Hi everyone.
It’s a general question…
I designed a balcony and applied a load to it.
In the first simulation (mesh max. 80 mm, min. 20 mm), the maximum stress was 67 MPa.
In the second simulation (mesh max. 10 mm, min. 5 mm), the maximum stress is 238 MPa, as shown in the figure.
What mesh size should I use to get reliable results?
Many thanks to everyone.
Giovanni Di Maria
First of all, you should use hexahedral elements whenever possible. These parts seem simple enough for that. And it would be good to create surface partitions to apply load to more accurately defined patches instead of relying on manyually selected element faces.
But when it comes to mesh density, you should perform a mesh convergence study. So basically what you’ve already started - run with a coarser mesh and check the maximum stress and displacement, refine the mesh, recheck the results and refine again if needed. The difference between the subsequent runs should be around 5%.
In some cases you may encounter stress singularities - stresses will keep increasing indefinitely with mesh refinement. This happens when you have sharp notches and point BCs/loads for instance. But then you can add plasticity or fillets or even ignore these peaks sometimes.
In this case you have a stress concentration at the tied interface. Consider using matching meshes or possibly compound parts instead. Currently, you have a very large difference in mesh densities between both parts. If you use hex elements and more compatible mesh sizes, the results should be better. Of course, for tie constraints the coarser side should be the master, but ties themselves may introduce stress concentrafions and it’s often better to use contact (if relative motions are allowable) or merge/compound the geometries (if relative motions are not permitted).
Perfect. , very clear.
Thank you so much from the bottom of my heart.
Giovanni Di Maria
