I have managed to make my model converge fairly well and achieve large displacements and deformations. It exhibits stress and strain good continuity by solving it under small displacement and deformation assumption. In other terms, engineering strain is computed instead of Green Lagrange strain, stress tensor is Cauchy and not Piola Kirchhoff, and material frame is associated to spatial frame.

I know the small displacement/deformation assumption is only for no more than 5% strain, but actually, the strain reaches 50% ; it moves 1cm into an 8cm solid box.

I know also that every single FEM can only be an approximation of reality.

What can I expect about the validity of the model ? Does it mean absolutely nothing because it is quite nonsense (but the only thing is that the error is highered) ?

  • 1
    $\begingroup$ The way I see it is, if you're using a model under certain assumptions and yet those assumptions aren't met, then you should be expected more error than the error the FEM would give you alone. It might be very wrong or only slightly incorrect, depending on your problem. Based on how large the strain is relative to the strain assumption of the model, I would suspect the results aren't really a good predictor for reality. $\endgroup$
    – spektr
    Commented Jul 21, 2016 at 16:33
  • 1
    $\begingroup$ If you change the length of a 8cm box by 1cm that would be a 12.5% strain rather than 50% strain wouldn't it? Even so, the error in the solution based on a small-strain assumption is likely to be very large. Beyond the error due to the small-strain kinematic relations, there will also be significant errors due to the incorrect modeling of the material behavior (you did not state the material of your part). $\endgroup$ Commented Jul 21, 2016 at 17:17
  • 1
    $\begingroup$ @BillGreene You're right, it's actually 1mm into something like 4-5. My material is assumed to be linear viscoelastic. Do you have an idea how can I at least measure the error ? $\endgroup$ Commented Jul 21, 2016 at 18:58
  • $\begingroup$ @Blue_Elephant, solve a problem you know the answer to using the Method of Manufactured Solutions or an analytical solution. $\endgroup$
    – Bill Barth
    Commented Jul 21, 2016 at 19:40
  • $\begingroup$ Without knowing more, it is difficult to say. How is that you happened to be using a FE formulation that seems to be so ill-suited to the particular problem you are trying to solve? Is this an assignment where you have to implement your own FE code? If you are a student, do you have access to any commercial FE solvers e.g. Abaqus? $\endgroup$ Commented Jul 21, 2016 at 23:59

2 Answers 2


I know also that every single FEM can only be an approximation of reality.

By the FEM you just obtain an approximation to an (hopefully) well posed problem.

Logical steps are as follows.

  1. You first set a problem by choosing appropriate equations (congruence, constitutive equations, balance), a geometric domain, material constitutive parameters, and appropriate boundary and initial conditions. If the problem is well-posed this defines a unique solution $L$.
  2. By the FEM you obtain an approximation $L_\text{FEM} \approx L$.

The small strain/displacement assumption affect the equations that define $L$ (in the sense that you end up with a set of linear congruence and balance equations), and presumably you have a well-defined problem, and therefore are able to easily compute a converged solution $L_\text{FEM}$.

The real question is if $L$ is physically meaningful or not, and of course this question has nothing to do with the particular method you used to compute an approximation to it. This is a question about the equations you are going to solve: are they able to model the physics of your problem?

It is impossible to answer this question without analysing your specific problem and your solution. However in general it is very dangerous to apply continuum mechanics equations outside their domain of validity: why a solution $L$ defined under small displacement assumptions should be physically valid for finite displacements? In my own experience this is almost never the case, apart from some trivial problems.

The equations of linear mechanics can be presented as the linearisation of more general non-linear equations. Intuitively this means that you search for a solution on the tangent to a curve, instead of for a solution on the curve itself: you can make a strong point about the fact that you will end very far from the correct solution.


When you mention the convergence of the model, do you mean that you have used some form of iterative method? In that case, it is likely that you were using some non-linear model (unadvertely?).

The following is a list of possible non-linearities one can encounter based on the ubiquitous "Governing Equations":

  • System's internal balance equations (Statics or dynamics)

       Nonlinear damping
  • Constitutive equations (Material)

  • Kinematic equations (Geometry)

       Large deformations with small strains
       Large strains
  • Boundary conditions

           Link rupture

As you can see, large strains (the problem that you seem to be studying) is only one of the many cases where the assumption of linear behaviour just limits the validity of a model. In the image below, you can see that the linear hypothesis is valid only within the orange triangle. If you were to continue pulling the spring assuming that your real behaviour is on the line, the amount of energy that you would be creating from 'nothing' would grow quadratically once you enter in the non-linear regime.

Strain energy of a stress experiment

FEM is generally formulated on variational principles (balance of energies), so (in my opinion) the error should be accounted for in the energy level. In this case, your error would grow in a quadratic form.


Your Answer

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

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