Let's Share it

In this whitepaper we are going to investigate how to find and deal with stress concentrations, review mesh control and how it affects stress results.

For beginners: before starting this practice, it is recommended to read the previous whitepapers, first.

Problem Description

During this study we analyse a rail support- simplified assembly is presented in figure (1)- under normal and horizontal load of F=2.7kN. Support is laser cut from 16mm plate, material is AS3678-250.

FEA geometry description — *Figure (1)- Simplified Geometry of support and rail*

As mentioned in the introductory of this study we are focusing on stress concentration, to achieve this goal a reference point at middle of bend line (Point 1) is defined, figure (2).

Shows point in the middle of the stress concentration line — *Figure(2)- Reference Point on the middle of bend line*

To obtain stress value of point 1 at each study, we define a sensor for this point, right click on the Sensors folder in the model tree and select “Add Sensor…”, figure (3).

add sensor to the model — *Figure (3)- Add Sensor to the model*

On the Sensor Type section “Simulation Data“, on Data Quality select “Workflow Sensitive“, for “Properties” select Point1, figure (4).

Steps for creating sensor on point1 — Figure (4)- Steps to create sensor on point1

Finite Element Analysis

Create Study

Create a static study and name it “Stress Concentration“, figure (5).

Stress Concentration Study — *Figure (5)- Create Stress Concentration study*

Apply Material

First create a custom material named AS3678-250 with properties shown in figure (6), then assign it to the model.

If you don’t know how to create custom material, follow steps in this link.

Set the Connections

Not applicable for sole part.

Apply Fixtures

Apply fixed fixture to the end of the support, figure (7).

How to add fixing to the support — *Figure (7)- Apply fixed geometry to the end of support*

Define The Loads

Add 2700N normal and horizontal to the end of support, figure (8).

How to apply load on the end face — *Figure (8)- Apply load on the support*

Mesh the Model

Apply mesh to the model, Curvature-based Mesh with the default size of 3.7mm, figure (9).

Mesh size and type illustrated — *Figure (9)- Mesh Size and Type*

Run the Analysis

FEA results of Von Mises stress for the analysis is presented in figure (10).

Figure (10)- Von Mises stress results of the analysis

To get the exact amount of stress, use probe tool, on options select from sensors, stress in Point1 is 119.8MPa, figure (11).

Steps in probe — *Figure(11)- Probe Stress on Point1*

Evaluate the Results

To have confidence in FEA results, check the stress Error plot, figure (12).

Stress Error Plot, maximum 93.25% — *Figure (12)- Stress Error Plot*

Due to high percentage error in the stress concentrated areas, we use mesh control to reduce the mesh element size in that area and check again the stress results.

To have a record of what has been done, copy this study, to do that, right click on the study name and select “Copy Study”, figure (13).

Copy Study icon — *Figure (13)- Copy Study*

Select a name for the study as you like, something like “Mesh Control 01”. In the new study apply mesh control to the edge with the default numbers, figure (14). Then run the analysis and see the stress in Point1.

How to add mesh control on high stress area — *Figure (14)- Apply Mesh control on stress concentration area*

The stress in point1 is 159MPa, about 33% increase in the stress. During each study if you see such a big stress difference by changing mesh size, you normally refine the mesh in that area more to see how stress changes in that area.

To do that, copy the study again, names it “Mesh Control 02”, modify the mesh control and slide the mesh density bar to right (fine side), run the analysis and check the stress in Point1, the stress in Point1 is 213.4MPa (34% increase). Meanwhile, if you check the stress Error plot you would see that the error percentage in the high stress area is reducing!

Based on elasticity stress in sharp corners, stress is division of load on a point (no area) so that it is infinite. But the software couldn’t generate infinite stress due to discretization error.

To obtain correct amount of stress in this area just add a small fillet there, for example add 1mm fillet to the line and repeat this three studies again. Comparison between stress value in these six studies are presented in chart (1) and the trend is displayed in chart (2).

Stress Values for each study
for no mesh control study:
without fillet: 119.8MPa
with fillet: 188.9MPa
Mesh control 01 study:
without fillet: 159MPa
with fillet: 114.3MPa
Mesh control 02 study:
without fillet: 213.4MPa
with fillet: 114.3MPa — *Chart (1)- Stress Values for Each Study*

two different trends, converging results for fillet studies and diverging results for no fillet studies — *Chart (2)- Stress trend summary for all studies*

As it could be understood from chart (2), the stress value is converging to a constant value, the mesh control size 01 is accurate enough and the obtained result is reliable.

Finite Element Analysis- Stress Concentration