0
$\begingroup$

There are many types of surface elements which exist in most of the Finite Element softwares. In ANSYS, I have the option to make my surface element to behave as a plane stress element, plane strain element, membrane element, plate element or shell element. But I cannot decide which element type should be chosen for what purpose?

Can anyone provide an elaboration on this please?

Improve this question
$\endgroup$
1
  • 2
    $\begingroup$ How are each of those elements defined in the instructions? And, sure as eggs are eggs, the definitions of each element are in the instructions. $\endgroup$
    – Solar Mike
    Oct 7, 2021 at 19:28

3 Answers 3

Reset to default
2
$\begingroup$

Your method of categorizing different types of elements seems confused. It is a "two-dimensional" set of categories, not a "one-dimensional" list.

First, geometry:

  • Plate elements are always flat.
  • Shell elements can be curved, though they can be flat as a special case.

Second, what stress and strain components do they carry:

  • Membrane elements can only carry direct and shear stresses in the plane of the element. That is easy to understand if the element is flat, but curved membrane elements can also exist - for example, to model a thin walled pressure vessel where the direct stress in the curved wall is balanced by the internal pressure.
  • Plate and shell elements can both carry bending loads as well as direct loads.

You should have learned the difference between plane stress and plane strain in a "strength of materials" course on statics, before attempting to do any finite element modelling.

  • In plane stress, there is no direct stress component through the thickness of the element. If Poisson's ratio is non-zero, the thickness of the element will change because of the other stress components.
  • In plane strain, there is no direct strain component through the thickness of the element. If Poisson's ratio is non-zero, there will be a compressive or tensile stress through the thickness.

Plane strain elements are only used to model situations where this makes physical sense, so as a general guideline, "if you don't know why you want to use plane strain elements, then you don't want to use them at all".

Improve this answer
$\endgroup$
2
  • $\begingroup$ I actually have read and understood the plane stress/strain theory in the course you have mentioned, in my undergraduate studies. Infact, it was Elasticity and not Mechanics of Materials. But I haven't taken the advanced courses which mentions the differences between the membrane element and plane stress/strain element, or difference between plate and shell element, since I have just graduated. So only if plane stress/strain elements were available, I wouldn't had posted this question at all, but there exists much more varieties than these so it was slightly confusing. $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 21:36
  • $\begingroup$ And I could had read the guide manual for ANSYS only, but I wanted to get a general overview for these elements so that even if I progress to a different software, I still would have an overall idea about these elements. Because the FEA softwares sometimes can be different from each other in some ways they work. $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 21:37
1
$\begingroup$

Membrane Element - Membrane elements are used to represent thin surfaces in space that offer strength in the plane of the element but have no bending stiffness.

Plate Element - The plate element is one of the more important structural elements and is used to model and analyze such structures as pressure vessels, chimney stacks, and automobile parts.

Shell Element - Shell elements are used to model structures in which one dimension, the thickness, is significantly smaller than the other dimensions.

Note: Shell elements are different from plate elements in that:

– They carry membrane AND bending forces

– They can be curved

PLane Strain/stress Element - They must be positioned in the model XY -plane, i.e., the Z coordinate of the element nodes must be zero. Loading F must act in the plane of the element.

Improve this answer
$\endgroup$
14
  • $\begingroup$ what would be the difference between membrane element and plane stress/strain element then? $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 20:36
  • $\begingroup$ Does all of these element types require thickness as an input in FEA? Or some of them can work without need for a thickness input? Plus, can we say that Shell element is somewhat the combination of membrane and plate element? What would happen if I apply a load to a membrane or plane stress/strain element, like it won't work and FEA software should return me an error or something? $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 20:40
  • 1
    $\begingroup$ "Plane Strain/stress Element - They must be positioned in the model XY -plane," Is that a statement specifically about ANSYS? It is certainly not true for other FEA programs (and if it was true for ANSYS, it makes the elements next to useless for real-world modelling IMO). $\endgroup$
    – alephzero
    Oct 7, 2021 at 21:11
  • 1
    $\begingroup$ Plate and shell elements need to assign a thickness, membrane, and plane strain/stress elements default to the unit. Yes and yes. $\endgroup$
    – r13
    Oct 7, 2021 at 21:17
  • 1
    $\begingroup$ OK, so Abaqus has a plane stress element with a pile of restrictions that make is useless in many situations. Big deal. I have no idea about Ansys, but NASTRAN plane stress elements certainly do not have the same restrictions as Abaqus - and also NASTRAN plane strain elements can be of any thickness, not just unity. To repeat, the OP's question is about ANSYS. Technical details about Abaqus are irrelevant. $\endgroup$
    – alephzero
    Oct 7, 2021 at 21:38
0
$\begingroup$

So I will give you a quick overview of relevant element types.

  1. The most natural element are solid elements. Either in 2D or 3D they can be used to display stresses/strains in either 2 or 3 dimensions. This should mostly be your element of choice for solid bodies.

  2. There may be vey thin elements. it me smart here to apply something like the plate theory. this is particularly usefull if your thickness is way lower so than any other size so that any stresses in that direction can be ignored.

Very often you will also see a difference between linear and quadratic elements. This usually refers to the shape functions. If you dont want to go into detail too much, here is a quick explanation: elements try to find a polynomial which will describe the displacement inside that element. This polynomial may be either linear or quadratic. Since the strain is the derivative (kinda) of the displacement, you will end up with constant strain across elements for linear shape functions and with linear strain for quadratic shape functions. constant strain is very bad for modelling usually so you should always try to go for elements of 2nd order.

Improve this answer
$\endgroup$
11
  • $\begingroup$ This explanation is completely different than what I was looking for and what I have asked in my question. I usually use ANSYS default element types and I don't mess with them since there further exists hundreds of types for each of the types that I have mentioned it, so I keep it to ANSYS to decide the best available depending upon the model. $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 20:59
  • $\begingroup$ But let me ask you this for the answer that you have given. Since quadratic order means that there now exists an extra node between two nodes (i.e. now there are 8 nodes in a quad element rather than 4 nodes), so the strain between each of the nodes is still going to linear, right? What I mean is that we have now replaced a linear strain over the element with two linear strains, isn't it? $\endgroup$
    – Rameez Ul Haq
    Oct 7, 2021 at 21:04
  • $\begingroup$ @RameezUlHaq "so the strain between each of the nodes is still going to linear, right?" No. The displacement along the edge of an 8-node element is quadratic. The strain is the derivative of the displacement and therefore a single linear function. (And the strain along the edge of a 4-node element is constant, not linear.) $\endgroup$
    – alephzero
    Oct 7, 2021 at 21:45
  • $\begingroup$ @RameezUlHaq "I keep it to ANSYS to decide the best available depending upon the model." That is a recipe for disaster. You are the person who has to make the decisions about how to model the structure and what element types to use. The software can't do it for you. $\endgroup$
    – alephzero
    Oct 7, 2021 at 21:47
  • $\begingroup$ An engineer who understands FEM will become a better engineer, one who doesn’t will become a dangerous engineer. FEM is not always correct. It’s not god and only works if used properly. $\endgroup$
    – Finn Eggers
    Oct 8, 2021 at 4:22

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

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