Placement 2025 Scholarship: Your Future Starts Here | 6 Guaranteed Job Interviews | 1̶0̶0̶ 29 seats only. Apply Now

00D 00H 00M 00S

Menu

Executive Programs

Workshops

Projects

Blogs

Careers

Placements

Student Reviews


For Business


More

Academic Training

Informative Articles

Find Jobs

We are Hiring!


All Courses

Choose a category

Mechanical

Electrical

Civil

Computer Science

Electronics

Offline Program

All Courses

All Courses

logo

CHOOSE A CATEGORY

Mechanical

Electrical

Civil

Computer Science

Electronics

Offline Program

Top Job Leading Courses

Automotive

CFD

FEA

Design

MBD

Med Tech

Courses by Software

Design

Solver

Automation

Vehicle Dynamics

CFD Solver

Preprocessor

Courses by Semester

First Year

Second Year

Third Year

Fourth Year

Courses by Domain

Automotive

CFD

Design

FEA

Tool-focused Courses

Design

Solver

Automation

Preprocessor

CFD Solver

Vehicle Dynamics

Machine learning

Machine Learning and AI

POPULAR COURSES

coursePost Graduate Program in Hybrid Electric Vehicle Design and Analysis
coursePost Graduate Program in Computational Fluid Dynamics
coursePost Graduate Program in CAD
coursePost Graduate Program in CAE
coursePost Graduate Program in Manufacturing Design
coursePost Graduate Program in Computational Design and Pre-processing
coursePost Graduate Program in Complete Passenger Car Design & Product Development
Executive Programs
Workshops
For Business

Success Stories

Placements

Student Reviews

More

Projects

Blogs

Academic Training

Find Jobs

Informative Articles

We're Hiring!

phone+91 9342691281Log in
  1. Home/
  2. Anish Augustine/
  3. Week 4 -Wire Bending Challenge

Week 4 -Wire Bending Challenge

SIMULATION OF WIRE BENDING USING ANSYS WORKBENCH OBJECTIVE 1. To simulate bending of wire for different cases of wire material, Case-1: Copper Alloy NL Case-2: Aluminium Alloy NL Case-3: Magnesium Alloy NL 2. To find out Equivalent stress and Equivalent strain developed in wire for each case and compare the results. 1.…

    • Anish Augustine

      updated on 27 Mar 2021

    SIMULATION OF WIRE BENDING USING ANSYS WORKBENCH

    OBJECTIVE

    1. To simulate bending of wire for different cases of wire material,

    1. Case-1: Copper Alloy NL
    2. Case-2: Aluminium Alloy NL
    3. Case-3: Magnesium Alloy NL

    2. To find out Equivalent stress and Equivalent strain developed in wire for each case and compare the results.

    1. THEORY

    1.1 Wire Bending:

    The process of wire bending involves using mechanical force to push wire against a die, forcing the wire to conform to the shape of the die. Often, it is held firmly in place while the end is rotated and rolled around the die. Other forms of processing including pushing stock through rollers that bend it into a simple curve.

    Rotary draw bending (RDB) is a precise technology, since it bends using tooling or "die sets" which have a constant centre line radius, alternatively indicated as mean bending radius. Rotary draw benders can be programmable to store multiple bend jobs with varying degrees of bending. The rotary-draw-bending method is a complex physical process with multi-factor interactive effects and is one of the advanced tube or wire forming processes with high efficiency, high forming precision, low consumption and good flexibility for bending angle changes. However, it may cause a wrinkling phenomenon, over thinning and cross-section distortion if the process parameters are inappropriate. Wrinkles propagate, but in some cases, localize in a finite zone and lead to failure.

    Rotary draw benders create aesthetically pleasing bends when the right tooling is matched to the application. CNC rotary draw bending machines can be very complex and use sophisticated tooling to produce severe bends with high quality requirements. Rotary draw benders are the most popular machines for use in bending tube, pipe and wires for applications like: handrails, frames, motor vehicle roll cages, handles, light fittings, hanger hooks, key chains, refrigerator rack, stainless steel fruit baskets, and other metal wire and strip forming and bending.

