3.6 Three-dimensional stress analysis: Stress concentration in a stepped round bar subjected to torsion

Stepped round bars are also important fundamental structural and/or machine elements; they are found in automobile axels, pump shafts, shafts in other rotary machines, etc. Such shafts are subjected to torsion.

Torsion problems of circular shafts are one of the most important problems in engineering.

3.6.1 Example problem: A stepped round bar subjected to torsion

Perform an FEM analysis of a 3D stepped round bar subjected to an applied torque at the free end and clamped to the rigid wall at the other end, as shown in Fig. 3.128. Calculate the stress concentration at the foot of the fillet of the bar and the shear stress distribution on a cross section of the bar.

Fig. 3.128
Fig. 3.128 Stepped round bar subjected to the applied torque T.

3.6.2 Problem description

  • Geometry: lengths l1 = 50 mm, l2 = 50 mm, diameters D = 40 mm, d = 20 mm, fillet radius ρ = 3 mm.
  • Material: mild steel having Young's modulus E = 210 GPa and Poisson's ratio ν = 0.3.
  • Boundary conditions: A stepped bar is rigidly clamped to a wall at the left end and twisted at the right free end by a torque (twisting moment) of T = 100 N mm applied in a plane perpendicular to the central axis of the bar, as shown in Fig. 3.128.

3.6.3 Review of the solutions obtained by the elementary mechanics of materials

Before proceeding to the FEM analysis of the stepped round bar, let us review the solution to the torsion problem of a straight cylindrical bar obtained by the elementary mechanics of materials, as shown in Fig. 3.129.

Fig. 3.129
Fig. 3.129 A circular cylindrical bar subjected to the applied torque T.

In a circular cylindrical bar subjected to the applied torque, shear strain γ is induced and varies linearly from the central axis reaching its maximum value γmax at the periphery of the bar, as given by Eq. (3.23).

γmax=γr=d/2=dθ2l

si40_e  (3.23)

where d is the diameter of the bar, l is its length, and θ is the angle of twist. The twist angle θ is obtained by the following equation:

θ=32TπGd4=TGIpwhereIp=πd432

si41_e  (3.24)

where G is the shear modulus and Ip is the polar moment of inertia of area of the bar.

The maximum shearing stress τ0 is thus obtained on the periphery of the bar at the right end where the torque T is applied, and is given by the following equation:

τ0=τθzr=d/2=16Tπd3

si42_e  (3.25)

3.6.4 Analytical procedures

3.6.4.1 Creation of an analytical model

A 3D stepped round bar can be created by rotating the 2D stepped beam described in Section A.1.1 around the longitudinal axis, or the x-axis. At first, create a 2D stepped beam having a rounded fillet referring to the operations described in Section A.1.1.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Create →Areas → Rectangle → By 2 Corners
  1. 1. Input two 0s into the WP X and WP Y boxes in the Rectangle by 2 Corners window to determine the lower left corner point of the thicker portion of the bar on the Cartesian coordinates of the working plane.
  2. 2. Input 100 and 20 (mm) into the Width and Height boxes, respectively, to determine the shape of the length and the radius of the thicker portion of the bar.
  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Create →Areas → Circle → Solid Circle
  1. 1. Input 53, 13, and 3 (mm) into the WP X, WP Y, and Radius boxes, respectively, in the Solid Circular Area window to create the rounded fillet having the curvature radius of 3 (mm).

Two more rectangles are needed to create a stepped beam with a rounded fillet. Create two rectangles by carrying out the following commands:

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Create →Areas → Rectangle → By 2 Corners
  1. 1. Input 53 and 10 (mm) into the WP X and WP Y boxes in the Rectangle by 2 Corners window, and 50 and 15 (mm) into the Width and Height boxes, respectively. Press the Apply button.
  2. 2. Input 50 and 13 (mm) into the WP X and WP Y boxes in the Rectangle by 2 Corners window, and 10 and 15 (mm) into the Width and Height boxes, respectively. Press the OK button.

The stepped beam with a rounded fillet can be obtained by subtracting the solid circle and the two small rectangles from the 100 by 20 (mm) rectangle created by the operations mentioned above.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Operate →Booleans → Subtract > Areas
  1. 1. Pick the largest rectangular area by the upward arrow to turn the colour of the rectangular area to pink. Click the OK button.
  2. 2. Pick the solid circular area and the two smaller rectangular areas by the upward arrow to turn the colour of the areas to pink. Click the OK button to get the stepped beam with a rounded fillet, as shown in Fig. 3.130.
Fig. 3.130
Fig. 3.130 2D stepped beam with a rounded fillet.

