One end of a steel pin is rigidly fixed into the solid plate while its other end is force fitted into the steel arm. The configuration is shown in Fig. 7.1.

This is a three-dimensional analysis but because of the inherent symmetry of the model, analysis will be carried out for a quarter symmetry model only. There are two objectives of the analysis. The first objective is to observe the force fit stresses of the pin, which is pushed into the arm's hole with geometric interference. The second objective of the analysis is to find out stresses, contact pressures, and reaction forces due to a torque applied to the arm (force acting at the arm's end) and causing rotation of the arm. Stresses resulting from shearing of the pin and bending of the pin will be neglected purposefully.

The dimensions of the model are as follows:

• Pin radius = 1 cm, pin length = 3 cm. Arm width = 4 cm, arm length = 12 cm, arm thickness = 2 cm. Hole in the arm: radius = 0.99 cm, depth = 2 cm (through thickness hole).

Both elements are made of steel with Young's modulus = 2.1 × 10⁹ N/m², Poisson's ratio = 0.3 and are assumed to be elastic.

7.2.1.2 Construction of the model

In order to analyse the contact between the pin and the hole, a quarter symmetry model is appropriate. This is shown in Fig. 7.2.

In order to create a model shown in Fig. 7.2, two 3D (three-dimensional) primitives are used: block and cylinder. The model is constructed using GUI (graphic user interface) only. For carrying out Boolean operations, it is convenient to have volumes numbered. This can be done by selecting from the Utility Menu PlotCtrls → Numbering and checking the appropriate box to activate VOLU (volume numbers) option.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Block → By Dimensions. In response, a frame shown in Fig. 7.3 appears.

It can be seen from Fig. 7.3 that appropriate X, Y, Z coordinates were entered. Clicking the [A] OK button implements the entries. A block with the length 5, width 5, and thickness 2 (vol. 1) is created.

Next, from the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. In response, a frame shown in Fig. 7.4 appears.

The inputs are shown in Fig. 7.4. Clicking the [A] OK button implements the entries and creates a solid cylinder sector with a radius 1 cm, length 5.5 cm, starting angle 270 degrees, and ending angle 360 degrees (vol. 2).

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Overlap → Volumes. A frame shown in Fig. 7.5 appears.

Block (vol. 1) and cylinder (vol.2) should be picked and [A] OK button pressed. As a result of that block and cylinder are overlapped.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Block → By Dimensions. The frame shown in Fig. 7.6 appears.

Coordinates X, Y, Z were used as shown in Fig. 7.6. Clicking the [A] OK button implements the entries and, as a result, a block volume was created with the length 10 cm, width 2 cm and thickness 2 cm (vol. 2).

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. The frame shown in Fig. 7.7 appears.

Input data entered are shown in Fig. 7.7. Clicking the [A] OK button implements the entries. As a result, a solid cylinder sector with radius 0.99 cm, length 2 cm, starting angle 270 degrees, and ending angle 360 degrees (vol. 2) is produced. Next, volume 2 must be subtracted from volume 1 in order to produce a hole in the arm with the radius of 0.99 cm, which is smaller than the radius of the pin. In this way, an interference fit between the pin and the arm is created.

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate→ Booleans → Subtract → Volumes. The frame shown in Fig. 7.8 appears.

Volume 2 (short solid cylinder sector with radius 0.99 cm) is subtracted from volume 1 (the arm) by picking them in turn and pressing the [A] OK button. As a result, volume 6 is created.

From the ANSYS Main Menu, select Modelling → Move/Modify → Volumes. Then pick volume 6 (the arm), which is to be moved, and click OK. The frame shown in Fig. 7.9 appears.

In order to move the arm (vol. 6) into the required position, coordinates shown in Fig. 7.9 should be used. Clicking the [A] OK button implements the move action.

From the Utility Menu, select Plot → Replot to view the arm positioned in the required location. Finally, from the Utility Menu, select PlotCtrls → View Settings → Viewing Direction. The frame shown in Fig. 7.10 appears.

By selecting coordinates X, Y, Z as shown in Fig. 7.10 and activating [A] Plot → Replot command (Utility Menu), a quarter symmetry model, shown in Fig. 7.2, is finally created.

7.2.1.3 Material properties and element type

The next step in the analysis is to define the properties of the material used to make the pin and the arm.

From the ANSYS Main Menu, select Preferences. The frame shown in Fig. 7.11 is produced.

From the Preferences list, [A] Structural option was selected as shown in Fig. 7.11.

From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models.

Click in turn: Structural: Linear: Elastic: Isotropic. A frame shown in Fig. 7.12 appears.

Enter [A] EX = 2.1 × 10⁹ for Young's modulus and [B] PRXY = 0.3 for Poisson's ratio. Then click [C] OK and afterwards Material: Exit.

After defining properties of the material, the next step is to select the element type appropriate for the analysis.

From the ANSYS Main Menu, select Preprocessor: Element Type: Add/Edit/Delete. The frame shown in Fig. 7.13 appears.

Click [A] Add in order to pull down another frame, shown in Fig. 7.14.

In the left column click [A] Structural Solid and in the right column click [B] Brick 8node 185. After that click [C] OK and [B] Close in the frame shown in Fig. 7.13. This completes the element type selection.

7.2.1.4 Meshing

From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh Tool. The frame shown in Fig. 7.15 appears.

There are a number of options available. The first step is to go to [A] Size Control → Lines option and click the [B] Set button. This opens another frame (shown in Fig. 7.16) prompting to pick lines on which element size is going to be controlled.

Pick the horizontal and vertical lines on the front edge of the pin and click [A] OK. The frame shown in Fig. 7.17 appears. In the box [A] No. of element divisions, type 3 and change selection [B] SIZE, NDIV can be changed to No by checking the box and, finally, click [C] OK.

Using the MeshTool frame again, shown in Fig. 7.18, click button [A] Set in the Size Controls → Lines option and pick the curved line on the front of the arm. Click OK afterwards. The frame shown in Fig. 7.17 appears. In the box No. of element divisions, type 4 this time and press the [C] OK button.

In the frame MeshTool (see Fig. 7.18), pull down [B] Volumes in the option Mesh.

Check [C] Hex/Wedge and [D] Sweep options. This is shown in Fig. 7.18.

Pressing the [E] Sweep button brings another frame asking to pick the pin and the arm volumes (see Fig. 7.19).

Selecting first [A] Pick All and then pressing the [B] OK button initiates the meshing process. The model after meshing looks like the image in Fig. 7.20.

Pressing the [F] Close button on MeshTool frame (see Fig. 7.18) ends the mesh generation stage.

After meshing is complete, it is usually necessary to smooth element edges in order to improve the graphic display. This can be accomplished using the PlotCtrls facility in the Utility Menu.

From the Utility Menu, select PlotCtrls → Style → Size and Shape. The frame shown in Fig. 7.21 appears.

In the option [A] Facets/element edge, select 2 facets/edge, which is shown in Fig. 7.21.

7.2.1.5 Creation of contact pair

In solving the problem of contact between two elements, it is necessary to create a contact pair. Contact Wizard is the facility offered by ANSYS.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Contact Pair. As a result of this selection, a frame shown in Fig. 7.22 appears.

The location of [A] Contact Wizard button is in the upper left-hand corner of the frame. By clicking on this button a new frame, shown in Fig. 7.23, is produced.

In the frame shown in Fig. 7.23, select [A] Areas, [B] Flexible and press the [C] Pick Target button. As a result of that selection, the frame shown in Fig. 7.24 is produced.

The target area is the surface of pin hole in the arm and it should be picked and the [A] OK button pressed. In the Contact Wizard frame (see Fig. 7.23), press the [D] Next button (which should be highlighted when the target area is picked) and the Pick Contact button to obtain another frame, shown in Fig. 7.25.

The surface area of the pin should be picked as the area for contact. When this is done and the [A] OK button pressed, the Contact Wizard frame appears (see Fig. 7.23). Pressing the Next [D] button produces a frame in which Material ID = 1, Coefficient of friction = 0.2 should be selected. Also the Include Initial penetration option should be checked. Next, the Optional settings button should be pressed in order to refine contact parameters further. In the new frame, Normal penalty stiffness = 0.1 should be selected. Also, the Friction tab located in the top of the frame menu should be activated and Stiffness matrix = Unsymmetric selected. Afterwards, pressing the OK button and then Create results in the image shown in Fig. 7.26.

