(function(w,d,s,l,i){w[l]=w[l]||[];w[l].push({'gtm.start': new Date().getTime(),event:'gtm.js'});var f=d.getElementsByTagName(s)[0], j=d.createElement(s),dl=l!='dataLayer'?'&l='+l:'';j.async=true;j.src= 'https://www.googletagmanager.com/gtm.js?id='+i+dl;f.parentNode.insertBefore(j,f); })(window,document,'script','dataLayer','GTM-PM5M9PRG');
6 June 2017

# When to ignore material nonlinearity?

Linear FEA calculations are the most common type of static analysis done with finite elements. There are a lot of benefits to the method itself, but of course, there are risks involved as well. Today you will learn when it is safe to ignore material nonlinearity. I will also tell you what things you should watch out for!

## Linear FEA approach to static design

When your task is to assess the capacity of any given element/structure, you will automatically think about linear static. The name already suggests several very important things about calculations you are about to make.

Firstly “static” indicates that you don’t consider dynamic effects in the analysis. This is, however, a topic of its own and I won’t discuss it here.

What we will focus on is the “linear” approach:

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 avaiable and a lot of settings needed. It is good to know when you can ignore this effect and simply use 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 make 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 linear zone today.

Since you already learned what problems you must consider let’s discuss how to deal with them. Today I will describe material nonlinearity, and when it is ok to ignore it.

## When can you ignore material nonlinearity?

First of all, it would be great to understand what material nonlinearity does. In short, FEA calculates deformations of the model first. Then it calculates strain and based on this strain it calculates stress. If you follow Hooke’s law, the relation between stress and strain is linear. However, most materials show a nonlinear relation between stress and strain after the initial linear part of this relationship. This means that the initial material is “linear” but when strain gets bigger material starts to be “nonlinear”:

This means that when you define the linear case, you basically assume that you will always have “small strain”. Small here means that strain will never get high enough in your model to “reach” the nonlinear part. In essence, instead of a “real” material (marked in green below), you model a “fake” material (broken line below). In the small strain region, they have identical properties – so everything is well!

Unfortunately, there is no safety net here. If your model will get higher strains there are no “warning messages” – you will simply get unrealistically high stress. The mechanism of how the solver does those calculations is simple. Look at the schematic below. Assume that the analyzed point in your structure has a certain strain, higher than the “linear limit”. In reality, the nonlinear material would display stress marked in green. Since we are using linear material solver will “blindly” believe that the relation between strain and stress is linear and will produce a much higher value!

This is why you often get stresses in GPa instead of MPa in linear FEA. They are simply calculated with the assumption that stress always depends linearly on the strain.

## Material nonlinearity – summary

You can safely ignore material nonlinearity when strains in the model (and resulting stresses) do not go out of the “linear zone”. The further away you get from the limit, the worse outcomes you get.

Just be aware that such conditions aren’t met in many models. You need to be aware that there are stress concentrations in some places. In those regions, stress will reach higher values. Of course, it is best to use nonlinear analysis in such cases. There are however code rules and “best practices” that allow you to estimate if the stress you have obtained is “dangerous or not” even if it is higher than yield (or even higher than ultimate stress). Such analysis requires vast post-processing time (where you analyze outcomes by hand) but is doable and quite popular.

In essence, when you use linear material and the strains are high you will have to spend a lot of time on post-processing to check (according to various standards) if the stress is “acceptable”. Code rules are based on experience in this regard as there is no good way to build a mathematical model for such checks. In my personal opinion, if post-processing takes a lot of time it is more effective to use a nonlinear approach where all you need to do is to check capacity and maximal plastic strain.

Definitely check out my FREE FEA course. You can get it by subscribing below.

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.

#### Author:Łukasz Skotny Ph.D.

I have over 10 years of practical FEA experience (I'm running my own Engineering Consultancy), and I've been an academic teacher for a decade. Here, I gladly share my engineering knowledge through courses, and on the blog!

### Get my 1h video Lecture on Nonlinear Material

Your personal data administrator is Enterfea Łukasz Skotny, Skrzydlata 1/7, 54-129 Wrocław/POLAND, Email. By subscribing to the newsletter that includes marketing messages you consent to your personal data processing in accordance with this privacy policy

### Join the discussion

Martin - 2023-02-24 12:28:26

Hi Lukasz,

in my daily work I come often to the point to use a nonilearity material model.
In my opinion, there is no way around a nonlinear calculation in order to fully exploit the limits of feasibility.
Which standard or maximum values do you use for the evaluation of nonlinear analyses? There are significantly fewer standards available here, aren't there?
I think below 3% plastic deformation everything is uncritical.
Regards
Martin

Łukasz Skotny Ph.D. - 2023-02-28 11:04:13

Hey Martin!

