When making structural analysis with FEM, do we normally use plate or shell elements to represent slabs? I checked and did some reading for the difference between shell and plate elements in FEM in general but particularly I am trying to understand the differences between the two as far as representing a slab in a structure such as a building or bridge.

Also does the type of slab make a difference, such as RC concrete, metal deck or post-tensioned?

Also, the difference should also depend on the software we use right? I mean as far as how the calculations are formulated in each software, so may be there is no definite answer to this and we go case by case for each software?


The general rule of thumb is never to introduce a degree of complexity you don't need.

Use the expected behaviour of the structure to determine the element type. A two-way slab is usually best modelled as 2D elements (plate elements) and an orthotropic bridge deck is often best modelled using 1D elements (beam elements) because it consists of elements which only have one span direction each.

This makes the model easy to create, and what is perhaps even more important, it makes the model easier to check. The closer the model is to a manageable hand calculation method, the more realistic it is to do spot calculations that verify the results of the model.

The use of 3D elements may also be problematic because the software will often assume the material is able to transfer the same stress in each of the three directions. Rolled steel is an example of a material which isn't isotropic and may have very low tension capacity in the thickness direction due to various defects (lamellar tearing). The easy fix is to only use 2D elements that will automatically assume zero stresses in the thickness direction.

For reinforced concrete, making a design based on 3D elements will be a bit a nightmare unless you make an extremely detailed model that include the reinforcement and take cracking of concrete in tension correctly into account, because otherwise you will have tension stresses in concrete that exceed its tension capacity and you will have to convert the stresses in the 3D elements to equivalent section forces corresponding the results of 2D elements in order to do a reinforcement design. To correctly account for concrete cracking in three dimensions is a complicated problem and to attempt this in a model of the global behaviour of a structure is a challenge that is best avoided if at all possible.

In most cases, I will only recommend using 3D elements for two situations:

  • Local models of complex details in steel structures and similar. This includes cases where you to need to know the exact peak stresses to account for fatigue effects.

  • Soil in geotechnical problems with significant 3D effect.

  • $\begingroup$ Thanks a lot, so I understand plate elements are fine, so you mean shell element is a 3D element correct? Also I didnt understand the relation here with cracking of concrete by the way, so when concrete cracks, can we not simply reduce stiffness of section to represent that (even when we do simple analysis with 2D elements)? $\endgroup$ May 9 '20 at 9:27
  • $\begingroup$ Yes, shell elements are another term for what I called 3D elements. Modelling of cracks and their influence on the distribution of forces by reducing the stiffness is a very good first approximation. The reduction factor should depend on the amount of reinforcement, and that becomes tricky for 3D elements if you don't have evenly distributed reinforcement in all three directions. But it works for slabs modelled as 2D elements. The influence of cracks on the strength is obviously not handled fully by simply reducing the stiffness. $\endgroup$
    – ingenørd
    May 9 '20 at 9:51

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). 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.



Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.