do you ever use solid elements for fea modeling

huangyhg

do you ever use solid elements for fea modeling?
i don’t think i ever have. for one thing, i think they tend to overestimate stiffness. another problem they present is interpreting results.
check out our whitepaper library.
since solid elements represent all degrees of freedom, unless you are using them in an application that is too demanding (like long thin beams or plates), then they should give you the correct stiffness. in general, more degrees of freedom translates into more compliant (that is, less stiff) response.
you have a point; it’s just that whenever i have used them (to model (concrete) pedestals for example) i have gotten stiffness that exceeds the theoretical value. meshing might be the problem there.
is your concrete constitutive model isotropic? sometimes anisotropy in the material model leads to unexpected stiffness.
in some cases, i have tried to use solid elements to model reinforced concrete pedestals. i have found that it overestimates stiffness (in comparison to using plate elements). i don’t consider r/c as isotropic.
of course in reality r/c isn't isotropic. the question is what is in the fe model? i was just raising the possibility that an anisotropic material constitutive relation in the fe model might cause some unexpected behavior.
in one model that comes to mind: i had nothing but solid elements. that's it. in fact i did a comparison once: i modeled a shear wall using plate elements, and another using solid elements. i got the more (theoretically) accurate results using plate elements (for lateral stiffness).
the (theoretically) accurate results are from what source?
roarks? or where?
from a concrete text i have which gives a shear wall deflection equation.
i may have an idea where the discrepancies in the computed stiffnesses originate. this might be a problem of comparing apples and oranges, but i can't say for sure since i don't have the text you are using i am sure.
the apples and oranges here are the kinematic formulation. the one dimensional analogy is the beam. say you had an easily derived analytic solution for the beam loaded with a constant traction, q. simply supported on the two ends. it is easy to derive the euler-bernoulli beam bending solution, since most of us have had some kind of basic mechanics of materials or "strengths" class where we learned how to do basic shear and moment diagrams. now analyze this with two fe models--one uses 'beam' elements, the other 2d solid elements. you get two fe solutions, which is correct? if the measure of correctness is comparison with that beam bending solution you derived, the fe model with the beam elements should always give you the best answer, because the beam elements are consistent with the beam bending solution you have derived--to derive the beam elements for the fe software, the fe software developers made the same assumptions as the bernoulli euler beam bending analytic solutions made, therefore the beam elements are more consistent with the beam bending analytic solutions than the 2d solids are.
i am guessing that the shear wall solution in your concrete text uses some kind of plate kinematics model (say timoshenko's plate model), which makes some key assumptions that eliminate degrees of freedom to simplify the equations (for instance, some plate models assume there is zero normal stress in the direction perpendicular to the plate surface, while clearly a plate loaded with a constant pressure normal to the surface has to have a normal stress varying from that constant pressure on the loaded surface to zero on the opposite surface). the plate elements in the fe software might use the very same assumptions your shear wall solution used, and therefore also ignore or eliminate the same degrees of freedom as the shear wall solution. since the shear wall solution and the fe plate elements use the same assumptions, you should be able to match the shear wall solution more easily with the fe plate elements than with the fe solid elements.
usually though a too stiff fe solution means not enough degrees of freedom, so that if you quadrupled the number of elements, you probably will get a more compliant fe model with the solid elements. it's kinda cool to play around with different fe element types to see how the answers change.
you generally use solid elements when all 3 dimensions are proportionally close (like a mechanical component). 2d (plate, shell) elements should be used when 1 of the 3 dimensions is disproportionate by a magnitude less (in other words for something like a wall or a slab). it all depends upon the relative proportions. i also suggest that you refer to the software users manual. it usually gives some guidance on this.