Thank you for writing :)

In my experience, there are just as many "linear" and "nonlinear" codes out there. The "nonlinear" parts are just shorter and easier to understand :)

Many codes that allow FEA for design will usually have a chapter about nonlinear calculations. Be it Chapter 5 in ASME VIII div. 2 or Annex B in EN 13445-3 or straight out most of EN 1993-1-6 (that doesn't really allow Linear FEA at all!). So I would say that the selection is big, to be honest. And for the most part, the nonlinear rules are "similar" in nature (while values of course change code to code, the "workflow" almost always stays the same). If I would have to learn "linear rules" from all the codes I'm using... I would most likely go crazy :)

As for specific plastic strain limits, this, of course, depends on a lot of factors, like what material you are using, what ruleset, if fatigue will be a problem, and how many load cycles are expected, etc. But in most cases, for "normal" structural steel without fatigue, 3% plastic strain would be a very reasonable call.

All the best!
Ł

Vikrant - 2021-10-01 12:36:51

Hi Lukasz!

Great article, thanks! Do you also have an article about "second order effects" that you mentioned in the geometry? Or any source as simple/interesting as yours :-)

Best,
Vikrant

Łukasz Skotny Ph.D. - 2021-10-01 17:55:55

Hey Vikrant!

Thank you for the kind words!

Sadly, I don't think I did such a thing for "second-order effects", however, based on your question you are doing beam/member steel structures aren't you?

I don't think that second-order effects will make the calculation super longer (I mean, the difference between linear and nonlinear will be there for sure, but we run analysis here that take several hours each, I don't think you will get there unless you have HUGE models in beams). That being said, if you use 2-order and it has no influence... it won't influence the outcomes... if it does have influence, you will have that in your analysis... and all of that almost for "free" with just a bit more computing time!

I think "blindly assuming" that you should take second-order into account is actually a good strategy, as verification if you really need that will most likely take longer than the computing time you are trying to "save" :)

All the best!
Ł

Venugopal B - 2021-05-17 13:58:40

Hello sir,
It is very good post. However, I have few questions to ask.
1. composite materials has different S-S curve in different directions. Which one I need consider for material nonlinearity.
2. It's very hard to separate elastic and plastic regime in GFRP S-S curve. How can I do that?

Thank you very much
regards
Venugopal B

B.Jacobse - 2020-09-08 07:07:46

Hey Lukasz,

Thank you for sharing your idea! The goal of my research is to check whether the layer of hardwood is damaged by the load of the ship. So as the keel of the ship rest on the dock blocks the soft wood is compressed, however if this displacement is too large the hardwood will be damaged as well. To distribute the load on the softwood a steel plate is often placed on top of it. Indeed, the assumption to model the whole keel of the ship as a beam is a simplified start, from this point I'll add the complexity of the ships weight distribution. I was wondering if could use the same DNV approach as you discussed before to model the non-linearity. So basically what I ask is if in this case I check whether the load is exceeding the linear limit and I evaluate the stress-strain graph from this soft wood. Indeed as you mention the grain is of importance and I will take this into account. For me it is difficult to see how the non-linearity in the softwood behaves and how I should model this.

Thank you for sharing your thoughts with me, very interesting to hear your point of view!

Best regards,

Bart

Łukasz Skotny Ph.D. - 2020-09-09 06:37:27

Hey Bart!

Starting with a super-simple model just to see if all of the important "components" work is always a good idea!

Sadly, when it comes to the stress-strain curve for wood in various directions of grain... I simply don't have any answers for you. Heck, I don't know anyone I could ask about such things either, but I hope there are answers out there. Someone had to search for that in the past I think, so you will have to simply find that person or their work.

You mention 'research" - if you are at Uni, try web of knowledge (the elsevier thingy where you can search for scientific articles) - maybe something interesting will come up!

