Static Structural Analysis on the Wire Bending Model

Static Structural Analysis on the Wire Bending Model.

Aim :

• To perform Static Structural Analysis on the Wire Bending Model with three different materials.

Objective :

• To define appropriate materials to the Wire Bending Model.
• To define connections between them.
• To perform mesh on the Wire Bending Model.
• To define appropriate Boundary Conditions to the Model.
• To solve and compare the results of the three cases for Total Deformation, Von-Mises Stress, and Equivalent Elastic Strain.

Figure 1-Wire Bending.

Figure 2-Wire Bending Animation.

Procedure :

Phase 1- Material Set-Up :

• To set up the material for the Rolling Operation Model. First, drag and drop the static structural analysis workspace into the project schematic from the analysis system. This is shown in below Figure 3.

Figure 3-Ansys Workbench Workspace.

• After deploying the static structural analysis system in the project schematic workspace.
• Define the Engineering Data and geometry, To define the Geometry and Engineering Data, Right Click on the Engineering Data and click to edit, it will take to the Engineering Tab.
• There Right Click on the Material Tab, A window will Pop-Up stating Engineering data sources.
• Click on the Engineering Data Sources, There go and select the material to define the engineering data. This is shown in below Figures 4,5,6.

Figure 4-Right Click on the Engineering Data.

Figure 5-Right Click on the Material Tab.

Figure 6-Select these Materials to define the Model.

Phase 2-Geometry Set Up :

• Next set up the geometry. To set up the geometry, Right-Click on the Geometry option >> Import Geometry. This is shown in below Figure 7.

Figure 7-Importing Geometry.

Figure 8-Selecting the Geometry to Import.

• Next double click on the geometry to check, Whether the model imported, is Wire Bending Model or not. Space Claim Workspace will open. The model will be imported in the space claim, Which is shown in below Figure 9.

Figure 9-Wire Bending Model in the Space Claim.

Phase 3-Model Set-Up :

• Next, define the model, Double click on the model, The Mechanical Workspace will open, There go and define the material, set up the load case for the model.
• The Model loaded in the mechanical workspace is shown in below Figure 10.

Figure 10-Model Loaded in Mechanical Workspace.

3:1 Assign Material :

• Next, define the material as Copper Alloy for the Wire alone which is shown in below Figure 14.
• Similarly, define the Structural Steel as material for the Wheel and Lever. The material properties are shown in below Figures 12 and 13.
• To assign a material,Click on the Geometry >> Select the Wire Geometry >> Parameter Window >> Assignment >>Copper Alloy.
• Similarly, assign for the Wheel and Lever also.

Figure 11-Assign Material to the Wire.

Figure 12-Mechanical Properties of Structural Steel.

Figure 13-Mechanical Properties of Copper Alloy.

3:2 Define Connections :

• For this Rolling Operation Model, We have to Create two contacts, One is between Wire and Lever and the other one is between Wheel and Wire.

1) Contact Between Wire and Lever :

• In this contact, Select the wire outer face for the contact and select the lever outer face for the target. This is shown in below Figure 14.
• Contact Type-Frictional.
• Frictional Coefficient -0.2.
• Formulation Type-Augmented Lagrange.
• Enable Normal Stiffness-Factor.
• Normal Stiffness-Factor-0.1.
• Update Stiffness-Each Iteration.
• Interface Treatment-Add Offset, Ramped Effects.

Figure 14-Contact Between Wire and Lever.

2) Contact Between Wheel and Wire :

• In this contact, Select the wheel outer face for the contact and select the wire outer face for the target. This is shown in below Figure 15.
• Contact Type-Frictional.
• Frictional Coefficient -0.2.
• Formulation Type-Augmented Lagrange.
• Enable Normal Stiffness-Factor.
• Normal Stiffness-Factor-0.1.
• Update Stiffness-Each Iteration.
• Interface Treatment-Add Offset, Ramped Effects.

Figure 15-Contact Between Wheel and Wire.

Figure 16-Connections Defined.

