I started paying attention to meshing way too late I think. When I started my Ph.D. I literally divided elements into two categories: those that throw errors and those that don’t! But even then I was lucky – I could simply check scientific papers on similar topics and use the elements that someone else used before. In “normal” work you usually don’t have such a luxury! So let’s take a look at various elements types used in FEA!
There are several types of Finite Elements. You can use beams/plates/solids depending on your model. With plates/solids, you can use easier to mesh triangular elements (TRI/TET), or more robust quadratic elements (QUAD/HEX). All elements can be linear or quadratic (the second computing longer but with nice perks in return).
As you can see, there are several things we need to discuss – let’s jump in!
The Biggest Problem with Meshing Today!
Sadly, I see it more and more often and we need to address this first. We can discuss TET and HEX elements all day, but there is a choice that is often skipped. Unfortunately, it’s the most important one!
It’s clear that CAD tools are everywhere in an industry. When I was moving to my students’ apartment I designed my furniture on paper with a humble pencil, I went to a store that cut plywood and ordered the needed parts having several sheets of hand drawings with me. I’m not even sure if they would take my order today without some sort of a CAD model or maybe even a CNC file.
Nowadays each engineer has easy access to a full 3D geometry of whatever is there to design. No surprise – everybody uses CAD models for manufacturing at least! Most of my Customers send me a 3D CAD files of structure/elements I should verify – it’s more convenient for them, and they have those anyway!
This means that “technically” geometry is already made for you! All you need to do is just to load/support/mesh it and you are set, right?!
Well… How About “No”?!
Those 3D models were usually created with manufacturing in mind. All the beams and plates are modeled as solid, this serves that purpose better. Also, every detail, bend, undercut, fillet, and hole (however small) is there in the model… it’s needed in manufacturing after all!
This means that you get an incredibly detailed and complex 3D solid geometry… and this is a trap!
Does this mean that those models are “wrong”? Of course not – they just serve a different purpose! They are great for manufacturing, but those are not “FEA models” by a long shot!
I often see that people start to mesh such geometries (they are already there!), and sometimes even spend a lot of time “defeaturing” them (removing those small geometric details). In most of the models I did, that is not the best approach.
You see, the analysis model must be simplified and idealized for the analysis to actually “work” properly. In the above cases switching to 2D mesh in most parts (and beam elements for supports) is a must! You would need at least a few solid (HEX) elements through plate thickness… so with solid mesh, the element count would be *INSANE*! Not to mention that a lot of details only make the analysis last longer not contributing anything useful!
My experience is, that in most cases it’s actually faster to do the model from scratch with the analysis in mind, rather than work on changing the 3D geometry you’ve got! Either way, this is a process that will take time, and simply meshing the CAD model is definitely not the best approach (unless of course this CAD model was done directly for design purposes… but that never happened for me so far!).
So now, knowing that you really have to work up front on your model geometry it’s high time that we actually discuss various element types in FEA!
The Biggest Choice for Your Finite Elements Mesh!
Since it’s clear that working on geometry will be required, the biggest issue without a doubt is: should you use the beam, plate or solid elements.
All of those have advantages and my thinking usually is like this:
Of course, this makes sense only if you can reasonably make a call whether some elements could, or could not be used. Let’s take a closer look then!
Beam Elements – what, why, when?!
My initial question is always about beams, and there is a good reason for it. Beams have a lot of great advantages:
- Modeling and computing are so fast! I mean a beam is literally a few clicks away, and in the worst case have only a few elements along the length!
- Changes in the model are almost for free! Just click on the beam, change the assigned cross-section and relax… you just worked very hard!
- Lot’s of cool rules that can get automated! No one in their right mind would like to calculate beam models using “pure FEA” approach. There are a lot of codes and design guidelines guiding you with beam design. But it’s even better – a lot of software have those automated, so you just pick a few settings for each member and in return, you get its capacity ratio. No need to wonder about stress levels, interpreting outcomes and all the jazz… a straight capacity is at 93% answer is waiting for you at the ends!