A stepped round bar with a rounded fillet can be obtained by rotating the 2D stepped beam around the x-axis.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Operate →Extrude → Areas → About Axis
  1. 1. The Sweep Areas about Axis window appears, as shown in Fig. 3.131. Pick the stepped beam area by the upward arrow to turn the colour of the rectangular area to pink. Click the OK button of the window.
  2. 2. Pick the two corner points of the bottom side of the stepped beam area by the upward arrow and click the OK button of the window.
  3. 3. Another Sweep Areas about Axis window appears, as shown in Fig. 3.132. Input 360 (degrees) into the ARC box to rotate the 2D stepped beam at 360 degrees about the x-axis to get the 3D stepped round bar with circumferential shoulder fillet, as shown in Fig. 3.133.
Fig. 3.131
Fig. 3.131 Sweep Areas about Axis window.
Fig. 3.132
Fig. 3.132 Another Sweep Areas about Axis window appearing after the window shown in Fig. 3.131.
Fig. 3.133
Fig. 3.133 3D stepped round bar with circumferential shoulder fillet created.

3.6.4.2 Input of the elastic properties of the stepped round bar material

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Material Props → Material Models
  1. 1. The Define Material Model Behavior window opens.
  2. 2. Double-click the Structural, Linear, Elastic, and Isotropic buttons one after another.
  3. 3. Input the value of Young's modulus, 2.1e5 (MPa), and that of Poisson's ratio, 0.3, into the EX and the PRXY boxes, respectively, and click the OK button of the Linear Isotropic Properties for Materials Number 1 window.
  4. 4. Exit from the Define Material Model Behavior window by selecting Exit in the Material menu of the window.

3.6.4.3 Finite-element discretisation of the round bar volume

  1. (1) Selection of the element type
  • [COMMAND]    ANSYS Main Menu → Preprocessor → Element Type → Add/Edit/ Delete
  1. 1. The Element Types window opens.
  2. 2. Click the Add … button in the Element Types window to open the Library of Element Types window and select the element type to use.
  3. 3. Select Structural Mass – Solid and Tet 10 node 187.
  4. 4. Click the OK button in the Library of Element Types window to use the 10-node isoparametric tetrahedral element.
  5. (2) Sizing of the elements
  • [COMMAND]    ANSYS Main Menu → Preprocessor → Meshing → Size Cntrls →Manual Size → Global → Size
  1. 1. The Global Element Sizes window opens.
  2. 2. Input 2 in the SIZE box and click the OK button.
  3. (3) Meshing
    [COMMAND]    ANSYS Main Menu → Preprocessor → Meshing → Mesh → Volumes → Free
  4. 1. The Mesh Volumes window opens.
  5. 2. The upward arrow appears in the ANSYS Graphics window. The stepped bar volume is quadrisected, as shown in Fig. 3.134. Point the arrow at each quarter volume and click one by one.
  6. 3. After the colour of the whole volume turns from light blue to pink, click the OK button to see the whole stepped round bar model meshed by 10-node tetrahedral isoparametric elements, as shown in Fig. 3.135.
Fig. 3.134
Fig. 3.134 A quadrisected volume of the stepped bar model selected for finite-element discretisation.
Fig. 3.135
Fig. 3.135 A whole view of the present stepped bar model discretised by 10-node tetrahedral isoparametric elements.

3.6.4.4 Input of boundary conditions

  1. (1) Imposing constraint conditions on the left-end face of the stepped round bar

Click the [A] Dynamic Model Mode button and drag the mouse while pressing its right button to rotate the round bar model to display the left end face, as shown in Fig. 3.136.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Loads → Define Loads →Apply → Structural → Displacement → On Areas
  1. 1. The Apply U, ROT on Areas window opens and the upward arrow appears when the mouse cursor is moved to the ANSYS Graphics window.
  2. 2. Click and select the four quadrants into which the left face is divided. Click the OK button in the Apply U, ROT on Areas window. Another Apply U, ROT on Areas window opens, as shown in Fig. 3.137. Select [A] All DOF in the Lab2 box and click the OK button.
  3. (2) Applying torque to the right-end face of the stepped round bar
Fig. 3.136
Fig. 3.136 Selected one of the four quadrants of the left-end face of the stepped bar model.
Fig. 3.137
Fig. 3.137 Apply U, ROT on Areas window.

