When to ignore geometric nonlinearity?

Linear FEA calculations are the most common type of static analysis done with finite elements. Last week we have discussed when it is safe to ignore material nonlinearity to use this simple yet robust tool. Today I will describe when we can safely ignore material nonlinearity.

A short remainder

There are several things you should consider when you want to use linear static design. We won’t discuss dynamics here, but “linear” means that you are omitting some key things in linear FEA.

Depending on whom you ask there are several “aspects” that can be treated as linear in the analysis:

  • Material – an obvious choice. I think that most engineers automatically think about material nonlinearity when they are asked what nonlinearity is. This is a big thing, as there are many different material models available and a lot of settings needed. It is good to know when you can ignore this effect and simply use the linear material.
  • Geometry – second obvious aspect. Nonlinear geometry can help you with buckling design or second-order effects in the analysis. Unfortunately defining a case usually takes some time, also computing alone is much longer. This makes it seems like a great idea to wonder when you can avoid all this trouble safely!
  • Contact – this is a tricky one. Depending on the source you may have issues to determine if contact is always nonlinear, or can it be linear as well. I won’t take part in the discussion about definition – I hate argues about semantics! Whatever side of the fence you will take, contact can be nonlinear – so we will try to answer when ignoring it makes sense.
  • Follower forces – this is a relatively small thing. If this is a “nonlinearity” at all again is a discussion I would say. If we will “clear” geometrical nonlinearity we are certain that deformations in the model are small. In such cases, it doesn’t really matter if the loads follow the shape of the geometry or not. This would play a role in geometrical nonlinear analysis, but we are staying in the linear zone today.

As I mentioned before, last week we have discusses when it is safe to ignore material nonlinearity. Today I will shortly describe when you can ignore geometric nonlinearity. Since follower forces are closely connected with geometric nonlinearity they come “free” with this topic!

When can you ignore geometrical nonlinearity?

This is a very tricky question. If you know how geometrical nonlinearity works you understand that it is more subtle than material nonlinearity. The easiest way to check would be to perform a geometrically nonlinear analysis and simply compare the outcomes. Of course, that would be a very ineffective check. There are easier ways to do it, even if they require certain experience.

The easiest would be to perform a linear buckling analysis. If you want to learn more about it, you can try my free online course:
Usually, when something is susceptible to nonlinear geometry (large deformations) it is connected with small bending rigidity. The analyzed element cannot withstand the load in a “rigid enough” way and change the “form” in which it carries the load. Such effects will result in a low eigenvalue from Linear Buckling Analysis (LBA). If you have certain experience and you know what you are looking for, analyzing LBA outcomes seems like a great start.

To be more specific you should be cautious when the eigenvalue of your model is smaller than 10. This is a “popular” value. It is even listed as one of the checks in Eurocode 3 for steel structures. This code also mentions that if you are using the plastic design you should aim for eigenvalues higher than 15.

A (not so) simple LBA example

I’m always reluctant to give such information without further comment. You see – this is not a “perfect solution”. I will show it on a simple example. Imagine you are designing a steel truss with reasonable beams. All checks according to EC (including buckling of elements) are ok, and capacity ration is maximally 0.96:Truss example on when to use linear FEA

For short members in compression limit capacity is around 2-2.5 times lower than ideal Euler force (due to imperfections etc.). This means that if you have a simple truss you will get a lot of eigenvalues around 2.0 – 2.5. To be exact first… 96 forms have eigenvalues between 2.01 – 5.4 that look more or less like this:

First eigenmode of a 3D truss

This doesn’t mean however that your truss is susceptible to large deformation… even though this seems so based on the criteria I just described. It is, of course, easy to prove. All I have to do is to make a linear calculation. Note that the maximal deformation is 64.4mm (maximal capacity ratio as mentioned above is 0.96):

Linear static calculation of a 3D truss (linear FEA)

Then I will do a geometrically nonlinear analysis. Note that maximal deformation is 67.8mm:

Geometrically nonlinear analysis of a 3D truss

The maximal capacity ratio is in this case 100%.

In summary, I got almost 100 eigenvalues below 5.4 which are far below recommended 10 (lowest being 2.01). This would suggest that nonlinear geometry should be significant in the model. This is however not the case since with nonlinear geometry both deformations and stresses increased around 5%. Not an astonishing change isn’t it?

This is the problem with geometric nonlinearity – it requires experience to spot when it can be ignored. This is why I usually use geometric nonlinearity calculations in FEA… just in case. I still get surprised after 10 years of experience in FEA field! When using LBA for testing it is always good to check if your FEA solver includes warping-torsion commonly referred to as a “7th degree of freedom”. If you don’t have such possibilities, your LBA won’t be able to find lateral torsion buckling in beam models. It will work just fine in plate/shell/solid models through.

Check deformations!

Another good idea is to fulfill code criteria for maximal deformations. Sure there are no criteria for many elements. Luckily you can find similarities of what you are calculating to other defined cases. This way when you know you are within “allowable” deformations for your type of structure this means that you are safe from large deformations problems (unless the code you are using defines it differently of course).

Usually, those criteria provide allowable deformation. Usually, this is the length of the element divided by a certain value (like L/250). Such approach is very common in civil engineering. According to Eurocodes such checks are called SLS (serviceability limit state). When you do those checks just remember that for cantilevers the allowable deformation is twice as high!

When I’m in doubt about what limit to use I follow a simple guideline:

  • If element is “unimportant” I go with maximal deformation of L/200
  • If this is something that can go into membrane state (thin plates i.e.) I allow L/150 (sometimes L/200)
  • For more important elements (that should be rigid) I would go with L/350
  • If deformations aren’t allowed almost “at all” to me that would mean L/500 or in extreme cases L/1000

The above are just a rule of thumb obviously but should give you the general “range” of allowed deformation.

