes.
This example shows how to setup a two-stage compaction process of metal powder for a simple geometry, and compares the outcome with the results of a single-stage process. The Gurson–Tvergaard–Needleman (GTN) model is used as constitutive model for the porous powder. Friction between the metal powder and the die is taken into account, while perfect bonding between two powder molds is assumed.
Model Definition
The 2D axisymmetric geometry of the workpiece (metal powder) and die are shown in Figure 1. The workpiece geometry is divided into two different domains, for a two-stage compaction process these two domains represent two powder molds at two distinct stages. For the single-stage compaction they represent one powder mold. The punch geometry is not included. Instead, a prescribed displacement at the top boundary is used to compact the powder.
Figure 1: Geometry of the workpiece (metal powder) and die.
Material Properties
The Gurson–Tvergaard–Needleman (GTN) material model is used for the aluminum metal powder, whereas the die is assumed to be rigid. The parameters for the 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
Critical void volume fraction
0.36
Failure void volume fraction
0.4
Boundary Conditions
The applied boundary conditions are:
•
The die is fixed.
•
The axial displacement on the lower face of the metal powder is constrained.
•
For the single-stage compaction process, the axial displacement of the upper face is controlled by a parameter called disp.
•
For the two-stage compaction process, the first compaction stage applies an axial load on the upper boundary of the first powder mold, while in the second stage, the load is applied on the upper boundary of the second powder mold.
Results and Discussion
Figure 2 shows the volumetric plastic strain at the end of the compaction for two-stage and single-stage processes. For the two-stage process there is layer-wise uniformity in the volumetric plastic strain distribution, while for the single-stage compaction there is a large variation in volumetric plastic strain between the upper and lower boundaries.
Figure 2: Volumetric plastic strain at the end of compaction.
The relative density distribution at the end of the two-stage and single-stage processes are shown in Figure 3 and Figure 4, respectively. The layer-wise uniformity is observed in the relative density for the two-stage process, while for the single-stage process there is a clear variation in density from top to bottom. For the two-stage process, the variation in relative density is smaller compared to that after the single-stage process.
Figure 3: Relative density at the end of compaction for the two-stage process.
Figure 4: Relative density at the end of the compaction for the single-stage process.
The variation of the average volumetric elastic strain for the two-stage process is shown in Figure 5. During the first stage of compaction (parameter para between 0 and 1) there is a linear variation of volumetric elastic strain in the first powder mold and no strain in the second one. This is expected as the upper portion of powder is not present in the first stage of compaction. There is elastic recovery in the first powder mold when the parameter para increases from 1 to 1.1 (punch retraction after first stage of compaction). The second stage of compaction starts when the parameter para reaches the value of 1.1, and ends at the value of 2. In this loading step there is a linear variation in the volumetric elastic strain in both powder molds.
Figure 6 shows the punch force versus axial compaction for the two-stage and single-stage processes. The yield point and the end point are almost the same for both cases, but the intermediate states are different. For the two-stage process, there are three stages of punch movement: a first forward movement of the punch on the first powder mold, a retraction of the punch, and finally the forward movement of the punch on the second powder mold. For the single-stage process there is only a forward movement of the punch on the mold.
Figure 5: Variation of average volumetric elastic strain in the two-stage process.
Figure 6: Punch force versus axial compaction.
Notes About the COMSOL Implementation
In the two-stage compaction process analysis, the second powder mold is only present during the second stage of compaction. The activation of this mold is performed using the Activation subnode under Linear Elastic Material. Note that the mold will be activated in a stress-free state. The stresses and strains are not considered when the domain is deactivated.
Application Library path: Nonlinear_Structural_Materials_Module/Porous_Plasticity/two_stage_compaction
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 Select Physics tree, select Structural Mechanics > Solid Mechanics (solid).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies > Stationary.
8
Click  Done.
For convenience, the model parameters are available in a text file.
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
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file two_stage_compaction_parameters.txt.
Punch Force
1
In the Home toolbar, click  Functions and choose Global > Interpolation.