Also, the Contact Wizard frame appears in the form shown in Fig. 7.27.

The message is that the contact pair has been created. Pressing the [A] Finish button closes the Contact Wizard tool.

The Contact Manager frame appears again with the information pertinent to the problem considered. It is shown in Fig. 7.28.

7.2.1.6 Solution

In the solution stage, solution criteria have to be specified first. As a first step in that process, symmetry constraints are applied on the quarter symmetry model.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → Symmetry BC → On Areas. A frame shown in Fig. 7.29 appears.

Four areas which were created when the full configuration model was sectioned to produce quarter symmetry model should be picked. When that is done, click the [A] OK button in the frame of Fig. 7.29.

The next step is to apply boundary constraints on the block of which the pin is an integral part.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On Areas. Fig. 7.30 showing quarter symmetry model appears.

The back side of the block should be picked and then the OK button pressed. The frame shown in Fig. 7.31 appears.

All degrees of freedom [A] All DOF should be constrained with the displacement value equal to zero (see Fig. 7.31). Clicking the [B] OK button applies the constraints.

Because the original problem formulation asks for stress analysis when the arm is pulled out of the pin, the analysis involves large displacement effects. The first type of load results from the interference fit between the pin and arm.

From the ANSYS Main Menu, select Solution → Analysis Type → Sol’n Controls. A frame shown in Fig. 7.32 appears. In the pull-down menu, select [A] Large Displacement Static. Further selected options should be: [B] Time at end of load step = 100; [C] Automatic time stepping (pull-down menu) = Off; [D] Number of substeps = 1. All specified selections are shown in Fig. 7.32. Pressing the [E] OK button applies the settings and closes the frame.

The next action is to solve for the first type of load, which is interference fit.

From the ANSYS Main Menu, select Solution → Solve → Current LS. A frame showing review of information pertaining to the planned solution action appears. After checking that everything is correct, select File → Close to close that frame. Pressing the OK button starts the solution. When the solution is completed, press the Close button.

In order to return to the previous image of the model, select Utility Menu → Plot → Replot.

The second type of load is created when the arm is pulled out of the pin. A number of actions have to be taken in order to prepare the model for the solution. The first action is to apply a displacement along Z axis equal to 2 cm (thickness of the arm) to all nodes on the front of the pin in order to observe this effect.

From the Utility Menu, choose Select → Entities. A frame shown in Fig. 7.33 appears.

In this frame, the following selections should be made: [A] Nodes (from pull-down menu); [B] By Location (pull-down menu); [C] Z coordinates (to be checked); Min, Max = 4, 5. Pressing the [D] OK button implements the selections made.

Next, degrees of freedom in the Z direction should be constrained with the displacement value of 2 (thickness of the arm).

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On Nodes. In response, a frame shown in Fig. 7.34 appears.

By pressing the [A] Pick All button, a frame shown in Fig. 7.35 is called up.

As shown in Fig. 7.35, [A] DOF to be constrained = UZ and the [B] Displacement value = 2. Pressing the [C] OK button applies selected constraints.

Options for the analysis of pull-out operation have to be defined now.

From the ANSYS Main Menu, select Solution → Analysis Type → Sol’n Controls. A frame shown in Fig. 7.36 appears in response.

As shown in Fig. 7.36, the following selections defining solution controls were made: [A] Time at end of load step = 200; [B] Automatic time stepping (pull-down menu) = On; [C] Number of substeps = 100; [D] Max no. of substeps = 10,000; [E] Min no. of substeps = 10; Frequency (pull-down menu) = Write every Nth substep; where N = − 10. Pressing the [F] OK button applies selected controls.

Now the model is ready to be solved for the load resulting from pulling the arm out.

From the ANSYS Main Menu, select Solution: Solve: Current LS. A frame giving summary information pertinent to the solution appears. After reviewing the information select File: Close to close the frame. After that, pressing the OK button starts the solution. When the solution is done, press the Close button.

During solution process warning messages could appear. In order to make sure that the solution is done, it is practical to issue the command in the input box: /NERR, 100, 100, 0FF. This ensures that the ANSYS programme does not abort if it encounters a considerable number of errors.

7.2.1.7 Postprocessing

The postprocessing stage is used to display solution results in a variety of forms.

The first thing to do is to expand the quarter symmetry model into the full configuration model.

From the Utility Menu, select PlotCtrls → Style → Symmetry Expansion → Periodic/Cyclic Symmetry. Fig. 7.37 shows the resulting frame.

Check the [A] ¼ Dihedral Sym button as shown in Fig. 7.37 and press the [B] OK button.

From the Utility Menu, select Plot → Elements. An image of the full configuration model appears, as shown in Fig. 7.38.

The first set of results to observe in the postprocessing stage is the state of stress due to interference fit between the pin and the hole in the arm.

From the ANSYS Main Menu, select General Postproc → Read results → By Load Step. The frame shown in Fig. 7.39 is produced.

The selection [A] Load step number = 1 is shown in Fig. 7.39. By clicking the [B] OK button, the selection is implemented.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. In the resulting frame (see Fig. 7.40), the following selections are made: [A] Item to be contoured = Stress; [B] Item to be contoured = von Mises (SEQV). Pressing the [C] OK button implements the selections made.

A contour plot of von Mises stress (nodal solution) is shown in Fig. 7.41.

Fig. 7.41 shows a stress contour plot for the assembly of the pin in the hole. In order to observe contact pressure on the pin resulting from the interference fit, it is necessary to read results by time/frequency.

From the ANSYS Main Menu, select General Postproc → Read Results → By Time/Freq.

In the resulting frame, shown in Fig. 7.42, the selection to be made is: [A] Value of time or freq = 120. Pressing the [B] OK button implements the selection.

From the Utility Menu, choose Select: Entities. The frame shown in Fig. 7.43 appears.

In the frame shown in Fig. 7.43, the following selections are made: [A] Elements (from pull-down menu); [B] By Elem Name (from pull-down menu); [C] Element Name = 174. The element with the number 174 was introduced automatically during the process of creation of contact pairs described earlier. It is listed in the Preprocessor → Element Type → Add/Edit/Delete option. Selections are implemented by pressing the [D] OK button.

From the Utility Menu, select Plot → Elements. An image of the pin with surface elements is produced (see Fig. 7.44).

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The frame shown in Fig. 7.45 appears.

In the frame shown in Fig. 7.45, the following selections are made: [A] Contact and [B] Pressure. These are items to be contoured. Pressing the [C] OK button implements the selections made. Fig. 7.46 shows an image of the pin with pressure contours.

The last action to be taken is to observe the state of stress resulting from pulling out the arm from the pin.

From the Utility Menu, choose Select → Everything. Next, from the ANSYS Main Menu, select General Postproc: Read Results: By Load Step. The frame shown in Fig. 7.47 appears.

As shown in Fig. 7.47, [A] Load step number = 2″ was selected. Pressing the [B] OK button implements the selection.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. In the appearing frame (see Fig. 7.40), the following are selected as items to be contoured: [A] Stress; [B] von Mises (SEQV). Pressing the [C] OK button implements the selections made. Fig. 7.48 shows stress contours on the pin resulting from pulling out the arm.

The configuration of the contact between a cylinder and two blocks is shown in Fig. 7.49.

This is a typical contact problem, which in engineering applications is represented by a cylindrical rolling contact bearing. Also, the characteristic feature of the contact is that, nominally, surface contact takes place between elements. In reality, this is never the case due to surface roughness and unavoidable machining errors and dimensional tolerance. There is no geometrical interference when the cylinder and two blocks are assembled.

This is a 3D analysis and advantage could be taken of the inherent symmetry of the model. Therefore, the analysis will be carried out on a half symmetry model only. The objective of the analysis is to observe the stresses in the cylinder when the initial gap between two blocks is decreased by 0.05 cm.

The dimensions of the model are as follows:

• Cylinder radius = 0.5 cm; cylinder length = 1 cm; block length = 2 cm; block width = 1 cm; block thickness = 0.75 cm. Both blocks are geometrically identical. All elements are made of steel with Young's modulus = 2.1 × 10⁹ N/m², Poisson's ratio = 0.3 and are assumed elastic. The friction coefficient at the interface between cylinder and the block is 0.2.

7.2.2.2 Model construction

For the intended analysis, a half symmetry model is appropriate. This is shown in Fig. 7.50.

