This content has been marked as final. Show 3 replies
The problem is the lack of elements through the thickness of the tank. You need at least 3 to 4 parabolic (cosmos use term high instead of parabolic) solid elements through the thickness to get accurate natural frequencies. As the number of solid elements through the thickness increases, the natural frequencies and mode shapes should converge toward the shell element solution. This assumes your boundary conditions are consistent and appropriate between the solid element model and the shell element model.
Shell elements are well suited for thin structures. They reduce the computation effort and maintain accuracy for thin structures.
1. What is the ratio of "next largest length" to thickness? nextLargestLength/thickness
2. What is the ratio of "largest length" to thickness? LargestLength/thickness
If you your up in the hundreds to one range or more, just use the shell elements. I am unsure of where the shell elements breakdown exactly. I will have to look into this in the future.
For static studies there are usually (from my previous experience) no difference using more than one element through the wall thickness of a tank (away from any discontinuities). For internal pressure load cases we ussually compares the FEA first principal stresses to the calculated hoop stresses (Pr/t). Which normally do not differ more than 1%.
Why the difference for the modal analysis as the same stifness matrix was used to calculate the eignvalues?
What do you mean by the next largest length? Do you mean the size of the elements in the other directions?
The "2-3" or "3-4" solids thru a thickness rule of thumb has been out there for as long as I've been using FEA (punch cards in Nastran). It is actually a little more complicated than that. Consider a thin member in pure tension, as you might expect in a classic pressure vessel that conforms to thn-walled pressure vessel calcs, or hoop stress = PR/t. (Note that if you expect shells are appropriate, you design should be in the thin walled category where R/t > 10) You'll get reasonable stress results with a low aspect ratio second order (High Quality) tet mesh where there is only one element thru the thickness.
As bending becomes a more dominant behavior, the solid mesh will deviate from the shell mesh as shells handle bending better. One way to understand this is to consider the way outer fiber stresses are calculated in a solid. stresses are calculated at points within the element, called Gauss points and then stresses are estimated at the outer nodes. For sharp discontinuities and bends, a single element doesn't have enough information or flexibility to correctly estimate what is happening at the outer surfaces.
A few years ago, before I joined SolidWorks, I tried to develop a mini-course on meshing where I was going to show clearly when solid tetrahedrons fell apart for thin walled bodies. I learned that it is really problem dependent and I got much better results for solid tets in tough problems than I ever expected.
My suggestion is that you spend some time exploring simplified versions of your design in solids and shells where a hand calc or other known solution is available and vary wall thickness to determine where each assumption breaks down. It isn't so neatly packaged in the "3-4 elements thru a thickness guideline" although if you can get that in your model (Good luck!) you can be reasonably comfortable that your stiffness will be good.
Why did solids seem to work for static pressure but not frequency? I would suspect it stems from the way the problem is solved. The frequency solver considers energy in bending as it determines natural frequencies, whereas the static solver wouldn't necessarily go there for the loading you described. You'd see the same thing with buckling (which was one of my eye openers to the limitations of tetrahedrons in thin walled structures 15+ years ago.)