    2. ANALYSIS SETUP

    2.1 Geometry:

    2.1

    Fig.2.1 3D model of wire bending setup.

    The given 3D model of wire bending setup assembly is imported into SpaceClaim. It consists of a wheel, lever and wire. The wire is held in the slot of the wheel and it is made to bend, forcing the wire to conform to the shape of the wheel using the rotating lever.

    2.2 Material Properties:

    2.2.a

    a. Copper Alloy NL.

    2.2.b

    b. Aluminum Alloy NL.

    2.2.c

    c. Magnesium Alloy NL

    Fig.2.2 Material property details of wire.

    The following materials are assigned for wire for each case,

    1. Case-1: Copper Alloy NL
    2. Case-2: Aluminium Alloy NL
    3. Case-3: Magnesium Alloy NL

    Note: The analysis setup of only case-1 is demonstrated.

    2.3 Connection Details:

    2.3.1 Contact details:

    2.3.1.a

    a. Contact between lever and wire.

    2.3.1.b

    b. Contact between wheel and wire.

    Fig.2.3.1 Contact details of wire bending.

    Contact between, (a) Lever (contact body) and wire (target body), (b) Wheel (contact body) and wire (target body) are assigned as frictional contact with coefficient of friction = 0.2. The formulation type of contact is set as ‘Augmented Lagrange’ and normal stiffness value is inputted as 0.1 factor with update stiffness set to as ‘each iteration’. The interface treatment is set as ‘Add Offset, Ramped Effects’.

    2.3.2 Joint Details:

    2.3.2.a

    Fig.2.3.2 Joint details of wire bending,

    The revolute type of joint is assigned for lever with connection type being body-ground, since only rotation is specified along Z-axis.

    2.4 Meshing:

    2.4.a2.4.b

    a. Patch conforming method (tetrahedron).                                                       b. Face sizing of contact region of lever and whole wire.

    2.4.c2.4.d

    c. Face sizing of contact region of wire and wheel.                                             d. Meshed model.

    Fig.2.4 Meshing details of wire bending.

    The element generated in meshing the model is ensured as tetrahedron elements by using patch conforming method. The mesh size of the contact regions of lever and wire is refined to 2 mm by using face sizing option. The mesh size of the contact region of wire and the curved region of wheel is refined to 0.8 mm using face sizing option with sphere centre being created using user defined coordinate system and sphere of influence radius being 7 mm. The total number of nodes and elements generated are 9067 and 4554 respectively.

    Note: The academic version of software has the problem size limit of 128k nodes or elements.

    2.5 Boundary Conditions:

    2.5.1 Analysis settings:

    2.5.1.12.5.1.2

    a. Analysis setting for step 1.                                        b. Analysis setting for step 2 to step 8.

    Fig.2.5.1 Analysis settings.

    In the analysis settings the number of steps considered is 8 and auto time stepping is set to ‘On’ which is defined by ‘time’. For step 1, the initial, minimum and maximum time step is considered as 0.1s, 1e-2s and 0.2s respectively. For step 2 to step 8, the minimum and maximum time step is 1e-2s and 1s respectively. In the solver controls, solver type is chosen as ‘Direct’ and large deflection is set to ‘On’. Under the output controls, all the results are set to ‘Yes’.

    2.5.2 Boundary condition for wire bending:

    2.5.2.a2.5.2.b

    a. Fixed support.

    2.5.2.b

    b. Joint load applied to lever along Z-axis.

    Fig.2.5.2 Boundary conditions for wire bending.

    Since, the wheel is stationary and to avoid slippage of wire while bending, fixed support is assigned to the surface of the wheel and wire as shown in fig. 2.5.2 a. In order to bend wire, the lever is made to rotate in clockwise direction from 00 to 1400, with an increment of 200 in each step.