An element called MPC184 rigid link/beam element is used to apply torque to the right-end face of the stepped round bar. This element is used as a rigid component to transmit forces, moments, and torques as in the present case, and is well suited for linear, large rotation, and/or large strain nonlinear applications [12].

Create the MPC184 element, or the multipoint constraint element, and apply torque via this element to the stepped round bar around its centre axis, or the x-axis. For this purpose, the pilot node will be defined first.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Modeling → Create →Nodes → In Active CS
  1. 1. The Create Nodes in Active Coordinate System window opens as shown in Fig. 3.138.
  2. 2. Input, say 150000, the node number which does not exist in the present model, in the NODE box and input the coordinates (100, 0, 0) of the centre of the right-end face in the X, Y, Z window, then click the OK button. Fig. 3.139 shows the pilot node number 150000 depicted on the right-end face of the stepped bar model.
Fig. 3.138
Fig. 3.138 Create Nodes in Active Coordinate System window.
Fig. 3.139
Fig. 3.139 Pilot node number 150000 depicted on the right-end face of the stepped bar model.

Click the Pair Based Contact Manager button shown by [B] in Fig. 3.136, and the Pair Based Contact Manager window opens. Click the [A] Contact Wizard button shown in Fig. 3.140.

Fig. 3.140
Fig. 3.140 Pair Based Contact Manager window and Contact Wizard button.

The Contact Wizard window opens. Choose Areas as the Target Surface and Pilot Node Only as the Target Type. Click the Next > button. Input N_PILOT in the Pilot name box, choose Pick existing node …, and click the Pick Entity … button. The Select Node for Pilot Node window opens as shown in Fig. 3.141. Input the pilot node number, i.e. 150000, in the List of Items box and click the OK button to return to the Contact Wizard window. Click the Next > button in the window.

Fig. 3.141
Fig. 3.141 Select Node for Pilot Node window.

The next screen of the Contact Wizard window appears. Choose Areas as the Contact Surface and Surface-to-Surface as the Contact Element Type. Click the Pick Contact … button. The Select Areas for Contact window opens, as shown in Fig. 3.142. Pick the four quadrants of the right-end face of the stepped bar to which the torque is to be applied to in the ANSYS Graphics window, and click the OK button to come back to the Contact Wizard window. Click the Next > button.

Fig. 3.142
Fig. 3.142 Select Areas for Contact window.

The next screen of the Contact Wizard window appears. Choose Rigid constraint as the Constraint Surface Type and User specified as the Boundary conditions on target. Click the Create > button. The message ‘The contact pair has been created. To interact with the contact pair use real set ID 3’ appears in the Contact Wizard window. Click the Finish button.

The Pair Based Contact Manager window opens, as shown in Fig. 3.143, describing the specifications of the contact pairs created. Fig. 3.144 shows in red the right-end face of the stepped bar to which the torque is applied.

  • [COMMAND]    ANSYS Utility Menu → Plot → Elements
Fig. 3.143
Fig. 3.143 Pair Based Contact Manager window describing the specifications of the contact pairs created.
Fig. 3.144
Fig. 3.144 Highlighted right-end face of the stepped bar to which the torque is applied.

The finite element mesh of the model is then recovered.

  • [COMMAND]    ANSYS Main Menu → Preprocessor → Loads → Define Loads → Apply → Structural → Force/Element → On Nodes
  1. 1. The Apply F/M on Nodes window opens as shown in Fig. 3.145. Input the pilot node number, i.e. 150000, in the List of Items box and click the OK button.
  2. 2. Another Apply F/M on Nodes window opens as shown in Fig. 3.146. Choose MX, or torsional moment around the x-axis, from among the items listed in the Lab box and Constant Value in the Apply as box. Input 100 (N mm) in the VALUE box, then click the OK button.
Fig. 3.145
Fig. 3.145 Apply F/M on Nodes window.
Fig. 3.146
Fig. 3.146 Next scene of the Apply F/M on Nodes window.

3.6.4.5 Solution procedures

Torsion analysis often needs the large rotation/displacement analysis. Without the large rotation/displacement option, the result of the torsion analysis brings about anomalous deformation as depicted in Fig. 3.147, where the deformation is enlarged to approximately 302 times the true scale and found to become larger for approaching the torque-bearing right-end face.

Fig. 3.147
Fig. 3.147 Anomalous deformation of the circular cylindrical bar as a result of torsion analysis without the large rotation/displacement option.

