Reply To: Bearing Stress Simulation

[peteroznewman]

Thanks for the detailed information!

Bearing Stress is calculated using the definition that you have shown and is useful for hand calculations for a first order analysis prior to an FEA model. 

The experiment is a physical test that creates some data which an FEA model can attempt to simulate.

An ANSYS Bearing Load applies forces to one half of a cylindrical face in a radial direction on the face with a magnitude proportional to the cosine of the angle of the face normal to the load direction. This means a factor of 1 on the top of the hole at a 0 degree angle to the load direction and a factor of 0.5 at a 60 degree angle and zero at 90 degrees and beyond. That force profile is much better than just putting equal parallel forces on all the nodes around the entire cylindrical face which is what a Force Load would do and creates tension on the opposite side of the hole!

A more accurate representation of the stress in the part than the Bearing Load is to model a cylindrical pin and use contact.

One missing dimension is from the edge of the hole to the top of the plate. Recommendations are 1.5 to 2 diameters, but looking at your images, it looks like you are at 1.0 diameters or 6.35 mm, so I created a model at that dimension.

You should always take advantage of symmetry in your models. I can slice this model down the center twice, and keep the left rear quarter, the other quarters have identical stress, however, a quarter model will only show a quarter of the load, so if you pull the pin 1 mm up, the model would show 3 kN not 12 kN that the experiment delivered.

You should also try to get brick-shaped hex elements, rather than tetrahedral elements because they deliver higher quality results for the same number of nodes. You should also have smaller elements where the stress changes rapidly. The image below is a quarter model of your plate. A pin of the same diameter is hidden in this view and is modeled as a rigid body.

The experiment included taking the material past yield and into plastic deformation. When you build a model you can add plasticity to the material model. There are several types of plasticity and I chose a simple Bilinear Kinematic Plasticity. The model displaces the pin up 1 mm and the resultant force required to do that is plotted below. Remember: 3 kN in the model = 12 kN in the test.

The plasticity model used a Yield Strength of 450 MPa and a Tangent Modulus of 300 MPa.
A multilinear plasticity model would do a better job of creating the more gradual curve shown in the experimental data.

You are welcome to have a copy of this model but it was built in ANSYS 17.2 so you would have to upgrade to open it.

Regards, Peter