How much mesh refinement should I do?
A linear statics model calculates a maximum equivalent stress, which is compared with a yield strength.
An initial mesh has a certain element size around the point of maximum stress.
A second mesh with smaller elements is solved and gives a new value of maximum stress.
A third mesh with even smaller elements gives a third value of maximum stress.
How do you decide when to stop refining?
One method is described in ASME V&V10.1 “Illustration on V&V for Computational Solid Mechanics” and is called Calculation Verification, one small part of the entire Verification and Validation process.
Below is an example using a tetrahedral mesh with a Sizing Mesh Control on a Sphere of Influence.
Maximum Stress from six mesh sizes were plotted. The red line is a best fit line through the three smallest element sizes. This line, or the calculation in Section 7.2 of V&V10.1, can be used to extrapolate the maximum stress to a zero-size element. This is the estimate for the exact maximum stress, but is only valid when the results are being calculated in the asymptotic convergence regime. The line estimates the maximum stress is 607 MPa. See this discussion for an alternative mesh control using inflation.
The three largest element sizes are clearly trending toward a very different zero-size element value and should not be used since those results are not in the asymptotic convergence regime. V&V10.1 has more information on how to determine if you are in that regime.
In this example, I used a factor of 1.5 to change each successive element size. V&V10.1 recommends the factor be > 1.3.