In order to create a model shown in Fig. 7.50, the use of two 3D (three-dimensional) primitives, namely block and cylinder, is made. The model is constructed using GUI facilities only. When carrying out Boolean operations on volumes, it is quite convenient to number them. This is done by selecting from the Utility Menu → PlotCtrls → Numbering and checking the appropriate box to activate the VOLU (volume numbers) option.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Block → By Dimensions. In response, a frame shown in Fig. 7.51 appears.

It can be seen from Fig. 7.51 that appropriate X, Y, Z coordinates were entered to create a block (vol. 1) with the length 2 cm ([A] X1 = − 1; X2 = 1), width 1 cm ([B] Z1 = 0; Z2 = 1), and thickness 0.75 cm ([C] Y1 = − 0.25; Y2 = − 1). Next, from the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. In response, a frame shown in Fig. 7.52 appears.

The input into the frame, shown in Fig. 7.52, created a solid cylinder sector with the [A] radius 0.5 cm, [B] length 1 cm, [C] starting angle 180 degrees, and [D] ending angle 360 degrees (vol. 2).

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Overlap → Volumes. A frame shown in Fig. 7.53 appears.

Block (vol. 1) and cylinder (vol.2) should be picked and the [A] OK button pressed. As a result of that, the block and cylinder are overlapped and three volumes created: vol. 5 (block), vol. 3 (section of the cylinder within the block), and vol. 4 (remaining of the cylinder after a section of it has been subtracted).

From the ANSYS Main Menu, select Modelling → Delete → Volume and Below. The frame shown in Fig. 7.54 appears.

Picking vol. 4 and clicking the [A] OK button deletes it. The same operation should be repeated to delete vol. 3. As a result of that, a block should be produced. The front view of the block is shown in Fig. 7.55.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Volumes → Cylinder → By Dimensions. In response, a frame shown in Fig. 7.56 appears.

A cylinder created earlier (see Fig. 7.52 for inputs) is reproduced (vol. 1).

In order to create loading conditions at the contact interface, the cylinder is moved towards the block by 0.05 units.

From the ANSYS Main Menu, select Modelling → Move/Modify → Volumes. A frame shown in Fig. 7.57 appears.

Selecting vol. 1 and clicking the [A] OK button calls up another frame shown in Fig. 7.58.

Fig. 7.58 shows that the cylinder was moved by [A] 0.05 cm downwards—that is, towards the block, after clicking the [B] OK button.

From the Utility Menu, select Plot → Replot to view the cylinder positioned in the required location. Finally, from the Utility Menu, select PlotCtrls → View Settings → Viewing Direction. The frame shown in Fig. 7.59 appears.

By selecting coordinates [A] X, Y, Z, as shown in Fig. 7.59, clicking the [B] OK button, and activating the Plot → Replot command (Utility Menu), a half symmetry model, shown in Fig. 7.50, is finally created.

7.2.2.3 Material properties

Before any analysis is attempted, it is necessary to define the properties of the material to be used.

From the ANSYS Main Menu, select Preferences. The frame shown in Fig. 7.60 is produced.

From the Preferences list, [A] Structural option was selected, as shown in Fig. 7.60. From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models. Click in turn: Structural → Linear → Elastic → Isotropic. A frame shown in Fig. 7.61 appears.

Enter [A] EX = 2.1 × 10⁹ for Young's modulus and [B] PRXY = 0.3 for Poisson's ratio. Then click the [C] OK button and afterwards Material → Exit. After defining properties of the material, the next step is to select element type appropriate for the analysis performed. From the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 7.62 appears.

Click [A] Add in order to pull down another frame, shown in Fig. 7.63.

In the left column click [A] Structural Solid and in the right column click [B] Brick 8node 185. After that click [C] OK and Close in order to finish the element type selection.

7.2.2.4 Meshing

From the ANSYS Main Menu, select Preprocessor: → Meshing → Mesh Tool. The frame shown in Fig. 7.64 appears.

There are a number of options available. The first step is to go to Size Control → Lines option and click the [A] Set button. This opens another frame (shown in Fig. 7.65), prompting you to pick lines on which element size is going to be controlled.

Pick two horizontal lines on the front edge of the cylinder and click the [A] OK button. The frame shown in Fig. 7.66 appears.

In the box [A] No. of element divisions, type 3 and change selection [B] SIZE, NDIV can be changed to No by checking the box and click the [C] OK button. Both selections are shown in Fig. 7.66.

Similarly, using Mesh Tool frame, click button Set in the Size Controls: Lines option and pick the curved line on the front of the block. Click OK afterwards. The frame shown in Fig. 7.66 appears. In the box [A] No. of element divisions, type 4 this time and press the [C] OK button.

In the frame Mesh Tool (see Fig. 7.67), pull down [A] Volumes in the option Mesh.

Check [B] Hex/Wedge and [C] Sweep options. This is shown in Fig. 7.67.

Pressing the [D] Sweep button brings another frame asking you to pick volumes to be swept (see Fig. 7.68).

Pressing the [A] Pick All button initiates the meshing process. After meshing, the model looks like the image in Fig. 7.69. Pressing the [E] Close button in Mesh Tool frame ends the mesh generation stage.

After meshing is complete, it is usually necessary to smooth element edges in order to improve the graphic display. This can be accomplished using the PlotCtrls facility in the Utility Menu. From the Utility Menu, select PlotCtrls → Style → Size and Shape. The frame shown in Fig. 7.70 appears.

In the option [A] Facets/element edge, select 2 facets/edge and click the [B] OK button to implement the selection, as shown in Fig. 7.70.

In solving the problem of contact between two elements, it is necessary to create a contact pair. Contact Wizard is the facility offered by ANSYS.

7.2.2.5 Creation of a contact pair

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Contact Pair. As a result of this selection, a frame shown in Fig. 7.71 appears.

The Contact Wizard button is located in the upper left-hand corner of the frame. By clicking the [A] on this button, a Contact Wizard frame, shown in Fig. 7.72, is produced.

In the frame shown in Fig. 7.72, select [A] Areas, [B] Flexible, and press the [C] Pick Target button. The frame shown in Fig. 7.73 is produced.

Select the curved surface in the block as a target and press the [A] OK button in the frame of Fig. 7.73. Again the Contact Wizard frame appears, and this time the Next button should be pressed to obtain the frame shown in Fig. 7.74.

Press the [A] Pick Contact button to create the frame shown in Fig. 7.75.

Pick the area of the cylinder in contact with the concave area in the block as a contact and press the OK button. Again the Contact Wizard frame appears, and the Next button should be clicked. The frame shown in Fig. 7.76 appears.

In this frame, select [A] Coefficient of Friction = 0.2, check box [B] Include initial penetration. Next, press the [C] Optional settings button to call up another frame. In the new frame (Fig. 7.77), Normal penalty stiffness = 0.1 should be selected. Also, the Friction tab located in the top of the frame menu should be activated and Stiffness matrix = Unsymmetric selected.

Pressing the [A] OK button brings back Contact Wizard frame (see Fig. 7.76); the [D] Create button should be pressed.

A created contact pair is shown in Fig. 7.78.

Finally, the Contact Wizard frame should be closed by pressing the Finish button. Also, the Contact Manager summary information frame should be closed.

7.2.2.6 Solution

Before the solution process can be attempted, solution criteria have to be specified. As a first step in that process, symmetry constraints are applied on the half symmetry model.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → Symmetry BC → On Areas. A frame shown in Fig. 7.79 appears.

Three horizontal surfaces should be selected by picking them and then clicking the [A] OK button. As a result, an image shown in Fig. 7.80 appears.

The next step is to apply constraints on the bottom surface of the block. From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On Areas. The frame shown in Fig. 7.81 appears.

After selecting the required surface (bottom surface of the block) and pressing the [A] OK button, another frame appears, in which the following should be selected: DOFs to be constrained = All DOF and Displacement value = 0. Selections are implemented by pressing the OK button in the frame.

Because the cylinder has been moved towards the block by 0.05 cm, in order to create an interference load, the analysis involves large displacement effects.

From the ANSYS Main Menu, select Solution → Analysis Type → Sol’n Controls. A frame shown in Fig. 7.82 appears.

