Week 2 Railwheel and Track

OBJECTIVE

To perform a static structural analysis on a railwheel and track setup and to compare the outputs of two different bearing loads of 100 kN and 500 kN. The outputs to be requested are that of total deformation, equivalent stress and life under both loads. In addition to that, a user-defined result for the total deformation is to be requested and verified with the original deformation output for correctness.

MODEL IMAGE

PROCEDURE

1. After opening ANSYS Workbench, we are met with the Project Schematic window. Here, we can select the 'System Structural' analysis system on the left. Doing so creates a new project. Here, we can rename the project and also change the material if needed. We will need to right-click 'Geometry' and select 'import'. The STP file provided for this project should be selected.

Since the material is to be structural steel (which is the default), we needn't worry about applying any for this challenge. We can then right-click 'Model' and select 'edit'. This will bring the model up in the Mechanical interface.

2. First thing we need to do is set up the contact between the multiple components of this assembly - namely the wheel and the track & the wheel and the shaft. The given model already has rudimentary contacts defined between these parts' surfaces, we need to further define them.

For the contact between the wheel and the track, we shall be assigning a frictional type contact between the two with a frictional coefficient of 0.3 as shown:

For the wheel and shaft contact, it will merely be changed into a frictionless type contact. No other settings are to be changed:

3. The next step is to add joints. The following procedure will therefore be repeated for each joint. Right-clicking the Contact entity again, we can then go to Insert > Joint.

The first one is a fixed joint for the track.

For scope, both sides of the track are selected as shown.

The next joint is a translational joint that is to be applied on the shaft's curved surface:

Care must be taken to ensure the translational motion's direction is specified correctly as seen above. If not, simply clicking the required axis on the local coordinate system will correct it.

Finally, a planar joint is to be assigned on the following region of the wheel:

4. Moving on to the mesh, we can selectively refine the mesh in the regions where there are wheel and track contact using the 'sizing' option (right-click Mesh in outline > insert > sizing). The surfaces are selected as shown and a mesh size of 25mm is assigned:

After this, we can go back to 'mesh' in the outline and edit the entity in its window on the bottom left. Going to the 'Defaults' section, here we can change the mesh size to 35mm.

5. Next, we shall work on the analysis settings. The number of steps would be 5. Selecting the 1st step only from the bottom toolbar, we can edit this particular step's properties in the entity window on the bottom left. Auto time-stepping would be program-controlled and the solver type would be direct.

For time steps 2 to 5, the Auto Time Stepping option would be 'on', it would be defined by time, the carryover time step would be on, Min. time step = 0.001s and Max. time step = 0.1s and the Solver type would be 'Direct'. Large Deflection would be turned on.

For both time step settings, 'force convergence' would be turned on and all the settings for the output controls would be turned on as well.

6. Next, we need to right-click static structural > Insert > Joint Load. We are to add a joint load for the translational joint we created earlier on the shaft. The type would be displacement and we need to create a displacement-time table with increments of 100mm for each second as shown:

Then, we will need to create a bearing load on the surface where the shaft interacts with the wheel. We can create one by right-clicking static structural > create > bearing load. The specified region will be selected for the geometry option and this load will be defined by components. Checking the global coordinate system, we can see that the load would be in the negative y direction. Hence, the magnitude to be entered for y-coordinate would be negative, which in this case would be -100000 N (this value needs to be changed for the next case, where the bearing load would be five times, which is -500000 N, as shown in the screenshot).

7. Now we can generate the outputs. To do this, we can right-click Solution > Insert > Deformation > Total (for maximum deformation), right-click Solution > Insert > Stress > Equivalent (Von-Mises) (for stress) and, right-click Solution > Insert > Strain> Equivalent (Von Mises) (for strain) and right-click Solution > Insert > Fatigue > Fatigue Tool (and select 'stress life' for its Analysis Type).

We also need to create a user-defined output result for total deformation in the analysis. To do this, we simply need to right-click Solution > Insert > User Defined Result. In its entity box, we need to define it by giving it an expression. Checking the worksheet for Solution (worksheet option from top toolbar), we can see that deformation is denoted by UX, UY and UY (for deformation in all directions). The magnitude would therefore be:

Total Deformation, `U = sqrt(U_x^2 + U_y^2 + U_z^2)`

So, this would be the expression we need to input.

Now, all we need to do is right-click solution again and click 'Evaluate all results'. It must be reiterated that after reaching the solutions, we must go back to the bearing load entity and change the magnitude to cover both cases (so the file will be saved after each iteration) and we will need to run result evaluation again. So there would be two cases - one for 100000 N and one for 500000 N.

Finally, when the analysis is done, we can view the results by simply clicking each of these solution entities we created, in the Outline menu.

OUTPUTS

100000N BEARING LOAD

EQUIVALENT STRESS

Maximum & Minimum

TOTAL DEFORMATION

Maximum & Minimum

LIFE

USER-DEFINED RESULT - TOTAL DEFORMATION

Maximum & Minimum

500000N BEARING LOAD

EQUIVALENT STRESS

Maximum & Minimum

TOTAL DEFORMATION

Maximum & Minimum

LIFE

USER-DEFINED RESULT - TOTAL DEFORMATION

Maximum & Minimum

OBSERVATIONS

As we can see, there's an obvious increase in stresses generated with an increase in the bearing load. There is a direct relation between the two. The deformation although remains relatively the same (the difference between minimum deformation values is very minimal magnitude-wise).

Fatigue life is such a number of cycles of stress or strain of a specified character that a given specimen sustains before the occurrence of failure due to fatigue. Here, we can see that the case with lesser load has a larger fatigue life threshold of 95145 cycles minimum. Whereas, in case 2 where the load is 5 times the load of case 1, there is a drastic drop in fatigue life with a measly 1151.4 minimum cycles.

Coming to the user-defined result, we can see that the maximum and minimum values are 1001.5 mm and 5.684e-14 mm for 100kN and 1001.9 mm and 4.766e-14 mm for 500kN respectively. These are the exact same values as that of the total deformation outputs in the table above.

RESULTS

Static structural analysis was carried out on this railwheel and track system with the required outputs of Von-Mises stress, total deformation and fatigue life being generated. Analysis was carried out for loads 100 kN and 500 kN. In addition to that, an additional user-defined output was created to calculate the total deformation in the system. It was also proven to be the same as the values generated through the total deformation output.