When making structural analysis with FEM, do we normally use plate or shell elements to represent slabs?
You really need to specify what software you are using. The names "plates" and "shells" may be used for very different finite element formulations. Another name sometimes used is "membrane element". Since you have specified the "structural engineering" tag, you are probably using something like STAAD, ETABS, SAP2000, MIDAS, LS-Dyna or Oasys GSA, and your shell and plate formulations are probably both 2D elements (not 3D) - since they have only 2D geometrical connectivity, and the formulation typically is based on shape functions based on two-dimensional local coordinates. The difference between "plates" and "shells" will depend upon the software you are using, but typically there are three types of behaviour in most structural analysis software:
1. In-plane properties only - sometimes called membrane elements as they have no flexural stiffness. They can be used for shear wall analysis - the benefit for design calculations being that they do not generate minor axis shears or bending moments. This may be a disadvantage in some cases though. They should not be used for slab design (although they may be used as diaphragm elements to tie lateral system elements together).
2. Out-of-plane properties only - sometimes called grid or plate elements, and are used for flexural analysis (I don't think these are commonly used these days). 296
These may be used for design of floor slabs without significant in-plane forces, with the advantage being that they don't generate axial loads, which makes design easier. However, in some cases, this can be a disadvantage - they cannot be used to model slab and beam acting compositely. Also they will not provide diaphragm action to tie lateral systems together (shear walls, braced frames and moment frames).
3. In-plane AND out-of-plane properties - these are more general than the first two, and may be used for wall and slab and beam and slab design. However, the engineer must be aware of the larger matrix of forces and moments that they carry and will need to design for them. In their most basic formulation they do not account for through thickness shear or "drilling moments" at the nodes, although some do (for example the Allman-Cook formulation). You will need drilling stiffness if you want to directly connect 1D beam elements to your 2D mesh at a node.
You may also come across "thick shell formulations" which explicitly account for through thickness shear (good for transfer plates and flat slabs).
For slab design you will also need to look out for formulations or tools that convert torsional moments (Mxy and Myx) into direct moments - such as by means of the Wood and Armer method. If you ignore these you may under-design your slabs for flexure. Alternatively you can look for design software that creates strips for design (they will handle the torsional moments I mentioned).
There are other formulations for 2D elements - depending on whether they have linear or parabolic shape functions, or even more exotic. Note that I have not covered plane stress, plane strain or axisymmetric 2D element types.
STRONG REMINDER: You need to check the user manual of the software that you are using in order to fully understand what the implementation is in that particular software.
Resources:
* https://www.oasys-software.com/help/gsa/10.0/GSA_Manual.pdf (section 3.6.1 from page 78 onward)
* https://www.oasys-software.com/help/gsa/10.0/GSA_Theory.pdf (from page 61)
* https://ocw.mit.edu/resources/res-2-002-finite-element-procedures-for-solids-and-structures-spring-2010/nonlinear/lecture-19/MITRES2_002S10_lec19.pdf 296