In the pull-down menu, select [A] Large Displacement Static. Further selected options should be: [B] Time at end of load step = 100; [C] Automatic time stepping (pull-down menu) = Off; [D] Number of substeps = 1. All specified selections are shown in Fig. 7.82. Pressing the [E] OK button implements the settings and closes the frame.

Now the modelling stage is completed and the solution can be attempted. From the ANSYS Main Menu, select Solution → Solve → Current LS. A frame showing a review of information pertaining to the planned solution action appears. After checking that everything is correct, select File: Close to close that frame. Pressing the OK button starts the solution. When the solution is completed, press the Close button.

In order to return to the previous image of the model, select Utility Menu → Plot → Replot.

7.2.2.7 Postprocessing

Solution results can be displayed in a variety of forms using postprocessing facility. For the results to be viewed for the full model, the half symmetry model used for analysis has to be expanded.

From the Utility Menu, select PlotCtrls → Style → Symmetry Expansion → Periodic/Cyclic Symmetry. Fig. 7.83 shows the resulting frame.

In the frame shown in Fig. 7.83, [A] Reflect about XZ was selected. After clicking the [B] OK button in the frame and selecting Plot: Elements from the Utility Menu, an image of a full model, shown in Fig. 7.84, is produced.

The objective of the analysis presented here was to observe stresses in the cylinder produced by the reduction of the initial gap between two blocks by 0.05 cm (an interference fit). Therefore, from the ANSYS Main Menu, select General Postproc → Read results → By Load Step. The frame shown in Fig. 7.85 is produced.

The selection [A] Load step number = 1, shown in Fig. 7.85, is implemented by clicking the [B] OK button.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. In the resulting frame (see Fig. 7.86), the following selections are made: [A] Item to be contoured = Stress; [B] Item to be contoured = von Mises (SEQV). Pressing the [C] OK button implements the selections made.

A contour plot of von Mises stress (nodal solution) is shown in Fig. 7.87.

Fig. 7.87 shows a von Mises stress contour for the whole assembly. If one is interested in observing contact pressure on the cylinder alone, then a different presentation of solution results is required.

From the Utility Menu, choose Select → Entities. The frame shown in Fig. 7.88 appears.

In the frame shown in Fig. 7.88, the following selections are made: [A] Elements (first pull-down menu); [B] By Elem Name (second pull-down menu); [C] Element Name = 174. The element with the number 174 was introduced automatically during the process of creation of contact pairs described earlier. It is listed in the Preprocessor → Element Type → Add/Edit/Delete option. Selections are implemented by pressing the [D] OK button.

From the Utility Menu, select Plot → Elements. An image of the cylinder surface with a mesh of elements is produced (see Fig. 7.89).

It is seen that the gap equal to 0.05 units exists between two half of the cylinder. It is the result of moving half of the cylinder towards the block (by 0.05 cm) in order to create loading at the interface.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The frame shown in Fig. 7.90 appears.

In the frame, shown in Fig. 7.90, the following selections are made: [A] Contact and [B] Pressure. These are items to be contoured. Pressing the [C] OK button implements the selections made. In response to that, an image of the cylinder surface with pressure contours on it is produced, as shown in Fig. 7.91.

The configuration of the contact to be analysed is shown in Fig. 7.92.

This contact problem, which in practice is represented by a wheel-on-rail configuration, is well known in engineering. Also, the characteristic feature of the contact is that, nominally, contact between elements takes place along line. In reality, this is never the case due to unavoidable elastic deformations and surface roughness. As a consequence of that, surface contact is established between elements.

This is a 3D analysis and advantage could be taken of the inherent symmetry of the model. Therefore, the analysis will be carried out on a quarter symmetry model only. The objective of the analysis is to observe the stresses in the cylinder and the rail when an external load is imposed on them.

The dimensions of the model are as follows:

• Diameter of the cylinder = 1 cm; cylinder length = 2 cm. Rail dimensions: base width = 4 cm; head width = 2 cm; head thickness = 0.5 cm; rail height = 2 cm.

Both elements are made of steel with Young's modulus = 2.1 × 10⁹ N/m², Poisson's ratio = 0.3 and are assumed elastic. The friction coefficient at the interface between cylinder and the rail is 0.1.

7.2.3.2 Model construction

For the intended analysis, a half symmetry model is appropriate. This is shown in Fig. 7.93.

The model is constructed using GUI facilities only. First, a 2D model is created (using rectangles and circles as primitives). This is shown in Fig. 7.94.

Next, using the ‘extrude’ facility, areas are converted into volumes and a 3D model constructed. When carrying out Boolean operations on areas or volumes, it is convenient to number them. This is done by selecting from the Utility Menu → PlotCtrls → Numbering and checking the appropriate box to activate the AREA (area numbers) or VOLU (volume numbers) option.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. A frame shown in Fig. 7.95 appears.

Entered coordinates, [A] (X1 = 0; X2 = 2) and [B] (Y1 = − 0.5; Y2 = − 2.5), are shown in Fig. 7.95. This creates area A1.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. A frame with entered coordinates, [A] (X1 = 1; X2 = 2) and [B] (Y1 = − 0.5; Y2 = − 1.5), is shown in Fig. 7.96. This creates area A2.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By Dimensions. A frame with entered coordinates, [A] (X1 = 0.5; X2 = 2) and [B] (Y1 = − 1; Y2 = − 1.5), is shown in Fig. 7.97. This creates area A3.

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Booleans → Subtract → Areas. A frame shown in Fig. 7.98 appears, asking for selection of areas to be subtracted.

Select the first area, A1, by clicking on it. Then click the [A] OK button in the frame of Fig. 7.98. Next, select area A3 by clicking on it and pressing the [A] OK button. Area A3 is subtracted from area A1. This operation creates area A4.

Repeat all the above steps in order to subtract area A2 from area A4. As a result of this operation, a cross-section of half of the rail's area is created. Its assigned number is A1.

Next, a quarter of a circle is created, which will be extruded into a quarter of the cylinder. To do that, it is necessary to offset WP (work plane) by 90 degrees, so that the quarter circle will have the required orientation.

From the Utility Menu, select WorkPlane → Offset WP by Increments. Fig. 7.99 shows the frame resulting from the selection.

It can be seen from Fig. 7.99 that the ZX plane was offset by [A] 90 degrees clockwise (the clockwise direction is negative).

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Circle → By Dimensions. The frame shown in Fig. 7.100 appears where appropriate data were entered to create a solid quarter of a circle with [A] outer radius of 0.5 cm, [B] starting angle 270 degrees, and [C] ending angle 360 degrees.

When the solid quarter circular area is created, it is important to restore WP offset to its original setting. This can be done by following steps associated with Fig. 7.99 and selecting, XY, YZ, ZX angles as 0, 0, and 90 degrees, respectively.

In an isometric view, the 2D quarter model is shown in Fig. 7.101.

It can be seen that the cross-section of the rail is assigned number A1 and the quarter of the solid circle is given number A2.

The next step is to extrude both areas, A1 and A2, into volumes.

From the ANSYS Main Menu, select Preprocessor → Modelling → Operate → Extrude → Areas → Along Normal. The frame shown in Fig. 7.102 appears.

Pick area A1 and click the [A] OK button to pull down another frame shown in Fig. 7.103.

Selections made are shown in Fig. 7.103. By clicking the [A] OK button, a 2D cross-section of the rail is extruded by [B] 1 cm (length of extrusion) into a volume. The direction of extrusion is normal to the rail's cross-section.

In a similar way, a quarter solid circle can be extruded to create a quarter of the cylinder with 1 cm length. Fig. 7.104 shows the frame and selections made.

It should be noted that in order to have the quarter cylinder oriented as required, [A] length of extrusion = − 1 cm should be selected. The minus sign denotes the direction of extrusion.

From the Utility Menu, select PlotCtrls → Numbering and check in VOLU and check out AREA. This will change the system of numbering from areas to volumes. The rail is allocated number V1 and cylinder number V2. This completes the construction of a quarter symmetry model, shown in Fig. 7.93.

7.2.3.3 Properties of material

Before any analysis is attempted, it is necessary to define the properties of the material to be used.

From the ANSYS Main Menu, select Preferences. The frame in Fig. 7.105 is produced.

As shown in Fig. 7.105, [A] Structural was the option selected.

From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models. Double-click Structural → Linear → Elastic → Isotropic. A frame shown in Fig. 7.106 appears.