3:3 Define Joints :

1) Revolute Joint :

• After creating the connections, Go and create a Revolute Joint.
• Select the inner face of the Lever and keep the Type as Body to Ground.
• Type of Joint-Revolute.
• Connection Type-Body to Ground.

Figure 17-Revolute Joint Defined.

3:4 Meshing :

• After defining the connections, We have to define mesh for the Rolling Operation Model.
• There will be a default mesh created for the Rolling Operation model.
• But we have to insert body sizing and face sizing to refine the mesh of WorkPiece.
• To Insert Body Sizing >> Right Click on Mesh >> Insert >> Sizing >> Select Wire and Lever Faces.Which is shown in below Figure 18.

Figure 18-Insert Face Sizing to Refine the Mesh of Wire and Lever.

1) Patch Conforming Method :

• Here for this wire bending model, We are meshing the components with tetrahedral elements.
• To mesh the component with tetrahedral elements, We have to insert the patch conforming method.
• To do Right Click on Mesh >> Insert >> Patch Conforming Method >> Select the Geometry >> Type-Tetrahedrons,Which is shown in below Figure 19.

Figure 19-Insert Patch Conforming Method.

Figure 20-Selected the Geometry to Mesh with Tetrahedral Elements.

2) Face Sizing between Wire and Lever :

• Select the faces of the lever and wire to refine the mesh with a 2.2 mm element size which is shown in below Figure 21.

Figure 21-Face Sizing between Wire and Lever.

3) Mesh by using Sphere of Influence :

• Here, Create a new coordinate system between the wire and fillet region. This is shown in below Figure
• To create Coordinate System, Select the Fillet region Face >> Right Click >> Create Coordinate System, Which is shown in below Figure 22.
• Change the Type to Sphere of Influence in Face Sizing2.
• Give the radius of the sphere as 7 mm and the size of the element as 0.8 mm. This is shown in below Figure 25.

Figure 22-Create New Coordinate System.

Figure 23-Select the X and Z Offset to Create New Coordinate System.

Figure 24-Coordinate System Created.

Figure 25-Created the Sphere.

• The Whole Wire Bending Component is Meshed, Which is shown in below Figure 26.
• No of Nodes =8101
• No of Elements =4058
• The whole Model has meshed with Tetrahedral Elements.

Figure 26-Final Meshed Model.

3:5 Analysis Settings :

• Here for this Wire Bending Model, We are giving 8 steps to run the simulation.

Step 1-

• Auto Time Stepping-ON

• Define By-Time

• The initial Time Step is 0.1 sec.

• The minimum Time Step is 0.01 sec.

• The maximum Time Step is 0.2 sec.

• Solver Type-Direct

• Large Deformation-ON

• Output Controls-Change all the parameters to Yes.

Figure 27-Analysis Settings for Step-1.

Step 2-8 :

• Auto Time Stepping-ON.
• Define By-Time.
• Carry Over Time Step-ON.
• The minimum Time Step-0.01.
• Maximum TimeStep-1.
• Solver Type-Direct.
• Large Deformation-ON.

Figure 28-Analysis Settings for Step 2-8.

3:5 Boundary Conditions :

• After giving some parameters in the analysis settings, We have to give boundary conditions.
• Here we have to create two boundary conditions, Two Fixed Supports and the other is we have to create Joint Rotation.
• To give Fixed Support, Right Click on the Static Structural >> Insert >>Fixed Support. This is shown in below Figure 29.

Figure 29-Give Fixed Support.

1) Fixed Support 1 :

• Here the wheel should be rigid, So select the inner face of the wheel to be fixed, Which is shown in below Figure 30.

Figure 30-Defined Fixed Support for the Wheel.

2) Fixed Support 2 :

• Here the wire will be slipping out of the slot, So we have to fix this also.
• To fix, Select the inner circular flat face of the wire, Which is shown in below Figure 31.

Figure 31-Defined Fixed Support for the Wire.

3) Rotational Joint :

• Here we have to give the Rotational Joint for the lever.
• We have to provide a rotation value from 0 to 145 degrees in the time interval of 8 steps.
• Select the inner circular hole face of the lever to give the rotational value, Which is shown in below Figure 32.