All the best, and good luck! Definitely let me know when you find something!
Ł

B.Jacobse - 2020-09-07 11:41:44

Hello Lukasz,

Currently I am investigating the loading on dock blocks for ships. As these blocks are build from different layers of different materials I'm planning to model a beam of different layers as well. So the ship will be modeled as a beam, the bottom layer of the dock blocks are made of concrete and will be assumed rigid and therefore also modeled as a beam. The problem arise in the top 2 layers, respectively soft wood and hard wood. These layers will be modeled as a spring damping system between the two beams. My question is how to take the non-linear behavior of the soft wood into account in my model. I want a precise prediction of the displacement of this layer, in this way damage on the hard wood will be prevented. Hopefully you can help me with the non-linearity of the wood and the approach to be taken.

Łukasz Skotny Ph.D. - 2020-09-07 19:05:32

Hey Bart!

I'm so sorry Mate, but I will disappoint you. I never worked with wood on anything "real". I can assume that this is a rather complex topic, but what struck me is that you will model an entire ship as a beam... I most likely simply do not understand what you are up to, but this sounds odd to me. I'm first to admit that I never did any naval work so maybe this is something like "how to assess rigidity of the support or something similar".

I guess that both hardwood and softwood have different young modulus - that would be the first iteration right? I'm not sure how much you want to go "in" the complexity of wood modeling (considering that the ship is a beam) but I'm pretty certain it is not the same whether the load is along or perpendicular to the grain (I would bet that Young Modulus change too). Then, there is the splitting of wood on impact, maybe even buckling of the grain (I admit this is a rather sci-fi problem, but hey!) but those would be complex phenomena for sure - maybe different Young modulus is enough?

Let me know what you think about it in the spare time - I'm pretty curious how the whole thing works, and it definitely sounds intriguing :)

All the best!
Ł

Sandeep P - 2020-05-19 09:20:35

Hello Lukasz,

To model material non-linearity we can proceed with Bilinear isotropic hardenig (BISO) or Multilinear isotropic hardenig (MISO). right? by aproaching with MISO is fine to me till now.

But, if i want to go with Bilinear isotropic hardenig (BISO) approach. it needs tangent modulus value. right?
so to get this have you have any calculation/formulae for this. please share.

Łukasz Skotny Ph.D. - 2020-05-19 16:50:52

Hey!

I think it is best that you check your FEA solver manual. Usually, the show very effective ways to calculate parameters and where to get them from. I try not to say what to input in any given field in software I don't know, as sometimes they don't ask you "directly" about value but about some parameter derived from that value... so it's always better to check in the solver manual :)

Hope this helps!
Ł

Sandeep P - 2020-05-21 04:43:53

ok, i will try to check

Łukasz Skotny Ph.D. - 2020-05-24 09:48:09

Awesome,

If you won't understand something from that let me know - we will work this out :)

All the best!
Ł

Sandeep P - 2020-06-22 09:27:43

Sure Lukasz. thank you

prashant - 2018-04-05 17:39:33

should we add material non linearity in composite materials? As it doesn't have any yield stress.

Łukasz Skotny Ph.D. - 2018-04-05 17:51:49

Hey!

This post is geared toward yielding materials. However, there can be different forms of nonlinearity (yielding is just the most popular one). If the material you are using display nonlinear dependency between stress and strain (and it is not "almost linear" for practical purposes) you should use nonlinear material.

Have a great day!
Ł

Tien - 2017-11-01 23:08:12

Hi Lukasz,
This means if the equivalent stresses everywhere in the model is below the yield stress, then we don't even need to worry about material nonlinearity ?

Łukasz Skotny Ph.D. - 2017-11-01 23:16:58

Hey Tien,

In most cases... yes :) There are of course materials that have nonlinear behavior not necessarily connected to yielding but then you will know how much "linear chart" you have before you reach the "nonlinear" territory. Yielding can also have several criteria, so one should be careful when calculating equivalent stress - but if done right, I would say you are right :)

All the best
Ł

Sandeep - 2017-08-31 16:56:41

Good article and very valuable information for the complicated subject of non linearity..

Łukasz Skotny Ph.D. - 2017-08-31 17:50:44

Hey, Sandeep!

I'm very happy that you like it!

All the best
Ł

yudhi - 2017-06-10 05:27:48

Hi Lukasz,

Thanks for sharing this post. It helps me to get better understanding when dealing with non-linearity in FEA. i have two questions related to this non-linearity, if you dont mind to share your thought based on your expertise.
1. lets say we're dealing with non-linearity, we need to put stress-strain data based on test result to our FEA program or develop this data (i saw people use ASME BPVC method to generate stress-strain curve). some software demand the input data in nominal stress vs nominal strain, but some also demand yield stress vs plastic strain, in which we have to translate to match FEA software demand.
Given we got the raw data in metric unit, rather than USC unit, i.e. stress [MPa] vs strain [unitless, but most probably in mm/mm]. is that okay if we convert it directly into PSI vs [- or in/in] given i want to get the result in USC unit. We only need to convert MPa to PSI, as strain is unitless. the translation process will follow USC unit afterwards.