    3. RESULTS AND DISCUSSIONS

    3.1 Case-1: Wire material; Copper Alloy NL.

    3.1.a3.1.b

    a. Equivalent (v-m) Stress.                                                                                      b. Equivalent Elastic Strain

    3.2 Case-2: Wire material; Aluminum Alloy NL.

    3.2.a3.2.b

    a. Equivalent (v-m) Stress.                                                                                       b. Equivalent Elastic Strain.

    3.3 Case-3: Wire material; Magnesium Alloy NL.

    3.3.a3.3.b

    a. Equivalent (v-m) Stress.                                                                                       b. Equivalent Elastic Strain.

    3.4 Comparison of Results:

    3.4

    During the initial process of bending, the sharp bend of wire is experiencing maximum stress and strain. The results tabulated are pertaining to the step 8 (after bending).

    From table, it is observed that the maximum v-m stress developed in wire material of magnesium alloy NL is least compared to other wire materials. For all the three cases of wire material the maximum v-m stress developed is more than its yield strength value, hence it undergoes plastic deformation and conforms to the shape of the wheel while bending. The maximum equivalent elastic strain developed in wire material of copper alloy NL is least compared to other wire materials which indicates that it is least deformed, hence it is preferred wire material among the given wire materials.  

    4. ANIMATION OF RESULTS:

    4.1 Case-1: Wire material; Copper Alloy NL.

    4.1.a

    a. Total Deformation.

    4.1.b

    b. Equivalent (v-m) Stress.

    4.1.c

    c. Equivalent Elastic Strain

    4.2 Case-2: Wire material; Aluminum Alloy NL.

    4.2.a

    a. Total Deformation.

    4.2.b

    b. Equivalent (v-m) Stress.

    4.2.c

    c. Equivalent Elastic Strain

    4.3 Case-3: Wire material; Magnesium Alloy NL.

    4.3.a

    a. Total Deformation.

    4.3.b

    b. Equivalent (v-m) Stress.

    4.3.c

    c. Equivalent Elastic Strain

    CONCLUSION

    1. Simulation of bending of wire was carried out successfully for the following cases of wire material,

    1. Case-1: Copper Alloy NL
    2. Case-2: Aluminium Alloy NL
    3. Case-3: Magnesium Alloy NL

    2. The maximum Equivalent (v-m) stress developed in Magnesium Alloy NL wire material is least compared to other wire materials.

    3. For all the three cases of wire material the maximum v-m stress developed is more than its yield strength value, hence it undergoes plastic deformation and conforms to the shape of the wheel while bending.

    4. The maximum Equivalent strain developed in Copper Alloy NL wire material is least compared to other wire materials. Hence, it is least deformed and preferred choice of material among the given wire materials.  

    Leave a comment

    Thanks for choosing to leave a comment. Please keep in mind that all the comments are moderated as per our comment policy, and your email will not be published for privacy reasons. Please leave a personal & meaningful conversation.

    Please  login to add a comment

    Other comments...

    No comments yet!
    Be the first to add a comment

    Read more Projects by Anish Augustine (38)

    Week 11 Car Crash simulation

    Objective:

    CAR CRASH SIMULATION USING ANSYS WORKBENCH OBJECTIVE 1. To simulate car crash for different thickness of car body, Case-1: Thickness=0.3 mm. Case-2: Thickness=0.7 mm. Case-3: Thickness=1.5 mm. 2. To find out Total deformation and Equivalent stress developed in car body for each case and compare the results. 1. THEORY 1.1…

    calendar

    14 Jul 2021 09:52 AM IST

    • CAE
    Read more

    Week 10 Bullet penetrating a Bucket Challenge

    Objective:

    SIMULATION OF BULLET PENETRATING INTO A BUCKET USING ANSYS WORKBENCH OBJECTIVE To simulate bullet penetrating into a bucket for different cases of bucket material, Case-1: Aluminium Alloy NL Case-2: Copper Alloy NL Case-3: Stainless Steel NL To find out Total deformation and Equivalent stress developed in bucket for…

    calendar

    19 Jun 2021 08:51 AM IST

      Read more

      Week 9 Tension and Torsion test challenge

      Objective:

      SIMULATION OF TENSION AND TORSION TEST ON A SPECIMEN USING ANSYS WORKBENCH OBJECTIVE To perform the tension and torsion test simulation on the specimen by following the necessary boundary conditions, For the tension test, one end of the specimen has to be displaced to 18mm while keeping the other end fixed. For the torsion…

      calendar

      11 Jun 2021 11:10 AM IST

        Read more

        Week 9 Machining with Planer Challenge

        Objective:

        EXPLICIT DYNAMIC ANALYSIS OF MACHINING WITH PLANER USING ANSYS WORKBENCH OBJECTIVE To perform explicit dynamic analysis of machining with planer for the following two different cases of cutting velocity, Case-1: Cutting velocity=20000 mm/s Case-2: Cutting velocity=15000 mm/s To find out Directional Deformation, Equivalent…

        calendar

        06 Jun 2021 03:39 AM IST

          Read more

          Schedule a counselling session

          Please enter your name
          Please enter a valid email
          Please enter a valid number

          Related Courses

          coursecard

          Design loads considered on bridges

          Recently launched

          10 Hours of Content

          coursecard

          Design of Steel Superstructure in Bridges

          Recently launched

          16 Hours of Content

          coursecard

          Design for Manufacturability (DFM)

          Recently launched

          11 Hours of Content

          coursecard

          CATIA for Medical Product Design

          Recently launched

          5 Hours of Content

          coursecardcoursetype

          Accelerated Career Program in Embedded Systems (On-Campus) Courseware Partner: IT-ITes SSC nasscom

          Recently launched

          0 Hours of Content

          Schedule a counselling session

          Please enter your name
          Please enter a valid email
          Please enter a valid number

          logo

          Skill-Lync offers industry relevant advanced engineering courses for engineering students by partnering with industry experts.

          https://d27yxarlh48w6q.cloudfront.net/web/v1/images/facebook.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/insta.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/twitter.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/youtube.svghttps://d27yxarlh48w6q.cloudfront.net/web/v1/images/linkedin.svg

          Our Company

          News & EventsBlogCareersGrievance RedressalSkill-Lync ReviewsTermsPrivacy PolicyBecome an Affiliate
          map
          EpowerX Learning Technologies Pvt Ltd.
          4th Floor, BLOCK-B, Velachery - Tambaram Main Rd, Ram Nagar South, Madipakkam, Chennai, Tamil Nadu 600042.
          mail
          info@skill-lync.com
          mail
          ITgrievance@skill-lync.com

          Top Individual Courses

          Computational Combustion Using Python and CanteraIntroduction to Physical Modeling using SimscapeIntroduction to Structural Analysis using ANSYS WorkbenchIntroduction to Structural Analysis using ANSYS Workbench

          Top PG Programs

          Post Graduate Program in Hybrid Electric Vehicle Design and AnalysisPost Graduate Program in Computational Fluid DynamicsPost Graduate Program in CADPost Graduate Program in Electric Vehicle Design & Development

          Skill-Lync Plus

          Executive Program in Electric Vehicle Embedded SoftwareExecutive Program in Electric Vehicle DesignExecutive Program in Cybersecurity

          Trending Blogs

          Heat Transfer Principles in Energy-Efficient Refrigerators and Air Conditioners Advanced Modeling and Result Visualization in Simscape Exploring Simulink and Library Browser in Simscape Advanced Simulink Tools and Libraries in SimscapeExploring Simulink Basics in Simscape

          © 2025 Skill-Lync Inc. All Rights Reserved.

                      Do You Want To Showcase Your Technical Skills?
                      Sign-Up for our projects.