Figure 32-Defined the Rotational Joint.

Figure 33-Values given in the Tabular Data.

Phase 4-Request for the Outputs :

• Here we have to request outputs for the VonMisses Stress, Strain, and for Total Deformation.
• To request Output for Stress,Right Click on the Solution >> Insert >> Stress >> Equivalent Von Misses Stress.
• To request Output for Strain,Right Click on the Solution >> Insert >> Strain >> Equivalent Von Misses Strain.
• To request Output for Total Deformation,Right Click on the Solution >> Insert >> Deformation >> Total Deformation.
• This is shown in below Figure 34.

Figure 34-Requesting Outputs for the Stress, Strain, and Deformation.

• Next request output for the contact.
• To request Contact Tool >> Right Click on the Solution >> Insert >> Contact Tool >> Pressure >> Status,Which is shown in below Figures 35 and 36.

Figure 35-Requesting Output for Contact.

Figure 36-Requesting Outputs for Contact Tool.

• Similarly request the output for the Force Reaction.
• The Output requested for the Wire Bending Model is shown in below Figure 37.
• After requesting all the outputs, Run the Simulation.

Figure 37-Required Outputs Requested.

• To run the simulation, Right Click on the Solution >> Solve. This is shown in below Figure 38.

Figure 38-Solve all the Outputs Requested.

• After solving the outputs requested, the simulation results for all three cases are shown below Figures.

Case1 [Equivalent Von Misses Stress Copper Alloy] :

Figure 39-Equivalent Von Misses Stress [Case 1-Copper Alloy].

Figure 40-Equivalent Von Misses Stress Simulation Animation [Case 1-Copper Alloy].

Case2 [Equivalent Von Misses Stress Aluminium Alloy] :

Figure 41-Equivalent Von Misses Stress [Case 2-Aluminium Alloy].

Figure 42-Equivalent Von Misses Stress Simulation Animation [Case 2-Aluminium Alloy].

Case3 [Equivalent Von Misses Stress Magnesium Alloy] :

Figure 43-Equivalent Von Misses Stress [Case 3-Magnesium Alloy].

Figure 44-Equivalent Von Misses Stress Simulation Animation [Case 3-Magnesium Alloy].

Case1 [Equivalent Elastic Strain Copper Alloy] :

Figure 45-Equivalent Elastic Strain [Case 1-Copper Alloy].

Figure 46-Equivalent Elastic Strain Simulation Animation [Case 1-Copper Alloy].

Case2 [Equivalent Elastic Strain Aluminium Alloy] :

Figure 47-Equivalent Elastic Strain [Case 2-Aluminium Alloy].

Figure 48-Equivalent Elastic Strain Simulation Animation [Case 2-Aluminium Alloy].

Case3 [Equivalent Elastic Strain Magnesium Alloy] :

Figure 49-Equivalent Elastic Strain [Case 3-Magnesium Alloy].

Figure 50-Equivalent Elastic Strain Simulation Animation [Case 3-Magnesium Alloy].

Case1 [Equivalent Elastic Strain of Wire (Copper Alloy)] :

Figure 51-Equivalent Elastic Strain of Wire [Case 1-Copper Alloy].

Figure 52-Equivalent Elastic Strain of Wire Simulation Animation [Case 1-Copper Alloy].

Case2 [Equivalent Elastic Strain of Wire (Aluminium Alloy)] :

Figure 53-Equivalent Elastic Strain of Wire [Case 2-Aluminium Alloy].

Figure 54-Equivalent Elastic Strain of Wire Simulation Animation [Case 2-Aluminium Alloy].

Case3 [Equivalent Elastic Strain of Wire (Magnesium Alloy)] :

Figure 55-Equivalent Elastic Strain of Wire [Case 3-Magnesium Alloy].

Figure 56-Equivalent Elastic Strain of Wire Simulation Animation [Case 3-Magnesium Alloy].

Case1 Total Deformation [Copper Alloy] :

Figure 57-Case1 Total Deformation [Copper Alloy].