2
In the Settings window for Interpolation, type Punch Force in the Label text field.
3
Locate the Definition section. In the Function name text field, type PunchForce.
4
In the table, enter the following settings:
t
f(t)
0
0
1
300
1.1
0
2
300
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
PunchForce
kN
Geometry 1
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 R0.
4
In the Height text field, type H0.
Rectangle 2 (r2)
1
Right-click Rectangle 1 (r1) and choose Duplicate.
2
In the Settings window for Rectangle, locate the Position section.
3
In the z text field, type H0.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Click in the Graphics window and then press Ctrl+A to select both objects.
3
In the Settings window for Union, click  Build Selected.
Rectangle 3 (r3)
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 R0/4.
4
In the Height text field, type 2.5*H0.
5
Locate the Position section. In the r text field, type R0.
6
In the z text field, type -H0/4.
7
Click  Build All Objects.
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.
Add an Integration operator to compute the axial force.
Definitions
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundary 5 only.
5
Locate the Advanced section. From the Method list, choose Summation over nodes.
Add another Integration operator to compute the axial compaction.
Integration 2 (intop2)
1
Right-click Integration 1 (intop1) and choose Duplicate.
2
In the Settings window for Integration, locate the Source Selection section.
3
Click  Clear Selection.
4
Select Boundaries 6 and 7 only.
5
Locate the Advanced section. From the Method list, choose Integration.
6
Clear the Compute integral in revolved geometry checkbox.
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
Force1
PunchForce(para)
N
Punch force, two-stage compaction
Force2
intop1(-solid2.RFz)
N
Punch force, single-stage compaction
delta
1-intop2(1)/(2*H0)
 
Axial compaction
Set up the physics interfaces for two-stage and single-stage compaction.
Solid Mechanics (solid)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) click Linear Elastic Material 1.
Porous Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Porous Plasticity.
2
In the Settings window for Porous Plasticity, locate the Porous Plasticity Model section.
3
From the Material model list, choose Gurson–Tvergaard–Needleman.
Linear Elastic Material 1
In the Model Builder window, click Linear Elastic Material 1.
Activation 1
1
In the Physics toolbar, click  Attributes and choose Activation.
2
In the Settings window for Activation, locate the Domain Selection section.
3
Click  Clear Selection.
4
Select Domain 2 only.
5
Locate the Activation section. In the Activation expression text field, type para>1.
Rigid Material 1
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
Select Domain 3 only.
Fixed Constraint 1
In the Physics toolbar, click  Attributes and choose Fixed Constraint.
Contact 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid) 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 0.05.
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
From the Displacement in z direction list, choose Prescribed.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 4 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
From the Load type list, choose Total force.
5
Specify the Ftot vector as
0
r
-PunchForce(para)*(para<=1)
z
Boundary Load 2
1
Right-click Boundary Load 1 and choose Duplicate.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
Click  Clear Selection.
4
Select Boundary 5 only.
5
Locate the Force section. Specify the Ftot vector as
0
r
-PunchForce(para)*(para>=1.1)
z
Solid Mechanics 2 (solid2)
Linear Elastic Material 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics 2 (solid2) click Linear Elastic Material 1.
Porous Plasticity 1
1
In the Physics toolbar, click  Attributes and choose Porous Plasticity.
2
In the Settings window for Porous Plasticity, locate the Porous Plasticity Model section.
3
From the Material model list, choose Gurson–Tvergaard–Needleman.
Rigid Material 1
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
Select Domain 3 only.
Fixed Constraint 1
In the Physics toolbar, click  Attributes and choose Fixed Constraint.
Contact 1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics 2 (solid2) 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 0.05.
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
From the Displacement in z direction list, choose Prescribed.
Prescribed Displacement 2
1
Right-click Prescribed Displacement 1 and choose Duplicate.
2
Select Boundary 5 only.
3
In the Settings window for Prescribed Displacement, locate the Prescribed Displacement section.
4
In the u 0 z text field, type -disp.
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 > Aluminum.
4
Right-click and choose Add to Component 1 (comp1).