Enter [A] EX = 2.1 × 10⁹ for Young's modulus and [B] PRXY = 0.3 for Poisson's ratio. Then click the [C] OK button and afterwards Material: Exit.

After defining properties of the material, the next step is to select element type appropriate for the analysis performed.

From the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 7.107 appears.

Click the [A] Add button in order to pull down another frame, shown in Fig. 7.108.

In the left column click [A] Structural Solid and in the right column click [B] Brick 8node 185. After that click [C] OK and Close in order to finish the element type selection.

7.2.3.4 Meshing

From the ANSYS Main Menu, select Preprocessor → Meshing → Mesh Tool. The frame shown in Fig. 7.109 appears.

There are a number of options available. The first step is to go to Size Control → Lines option and click the [A] Set button. This opens another frame (shown in Fig. 7.110) prompting you to pick lines on which element size is going to be controlled.

Pick two lines, one arcuate and the other horizontal in contact with the top surface of the rail, located on the front side of the cylinder, and click the [A] OK button. The frame shown in Fig. 7.111 appears.

In the box [A] No. of element divisions, type 30 and change selection [B] SIZE, NDIV can be changed to No by checking the box out and then click [C] OK. Both selections are shown in Fig. 7.111.

Similarly, using the MeshTool frame (see Fig. 7.109), click the [A] Set button in the Size Controls → Lines option and pick two lines located on the top surface of the rail: one coinciding with the line previously picked and the other at the right angle to the first one. Click [A] OK as shown in Fig. 7.110. The frame shown in Fig. 7.111 appears again. In the box [A] No. of element divisions, type 30 and press the [C] OK button.

In the frame MeshTool (see Fig. 7.112), pull down [A] Volumes in the option Mesh. Check the [B] Hex and [C] Sweep options.

Pressing the [D] Sweep button brings up another frame, shown in Fig. 7.113, asking you to pick volumes to sweep.

Pressing the [A] Pick All button initiates the meshing process. The model after meshing looks like the image in Fig. 7.114.

Pressing the Close button on the MeshTool frame ends the mesh generation stage.

After the meshing is complete, it is usually necessary to smooth element edges in order to improve the graphic display. This can be accomplished using the PlotCtrls facility in the Utility Menu.

From the Utility Menu, select PlotCtrls → Style → Size and Shape. The frame shown in Fig. 7.115 appears.

In the option [A] Facets/element edge, select 2 facets/edge and click the [B] OK button as shown in Fig. 7.115.

7.2.3.5 Creation of a contact pair

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Contact Pair. As a result of this selection, a frame shown in Fig. 7.116 appears.

The upper left-hand corner of the frame contains the [A] Contact Wizard button. By clicking on this button, a Contact Wizard frame, shown in Fig. 7.117, is produced.

In the frame shown in Fig. 7.117, select [A] Areas, [B] Flexible, and press the [C] Pick Target button. The frame shown in Fig. 7.118 is produced.

Select the top area of the rail by clicking on it and pressing the [A] OK button in the frame of Fig. 7.118. Again the Contact Wizard frame appears, and this time the Next button should be pressed to obtain the frame shown in Fig. 7.119.

Press the [A] Pick Contact button to create the frame in Fig. 7.120.

Select curved surface of the cylinder and press the [A] OK button. Contact Wizard frame appears again and Next button should be pressed to obtain frame shown in Fig. 7.121.

In the [A] Optional Settings frame, select set Coefficient of Friction = 0.1, check out box—Include initial penetration. Next, press the [A] Optional Settings button to call up another frame. In the new frame, Normal penalty stiffness = 0.1 should be selected. Also, the Friction tab located in the top of the frame menu should be activated and Stiffness matrix = Unsymmetric selected. The Initial Adjustment tab, also located at the top of the menu, should be pressed and in the box [A] Automatic Contact Adjustment, Close gap should be selected, as shown in Fig. 7.122.

This will prevent solution crushing due to the gap between target and contact surfaces being greater than allowed by the programme.

Pressing the [B] OK button brings back the Contact Wizard frame (see Fig. 7.121), and the [B] Create button should then be pressed. The created contact pair is shown in Fig. 7.123.

Finally, the Contact Wizard frame should be closed by pressing the Finish button. Also, the Contact Manager summary information frame should be closed.

7.2.3.6 Solution

Before the solution can be attempted, solution criteria have to be specified. As a first step in that process, symmetry constraints are applied on the half symmetry model.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → Symmetry BC → On Areas. A frame shown in Fig. 7.124 appears.

Four surfaces at the back of the quarter symmetry model should be selected and the [A] OK button clicked. Symmetry constraints applied to the model are shown in Fig. 7.125.

The next step is to apply constraints on the bottom surface of the block. From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On Areas. The frame shown in Fig. 7.126 appears.

The bottom surface of the rail should be selected. After selecting the required surface and pressing the [A] OK button, another frame appears in which the following should be selected: DOFs to be constrained = All DOF and Displacement value = 0. Selections are implemented by pressing the OK button in the frame.

The final action is to apply external loads. In the case considered here, a pressure acting on the top surface of the cylinder will be used.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Pressure → On Areas. A frame shown in Fig. 7.127 appears.

The top surface of the cylinder should be selected and the [A] OK button pressed to pull down another frame, shown in Fig. 7.128.

It can be seen from Fig. 7.128 that the [A] constant pressure of 0.5 MPa was applied to the selected surface. Fig. 7.129 shows the model ready for solution with constraints and applied load.

Now the modelling stage is completed and the solution can be attempted. From the ANSYS Main Menu, select Solution → Solve → Current LS. A frame showing a review of information pertaining to the planned solution action appears. After checking that everything is correct, select File: Close to close that frame. Pressing the OK button starts the solution. When the solution is completed, press the Close button.

In order to return to the previous image of the model, select Utility Menu → Plot → Replot.

7.2.3.7 Postprocessing

In order to display solution results in a variety of forms, the postprocessing facility is used. In the example solved here, there is no need to expand the quarter symmetry model into the half symmetry or full model because the contact stresses are best observed from a quarter symmetry model. Furthermore, the isometric viewing direction used so far should be changed in the following way. From the Utility Menu, select PlotCtrls → View Settings → Viewing Direction. In the resulting frame, shown in Fig. 7.130, set View direction: [A] XV = − 1, [B] YV = 1, [C] ZV = − 1 and click the [D] OK button.

The quarter symmetry model in the selected viewing direction is shown in Fig. 7.131.

From the ANSYS Main Menu, select General Postproc → Read results → By Load Step. The frame shown in Fig. 7.132 is produced. The selection [A] Load step number = 1, shown in Fig. 7.132, is implemented by clicking the [B] OK button.

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. In the resulting frame, the following selections are made: [A] Item to be contoured = Stress; [B] Item to be contoured = von Mises stress (see Fig. 7.133). Pressing the [C] OK button implements the selections made.

A contour plot of von Mises stress (nodal solution) is shown in Fig. 7.134.

Fig. 7.134 shows a von Mises stress contour for both the rail and cylinder. If one is interested in observing contact pressure on the cylinder surface alone, then a different presentation of solution results is required.

From the Utility Menu, choose Select: Entities. The frame shown in Fig. 7.135 appears.

In the frame shown in Fig. 7.135, the following selections are made: [A] Elements (first pull-down menu); [B] By Elem Name (second pull-down menu); [C] Element Name = 174. The element with the number 174 was introduced automatically during the process of creation of contact pairs described earlier. It is listed in the Preprocessor → Element Type → Add/Edit/Delete option. Pressing the [A] OK button in the frame shown in Fig. 7.135 implements the selections made.

From the Utility Menu, select Plot → Elements. An image of the cylinder with a mesh of elements is produced (see Fig. 7.136).

From the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The frame shown in Fig. 7.137 appears.

In the frame shown in Fig. 7.137, the following selections are made: [A] Contact and [B] Contact pressure. These are items to be contoured. Pressing the [C] OK button implements the selections made. In response to that, an image of the cylinder surface with pressure contours is produced, as shown in Fig. 7.138.

The configuration of the contact between an O-ring made of rubber (hyperelastic material) and the groove is shown in Fig. 7.139.

An O-ring of solid circular cross-section is forced to conform to the shape of a rectangular groove by a moving wall as schematically shown in Fig. 7.139.