2. Is it useful to enter density value? Lets say for linear static case, most tutorial that i saw, define elasticity modulus and poisson ratio is enough for this type of analysis. Do you have some thought for density value?

Łukasz Skotny Ph.D. - 2017-06-10 08:41:59

Hey Yudhi!

I'm glad you like the post ;)

1. Strain, as you said, is unitless - so when you define stress values in psi you will get a stress-strain chart in USC units. This follows a simple logic - in the tensile test you get force and elongation. This elongation is then divided by the length of the "base" of the model. If you measure 10mm of deformation in 1000mm long base the relative deformation (strain) is 10/1000 = 0.01. If you would measure the same in inches the elongation would be 0.394in and the base would be 39.4in. The relative deformation (strain) would be the same (0.394/39.4 = 0.01). But force divided by area is unit dependent, so you need to choose a correct unit to measure force/stress etc.

2. Density on its own is useless. You can also define acceleration (gravity) and such action will define a self-weight (you have volume with density and proper acceleration). Usually, however, self weight of the element is not the most important aspect. Ie. when I model a steel connection which is heavily loaded (to check force distribution in bolts) self-weight of the connection itself is irrelevant to the case. However, if I would analyze a big structure then self-weight might be important. It is very case dependent, when you feel like the self-weight might be important define density but also define proper acceleration!

All the best
Ł

Varun - 2017-06-08 18:05:57

Hi Łukasz,

Wonderful summary to brush up the fundamentals of FEA engineers. I have a question about material properties, particularly of plastic - PA66. I have the stress-strain curve of the material. What I do not know is if these are nominal values or true values. How do I verify these except asking the plastic supplier?

Łukasz Skotny Ph.D. - 2017-06-08 18:17:17

Hey Varun!

Thank you, I'm glad that you like the post.

About your question: I haven't used plastics in FEA as I deal with structural steel mostly (but I hope to go there in future as there are some fun buckling cases there :) ). At this point, I need to ask what do you understand under "nominal" or "true" values.

If by nominal you understand "engineering stress-strain" (as opposed to "true stress-strain") there are 2 ways I think:
1. If those were taken from a tensile test that would *most likely* be an engineering stress-strain. Sure someone could do the job and "translate" test results to "true strsss-strain" but I don't think it is a common practice...
2. Engineering stress-strain will drop down at some point because of the necking. True stress-strain will always be rising.

If you think about "nominal" as values that you can use in design (as opposed to "true" values taken straight from the test) there is no way of knowing that. The difference will be in statistics. Of course the "nominal" values will most likely be a more "smooth" line, but in plastics, as far as I know, the line is smooth anyway so this is not a perfect test. Apart from that maybe check if the curve consists of "straight lines". Usually, values for design tend to be curves consisting of straight lines to simplify implementation. This is, however, a long shot...

I hope this helps you a bit :)

All the best
Ł

Martin Cibulka - 2017-06-06 08:47:17

Hi Lukasz, Grear content as always. My question is how do you check capacity and limit strain? I tend to use from the Eurocode 5% plastic strain limit with stress limited to ultimate capacity. I suppose what I am trying to figure out is if by capacity you would look at global and local buckling of steel plates and how to do local buckling check as global I do via stability calc.
One more question is whether there is a way to account for plasticity in concrete to avoid peaks in reinforcement design?

Łukasz Skotny Ph.D. - 2017-06-06 13:35:23

Hey, Martin!
Thank you for kind words!
1. I usually use recommendations from DNV RP-C208 - there is a full stability path there and also recommendations for limits in strains. Try that :)
2. It is hard to answer the second question - what do you mean by "stability calc."? You mean line LBA (linear bifurcation analysis)? I usually do nonlinear buckling analysis and it takes local and global effects into account (of course if you are not using beam models). With beams, there are hand calculations you can make if you are not interested in building shell models :)
3. Peaks in reinforcement design are irritating - I would try to model supports (walls and columns) with actual width instead of lines or points - this should greatly help out and some software have such possibilities. I'm not sure about the concrete plasticity - I don't do those designs very often, and it never came up in any of the designs. I think you would have to make some tests in the soft you run to solve those problems - that is the most reasonable way.

All the best
Ł