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Aluminum (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
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
Critical void volume fraction
fc
Fc
1
Poroplastic material model
Failure void volume fraction
ff
Ff
1
Poroplastic material model
Mesh 1
Mapped 1
In the Mesh toolbar, click  Mapped.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Boundaries 10 and 11 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 1.
5
Click  Build All.
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
From the Predefined list, choose Finer.
4
Click  Build All.
Study: Two-Stage Compaction
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Study: Two-Stage Compaction in the Label text field.
Step 1: Stationary
1
In the Model Builder window, under Study: Two-Stage Compaction click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Solid Mechanics 2 (solid2), Controls spatial frame.
5
Click  Disable in Model.
6
Click to expand the Study Extensions section. Select the Auxiliary sweep checkbox.
7
Click  Add.
8
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
para (Parameter)
range(0,1e-1,2)
 
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study: Two-Stage Compaction > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Fully Coupled 1.
4
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
5
In the Maximum number of iterations text field, type 50.
6
In the Study toolbar, click  Compute.
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: Two-Stage Compaction/Solution 1 (sol1) > Solid Mechanics > Volumetric Plastic Strain (solid) and Study: Two-Stage Compaction/Solution 1 (sol1) > Solid Mechanics > Current Void Volume Fraction (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.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies > Stationary.
4
Right-click and choose Add Study.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study: Single-Stage Compaction
In the Settings window for Study, type Study: Single-Stage Compaction in the Label text field.
Step 1: Stationary
1
In the Model Builder window, under Study: Single-Stage Compaction click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step checkbox.
4
In the tree, select Component 1 (comp1) > Solid Mechanics (solid), Controls spatial frame.
5
Click  Disable in Model.
6
Locate the Study Extensions section. Select the Auxiliary sweep checkbox.
7
Click  Add.
8
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
disp (Displacement parameter)
range(0,0.1,6.2)
mm
Solution 2 (sol2)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 2 (sol2) node.
3
In the Model Builder window, expand the Study: Single-Stage Compaction > Solver Configurations > Solution 2 (sol2) > Stationary Solver 1 node, then click Fully Coupled 1.
4
In the Settings window for Fully Coupled, locate the Method and Termination section.
5
In the Maximum number of iterations text field, type 50.
6
In the Study toolbar, click  Compute.
Results
Stress (solid2)
First create the revolution datasets needed to create the plots used in the documentation.
Study: Two-Stage Compaction/Solution 1 (3) (sol1)
1
In the Model Builder window, expand the Results > Datasets node.
2
Right-click Results > Datasets > Study: Two-Stage Compaction/Solution 1 (sol1) and choose Duplicate.
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 3 only.
Revolution 2D 1
1
In the Model Builder window, right-click Revolution 2D and choose Duplicate.
2
In the Settings window for Revolution 2D, locate the Data section.
3
From the Dataset list, choose Study: Two-Stage Compaction/Solution 1 (3) (sol1).
Study: Single-Stage Compaction/Solution 2 (4) (sol2)
In the Model Builder window, under Results > Datasets right-click Study: Single-Stage Compaction/Solution 2 (sol2) and choose Duplicate.
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 3 only.
Revolution 2D 2a
1
In the Model Builder window, under Results > Datasets right-click Revolution 2D 1 and choose Duplicate.
2
In the Settings window for Revolution 2D, locate the Data section.
3
From the Dataset list, choose Study: Single-Stage Compaction/Solution 2 (4) (sol2).
Revolution 2D 1, Revolution 2D 2a, Study: Single-Stage Compaction/Solution 2 (4) (sol2), Study: Two-Stage Compaction/Solution 1 (3) (sol1)
1
In the Model Builder window, under Results > Datasets, Ctrl-click to select Study: Two-Stage Compaction/Solution 1 (3) (sol1), Revolution 2D 1, Study: Single-Stage Compaction/Solution 2 (4) (sol2), and Revolution 2D 2a.
2
Right-click and choose Group.
Datasets for Die
In the Settings window for Group, type Datasets for Die in the Label text field.