In order to set up the large deformation analysis, the following commands should be carried out:

  • [COMMAND]    ANSYS Main Menu → Solution → Analysis Type → Sol’n Controls
  1. 1. The Solution Controls window opens, as shown in Fig. 3.148.
  2. 2. Choose Large Displacement Static from among the items listed in the Analysis Options box and choose On in the Automatic time stepping box in the Time Control pane.
  3. 3. When the Automatic time stepping option is chosen to be On, the number, the maximum and the minimum numbers of substeps shall be specified. Specify 10, 100, and 5 as the three numbers, respectively, for the present analysis.
  4. 4. Click the OK button.
  • [COMMAND]    ANSYS Main Menu → Solution → Solve → Current LS
  1. (1) The Solve Current Load Step window opens.
  2. (2) Click the OK button.
Fig. 3.148
Fig. 3.148 Solution Controls window.

The ANSYS Process Status window appears, describing ‘Nonlinear Solution’ during the solution process. When the solution is complete, click the Close button in the Note window and close the /STATUS Command window by clicking the cross mark (‘x’) of the upper right corner of the window. The solution convergence diagram appears in the ANSYS Graphics window, as shown in Fig. 3.149.

  • [COMMAND]    ANSYS Utility Menu → Plot → Volumes
  1. 1. The 3D model of the stepped bar is displayed as shown in Fig. 3.150, where both the global coordinate system (X, Y, Z) and the local one (WX, WY, WZ) are depicted.
Fig. 3.149
Fig. 3.149 Solution convergence diagram displayed in the ANSYS Graphics window after the end of nonlinear analysis.
Fig. 3.150
Fig. 3.150 Global coordinate system (X, Y, Z) and local coordinate (WX, WY, WZ) depicted on the present 3D model of the stepped bar.

3.6.4.6 Contour plot of stress

  1. (1) Changing the coordinate system (CS): from the global Cartesian to the global cylindrical CS

It is preferable to present stress components induced in the present stepped round bar in the circular cylindrical coordinate system (r, θ, z) rather than by the usual Cartesian coordinate system (x, y, z).

Before changing the coordinate systems, the Cartesian coordinate system will be rotated around the y-axis by 90 degrees so that the new z-axis becomes the longitudinal axis of the stepped bar. On ANSYS, the x-, y-, and z-axes should be transformed to the radial axis r, the azimuthal axis θ, and the longitudinal axis z, respectively.

  • [COMMAND]    ANSYS Utility Menu → Work Plane → Offset WP by Increments …
  1. 1. The Offset WP window opens, as shown in Fig. 3.151.
  2. 2. Move the [A] slide bar for the coordinate rotation to 90 degrees.
  3. 3. Click the [B] + Y rotation button and then the OK button. The local coordinate system is rotated around the y-axis by 90 degrees.
Fig. 3.151
Fig. 3.151 Offset WP window.

The coordinate system can now be changed by the following commands:

  • [COMMAND]    ANSYS Utility Menu → Work Plane → Local Coordinate Systems →Create CS → At WP Origin
  1. 1. The Create Local CS at WP Origin window opens, as shown in Fig. 3.152.
  2. 2. Input any integer larger than 10 in the [A] KCN box and choose [B] Cylindrical 1 in the KCS box.
  3. 3. Click the OK button.
  • [COMMAND]    ANSYS Main Menu → General Postprocessor → Options for Output
  1. 1. The Options for Output window opens, as shown in Fig. 3.153.
  2. 2. Choose [A] Local system from among the items listed in the RSYS box, and input the [B] integer 11 in the Local system reference no. box.
  3. 3. Click the OK button to change the coordinate systems; i.e. from the Cartesian coordinate system to the local cylindrical one.
  4. (2) Contour plot of the shear stress τrθ component in the global cylindrical coordinate system
  • [COMMAND]    ANSYS Main Menu > General Postproc → Plot Results → Contour Plot → Nodal Solution
  1. 1. The Contour Nodal Solution Data window opens.
  2. 2. Select Stress and YZ Shear stress. Note that Y and Z are understood to be θ and z, respectively, after the coordinate transformation, although the label of each coordinate remains unchanged.
  3. 3. Click the OK button to display the contour map of the shear stress τrθ in the stepped round bar in the ANSYS Graphics window, as shown in Fig. 3.154.
Fig. 3.152
Fig. 3.152 Create Local CS at WP Origin window.
Fig. 3.153
Fig. 3.153 Options for Output window.
Fig. 3.154
Fig. 3.154 Contour map of the shear stress τrθ in the stepped round bar showing stress concentration at the foot of the circumferential shoulder fillet.