So what is the problem? Well… not everything is a beam! In the hopper example above it’s clear that the columns and horizontal members can be modeled as beams… but the hopper itself – no way! There are many things to consider when you decide if something can be modeled as a beam or not (like do I want to analyze web stability in my FEA model for instance). However, the simplest rule would be:
If the maximal dimension of the cross-section is at least 10 times lower than the length of the element… this may be modeled as a beam!
Sure, you need to watch out for changing cross-sections, cut-outs and similar. Sometimes they will play a role, sometimes they won’t. Also, this is not the most “strict” rule of all times. If you have a 3000mm long HEB 300 (its cross-section is 300x300mm) cutting the last 10mm won’t suddenly make you remodel everything for plate elements. I used beams in various occasions that were significantly shorter than 10 times their max cross-section dimension. Still, if you are above this limit, you may simply be sure that it’s a beam!
Plate Elements for the Win!
Of course, not everything is a beam, and the hopper above is the best proof of that! If you can’t use beams, the next check is “can I use plates”. Again, plates offer some nice features over solid elements, let’s take a look:
- Modeling and computing isn’t a nightmare! Especially if you want to make a 3D HEX mesh… meshing plates seem like a hobby in comparison! While solid elements may even compute the same amount of elements faster (they usually have only 3DOF each node, but more nodes per element), solid models have way more solid elements that a plate model would have QUAD elements… so the computing gain is there as well!
- Changes won’t make you cry! Sure it’s not just a click here or a click there, but at least you can change plate thickness without changing geometry and remeshing the whole thing… and trust me – that is a lot!
If I can, I always use plates instead of solids. I simply consider them superior. Not only modeling is significantly faster, meshing way easier and computing seems quicker. They can also produce more accurate outcomes! Let’s get back to the hopper for a second. It’s clear I could use plate elements there, and to be honest… I should! To properly catch actions such as out-of-plane-bending I would need to have a few solid elements through thickness! Think how small those elements would be! Computing of such a model would take ages! And to no significant gain! If you can use plate elements, those will outperform solid elements all the time! Again the same rule can be used:
x10 Rule – round 2!
If your part has a thickness that is 10 times lower that other two dimensions of the part – you can (and should!) use plate elements!
Again, the constant thickness is a nice bonus (even though there are ways around it) etc. Sure there are considerations, and sometimes even plates have to be modeled with solids due to various reasons. But this is a rare exception, not a general rule. I feel completely comfortable saying that most of my models are made with 2D mesh. I think around 80% of those. Most of the rest 20% are pure beam models, but while I was doing more of such designs before, somehow I get mostly “plate models” to calculate nowadays, so it influenced such statistics. Very few models required solid elements, but of course, those happen as well!
Solid Elements of Last Resort
It’s exactly that. If I can’t use beams nor plates definitely I will use solid elements. There isn’t really any choice. I completely get that in FEA world there is extremely a lot of things that can only be modeled with solid mesh. Starting from engine body and ending on teeth bulky stuff will require solid mesh. It’s so simple.
But when you can avoid using solid elements… you really should! Mostly because I don’t really see a lot of benefits for using solid elements. Apart from the fact that in many cases you just have to!
2D Mesh – Finite Element Types
There won’t be a chapter about beams. Usually, linear beam elements are used and those are fine. Sure there are many formulations that only carry tension, or normal forces etc. Those are however pretty self-explanatory most of the time.
With plate elements, you have of course the same thing. There are membrane elements, stuff can be axisymmetric etc. Such elements serve various purposes, and I assume you will know when to use them. There is however one thing that I guess is the biggest issue, and that is: should I use triangular or quadratic elements?
Without going into many details I would say this:
- TRI3 elements (3 Nodes triangles) suck! You can make them work of course, but with a huge amount of elements… not the best trade. Also, they may behave too rigidly, as you can read in this post!
