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=1385^oC

Transition Temperature=20^oC

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.