Structural Analysis on Rail wheel and Track Setup

Structural Analysis on Railwheel and Track Setup

Case 0 (Base Setup)

A static non-linear structural analysis is performed on a Railwheel and Track setup. The geometry is imported into Ansys Space Claim. No alterations are made to the geometry for the analysis.

Material Definition: The geometry is assigned Structural steel as the working material, which exhibits the following properties:

Sl. No	Particulars	Magnitude
1.	Density	7.85e-06 kg/mm3
2.	Young’s Modulus	2.00e+05MPa
3.	Bulk Modulus	1.6657e+05MPa
4.	Poisson’s Ratio	0.3
5.	Shear Modulus	76923MPa
6.	Yield Strength	250MPa
7.	Ultimate Strength	460MPa

Meshing: The geometry is meshed with an element size of 50mm. For the parts that are in contact and of interest for this simulation, a face size of 35mm is provided to obtain more accurate results in these regions.

The mesh sizes are selected keeping in mind, the node/element limit imposed by the student license. The smoothing Effect has been kept to low to capture the geometry better.

Contact Definition: Two contact regions are defined for this simulation-

A frictional contact between the railwheel and the track with a coefficient of friction value of 0.3.

A frictionless contact between the wheel shaft and the bearing (inner surface of the wheel).

The contact formulation and behaviour are left to \"Program Controlled\".

Joint Definition: For the simulation, three types of joints are defined-

A fixed joint for the track to constraint all its degrees of freedom.

A translational joint for the wheel shaft to constraint its motion along the X-direction only (in translation). The coordinate axes are adjusted accordingly.

A planar joint for the wheel surface that limits the wheel\'s degrees of freedom to Rotation along Z and Translation along X and Y axis.

Load Definition: The setup involves imposing a bearing load and a displacement. The shaft of the wheel is provided with a displacement of 500mm over 5 seconds with a 100mm displacement over each second.

A constant bearing load of 1e+005N is imposed on the inner surface of the wheel in the negative Y direction.

Analysis Settings: The simulation is run in 5 steps of 1 second each. For the first step, Auto Time Stepping is set to \"Program Controlled\". For all the subsequent steps, a minimum time step of 1e-003 second and a maximum time step of 0.1 second is imposed.

For all the steps, Large Deflection is kept on and the Solver Type is set to Direct.

Additional non-linear and output control settings for the analysis.

The simulation is run and the results are plotted.

Case 1

In this case, the bearing load applied on the inner surface of the wheel is increased by a factor of 5. Hence the total bearing load imposed is 5e+005N in the negative Y-direction.

The rest of the setup is exactly the same as in Case 0 or the base setup. The simulation is run and the results are plotted.

Case 2

In this case, the bearing load is reversed to its original value of 1e+005N in the negative Y-direction and a user defined output is requested in the solution. A user defined Displacement or Deformation is requested using the expression \"USUM\".

The rest of the setup is exactly the same as in Case 0 or the base setup. The simulation is run and the results are plotted.

Results: The Total Deformation, Equivalent Stress and Equivalent Strain obtained from the simulation are tabulate below.

Particulars (max value)	Case0	Case1	Case2
Total Deformation (mm)	1000.6	1000.7	1000.6
Equivalent Stress (MPa)	100.93	395.7	100.93
Equivalent Strain	6.1232e-4	2.5699e-3	6.1232e-4
Max Fatigue Life (cycles)	1e+6	1e+6	1e+6
Min Fatigue Life (cycles)	4.0323e+5	2795.8	4.0323e+5

1. Total Deformation: The total deformation in all the cases is almost the same and of the magnitude of 1000.6mm.

The Deformation vs Time graph shows the maximum, minimum and average deformations as green, red and blue lines respectively.

2. Equivalent Stress: The maximum equivalent stress is developed on the track at the point of contact with the wheel.

Case0

Case1

Case2

The red, blue and green lines indicate the maximum, average and minimum equivalent stresses computed for the geometry respectively.

3. Equivalent Elastic Strain: The maximum equivalent ealstic strain is developed on the track at the point of contact with the wheel, due to the presence of maximum elastic stress in that region.

Case0

Case1

Case2

The red, blue and green lines indicate the maximum, average and minimum equivalent strains computed for the geometry respectively.

4. Fatigue Life Cycle: The maximum life cycle under fatigue remains the same in all cases (of the magnitude of 1e+6 cycles, though the minimum life reduces when the bearing load is increased 5 fold.

5. User Defined Result (Displacement): This is defined only in Case 2. The requested output through this feauture was Total Deformation or Displacement.

Conclusion:

All the simulations terminate successfully. A number of program defined and user defined results have been requested from the solution. Apart from the overall stresses and strains, the same on individual parts of the assembly have also been requested.

Since the simulation setup in terms of constraints and loading is the same in case 0 and case 1, the results obtained are also exactly the same.

The analysis shows that increasing the bearing load in Case 1 to 5 times the bearing load in Case0, results in a four fold increase in both the Equivalent stress and Equivalent Elastic strain.

Increase in Equivalent Stress = (Equivalent Stress in Case1/Equivalent Stress in Case0)

= (395.7MPa/100.93MPa)

= 3.92

Increase in Equivalent Elastic Strain =(Equivalent Strain in Case1/Equivalent Strain in Case0)

= (2.5699e-03/6.1232e-04)

= 4.19 ~ 4.2

The Total Deformation value obtained from the runs is the displacement of any point on the wheel on a 500mm transllation of the wheel in the X-direction. This value is 1000.6mm for Case 0 and Case2 and 1000.7mm for Case1. The increase in deformation in case 1 is negligible.

It can be observed that the Deformation or Displacement value requested through the User Defined Result Expression \"USUM\" is exactly the same as that obtained from the default inbuilt Ansys result of Total Deformation.