Figure 58-Case1 Total Deformation Simulation Animation [Copper Alloy].

Case2 Total Deformation [Aluminium Alloy] :

Figure 59-Case2 Total Deformation [Aluminium Alloy].

Figure 60-Case2 Total Deformation Simulation Animation [Aluminium Alloy].

Case3 Total Deformation [Magnesium Alloy] :

Figure 61-Case3 Total Deformation [Magnesium Alloy].

Figure 62-Case3 Total Deformation Simulation Animation [Magnesium Alloy].

Case1 Pressure [Copper Alloy] :

Figure 63-Case1 Pressure [Copper Alloy].

Figure 64-Case1 Pressure Simulation Animation [Copper Alloy].

Case2 Pressure [Aluminium Alloy] :

Figure 65-Case2 Pressure [Aluminium Alloy].

Figure 66-Case2 Pressure Simulation Animation [Aluminium Alloy].

Case3 Pressure [Copper Alloy] :

Figure 67-Case3 Pressure [Magnesium Alloy].

Figure 68-Case3 Pressure Simulation Animation [Magnesium Alloy].

Force Reaction :

• The Force Reaction for the case 1 with copper alloy material is shown in below Figure 69.It is similar for other two cases.

Figure 69-Case 1 Force Reaction Simulation Animation [Copper Alloy].

Comparison of Results :

Cases	Von-Misses Stress (MPa)		Total Deformation (mm)		Equivalent Elastic Strain (mm/mm)		Equivalent Elastic Strain of Wire(mm/mm)
	Max.	Min.	Max.	Min.	Max.	Min.	Max.	Min.
Case-1 [Copper Alloy]	341.01 MPa	3.1709e-003 MPa	262.64 mm	0. mm	3.1749e-003 mm/mm	1.7253e-008 mm/mm	3.1749e-003 mm/mm	7.8642e-008 mm/mm
Case-2 [Aluminium Alloy]	320.59 MPa	2.5651e-003 MPa	262.64 mm	0. mm	4.5304e-003 mm/mm	1.4287e-008 mm/mm	4.5304e-003 mm/mm	7.9872e-008 mm/mm
Case-3 [Magnesium Alloy]	257.77 MPa	1.9407e-003 MPa	262.64 mm	0. mm	5.7676e-003 mm/mm	1.6952e-008 mm/mm	5.7676e-003 mm/mm	7.9424e-008 mm/mm

Table-1

• From the result,The Maximum Von Misses Stress is occured in the Case-1 with Copper Alloy Material.
• The Maximum Stress developed in the Copper Alloy Material is 341.01 MPa and the Maximum Equivalent Elastic Strain is 0.0031749 mm/mm.
• The Maximu Deformation is occured is 262.64 mm,It is same for all the three cases.
• The stress developed in the copper material is high when compared to the other two cases and the Maximum Equivalent Elastic Strain developed in the Copper Alloy is 0.003749 mm/mm,It is least when compared to the other two cases.
• The Maximum Stress developed in all the three materails are beyond the yield strength of the material and the FOS for every material is less than 1,FOS of Copper Alloy=0.8,Aluminium Alloy-0.8,Magnesium Alloy-0.7,So every material will undergo plastic deformation.

Results :

• Hence the material has been defined for Wire Bending Model.
• Hence the connections were defined to the Wire Bending Model.
• Hence the model was meshed with tetrahedral elements and refined with 2.2 mm size.
• Hence the Simulation was ran successfully with 8 number of time steps.
• Hence the model was defined with Fixed Support and Rotational Joint.
• Hence the model has been solved for Von-Misses Stress, Equivalent Elastic Strain,Stress Intensity,Contact Tool and Directional Deformation by applying appropriate boundary conditions.

Learning Outcome and Conclusion :

In this Week 4 Wire Bending Challenge, I came to know about

• Learned how to give Fixed Support and Rotational Joint to the Wire Bending model.
• Learned to define Rotational joints.
• Learned how to assign materials to the model.
• Learned how to apply boundary conditions to the model.
• Learned how to request outputs and solve them.
• Learned about the Force Convergence.