One principal stress on a free surface should be zero, but its not. Why?

[mlindqvist]

On a free boundary surface of a solid, one of the principal stresses should be zero (plane stress), or equal to the applied pressure, if there is a pressure load on it. This, seemingly simple boundary condition is not always satisfied and apparently not enforced by the solver. I'm currently working on a hydraulic valve with a high internal pressure load. On some internal radii where this pressure is applied, one of the principal stress should be equal to this pressure, according to theory. After having run a singla pass adaptive analysis with default mesh settings, max principal is +1418, min principal is about +200 in the same location, but should be -103 (= applied pressure) according to theory. What does the ptc community suggest? Refine mesh?

So we have some known information about the stress state at the boundary surface. I'm not a programmer, but I imagine it should be possible to enforce this plane stress state on the boundary surface ? Is there any ptc developer in this community who can shed some light on this?

/Best regards Mats Lindqvist, Avalon Innovation Sweden

[mlindqvist]

I have now made a second run with a mesh control, max element size 2*R on internal rounds plus "detailed fillet modelling" in AutoGEM settings. 168k element vs 43k elements in the first model. It's now better, min principal is -83 vs. theoretical -103. Max principal is just slightly higher, so it seems max principal converges better than min principal. The reason I look at min principal is that there is an ASME design rule that takes all principal stresses into account.

[ehaenen]

Hi Mats

Strictly speaking you need stress perpendicular to the surface on which you apply the pressure to be equal to the applied pressure. This could very well be the min principal but I do not know for sure whether this is essentially the min-principal, depending on complex shapes.

Anyway: This is in fact one that is difficult to converge for Mechanica, strangely enough. Similar with shear stress that needs to be zero on the surface. and stress perpendicular to the outer surface of a pressure vessel (needs to be zero).

A rule of thumb: I find you need three solid elements over the thickness to get the convergence you are looking for. This is not easy to achieve using "ordinary" mesh refinement.

I use volume regions built from an offset boundary. Bluntly spoken: add a slightly bigger inner volume end use this to make a thin boundary layer of elements: You'll see a great improvement without adding an enormous amount of elements.

Regards

Erik