Following the initial squeeze of the O-ring (through movement of the wall), pressure is applied to the surface of the O-ring. Because of the sealing provided by the intrusion of the side walls, the pressure is effective over less than 180 degrees of the O-ring top surface. It is necessary to observe the conformity of the O-ring with the groove walls and stresses created by the pressure acting over its top surface.

The contact is characterised by the following data:

• Young's modulus of the wall and groove material = 2.1 × 10⁹ Pa;
• surface pressure applied to the O-ring = 0.1 × 10³ Pa;
• material of the O-ring is modelled as hyperelastic material of Mooney-Rivlin (2 parameters) type with constants: C10 = 80, C01 = 20;
• coefficient of friction between O-ring and wall = 0.1;
• wall movement = 0.2 mm;
• radius of the O-ring = 2.5 mm;
• depth of the groove = 4.5 mm;
• width of the groove = 5.5 mm; and
• length of the wall = 10 mm.

7.2.4.2 Model construction

The O-ring is constructed using a hyperelastic element (Mooney-Rivlin), and the groove and movable wall, both considered to be rigid, are constructed using link elements. The contact elements are constructed using ANSYS facility—Contact Manager. The loads are applied by wall motion and groove cavity pressurisation. The pressure sealing on the O-ring is assumed to take place at 15 degrees off horizontal. The model is constructed using GUI facilities only.

From the ANSYS Main Menu, select Preferences and check the Structural option. Next, the elements to be used in the analysis are selected.

From the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 7.140 appears.

Pressing the [A] Add button calls up another frame as shown in Fig. 7.141.

Select the [A] Solid and [B] Quad 4 node 182 element and click the [C] OK button. This creates a frame shown in Fig. 7.142, where Type 1 PLANE182 is shown.

Click the [A] Add button as shown in Fig. 7.142, and select the element illustrated in Fig. 7.142.

Selections of [A] Link and [B] 3D finit stn 180 were made as shown in Fig. 7.143. The selection of elements is shown in Fig. 7.144.

In this figure, highlight [A] LINK180 and click [B] Options. The frame shown in Fig. 7.145 is called up; [A] Rigid (classic) should be selected from the pull-down menu and the [B] OK button clicked to implement that choice.

7.2.4.3 Selection of materials

The next step is to establish a database for materials used.

From the ANSYS Main Menu, select Preprocessor → Material Props → Material Models → Structural → Nonlinear → Elastic → Hyperelastic → Mooney-Rivlin (2 parameters).

As a result of the selection, a frame shown in Fig. 7.146 appears.

Double-click on selection [A] to call up the frame shown in Fig. 7.147. Enter for C10 = 80, C01 = 20 and click [A] to implement the selections.

Now, having selected material for the O-ring, the next task is to define material for the wall and the groove. Thus, select Material from the menu at the top of the frame shown in Fig. 7.146 and click the New Model option. In response a frame shown in Fig. 7.148 appears.

By clicking the [A] OK button, a new material model number 2 is created, as shown in Fig. 7.149.

Selections made are shown in Fig. 7.149. By double-clicking on [A] Isotropic, a frame shown in Fig. 7.150 appears.

The following selections are made: [A] EX = 2.1 × 10⁹ Pa, and [B] Poisson's coefficient PRXY = 0.33. By clicking the [C] OK button, the selections are implemented.

Having selected materials for the contact assembly, the frame should be closed by selecting Material and Exit.

The next step in the process of solving the problem is to characterise the link element which is used to mesh the wall and the groove.

From the ANSYS Main Menu, select Preprocessor → Sections → Link → Add. The frame shown in Fig. 7.151 appears.

Input [A] ID = 2 and [B] OK to implement the selection. Afterwards, the frame shown in Fig. 7.152 is called up.

The inputs are shown in the figure: [A] Section Name = Link, [B] Link area = 1 and [C] OK to implement selections.

7.2.4.4 Geometry of the O-ring and meshing

The next phase in the model creation process is to draw the components involved.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Circle → By Dimensions. As a result of the selection, a frame shown in Fig. 7.153 appears.

By entering RAD1 = 2.5, RAD2 = 0, THETA1 = 0, THETA2 = 360, and clicking the [A] OK button, a solid circular area is created.

Next, the circular area, representing the O-ring, is meshed. From the ANSYS Main Menu, select Preprocessor → Meshing → MeshTool. Fig. 7.154 shows the resulting frame.

In the frame of Fig. 7.154, select [A] Lines—Set and [B] Close. A new frame is produced (see Fig. 7.155).

Pick all four arcuate segments on the circumference of the circular area and click the [A] OK button. The new frame shown in Fig. 7.156 appears.

In the frame of Fig. 7.156, enter number of element divisions, [A] NDIV = 10 and uncheck box [B] NDIV can be changed. Clicking the [C] OK button implements the selections made.

In the frame shown in Fig. 7.154 (Mesh Tool), activate [C] Free button and click the [D] Mesh button. In the appearing frame (Fig. 7.157), click [A] Pick All to have the circular area meshed.

Fig. 7.158 shows the circular area after the meshing process.

7.2.4.5 Creating wall and groove

Next, the wall and the groove are modelled as link components with an area equal to 1.

From the ANSYS Main Menu, select Preprocessing → Modelling → Create → Keypoints → In Active CS. The frame shown in Fig. 7.159 appears.

The input into the frame of Fig. 7.159 is as follows: keypoint number = 401 (it is an arbitrary selection, but it has to be greater than any number allocated to existing keypoints), X = − 2; Y = − 2.5. In a similar way, the other keypoints required for the groove and the wall as link components are created. The input coordinates are as follows:

• Keypoint number = 402, X = 2.5, Y = − 2.5; keypoint number = 403, X = 2.5, Y = 3; keypoint number = 404, X = − 2, Y = 3; keypoint number 405, X = − 2.5, Y = 5; keypoint number = 406, X = − 2.5, Y = − 5.

The next lines will be created using defined keypoints. From the ANSYS Main Menu, select Modelling: Create → Lines → Straight Line. The frame shown in Fig. 7.160 appears.

Click in sequence on the keypoints defining the groove: 401, 402, 403, and 404 and then [A] OK as shown in Fig. 7.160. Afterwards, click in sequence on the keypoints defining the wall: 405 and 406 and then [A] OK as shown in Fig. 7.160. The resulting outline of the wall and the groove looks like that shown in Fig. 7.161.

The next step in the process of modelling is to mesh created lines using the LINK180 element selected earlier. From the ANSYS Main Menu, select Meshing → Size Cntrls → ManualSize → Lines → Picked Lines. In response, a frame shown in Fig. 7.162 is called up.

Pick all four lines defining the groove and the wall and click [A] OK. In response, a frame shown in Fig. 7.163 is created.

In the frame of Fig. 7.163, enter number of element divisions, [A] NDIV = 10 and uncheck box [B] NDIV can be changed. Clicking the [C] OK button implements the selections made.

From the ANSYS Main Menu, select Modelling → Create → Elements → Elem Attributes. In response, the frame shown in Fig. 7.164 is created. Make entries as shown in Fig. 7.164, as they define element type and material to be used when meshing the groove and the wall.

From the ANSYS Main Menu, select Meshing → Mesh → Lines. This selection creates the frame shown in Fig. 7.165. Pick all four lines belonging to the groove-wall assembly and click [A] OK.

The O-ring assembly when fully meshed looks like that shown in Fig. 7.166.

7.2.4.6 Creation of a contact pair

In solving contact problems, a contact pair has to be created. Contact Wizard is a useful facility provided by ANSYS.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Contact Pair. As a result, a frame shown in Fig. 7.167 appears.

Clicking on the [A] Contact Wizard button located in the upper left-hand corner of the frame calls up a new frame as shown in Fig. 7.168.

In the frame shown in Fig. 7.168, select [A] Lines, [B] Flexible, and press the [C] Pick Target button. As a result of this selection, the frame shown in Fig. 7.169 is produced.

Target lines are: vertical line of the wall, lower horizontal line of the groove, and vertical line of the groove. After highlighting those lines, the [A] OK button should be pressed, as instructed by Fig. 7.169. Next, in the Contact Wizard frame (see Fig. 7.168), press the [D] Next button (this should be highlighted when the target lines are picked) to obtain another frame as shown in Fig. 7.170.

The following selection should be made (as indicated in Fig. 7.170): [A] Body (area), [B] Node-to-Surface, [C] Pick Contact. In response, the frame shown in Fig. 7.171 is produced, prompting you to select a contact.