- TRI6 elements (6 Nodes triangles) aren’t bad. But they have an inherited problem: they are triangles. The “FEA People” like QUAD meshes, and even if your TRI6 mesh produces good outcomes, those will be met with reservations. I would also consider those pretty hipsterish!
- QUAD4 elements (4 Nodes quadrilaterals) are decent. I consider this to be the “generic” 2D elements. Sure the quadratic version (QUAB8) has more blows and whistles, but the computing cost for that pleasure is high!
- QUAD8 element (8 Nodes quadrilaterals) and super cool. They offer a decent accuracy in strain representation, and they even deform better (with each edge having the possibility to bend). Usually, you will have details in your models that will “force” you to use smaller elements anyway, and the accuracy advantage of QUAD8 elements won’t be as visible while computing time will still be a lot higher. This is of course case dependent.
It’s impossible to say if QUAD4 or QUAD8 elements are “better”. This is of course case dependent. After all, if one type of element would be clearly better than the other… who would bother with implementing the “worse” choice? If you struggle with this question just do a model that nicely represents the problems you are usually facing and check the performance of both element types. This way you will know which elements are better in your case!
3D Mesh – Finite Element Types
Usually, solids are a bit more straight forward than plates. There aren’t that many formulations apart maybe for those complex composites 3D elements. But of course the “main” question remains basically the same as with the plates: should I use tetrahedral or hexahedron mesh? It’s basically the same triangle/quad problem… but in 3D!
Again a few thoughts on the most popular choices:
- TET4 elements (4 Nodes tetrahedral) must be the most controversial element in the entire FEA universe! When it comes to performance they are terrible. But there is one thing that makes them “better”, and that is: creating a HEX mesh is a LOT of work! With 2D QUADs, you have to put in some effort, but it’s not the end of the world. With HEX things get “frustrating”. And this means that auto meshed TET4 models are popular… simply to avoid doing HEX mesh! Of course, this doesn’t help with the performance at all… but the alternative requires a lot of work! Do TET4 suck? Yea, they kind of do. But with enough of those elements, you will be completely fine… you just need A LOT of them!
- TET10 elements (10 Nodes tetrahedral) are surprisingly ok! It’s the same problem as with TRI6 – even when they perform quite ok, a lot of people will see only the “TET and forget” approach. Whatever you do, if you have to use TET mesh… go with TET10. That would be my take on this.
- HEX8 elements (8 Nodes hexahedron) are most likely the “iconic” finite elements. They share performance similarities to QUAD4 elements. What is important to remember is, that having a single HEX8 element through the thickness of an element is a really bad idea in most cases. Either use more of those elements, go with HEX20 or switch to plate model in that section of your model!
- HEX20 element (20 Nodes hexahedron) – the “big guns” of solid meshing. This is a pretty decent element, but computing starts to take awfully long, which may make it a bit less practical (depending on the size of the task!). I’ve heard people saying that they use a single HEX20 element through the thickness. While “technically” this may be ok in many cases… I don’t think I would ever consider such a thing (the same goes for one QUAD8 element threw plate width).
If I would have to choose my solid element of choice it would be HEX8. Mostly because if I use solid modeling (and I really rarely do that!) this usually means that I have a small detail and I need to have precise outcomes in that space. So mesh will be small anyway (to take into account all the geometric features). This means that there is no real advantage in using HEX20, considering how much more time computing will take.
But I would also point out that TET10 elements aren’t that bad in many situations. I try to create “elegant” meshes (I’m just like that), so I would steer away from TETs all together. But in a pinch, for a small and quick model… TET10 isn’t a tragic idea, which may not occur to many people. TET4 elements have terrible “press” and this somehow influence how people consider TET10 elements as well – I figured I will point this out here!
Linear and Higher Order Elements
I already discussed the most common element types, but I just want to wrap it up here. Sadly the names can be a bit confusing and I just want to clarify a few things.
