[FEA NX] Fatigue Analysis of a Truss Joint

Contents:

Overview:

1. Fatigue Definition
   Fatigue is a phenomenon associated with variable loading, or more precisely, cyclic stressing or straining of a material. Fatigue failure is defined as the tendency of a material to fracture through progressive cracking under repeated alternating or cyclic stresses of an intensity considerably below the normal strength. Although the fracture is of a brittle type, it may take some time to propagate, depending on both the intensity and frequency of the stress cycles.

2. All structural and mechanical components that are subjected to cyclic loading can fail due to fatigue. Fundamental requirements during design and manufacturing to avoid fatigue failure are different for each case and should be considered during the design phase.

3. Fatigue Loading

   Fatigue loading is primarily the type of loading that causes cyclic variations in the stress or strain on a component. The cyclic loading can be uniform or non-uniform. For simple cases, constant amplitude loading is used to obtain material fatigue behavior/properties for fatigue design. Some real-life load histories can occasionally be modeled with constant amplitude as well.

   

4. Fatigue Life Estimation Method

   Fatigue analysis is usually carried out using the following methods of analysis:

   • S-N Method

   • E-N Method

   • Crack Growth

   FEA NX can consider the S-N and the E-N methods for fatigue analysis.

   The stress-life (or S-N method) is commonly referred to as the total life method since it makes no distinction between initiating or growing a crack. This was the first fatigue analysis method to be developed, and it provides satisfactory results for fatigue analysis. It assumes the structure to be fully elastic. The initiation or growing phase of a crack is not considered in this method. Applicable to high cycle fatigue problems (low load-long life). This approach should not be used to estimate fatigue lives below 10,000 cycles. we can use the Goodman, Gerber, Soderberg, Morrow, or SWT method of fatigue life prediction in the case of the S-N approach.

   The local-strain or strain-life (E-N) method, commonly referred to as the crack initiation method, was more recently developed and is intended to describe only the ‘initiation’ of a crack. This approach is best suited for low-cycle fatigue problems, where the applied stresses have a significant plastic component. We can use the Morrow, SWT, and Manson-Halford method of fatigue life prediction in the case of the E-N approach.

    

    

   [Note: Kindly find attached zip folder containing Parasolid model file & FEA NX file.]

    

Modelling

1. Open FEA NX software & click on new file. Input the name for project and click on OK.

   

   To do fatigue analysis we need a particular joint of the global model. so there are three ways possible for that. First, we can create a geometry by ourselves in FEA NX. Second, we can select that particular joint in Midas CIVIL NX and then import it to FEA NX by using tool called "Frame to Solid" import. Third, we can import the geometry in FEA NX as a Parasolid file. This Parasolid file contains the geometry as in surfaces of the structure.

    Here are steps how we can import the Parasolid file into FEA NX.

   

   Once the file is imported into FEA NX, the geometry of the joint model becomes available in the project environment. At this stage, the imported bodies and surfaces can be renamed as per convenience to improve model clarity and organization. Proper naming conventions help in identifying parts easily during meshing, boundary condition assignment, and result interpretation.

   

    

   After importing the surfaces, we must connect them so that they share a common node when meshed. To connect the surfaces, we are having a command called "imprint". 

   

   Here we can see the changes, before & after using imprint command.

   

   likewise, we need to use imprint command to connect all the surfaces.

   Create a "Steel" material Property.

   

   As imported geometry is a surface having shell property, we need to define the same in the FEA NX also. Input the thickness as 40mm.

   

   Now, select all the surfaces and create a mesh of size 150mm. 

   

Boundary Conditions:

We have imported a specific connection from the global model and re-modeled it using shell elements in FEA NX. In this local model, nodes are distributed across the surfaces of the geometry. To apply a prescribed displacement load, we create a master node at the geometric center of the region of interest. The surface nodes at the loading end are then connected to this master node via Rigid Links. This setup ensures that any displacement applied to the master node is uniformly transferred to all connected slave nodes. Once the rigid links are established, the specified displacement can be directly applied to the master node, and the load will propagate correctly across the shell elements.

To create a master node at the geometric center, here are the steps we can follow:

1. Create a line joining two extremes end.

2. Create a point over the line at the mid.

3. Create a node exactly over the node created at the center.

Let's create a line joining two extreme ends. Follow the same step for other ends also.

Create a point over the line at the mid. Follow the same step for other ends also.

Create a node exactly over the node created at the center. Follow the same step for other ends also.

Create a rigid link property.

Create the rigid link.

Similarly, create a rigid link at other locations as well.

Now, as the selected joint of the bridge is present at bearing location, we need to create a node at the bottom at bearing height location, let's say 50mm.

Once the bottom bearing node is created, connect the two nodes with elastic link with specified stiffness values.

Give the fixed support at the bottom bearing node. 

Loading

To perform fatigue analysis on this connection model under a specific load case, we begin by extracting the nodal displacements from the global model corresponding to that load case. These displacements represent the boundary behavior of the connection in the global context. We then apply these extracted displacements as enforced boundary conditions (i.e., prescribed displacements) in the local shell model developed in FEA NX. This ensures that the local model experiences the same deformation pattern as it would in the global structure. Below are the nodal displacement values for two load cases:

First let's apply the "Disp" at all the four nodes. Following image shows how we can apply for the displacement at node 1. Similarly, we need to apply at node 2, node 3 and node 4 also.

Following image shows the displacement applied at node 1 due to self-weight. We need to apply the displacement at node 2, node 3 and node 4 too.

Linear analysis:

For doing linear analysis, we need to generate analysis case for the same.

We can check the result for both the created load case:

Fatigue analysis:

In FEA NX we can specify the S-N and E-N methods by using the loading, stress, or strain results based on the linear static analysis carried on the structure. Users can specify the following methods:
1. SN using loading history
2. EN using loading history
3. SN using stress history
4. EN using stress history
5. EN using stress/strain history

Experimental test data is mostly uniaxial whereas FE results are usually multiaxial. At some point, stress must be converted from a multiaxial stress state to a uniaxial one. In FEA NX Equivalent (Von Mises), Signed Von Mises, Absolute Maximum Principal, and Maximum Shear options are available for this purpose.

Here, we are using the "SN using load history" method. we can define S-N curve as function or we can define the material property date like yield strength, tensile strength, endurance limit and cycles at endurance, based on which software will generate S-N curve automatically. 

To simulate the fatigue loading conditions in FEA NX, we first need to define appropriate fatigue load functions that represent how each load case varies over time.

In this analysis, we will generate two fatigue load functions corresponding to the two load cases:

1. "Sine" Load Function

   • Associated with the "Disp" (Displacement) load case

   • Represents a cyclic (sinusoidal) loading pattern to simulate fluctuating service loads

2. "Constant" Load Function

   • Associated with the "SW" (Self-Weight) load case

   • Represents a steady, non-varying load applied throughout the fatigue cycles

These functions will be used to scale the displacement boundary conditions over time and are essential inputs for the fatigue analysis setup.

Assign the load function to the corresponding load case and perform the analysis.

Fatigue Result:

Fatigue results are calculated as Damage and Fatigue Life Cycle as per mean stress correction method.

Fatigue lifecycle as per Goodman mean stress correction.

Fatigue Damage as per Goodman mean stress correction.

Likewise, we can check for Fatigue lifecycle and fatigue damage as per Gerber mean stress correction too.