Stress, Two-Stage Compaction
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 2D Plot Group, type Stress, Two-Stage Compaction in the Label text field.
3
In the Model Builder window, expand the Stress, Two-Stage Compaction node.
Selection 1
1
In the Model Builder window, expand the Results > Stress, Two-Stage Compaction > Surface 1 node.
2
Right-click Surface 1 and choose Selection.
3
Select Domains 1 and 2 only.
Surface 2
In the Model Builder window, under Results > Stress, Two-Stage Compaction right-click Surface 1 and choose Duplicate.
Selection 1
1
In the Model Builder window, expand the Surface 2 node.
2
Right-click Selection 1 and choose Delete.
Surface 2
1
In the Model Builder window, under Results > Stress, Two-Stage Compaction click Surface 2.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Two-Stage Compaction/Solution 1 (3) (sol1).
4
Click to expand the Title section. From the Title type list, choose None.
Material Appearance 1
1
Right-click Surface 2 and choose Material Appearance.
2
In the Settings window for Material Appearance, locate the Appearance section.
3
From the Appearance list, choose Custom.
4
From the Material type list, choose Steel.
Stress, Two-Stage Compaction
1
In the Model Builder window, under Results click Stress, Two-Stage Compaction.
2
In the Stress, Two-Stage Compaction toolbar, click  Plot.
Stress, Single-Stage Compaction
1
In the Model Builder window, click Stress (solid2).
2
Drag and drop below Stress, Two-Stage Compaction.
3
In the Settings window for 2D Plot Group, type Stress, Single-Stage Compaction in the Label text field.
4
In the Model Builder window, expand the Stress, Single-Stage Compaction node.
Selection 1
1
In the Model Builder window, expand the Results > Stress, Single-Stage Compaction > Surface 1 node.
2
Right-click Surface 1 and choose Selection.
3
Select Domains 1 and 2 only.
Surface 2
In the Model Builder window, under Results > Stress, Single-Stage Compaction right-click Surface 1 and choose Duplicate.
Selection 1
1
In the Model Builder window, expand the Surface 2 node.
2
Right-click Selection 1 and choose Delete.
Surface 2
1
In the Model Builder window, under Results > Stress, Single-Stage Compaction click Surface 2.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Single-Stage Compaction/Solution 2 (4) (sol2).
4
Locate the Title section. From the Title type list, choose None.
Material Appearance 1
1
Right-click Surface 2 and choose Material Appearance.
2
In the Settings window for Material Appearance, locate the Appearance section.
3
From the Appearance list, choose Custom.
4
From the Material type list, choose Steel.
Stress, Single-Stage Compaction
1
In the Model Builder window, under Results click Stress, Single-Stage Compaction.
2
In the Stress, Single-Stage Compaction toolbar, click  Plot.
Relative Density, Two-Stage Compaction
1
In the Model Builder window, under Results click Stress, 3D (solid).
2
In the Settings window for 3D Plot Group, type Relative Density, Two-Stage Compaction in the Label text field.
Surface 1
1
In the Model Builder window, expand the Relative Density, Two-Stage Compaction node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Porous plasticity > solid.rhorelGp - Current relative density - 1.
Surface 2
1
Right-click Results > Relative Density, Two-Stage Compaction > Surface 1 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Revolution 2D 1.
4
From the Solution parameters list, choose From parent.
5
Locate the Expression section. In the Expression text field, type 1.
6
Click to expand the Title section. From the Title type list, choose None.
7
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
8
From the Color list, choose Gray.
Relative Density, Two-Stage Compaction
1
In the Model Builder window, click Relative Density, Two-Stage Compaction.
2
In the Relative Density, Two-Stage Compaction toolbar, click  Plot.
Relative Density, Single-Stage Compaction
1
In the Model Builder window, click Stress, 3D (solid2).
2
Drag and drop below Relative Density, Two-Stage Compaction.
3
In the Settings window for 3D Plot Group, type Relative Density, Single-Stage Compaction in the Label text field.
