S-Frame Shell analysis, node density vs result 1

[NorthCivil]

Hi all,

I'm running a simulation of a square sheet in S frame. The sheet has fixed supports at certain points on the sheet, and loads at other points.

I set it up as a shell, mixed triangular & quad mesh, with joint nodes evenly spaced throughout the sheet.

I was getting results that I thought were too low for stresses near the fixtures, so I decided to run it with closer joint spacing near the fixtures. it gave me a result with higher stress. I checked again with really tight spacing, and the stress came back even higher, this time, a practically unrealistic result. I discussed with colleagues, and an idea was put out, that as we approach an infinitesimal area, stress approaches infinity. Are we right in this assumption? or is the model flawed? from some research online, some reports have been that stresses should converge on a definite solution when node densities are high.

If a stress that approaches infinity is in fact a correct concept, what is a good level to take the density to to find a realistic, yet acceptable, level of stress...?

thanks

Northcivil

Northcivil

 

[rickfischer51]

If you are applying a force at a point, you have a stress singularity. A point has zero area, so the stress is 10000lbs/0in2 = infinity. Stresses at nodes are extrapolated from integration points. The smaller the element, the closer the interpolation point is to the node, so the closer it is to the singularity and the higher the computed stress. Same goes for a restrained point. If you need accurate stresses at these points, you need to accurately model the boundary condition.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[glass99]

NorthCivil,

I assume this is a point supported glass panel. Are they rotules or non-rotating fittings?

Is this a non-linear geometry analysis?

Are you meshing a hole at the corners?

Are the supports moment fixed? If yes, the stress concentration can be substantial.

Have you modeled a "spider" in the holes with single constrained point?

You should reference Peterson's Stress Concentration Factors for a baseline comparison.

 

[NorthCivil]

rickfischer: Thanks - I see more clearly what is happening. I will have to look deeper into how to avoid singularities to reach what I'm shooting for within S frame.

glass99: you got it. spider fittings, moment fixed, didn't mesh a hole. linear analysis. Its a pretty conservative way to go about it. I just started using new software, and i was getting similar results initially to my old standard software. Because of this, I assumed there was some idiot proofing build in. Once I started making my mesh denser, things started getting a little out of whack.

 

[jhardy1]

In your model, your supports are presumably modelled as fixed restraints at individual nodes. The restraints will attract a finite reaction load to each support node, and a finite load applied over the infinitesimal area of the support nodes (with infinite stiffness) creates a singularity, for which the computed stresses approach infinity - regardless of how fine you make the local mesh. (In the real world, your "point support" has a finite area, and also has finite stiffness, so there is no singularity.)

Two suggested methods of dealing with this:

1. Ignore the computed stresses at and very near to the singularity, and use alternate methods to determine the local stresses.

2. Model the supports using a more realistic mesh and restraint model - e.g. create a fine local mesh which can capture the geometry of the actual support detail, and apply a finite, realistic distributed stiffness over the support elements, so that the local stresses distribute more realistically around the supports.

http://julianh72.blogspot.com

 

[ShellsPlatesMeshes]

The nature of the issue is closely related to the Saint-Venant's principle (lots of info an examples in the internet).