3.6.5 Discussion

Fig. 3.155 shows the relationship between stress concentration factor α and radius of curvature 2ρ/d at the foot of shoulder fillet for torsion of a stepped round bar with the shoulder fillet [13]. The relationship can be approximated by Eq. (3.27) [12].

Fig. 3.155
Fig. 3.155 Relationship between stress concentration factor α and radius of curvature 2ρ/d at the shoulder fillet for torsion of a stepped round bar with a shoulder fillet [12].

α=τmax/τ0

si43_e  (3.26)

α=1+Kdρ0.65

si44_e  (3.27)

The maximum stress obtained by ANSYS for the present stepped bar is about 0.0852 MPa, as shown in Fig. 3.154. The value of the stress concentration factor α of about 1.34 is obtained by the α − 2ρ/d diagram for D/d = 2; i.e.

τmax=ατ0≈1.34×16×100π×203≈0.0853MPa

si45_e  (3.28)

The value of the maximum shear stress τθz |max is a little bit smaller than that obtained by the tensile stress concentration vs radius of curvature diagram [13], and the relative difference the two values is − 0.16%.

3.6.6 Problems to solve

Problem 3.19

Calculate the stress concentration factor at a foot of the circumferential rounded fillet in a stepped circular cylindrical bar subjected to uniform tensile stress σ0 on the right-end face of the bar. The bar has the same geometry and mechanical properties as described in Section 3.6.2 and shown in Fig. 3.128, and is rigidly clamped to the rigid wall at the other end. Note that the large displacement option is not necessary to be imposed in this case.

Answer: The tensile stress concentration factor is obtained as α = σmax/σ0 ≈ 1.78 by the tensile stress concentration vs radius of curvature diagram [13].

Problem 3.20

Calculate the stress concentration factor at a foot of the circumferential rounded fillet in a stepped circular cylindrical bar subjected to point load P perpendicular to the longitudinal axis of the bar at the periphery of the right-end face of the bar. The bar has the same geometry and mechanical properties as described in Section 3.6.2 and shown in Fig. 3.128, and is rigidly clamped to the rigid wall at the other end. Note that the large displacement option is not necessary to be imposed in this case, either.

Answer: The bending stress concentration factor is obtained as α = σmax/σ0 ≈ 1.55 where σ0 = 32Pl2/(πd3) by the bending stress concentration vs radius of curvature diagram [13].

References

[1] Yuuki R., Kisu H. Elastic Analysis With the Boundary Element Method. Tokyo: Baifukan Co., Ltd.; 1987 (in Japanese).

[2] Isida M. Elastic Analysis of Cracks and Their Stress Intensity Factors. Tokyo: Baifukan Co., Ltd.; 1976 (in Japanese).

[3] Isida M. Analysis of stress intensity factors for the tension of a centrally cracked strip with stiffened edges. Eng. Fract. Mech. 1973;5(3):647–665.

[4] R.E. Feddersen, Discussion, ASTM STP 410, 1967, pp. 77–79.

[5] W.T. Koiter, Delft Technological University, Department of Mechanical Engineering, Report, No. 314, 1965.

[6] Tada H. A note on the finite width corrections to the stress intensity factor. Eng. Fract. Mech. 1971;3(2):345–347.

[7] Okamura H. Introduction to the Linear Elastic Fracture Mechanics. Tokyo: Baifukan Co., Ltd.; 1976 (in Japanese).

[8] Ewalds H.L., Wanhill R.J.H. Fracture Mechanics. London: Edward Arnold, Ltd.; 1984.

[9] Saxena A. Nonlinear Fracture Mechanics for Engineers. Florida: CRC Press; 1997.

[10] Nakahara I. Strength of Materials. Tokyo: Yokendo Co., Ltd.; . 1966;vol. 2 (in Japanese).

[11] Timoshenko S.P., Goodier J.N. Theory of Elasticity. third ed. Tokyo: McGraw-Hill Kogakusha, Ltd.; 1971.

[12] ANSYS help documents, SAS IP, Inc., 2015.

[13] Nishida M. Stress Concentration. Tokyo: Morikita Pub. Co., Ltd.; 1967 (in Japanese).

..................Content has been hidden....................

You can't read the all page of ebook, please click here login for view all page.
Reset