Surface 1
1
In the Model Builder window, expand the Relative Density, Single-Stage Compaction node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics 2 > Porous plasticity > solid2.rhorelGp - Current relative density - 1.
Surface 2
1
Right-click Results > Relative Density, Single-Stage Compaction > Surface 1 and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Revolution 2D 2a.
4
From the Solution parameters list, choose From parent.
5
Locate the Expression section. In the Expression text field, type 1.
6
Locate the Title section. From the Title type list, choose None.
7
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
8
From the Color list, choose Gray.
Relative Density, Single-Stage Compaction
1
In the Model Builder window, click Relative Density, Single-Stage Compaction.
2
In the Relative Density, Single-Stage Compaction toolbar, click  Plot.
Volumetric Plastic Strain
1
In the Model Builder window, under Results click Volumetric Plastic Strain (solid).
2
In the Settings window for 2D Plot Group, type Volumetric Plastic Strain in the Label text field.
3
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Surface 2
1
In the Model Builder window, expand the Volumetric Plastic Strain node.
2
Right-click Results > Volumetric Plastic Strain > Surface 1 and choose Duplicate.
Filter 1
1
In the Model Builder window, expand the Surface 2 node.
2
Right-click Filter 1 and choose Delete.
Surface 2
1
In the Settings window for Surface, locate the Data section.
2
From the Dataset list, choose Study: Single-Stage Compaction/Solution 2 (2) (sol2).
3
Locate the Expression section. In the Expression text field, type if(isnan(solid2.epvol),NaN,solid2.epvol).
4
Locate the Title section. From the Title type list, choose None.
5
Click to expand the Inherit Style section. From the Plot list, choose Surface 1.
Transformation 1
1
Right-click Surface 2 and choose Transformation.
2
In the Settings window for Transformation, locate the Transformation section.
3
In the Z text field, type 50[mm].
Volumetric Plastic Strain
In the Model Builder window, under Results click Volumetric Plastic Strain.
Table Annotation 1
1
In the Volumetric Plastic Strain toolbar, click  More Plots and choose Table Annotation.
2
In the Settings window for Table Annotation, locate the Data section.
3
From the Source list, choose Local table.
4
In the table, enter the following settings:
x-coordinate
y-coordinate
Annotation
0.025
0.02
Two-stage compaction
0.025
0.07
Single-stage compaction
5
Locate the Coloring and Style section. Clear the Show point checkbox.
6
In the Volumetric Plastic Strain toolbar, click  Plot.
Void Volume Fraction
1
In the Model Builder window, under Results click Current Void Volume Fraction (solid).
2
In the Settings window for 2D Plot Group, type Void Volume Fraction in the Label text field.
3
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Surface 2
1
In the Model Builder window, expand the Void Volume Fraction node.
2
Right-click Results > Void Volume Fraction > Surface 1 and choose Duplicate.
Deformation
1
In the Model Builder window, expand the Results > Void Volume Fraction > Surface 1 node.
2
Right-click Deformation and choose Delete.
Surface 2
In the Model Builder window, expand the Surface 2 node.
Deformation, Filter 1
1
In the Model Builder window, under Results > Void Volume Fraction > Surface 2, Ctrl-click to select Filter 1 and Deformation.
2
Right-click and choose Delete.
Surface 2
1
In the Settings window for Surface, locate the Data section.
2
From the Dataset list, choose Study: Single-Stage Compaction/Solution 2 (2) (sol2).
3
Locate the Expression section. In the Expression text field, type if(isnan(solid2.fcv),NaN,solid2.fcv).
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Inherit Style section. From the Plot list, choose Surface 1.
Transformation 1
1
Right-click Surface 2 and choose Transformation.
2
In the Settings window for Transformation, locate the Transformation section.
3
In the Z text field, type 50[mm].
Void Volume Fraction
In the Model Builder window, under Results click Void Volume Fraction.
Table Annotation 1
1
In the Void Volume Fraction toolbar, click  More Plots and choose Table Annotation.
2
In the Settings window for Table Annotation, locate the Data section.
3
From the Source list, choose Local table.