The surface of the O-ring (circle) should be selected and [A] OK pressed. The Contact Wizard frame appears (see Fig. 7.170). Pressing the [D] Next button (this should be highlighted) results in a frame in which the following entries should be made. Material ID = 1, Coefficient of friction = 0.1. Also, Include Initial penetration option ought to be unchecked. Next, the Optional settings button should be pressed to refine contact parameters further. In the new frame, the following entries are required: Normal penalty stiffness = 0.1 and Behaviour of contact surface = No separation. Furthermore, the Friction tab located in the top of the frame menu should be activated and Stiffness matrix = Unsymmetric ought to be selected. Finally, the Initial Adjustment tab should be activated and Automatic contact adjustment = Close gap selected. The process of creating a contact pair ends by pressing the OK button to implement settings and in the Contact Manager frame pressing the Create button to generate a contact, as shown in Fig. 7.172.

At this stage, the Contact Wizard should be closed by pressing Finish as well as Contact Manager.

7.2.4.7 Solution—First stage of loading

In the solution stage, solution criteria have to be specified first. Thus, the first step constraints have to be applied to the groove and the wall has to be moved by 0.2 mm in the X-direction in order to apply a load on the O-ring.

From the ANSYS Main Menu, select Solution → Define Loads → Apply → Structural → Displacement → On lines. This selection generates the frame shown in Fig. 7.173.

All lines defining the groove should be highlighted and the [A] OK button pressed. In response, a frame shown in Fig. 7.174 appears where [A] All DOF, [B] Value = 0, and [C] OK should be selected.

Next, the wall should be moved by 0.2 mm. Recall the frame shown in Fig. 7.173 and select the vertical line defining the wall. Clicking [A] OK produces a frame as shown in Fig. 7.175.

Selections made are shown in Fig. 7.175: [A] UX, [B] Value = 0.2, [C] OK.

Before a solution is attempted, solution controls have to be selected. From the ANSYS Main Menu, select Solution → Analysis Type → Sol’n Controls. This selection produces the frame shown in Fig. 7.176. Selections made are shown in this figure: [A] Large Displacement Static, [B] Time at end of loadstep = 1, [C] Write every substep. Also ensure that Number of substeps = 25, Max no. of substeps = 2000, Min no. of substeps = 5.

From the ANSYS Main Menu, select Solution → Solve → Current LS. A frame showing review of information relevant for the planned solution action appears. After checking that everything is correct, select File and Close. Pressing the OK button initiates the solution. When the solution is complete, press the Close button.

7.2.4.8 Postprocessing—First stage of loading

In order to observe deformations and stresses produced by the load applied to the O-ring through the movement of the wall in X-direction by 0.2 mm, postprocessing facilities of ANSYS should be used.

From the ANSYS Main Menu, select General Postproc: Read Results: By Load Step. Fig. 7.177 shows the resulting frame.

Entries to the frame are shown in Fig. 7.177. Pressing the [A] OK button implements the selections made.

Next, from the ANSYS Main Menu, select General Postproc → Plot Results → Contour Plot → Nodal Solu. The frame shown in Fig. 7.178 appears.

Selections made are as follows: [A] Stress, [B] von Mises stress, [C] Deformed shape only, and to implement selections, click [D] OK. This results in the image shown in Fig. 7.179.

In order to see deformed and undeformed shapes simultaneously, a choice shown in Fig. 7.180 should be made.

The image of a deformed O-ring and its undeformed edge is shown in Fig. 7.181.

7.2.4.9 Solution—Second stage of loading

The second load step involves applying, in addition to the load due to the wall movement, pressure acting over the top surface of the O-ring. Because the pressure effectively acts over the angle from 14 to 166 degrees, in order to apply it properly it is convenient to change the coordinate system from Cartesian to Polar.

From the ANSYS Utility Menu, select WorkPlane → WP Settings. The frame shown in Fig. 7.182 appears.

In the frame, select [A] Polar and [B] OK to implement the choices. Next, from the ANSYS Utility Menu, select WorkPlane → Change Active CS to → Working Plane. This selection ensures that the active coordinate system is identical with that of the WP coordinate system, which is the Polar system.

From the ANSYS Utility Menu, select Select → Entities. This selection produces a frame shown in Fig. 7.183.

First, the elements belonging only to the O-ring should be selected. This is done by making the following selections shown in Fig. 7.183: [A] Elements, [B] By Elem Name, [C] 182 (element Plane 182 was used to mesh O-ring), [D] From Full, and [E] OK. Next, the nodes attached to the selected elements have to be chosen. Thus from the ANSYS Utility Menu, choose Select: Entities. The frame shown in Fig. 7.184 appears.

Fig. 7.184 shows that the following selections were made: [A] Nodes, [B] Attached to, [C] Elements, [D] From Full, and [E] OK to implement choices.

Again from the ANSYS Utility Menu, choose Select → Entities; this produces the frame shown in Fig. 7.185.

As shown in Fig. 7.185, the following entries were made: [A] Nodes, [B] Exterior, [C] From Full, and [D] OK to implement selections.

Finally, from the ANSYS Utility Menu, choose Select → Entities. Fig. 7.186 shows the resulting frame.

In order to select nodes belonging to the O-ring on which pressure is applied (second stage loading), the selections shown in Fig. 7.186 were made: [A] Nodes, [B] By Location, [C] Y coordinates, [D] 14, 166 (over this angle pressure acts on O-ring), [E] Reselect, and [F] OK to implement all choices made.

Next, all associated elements with nodes selected above should be picked up. Therefore, from the ANSYS Utility Menu, choose Select: Entities. The frame shown in Fig. 7.187 appears.

Selections made are as follows (see Fig. 7.187): [A] Elements, [B] Attached to, [C] Nodes, [D] From Full, and [E] OK to implement the selections.

Now is the right moment to deselect all contact elements, Type 4 Conta175 (this information can be found in the element type frame), from being involved in the load transmission. Thus, from the ANSYS Utility Menu, choose Select → Entities. The frame shown in Fig. 7.188 is produced.

All selections made are shown in Fig. 7.188: [A] Elements, [B] By Elem Name, [C] 175 (this is name of contact element), [D] Unselect, and [E] OK to implement choices.

In order to apply pressure to selected external nodes belonging to the O-ring, the following steps should be taken.

From the ANSYS Main Menu, select Preprocessor → Solution → Define Loads → Apply → Structural → Pressure → On Nodes. The frame shown in Fig. 7.189 appears.

Pressing the [A] Pick All button creates another frame, shown in Fig. 7.190.

The load value [A] VALUE = 0.1 × 10³ Pa is entered in the frame shown in Fig. 7.190. Pressing [B] OK implements the entry. Finally, from the ANSYS Utility Menu, choose Select: Everything.

This action recalls all elements and nodes belonging to the O-ring assembly. Usually, before the solution is attempted, solution options should be selected. However, in this case they are the same for those selected for the first stage of loading.

Now the solution of the problem ought to be attempted by selecting from the ANSYS Main Menu: Solution → Solve → Current LS. A frame showing a review of information relevant for the planned solution action appears. After checking that everything is correct, select File and Close. Pressing the OK button initiates the solution. When the solution is completed, press the Close button.

7.2.4.10 Postprocessing—Second stage of loading

In order to see stresses and deformations of the O-ring, follow the steps outlined in Section 7.2.4.8. Fig. 7.191 shows the von Mises stress due to squeeze and external pressure acting on the O-ring (deformed shape only), while Fig. 7.192 shows the von Mises stress and external pressure acting on the O-ring, but this time the undeformed edge of the assembly is visible.

Two beams, as shown in Fig. 7.193, are having the following dimensions: length = 100 mm, cross-section = 10 mm × 10 mm. They are made of a material with a Young's modulus E = 200,000 Pa, Poisson's ratio = 0.3, and are rigidly constrained at the ends (see Fig. 7.193). A load of 10 kN is applied halfway through the length of the upper beam, resulting in that beam bending and subsequently making contact with the lower beam. There are two objectives of the analysis. The first is to learn how to utilise contact elements in order to simulate how the two beams react when they come into contact with each other. The second objective is to find out stresses and displacements associated with the contact and at the location of the contact.

