It commonly stated and believed that the stress concentration factor for a plate with a hole in uniaxial tension is 3. This is certainly not always true. In this article I will show that in many real cases the stress concentration factor is significantly smaller than that!
Simple FE Solution
To test the textbook solution I created a simple FE model of a plate with a hole in uniaxial tension. The plate had a width of 50 mm, a height of 50 mm, and thickness of 5 mm. The hole diameter was 2 mm. According to the equation listed above, the stress concentration factor for this geometry should be 2.88.
The FE calculated Mises stress contours for of this configuration are shown in the figure below. Here I assume that the material is linear elastic with a Young’s modulus of 100 MPa, and the applied strain was 0.2%. The mesh consisted of 32,000 full integration quadratic elements (C3D20). The stress concentration factor in this case becomes 2.81, which is similar to the textbook solution. The reason the value is slightly too low is likely due to the limited mesh refinement close to the hole. But there is something else that is much more problematic with this calculation!
More Realistic FE Simulation
To make the FE simulation more realistic we need to use a better material model! In this example I will assume that the plate is made from PTFE (Teflon). The MCalibration software comes with excellent experimental data for a PTFE, and it is easy and quick to calibrate the PolyUMod TNV model to this experimental data set. The figure below shows the calibrated material model predictions.
I then repeated the same FE simulation using this more accurate material model, and I extracted the stress concentration factor as a function of the applied strain. The figure shows that the stress concentration factor is about 2.8 in the limit as the strain goes to zero, but at an applied strain of 1% the strain concentration factor is 1.9, and that at 2% strain the stress concentration factor is 1.6. These values are substantially lower than 3.
From the FE simulation I also extracted the strain concentration factor as a function of the applied strain. The figure below shows that the strain concentration factor is about 2.8 in the limit as the strain goes to zero, but then become about 4.5 at an applied strain of 2%.