BIKE CRANK ANALYSIS.

1. Objective

i. Develop the solution to a 3D structural mechanics problem in ANSYS Mechanical and get the following output.
a. Deformed shape and displacement field
b. Stress distribution in the crank

ii. Verify the results and compare them with expected trends, etc.

iii. Do Sensitivity Analysis by refining the mesh.

2. Problem Specification

Consider a crank mounted on a bicycle. When a rider is pedaling the bicycle, he or she is applying a variable force to this bike crank. To simplify the analysis, we'll neglect the variation of the force with time and focus on the response of the crank to a static force.
We will work with the following crank model. The crank is made of Aluminum 6061-T6 alloy. For this material, Young's modulus is 1x10⁷ psi and the Poisson's Ratio is 0.33. 

The left three-hole surfaces are fixed and a load of 100 lbf is applied on the right hole surface in the upward direction. Note that this is an approximation of the actual loads and constraints on the bike crank. 

3. Pre-Analysis

3.1. Governing Equations: 

In these structural mechanics, to understand what is happening under the hood in these ANSYS, we need to know what the mathematical model is that ANSYS is solving. In particular, we need to know what are the governing equations that it's solving? What are the physical principles embedded in those governing equations? And what are the assumptions contained in the governing equations?
      The governing equations are based on 3D elasticity. So here we need to take a look at the overview of what the governing equations are and the principles on which these governing equations are based which is coded into ANSYS.

These are general equations used to solve the Solid Mechanics problem which can be adjustable according to the problem requirement. 

a. 3D Differential Equations of Equilibrium:

In the formula of 3D Differential Equations of Equilibrium, we have three equations and six unknowns.
Three Equations are force balance equations in x,y, and z-direction respectively. The Six unknowns are   `sigma_x, sigma_y, sigma_z, tau_(xy), tau_(xz),tau_(yz)`  as shown below.

Where:- 
`sigma`  shows the stress in the particular direction `x,y,z` .
`tau`  Shows the strain on a plane in a particular direction `x,y,z` .
`f_x,f_y,f_z = 0`  which is a body force.

b. 2D and 3D Hooke's Law:

i. 2D Hooke's Law:

ii. 2D Hooke's Law in Matrix Form:

iii. 3D Hooke's Law (constructive model):

we need to bring in additional equations to close the equation set. And so we bring in the material properties through the constitutive model so that relates the stresses to the strains through the 3D version of Hooke's Law as follows.

c. Strain Displacement Relation:

.

We need to determine 15 unknown functions:

6 stress components: σx,σy,σz,τxy,τxz,τyzμ${\displaystyle \mu }$

6 strain components: ϵx,ϵy,ϵz,γxy,γxz,γyzσx${\displaystyle {\sigma }_x}$

3 displacement components: u,v,w

We have as many equations as unknown functions, so the problem is fully determined.

Note: The Major Difference between the Displacement and Stress is the displacements are defined at a point but stresses defined for an infinitesimal Element located at the point.

3.2. Boundary Conditions:

Essential boundary conditions are applied at the three holes on the crank where displacements are set to zero as shown in the figure below.

Natural boundary conditions are applied at all other boundary surfaces. The traction is non-zero for the surface at which the force is applied (see figure below). It is zero for the remaining surfaces.  

At Every point on the boundary the displacement (or) Traction has to be defined. Each point of boundary we have three components of the displacement. i.e we need to know normal and tangential direction components. we apply the boundary conditions as shown above but all the other part of body where we not defined anything is by default taken as a Zero Traction by Ansys. i.e traction in all the direction is zero.

Note: Traction is Natural Boundary Condition which satisfies partially.

3.3. Numerical Solution Strategy: 

We have a Mathematical model So, ansys is going to solve it as a Finite Element Method. It Discretized the domain and reduced the problem to determine the displacement values only at nodes. each node going to calculate the three components of displacement i.e. (u,v,w).

Note: In this project, the Ansys includes mid-side node also to get higher-order polynomial interpolation to relate displacement at any point within an element to its nodal displacement.

3.4. Hand Calculation and Expectation: 

Based on the Euler-Bernoulli beam theory we are going to find the stress at point A and Point B.

bending stress in the x-direction is given as 

`sigma_x = (M*Y)/I`

Where:
M = Moment
Y = distance from Neutral axis
I = Moment of inertia

we get `sigma_(x _ A)= 14,300`  psi

`sigma_(x _ B)= - 14,300`

We expect σx, the normal stress in the x-direction, at A to be tensile and at B it is compressive.

4. Procedure

4.1. Geometry Prepration:

i. Open Ansys Workbench and Select the Analysis type as a Static Structural.

ii. Import the geometry.

iii. Optimize the geometry by supressing the component using space claim or Design Moldeler.

Note: The geometry defines the domain over which the 3D equilibrium equations need to be solved.

