UNDERSTANDING THE EFFECTS OF PROCESS VARIABLES ON MACHINING PERFORMANCE
BY
Ali Akber Kapadia
Roll No. 08
Prepared in partial fulfillment of
the course
Industrial Engineering Concepts
AT
NATIONAL
INSTITUTE OF INDUSTRIAL ENGINEERING, MUMBAI
August,
2012
This article aims at replicating the results of
"Finite Element Analysis of Two-dimensional Metal Cutting process"
Publish Year :2008
Authors: Chong Su, Jun-ming Hou, Li-da Zhu, Wan-shan Wang
School of Mechanical Engineering & Automation, Northeastern University Shenyang
NOTE : All the figures here are the screenshots of the simulation done me
INTRODUCTION
Abaqus is a commercial software package for finite
element analysis developed by HKS Inc of Rhode Island, USA and now marketed
under the SIMULIA brand of Dassault Systemes S.A.
I have used the ABAQUS v 6.7 to study and replicate the results of the above mentioned paper.
ORTHOGONAL
METAL CUTTING OPERATION
In this model, a simulation of orthogonal metal
cutting operation is performed in ABAQUS 6.7 Student Edition so as to understand
how the tool chip interfacial friction and other cutting parameters affect the
metal cutting operation. Frictional interaction along the tool- chip interface
is modeled with Johnson-Cook criterion.
The procedure for simulation is described as
follows;
Creating Parts:
1) Go
to the start menu, and click on the Abaqus
6.7 Student Edition > Abaqus CAE. The software window will appear on the
screen. Click on Create Model Database. The
screen will then show a model tree on the left and a blue screen on the right.
2) Expand
the Model option in the model tree by clicking on the + sign on its left. It will then show all the options to be defined
for creating a model.
3) Now
right click on the Parts container
and select the create option. Create Part window will appear. Create a 2D
planar, deformable part named Workpiece.
4) Now
sketch a rectangle with 2540µm length and a height of 889µm.
Create a datum point on the right
edge of the rectangle by the following path:
Tools
> Datum Point > Offset from Point
Then the Abaqus will ask for a
point selection from where you want the offset. Select the rightmost corner of
the workpiece as the offset. Then give the coordinates (0,-1,0) when asked for
the offset coordinates.
Fig1.
Workpiece Geometry
5) Follow
the same steps to create a 2D Planar, Analytical rigid part named Tool with a
base length of 407µm and height of 762µm with a filleted nose.
Tools
>Reference Point >Make the centre of the nose as the reference point.
Fig.2 Tool Geometry
Defining
Materials
6) Now
right click on the Materials
container under the Model tree and select Create option.
Edit
Material dialog box will appear.
Name the material as
WorkPieceMaterial
Define the;
Density as 7850Kg/m3.
Young’s modulus to be temperature
dependent as;
Young’s
Modulus E (GPa)
|
Poisson’s
Ratio
|
Temperature
|
207
|
0.3
|
20
|
200
|
0.3
|
100
|
190
|
0.3
|
150
|
105
|
0.3
|
200
|
70
|
0.3
|
250
|
50
|
0.3
|
300
|
30
|
0.3
|
350
|
Temperature dependent thermal
expansion coefficient as;
Thermal
Expansion coefficient (α) (µm/mK)
|
Temperature (oC)
|
12.3
|
20
|
12.7
|
200
|
13.7
|
400
|
14.5
|
600
|
Thermal Conductivity as 50.8;
Under the Plastic properties select the Johnson-Cook
model and define the following parameters;
A=305000000
B=1161000000
n=0.61
m=0.517
Melting Temperature=1385oC
Transition Temperature=20oC
And make it rate dependent by defining;
C=0.01
and Epsilon dot zero=1
Section Creation and Assignment:
7) Right
click on the Sections container
under the Model Tree. Create Section
dialog box will appear. Create a Solid, Homogenous section with
WorkpieceMaterial as the material and Plane stress/strain thickness as 1. Name
the section as WorkPieceSection.
8) Expand
the Workpiece Container under parts and double click on the Section Assignment option.
9) Select
the whole workpiece when asked for the region to be assigned a section. Edit Section Assignment dialog box
appears. Select the WorkPieceSection from the dropdown list and click OK. The
WorkPieceSection then gets assigned to the workpiece.
Creation
and Translation of Assembly:
10) Expand
the Assembly container in the Model
tree and double click the Instances
option that appears.
11) Create Instance
dialog box appears. Select both Workpiece as well as Tool and check the
Independent (mesh or instance) option and then click Apply.