5% strain

In a Linkedin discussion, a friend of mine Leonardo Rosa pointed out that there is a popular “5% strain” rule. According to it, if in the linear analysis you get more than 5% strain you should perform a geometrically nonlinear analysis.

Definitelly an interesting concept – it never hurts to make this additional check!

Summary

To check if you can ignore geometric nonlinearity:

  • Do the LBA analysis – if the lowes eigenvalue is higher than 10 (elastic design) or 15 (plastic design) you are most likely fine.
  • If the lowest eigenvalue is lower than the value above be careful. This does not mean that you have to use geometric nonlinearity, but it is worht tryng.
  • Check deformations from linear static – they should fit into allowable criteria.
  • If you can ignore geometric nonlinearity, you can also ignore follower forces.
  • If you are not sure use geometric nonlinearity – better to wast time than be sorry later!

Want to learn more?

This is great! I have a free nonlinear FEA course just for you! Subscribe below to get it!

If you enjoyed the post you can share it with friends – that would be a great help! If you have a spare 15 seconds write a comment with your thoughts on the matter or any questions you might have. I have a good history of replying to each and every comment 🙂

Free nonlinear FEA course!


10 Comments

  1. Nikos June 13, 2017 at 8:41 am - Reply

    So illustrative again! Thank you so much for this blog Lucasz!

    • Łukasz Skotny June 13, 2017 at 9:15 am - Reply

      Nikos!

      I’m very happy that you like it 🙂 All the best 🙂

      Ł

  2. Jouni June 15, 2017 at 11:04 am - Reply

    “To be more specific you should be cautious when the eigenvalue of your model is smaller than 10. This is a “popular” value. It is even listed as one of the checks in Eurocode 3 for steel structures. This code also mentions that if you are using the plastic design you should aim for eigenvalues higher than 15.”

    Hi, in which sections of Eurocode are the values 10 & 15 mentioned? Thanks!

    • Łukasz Skotny June 15, 2017 at 12:29 pm - Reply

      Hey, Jouni!

      Values are given in EN 1993-1-1 (Steel Structures: General rules and rules for buildings) chapter 5.2.1 (equation 5.1).

      All the best
      Ł

  3. Przemek June 18, 2017 at 12:51 pm - Reply

    I have known different “5% strain” rule. EC3-1-5 C.8 limits maximum plastic strain to 5% assuming everything should be ok then… Have I misunderstood the concept?

    • Łukasz Skotny June 18, 2017 at 2:09 pm - Reply

      Hey,

      I think this is something else. There is a limit for allowable plastic strain in certain structures. Simply put you are not allowed to have a higher plastic strain at all.

      Here it is like this: If you make a linear analysis and total strain is 5% or higher use nonlinear geometry. This is something different, especially since you cannot obtain plastic strain as an outcome from the linear analysis.

      All the best
      Ł

  4. Dragostin September 17, 2017 at 1:37 pm - Reply

    Great discussion for structural engineers dealing with this problems daily! Keep up with the proffesional work! Greetings from Bulgaria 🙂

    • Łukasz Skotny September 17, 2017 at 5:14 pm - Reply

      Hey, Dragostin!

      I’m very happy that you like it, thank you for the kind words!

      If you have any questions about FEA and engineering let me know – I will gladly answer them in my QnA posts 🙂

      All the best
      Ł

  5. J. Voermans March 4, 2018 at 7:15 pm - Reply

    Hi,
    Pls distinguish global stability and local stability in your story. alpha_crit > 10 relates to global stability where the compressed upper chord of your truss wants to buckle as a whole.
    Regards,
    Jurgen

    • Łukasz Skotny March 5, 2018 at 4:08 am - Reply

      Hey!

      This is a good point, but sadly hard to cope with. “Global” and “local” tend to have a lot of meanings. I.e. local stability is not a stability of the “member” but rather a web of the element in class 4, or web over the support. Something that happens in the “portion” of a beam. While global stability can be a buckling failure of the column (from the column perspective) or of a frame (from a frame perspective).

      With this in mind buckling of the diagonal in a truss can be treated as global (entire member buckles) and local (piece of a truss buckle). I haven’t found yet a definition that would satisfy me. This is an issue with semantics, and in engineering, I usually don’t like to divide stuff into subcategories. Buckling is what it is, regardless of how we would call it. Sure, when I design a structure I know what types of buckling I have already “covered” with equations… and I simply ignore those eigenvalues (I even check with them if my calculations are ok). So here I agree with you. Sadly I don’t really know how to precisely describe what is “global” and what is “local” – do you have a satisfying definition? I would love to hear it!

      About your truss example, this is how I see it – I would love to know your opinion:

      The upper chord of a truss will buckle in the middle of the span between bracings (or in-plane depending on setup). It won’t do it “as a whole” unless you don’t have any bracings out of the plane which doesn’t happen all that often. This would mean that it can also be treated as “local” stability (part of the element buckled). Not to mention that in-plane it will always buckle like that… so if no bracings were present it would buckle locally in-plane and globally out of the plane?

      To sum this up:

      I know in my gut what people mean when they call something “global” in a specific situation. Then it is easy. When we are talking about a column local is a web failure in class 4, and global is entire column buckling. In a frame, global would be buckling failure of the frame… but I’m unsure if calling a column buckling “local” in this setup makes sense. I wouldn’t worry however about calling a diagonal buckling in a truss “local” when we discuss a big truss… tricky stuff isn’t it?

      Let me know what you think : )

      Thank you for dropping a comment – great stuff!
      Ł

Leave A Comment

Do NOT follow this link or you will be banned from the site!