Linear elements don’t have to be “beams”. By such name, people often refer to the “first order” elements, so those that only have Nodes in “corners” (or beam start and end). It’s easy to remember since the edges of those elements must always be a straight line (there are only nodes at the beginning and at the end of each line!). The classical 2D and 3D linear elements (let’s call them “basic”) are:
There is also an alternative, usually referenced as “quadratic”. Those would be the “second order” elements. Those have additional nodes in the middle of each side. This means that the TRI6 element would be a “quadratic triangular element” – how awesome is that! This is why usually it’s better to say “first order” or “second order”, but linear and quadratic names are still pretty common. Typical second order elements we have already discussed are:
As you see we already talked about each of those elements. It’s just another way to divide them into groups (rather than 2D and 3D mesh as I did at the beginning). I just wanted to point this out.
Also, I use pretty popular “element names” and by this, I mean i.e. QUAD8. Much industrial software will use other element names, and i.e. QUAD8 element would be S8 in Abaqus (if my memory serves… I haven’t used Abaqus in a decade!).
What we are Missing?
There are a lot of other element types out there. This is getting very long already, but let’s take a quick peek:
- RBE = Rigid Body Elements: Those are the “rigid” elements, and they come in various types. The most popular would be types 2 and type 3 (RBE2 and RBE3). The RBE2 is basically a “spider” of rigid connections that connect all of the selected nodes on a single central node. On another hand, RBE3 is the “interpolation” element. Again there is a “spider” of connections between selected nodes and the “central node”. However, those connections aren’t rigid. They will just “distribute” the load coming from the central node to other nodes… and nothing more. This means that they don’t introduce “additional” rigidity to the model. Of course, sometimes you need that rigidity, and both RBE2 and RBE3 have great uses in day-to-day FEA analysis.
- Axisymmetric Elements: If you have a purely axisymmetric model instead of doing the whole 3D thing you can model only one section with axisymmetric elements. This is a nice trick, but dangers come with it. First of all, stuff is almost never axisymmetric (you know, discrete supports, some openings etc.). But also, assuming axial symmetry you assume that your model response will be axially symmetric as well… in many shell problems that is simply not the case (like in classical shell buckling). Sure, the model may be axisymmetric, but the outcomes may not (this is a classical nonlinear geometry benchmark – you can read more here):
- Plain Strain Elements: Those ate a bit similar to axisymmetric elements. Use them if you have a very long, straight solid shape with a constant cross-section (not such a big demand huh?). Again, you will assume that response will behave in a plain strain way (no “weird” actions in the “in-depth” direction). This may greatly reduce the size of your “linear dam” model… which would be a classic example of a plane strain problem.
- Beam Elements Galore: There are so many of them! You know the “tension only” or “compression only” elements, along with “only axial forces”, “springs” and “rigid elements”. I’m inclined to say, that those are software-dependent in a sense, and checking your soft manual to learn what exactly they do seems like a good idea. But of course, the names are pretty self-explanatory I think!
If you have any other ideas about what element types to put in here – let me know. I’m sure we can work it out together!
Want to Learn More about FEA?
I really hope you like this small guide. If you want to learn more, definitely sign up for a free lesson from my FEA course. You can easily do it by signing up below:
Common Questions about Types of Elements in FEA:
Are triangular or tetrahedral elements always a bad choice?
Absolutely not. I even heard someone say “why complaint about TET4 elements… we have so strong computers right now!”. And this is a really good argument. The biggest drawback of TRI/TET mesh is that you will need a LOT of elements to produce a reasonable outcome. This means that computing will take a lot of time. But of course preparing the HEX mesh takes time as well, and it’s the time you have to work (not computer alone).
If you have a difficult to mesh geometry, and you only need to run a single instance of linear static on a strong machine… using insane amounts of TET elements may actually be a smart choice… computer will sweat, but you can read a book in the meantime!
If you do that though: don’t forget about mesh convergence!
Why is the triangular element stiffer?
Ach, this is a good one! I actually wrote a post about it – read it here!
What are nodes and elements in FEA?
I guess that would be the “origin” question for today’s post! Why we need nodes and elements and “what they do” is a long story – read the whole thing here!