4.2. Meshing:

i. Set the "Body Sizing" as 0.2 inches for the whole crank.

ii. Refine the mesh around the fixed holes to 0.1 inches using face meshing option.

iii. Use the Multi-Zone method to get hexahedral elements. multizone chops the part into smaller volumes to get the better accuracy with less nodes.

Now we have 6681 nodes and 1190 Elements. So as we know Ansys will find the three displacement values at each node. therefore total displacement values is 6681*3 = 20043. 

Out of all the Nodes we don't have to solve all the Nodes Because some displacement values known to us from Essential Boundary Condition.

4.2.1 Review Mesh Quality:

Reviewing meshes Quality skewness and we can see the very few elements is skewed

This low-quality mesh affects our result. So we need to fix it by refining the mesh. But we have a larger number of high-quality mesh so this is acceptable for us problem. quality plays a major role in the complex assembly. So we can move further.

4.3. Model setup:

1. Assign Material Property:

From the pre-analysis we  know the 3D version of hook's law. from the equation, we need to define the value of young's modulus and poission's ratio. The essential boundary conditions set the displacement values directly and are unaffected by material properties.
Note that the natural boundary conditions set the traction which will filter down to affect the displacement gradients. Thus, if we keep the non-zero traction at a boundary the same and change the material properties, we will in effect be changing the boundary conditions on the displacement gradients.
Hence applying the material in Engineering data as an Aluminium 6061 T6 having `E` = 1e7 and `mu` = 0.33

ii. applying for fixed support at one end and Upward force 1000 lbf in y-direction at other ends as shown in the figure.

5. Numerical Solution

Now we have 6681 nodes therefore as we know the number of displacements is thre times of the nodes. Let's say 500 of these nodes are on the three fixed holes. So, now we need to know How many algebraic equations would ANSYS need to solve SIMULTANEOUSLY to determine all the nodal displacements which is as follows.

(6681−500) *3 = 18543

Hence Ansys need 18543 algebraic equations need to solve SIMULTANEOUSLY to determine all the nodal displacements. Now, we want to get get the Deformation , Normal stress in x-direction results to observe.so defining it in the solution and results is discussed in next section.

6. Numerical Results

6.1 Total Deformation:

we can see that the deformation is low near where we fixed the model, and it's high where we applied the force. And the deformation is about 0.046 inches which is very small.

we can either read the maximum value directly from the legend or by highlighting "Total Deformation" and looking at the "Maximum" under "Details of Total Deformation" in the lower-left box.

6.2 Normal Stress in x-direction:

Let's next plot `sigma_x` distribution for the model. ANSYS takes the displacement field, differentiates it to get the strain field, and from that uses Hooke's Law to calculate the stress field.

From the contours, we can see that the bottom portion of the crank has positive stress (tensile) and the top portion, negative stress (compressive), as expected. But The maximum tensile value occurs at the sharp corner at C. 

Sharp corners can produce stress singularities i.e. stresses can increase in an unbounded fashion on continually refining the mesh in our linear model. Since sharp corners can yield high stresses, it is a good idea to smooth these corners using fillets.

Also from above result image of normal stress we can see that there's not much variation in the z-direction. So since this is almost in pure bending, the variation shows it's a plane stress situation. So a 3D analysis for this model is actually not requird we need to use 3D analysis for more complicated assembly.

6.3 Normal stress along path:

To get the Normal stress along path we need to Create Custom Coordinate Systems first and then define the path to get aacurate results.

a. Defining coordinate system:

we are going to define the two coordinate system from which which will define the path

coordinate system-1 

x = 3.3465 in
y = 0
z = 0.375 in

coordinate system-2

x = 3.3465 in
y = 0.45276 in
z = 0.375 in

b. Defining path:

by using the coordinate system we defined the path as shown below. here we want to know the stress variation in y-direction hence we are defining the path along it.

Y-start = 0.45276
Y- End = 0

Now we define the stress along that path and the following output is as follows.

Probing the value at the origin of the coordinate system created at A gives σx= +6530 psi (positive, so it's tensile). A good verification check would be to compare this value to the "hand calculation" value we'd get from Euler-Bernoulli beam theory.

7. Sensitivity Analysis

7.1. Mesh Refinement:

Refine the mesh by reducing the "Body Sizing" to 0.1 in and the "Face Sizing" to 0.075 in. Remember that the limit for the student version is 32,000. If we had reduced the "Face Sizing" to 0.05 in, we would get more nodes than allowed.

To calculate the percentage change, divide the absolute difference between the values by the value without mesh refinement. 

 A very important takeaway from this question is that stress is more sensitive than displacement to the mesh and has a larger relative error. 

References:
Course | ENGR2000X | edX

The Flow of report:-

1. Objective.
2. Problem Specification.
3. Pre-Analysis.
4. Procedure.
5. Numerical Solution.
6. Numerical Result.
7. Sensitivity Analysis.