peteroznewman
Subscriber
nIf you are interested, put a new Coordinate System at that vertex. Under the Solution branch, request Equivalent Stress, but scope it to that vertex, and click the box next to the Result to make that an output parameter. Under Mesh, add a Sizing on the Body, type = Sphere of Influence. Select that new Coordinate System and type a Radius large enough to reach the vertex on the other side of the rib, such as 10 mm. Now you can make Element Size an input Parameter. That will let you automatically solve the model with progressively smaller elements and create a table of element size vs stress at that point. You can plot this data to see if it behaves like a singularity or if it converges on a finite value at zero element size. nThe rib looks like it might be about 8 mm wide. What is the global element size in this mesh? Is it 5 mm? A good way to reduce element size is with a constant ratio. If you start at a 4 mm Body Sizing in the Sphere of Influence, you can go down by a factor of 2 on each row of the Parameter Set Table of Design Points. The rows will have 4, 2, 1, 0.5, 0.25. Click the Update All Design Points and let it run until it finishes. Copy that table and plot it in Excel. I would be interested to see that plot. You can add another row at 0.125 mm if the trend in the three smallest points is not definitive.n