7.2.5.2 Construction of the model

The model of the two beams to make a contact under a load is constructed using a GUI, which is the main approach. However, this is not the only approach used, and for the purposes of illustration, the command approach will be given as well. The model in this instance consists of two identical rectangles, which can be created as follows.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Areas → Rectangle → By 2 Corners. In response, a frame shown in Fig. 7.194 appears.

Input WPX = 0; WPY = 15; Width = 100; Height = 10, and press the OK button to create the first beam.

In order to create the second beam, the above procedure is repeated but the input data into the frame shown in Fig. 7.194 are: WPX = 50; WPY = 0; Width = 100; Height = 10. Again, the OK button should be pressed. The following geometry is created as a result (see Fig. 7.195).

7.2.5.3 Material properties and element type selection

The next step is to define the type of the analysis and the type of elements to be used.

From the ANSYS Main Menu, select Preferences, and in the appearing frame, tick Structural and then press the OK button.

Then, from the ANSYS Main Menu, select Preprocessor → Element Type → Add/Edit/Delete. The frame shown in Fig. 7.196 appears.

Click [A] Add in order to access another frame as shown in Fig. 7.197.

In the left column, select [A] Solid and in the right column choose the [B] Quad 4node 182 element. After that, click the [C] OK button.

While the Element Type window (see Fig. 7.196) is still open, click Options, and in the new appearing frame change [A] Element Behaviour K3 to Plane Strs w/thk and click [B] OK, as shown in Fig. 7.198.

This allows a thickness of the beams to be input for the elements.

For the thickness of the beam to be used in the analysis, real constants must be defined. From the ANSYS Main Menu, select Preprocessor → Real Constants → Add/Edit/Delete. The frame shown in Fig. 7.199 appears. In this frame, press the [A] Add button to pull down another frame as shown in Fig. 7.200.

Click the [A] OK button to generate a third frame shown in Fig. 7.201. In this frame, input [A] thickness THK = 10 mm as shown. After that, click the [B] OK button and close the other frames.

Now, the materials for the two beams ought to be defined. From the ANSYS Main Menu, select Preprocessor → Materials Props → Material Models. Next, click Structural → Linear → Elastic → Isotropic and in the generated frame, input [A] EX = 200,000 (for Young's modulus) and [B] PRXY = 0.3 (for Poisson's ratio). After that, click the [C] OK button. Fig. 7.202 shows the inputs.

It is important to close the window showing the selection of a material.

7.2.5.4 Meshing

From the ANSYS Main Menu, select Preprocessor → Meshing → Size Control → Manual Size → Areas → All Areas. The frame shown in Fig. 7.203 is generated. For this example, element edge length is [A] 2 mm, as shown in Fig. 7.203.

The next step is to mesh both beams. Therefore, from the ANSYS Main Menu, select Preprocessor → Meshing → Mesh → Areas → Free → Pick All. This is illustrated in Fig. 7.204.

Select [A] Pick All and press the [B] OK button to mesh the selected areas. The mesh resulting from this action in shown in Fig. 7.205.

7.2.5.5 Creation of a contact pair

It is very convenient, when solving contact problems, to use the Contact Wizard tool, available in ANSYS.

From the ANSYS Main Menu, select Preprocessor → Modelling → Create → Contact Pair. This action results in a frame shown in Fig. 7.206.

The location of the Contact Wizard button is in the upper left-hand corner of the frame. By clicking on button [A], a new frame, shown in Fig. 7.207, is generated.

In this frame, select [A] Lines (upper line of the lower beam) and [B] Flexible, and press the [C] Pick Target button. As a result of this selection, the frame shown in Fig. 7.208 is produced.

The target area is the surface of the lower beam and should be picked and the OK button pressed. In the Contact Wizard (see Fig. 7.207), press the Next button (which should be highlighted once the target area is selected) to obtain the frame shown in Fig. 7.209. In this frame, the following selections should be made: [A] contact surface—Nodes and contact element type [B]—Node-to-Surface, as shown in Fig. 7.209.

Pressing the [C] Pick Contact button results in the frame shown in Fig. 7.210.

Responding to the prompt of this frame, select the node located at the lower right-hand corner of the upper beam and press the [A] OK button. When this is done, the Contact Wizard frame appears (see Fig. 7.209), and the Next button should be pressed in order to generate the frame in Fig. 7.211.

The entries into this frame are: [A] material ID = 1, [B] coefficient of friction = 0 (frictionless contact is assumed). The Include initial penetration option should be checked. Pressing the [C] Optional settings button enables the making of further adjustments to the model. Especially important is changing the Stiffness matrix to Un-symmetric, and that option can be accessed by pressing first the Optional settings button (see Fig. 7.211) and in the new frame the Friction tab located in the top of that frame menu. When all the above is done, pressing the [D] Create button (see frame in Fig. 7.211) produces an image of the contact pair, as shown in Fig. 7.212.

When a contact pair image is created, it signifies the end of the contact pair creation process and the Contact Manager frame should be closed.

However, the contact elements created by the Contact Manager have to have real constants defined. This is done by selecting Preprocessor → Real Constants → Add/Edit/Delete. As a result, the frame shown in Fig. 7.213 appears.

Select [A] Set 3 (containing contact elements) and press the [B] Add button. In response, the frame shown in Fig. 7.214 is generated.

Select [A] Type 3 CONTACT175 and click [B] OK. In response, a frame shown in Fig. 7.215 is produced.

There are two important entries which have to be made. The first is to set normal penalty stiffness, [A] = FKN = 200,000 and target edge extension factor, and [B] = TOLS = 10 (this can be found by scrolling down the table shown in Fig. 7.215).

7.2.5.6 Solution

First, an analysis type should be defined. From the ANSYS Main Menu, select Preprocessor → Solution → Analysis Type → New Analysis → Static.

Next, select Preprocessor → Solution → Analysis Type → Solution Control. The image shown in Fig. 7.216 will appear.

Ensure the following selections are made under the [A] Basic tab as shown in Fig. 7.216.

Especially important is to set [B] Automatic time stepping = On. This allows ANSYS to determine appropriate sizes to break the load steps into. Decreasing the step size usually ensures better accuracy, although it increases computing time.

Additionally, activate the [C] Nonlinear tab located at the top of the frame shown in Fig. 7.216. A new frame of Solution Controls will appear (see Fig. 7.217).

Ensure that [A] Maximum number of iterations = 100 and [B] Line search is On, as shown in Fig. 7.217.

Next, from the ANSYS Main Menu, select Preprocessor → Solution → Define Loads → Apply → Structural → Displacement → On Lines.

Fix the left end of the upper beam and right end of the lower beam, choosing all DOF option. This means that the ends of both beams are constrained in all directions.

Furthermore, on selecting Preprocessor → Solution → Define Loads → Apply → Structural → Force/Moment → On Nodes, the frame shown in Fig. 7.218 appears.

Pick the node located on the upper line of the upper beam and halfway through its length. To do this, plot the images of the beam as nodes by selecting from the utility menu of ANSYS: Plot → Nodes. When the selection is done, pressing the [A] OK button in frame of Fig. 7.218 generates the frame shown in Fig. 7.219.

Apply [A] VALUE Force/moment = −10,000 N in [B] the FY direction to the centre of the top surface of the upper beam. Note that this is a point load on a 2D surface. The minus sign signifies the fact that the load is acting downwards.

Finally, select Preprocessor → Solution → Solve → Current LS. On pressing the Solve button, it takes some time to obtain the solution. When it is successful, the image shown in Fig. 7.220 appears, illustrating steps in consecutive iterations and convergence.

7.2.5.7 Postprocessing

In order to view the results and to present them in different formats, the ANSYS postprocessing stage is used.

From the ANSYS Main Menu, select General PostProc. Next, from the utility menu, select PlotCtrls → Style → Displacement Scaling. The frame shown in Fig. 7.221 will appear.

Click the [A]—1.0 (true scale) button (as shown in Fig. 7.221). This selection is very important.

In order to see the stress distribution in the beams, the following selections should be made:

From the Utility Menu, select PlotCtrls → Style → Contours → Non-Uniform Contours. This generates the frame shown in Fig. 7.222. Ensure that entries are as shown in that figure.

Next, select General Postproc → Plot Results → Contour Plot → Nodal Solution → Stress → von Mises. As a result, a frame showing stress distribution within both beams will be shown (see Fig. 7.223).

As can be seen in Fig. 7.223, the load on the upper beam caused it to deflect and come into contact with the lower beam, producing a state of stress in both of them.