Both the parts appear on the screen
and the module gets switched to Assembly.
12) Follow
Instance
> Translate
Select the Tool when asked for
instance to be translated.
Translate the tool by taking
Reference point as the start point and Datum Point as the end point. The
assembly will look like;
Fig.3 Assembly
Defining
Sets and Surfaces:
13) Double
click on the Sets option under Model
Tree. Create Set dialog box appears.
Provide the respective name to the set and click Continue. Make the selection
as;
bottom edge: Set name - bottom
left edge: Set name - left
workpiece: Set name - plate
reference point: Set name – tool
14) Create
two surfaces by double clicking the Surfaces option under the Model Tree and
making the following selection;
tool: Surface name – tool
right edge of workpiece: Surface
name – work
Creating
Step-1:
15) Double
click the Steps container under the
Model tree and create a new step after the Initial step with following
specifications;
Name: Step-1
Type: Dynamic,Explicit
Under Basic Tab
Time Period: 10
Under Incrementation Tab
Type: Automatic
Stable increment estimator: Global
Max. time increment: Unlimited
Time scaling factor: 1
Under Other Tab
Linear bulk viscosity parameter:
0.06
Quadratic bulk viscosity parameter:
1.2
Meshing
the workpiece:
16) Click
the Mesh option located at the top
of the window and select the Element
Type option.
17) Select
the Workpiece when asked for the regions for which the element type is to be
assigned. Element Type dialog box
appears.
18) Define
the element to be CPE4R.
19) Then,
create instance by Mesh>Instance.
Again select the whole Workpiece and seed the part. The meshed part will look
like;
Fig.4 Meshed part
Applying Boundary Conditions:
20) Double
click the BCs option under Model
Tree. Create Boundary Condition
dialog box appears. Apply the following boundary condition to the Set-bottom;
Name: BC1
Type: Displacement/Rotation
Step: Step-1 (Dynamic Explicit)
Region: bottom
Distribution : uniform
U1= 0
U2= 0
UR3= 0
Click OK
21) Apply
the same boundary conditions to the Set-left.
Name: BC2
Type: Displacement/Rotation
Step: Step-1 (Dynamic Explicit)
Region: left
Distribution : uniform
U1= 0
U2= 0
UR3= 0
Click OK
22) Repeat
the step (15) to apply the following boundary condition to the Set-tool
Name: BC3
Type: Velocity/Angular Velocity
Step: Step-1 (Dynamic Explicit)
Region: tool
CSYS: (Global)
V1= -1
V2= 0
VR3= 0
Click OK
Fig.5 Boundary Conditions
Defining Interaction properties:
23) Double
Click the Interaction Properties
option under the Model Tree. Create
Interaction Property dialog box appears.
24) Name
the property as IntProp-1 and define the following;
Contact Property Options:
Tangential Behavior
Friction formulation: Penalty
Under Friction tab
Directionality: Isotropic
Number of field variables = 0
Friction coefficient = 0.4
Under Elastic Slip tab
Fraction of characteristic surface
dimension= 0.005
25) Double
Click the Interactions container
under Model tree. Create Interaction
dialog box appears. Define the following;
Name: Int-1
Type: Surface-to-surface contact (Explicit)
Step: Step1 (Dynamic,Explicit)
First Surface: tool
Second surface: work
Mechanical constraint formulation:
Kinematic contact method
Sliding formulation: Finite sliding
Contact Interaction Property:
IntProp-1
Weighting factor: 1
Click OK.
Creating
Job:
26) Right
Click on the Jobs container under
the Model Tree and select the create option.
27) Name
the Job as OrthogonalMetalCutting and click Continue. A job with the specified
name gets created.
28) Right
Click on the created job and select Submit.
Then monitor the submission.
Animating
the Time History:
29) Right Click on the Completed job and select
Results. Then follow Animate>Time
History. Animation will be displayed as;
Fig.6 Animation showing the orthogonal metal cutting operations
CONCLUSION
Successful finite element
simulations of the orthogonal metal cutting process have been carried out using
ABAQUS 6.7 Student Edition. Several conclusions can be drawn from this study.
First, this study demonstrates that it is possible to carry out sophisticated
finite element simulation of metal cutting processes. Second, the finite
element simulations were able to reproduce experimentally observed phenomena in
orthogonal metal cutting. Third, the finite element simulation shows that
friction along the tool-chip interface strongly affects the distribution of
thermodynamic fields. It is believed that the details afforded by FEM
simulations will greatly benefit the engineer in gaining a better understanding
of metal cutting processes and in aiding the design and application of such
processes.