4
In the table, enter the following settings:
x-coordinate
y-coordinate
Annotation
0.025
0.02
Two-stage compaction
0.025
0.07
Single-stage compaction
5
Locate the Coloring and Style section. Clear the Show point checkbox.
6
In the Void Volume Fraction toolbar, click  Plot.
Create a 1D plot of the average elastic volumetric strain in the workpiece to show the elastic recovery during the two-stage compaction.
Average Elastic Volumetric Strain, Two-Stage Compaction
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Average Elastic Volumetric Strain, Two-Stage Compaction in the Label text field.
Surface Average 1
1
Right-click Average Elastic Volumetric Strain, Two-Stage Compaction and choose Average > Surface Average.
2
Select Domain 1 only.
3
In the Settings window for Surface Average, locate the Expressions section.
4
In the table, enter the following settings:
Expression
Unit
Description
para
1
Parameter
solid.eelvol*solid.isactive
1
Elastic volumetric strain
Surface Average 2
1
In the Model Builder window, right-click Average Elastic Volumetric Strain, Two-Stage Compaction and choose Average > Surface Average.
2
Select Domain 2 only.
3
In the Settings window for Surface Average, locate the Expressions section.
4
In the table, enter the following settings:
Expression
Unit
Description
solid.eelvol*solid.isactive
1
Elastic volumetric strain
Average Elastic Volumetric Strain, Two-Stage Compaction
1
In the Model Builder window, click Average Elastic Volumetric Strain, Two-Stage Compaction.
2
In the Settings window for Evaluation Group, click to expand the Format section.
3
From the Include parameters list, choose Off.
4
In the Average Elastic Volumetric Strain, Two-Stage Compaction toolbar, click  Evaluate.
Average Elastic Volumetric Strain, Two-Stage Compaction
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Average Elastic Volumetric Strain, Two-Stage Compaction in the Label text field.
3
Locate the Plot Settings section.
4
Select the y-axis label checkbox. In the associated text field, type Average elastic volumetric strain (1).
5
Drag and drop below Void Volume Fraction.
Table Graph 1
1
Right-click Average Elastic Volumetric Strain, Two-Stage Compaction and choose Table Graph.
2
In the Settings window for Table Graph, locate the Data section.
3
From the Source list, choose Evaluation group.
4
From the x-axis data list, choose Parameter (1).
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
First powder mold
Second powder mold
Annotation 1
1
In the Model Builder window, right-click Average Elastic Volumetric Strain, Two-Stage Compaction and choose Annotation.
2
In the Settings window for Annotation, locate the Annotation section.
3
In the Text text field, type Elastic recovery.
4
Locate the Position section. In the R text field, type 1.05.
5
In the Z text field, type -0.0015.
6
Locate the Coloring and Style section. Clear the Show point checkbox.
7
Select the Show frame checkbox.
8
In the Average Elastic Volumetric Strain, Two-Stage Compaction toolbar, click  Plot.
Create a 1D plot of the punch forces for both processes.
Punch Force vs. Axial Compaction
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Punch Force vs. Axial Compaction in the Label text field.
3
Locate the Plot Settings section. Select the x-axis label checkbox.
4
Select the y-axis label checkbox. In the associated text field, type Punch force (kN).
5
In the x-axis label text field, type Axial compaction (1).
6
Locate the Axis section. Select the Manual axis limits checkbox.
7
In the x minimum text field, type -0.003.
8
In the x maximum text field, type 0.16.
9
In the y minimum text field, type -10.
10
In the y maximum text field, type 320.
11
Locate the Legend section. From the Position list, choose Lower right.
Global 1
1
Right-click Punch Force vs. Axial Compaction 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
Force1
kN
Punch force, two-stage compaction
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type delta.
6
Click to expand the Legends section. From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Two-stage compaction
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study: Single-Stage Compaction/Solution 2 (2) (sol2).
4
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
Force2
kN
Punch force, single-stage compaction
5
Locate the Legends section. In the table, enter the following settings:
Legends
Single-stage compaction
6
In the Punch Force vs. Axial Compaction toolbar, click  Plot.