Since we have started having frost nights here in Sweden it came to me recently when I started looking over my tools required for shifting tyres on the car that I lack “trestle jacks” or any type of jack stand. Having buckling on my mind I also started wondering how the requirements regarding such equipment looked in terms of buckling dimensioning -wouldn’t want to have my hands under a 2 tonne car… A less severe example of when buckling comes into play is if you ever have had the misfortune of trying to push in a straw in a carton only to have it fold and crease instead of penetrating the plastic?
Both of these cases are occurrences of buckling. I.e. the sudden collapse of a structure when little to no increase in force results in large deformations. I bet there are other definitions, but in regards to structural analysis I think this one is on point. So, to present means of how the above situations can be modelled this blog post will sort out how to analyse buckling in Simcenter 3D using Simcenter Nastran.
Besides dimensioning structures to make sure the components will not yield under the applied loads it is also imperative that one controls other failure modes as well: buckling being one of them. If we restrain ourselves to linear analysis then the investigation ends with a SOL105 (linear buckling) in Simcenter Nastran and we just dimension the structure not to be at risk of buckling, usually by applying some safety factor. However, sometimes we want to go further.
Having knowledge of at which load a structure will buckle and how the buckled shape looks like we can proceed in investigating more closely both the more realistic load at which the buckling failure will take place (performing a limit load analysis), additionally we can look at the resulting post buckling behaviour, or deformation. This can easily be done in SOL401 (multi-step nonlinear solver) using a nonlinear buckling subcase.
The Most Simple Case: Euler’s Buckling Formula
Starting of with analysing the linear buckling of a 1 m tall UPE100 column we can use the well known Euler buckling formulas for columns to estimate the buckling load of the UPE column:
According to Euler’s formulas the UPE100 column should buckle for a compressive load of approximately 210 kN. The somewhat lower figure when using K = 2.1 should take imperfections and material uncertainties, which will reduce the stability of the column, into account.
Ramping up Complexity – Using FEM to Solve a Linear Buckling Problem
Now let’s set this up in SC3D and solve it using Simcenter Nastran. The way Nastran treats this is to turn it into an eigenvalue problem by adding the differential stiffness, [K_d], of the elements to the stiffness matrix, [K], as seen below in (1):
Next recognising that the internal energy, U, will be depending on the stiffness matrices and the displacements, u, of the structure -one can formulate a condition which must be true if the structure is stationary, (2). From (2) we can work the expression by knowing that the differential stiffness will be dependent on the applied load, P_a, (3). Finally, we arrive at the eigenvalue problem in (4) by stating that the critical load, P_cr:i, will be a multiple of the applied load. This multiple, λ_i, will be the eigenvalues of the equation in (4) of which there will be as many as the degrees of freedom, N_DOF, in the model.
This was presented in a simplified manner and in the Simcenter Nastran Users Guide you can read the full documentation, but it gives you a hint why you are forced to specify an eigenvalue method and a number of eigenvalues for which to solve. Moreover, it also gives an explanation for why the critical load will be the given eigenvalue multiplied with the applied loads. I write loads since the system of applied loads are considered, which can be a good reminder if you have several loads affecting your structure.
Some limitations in using SOL105 and resorting to linear buckling is that deformations are assumed to be small and material nonlinearity is not considered so element stresses must be elastic for the applied load. As a rule of thumb, the loads should not impose visible deformations on the structure, and the maximum stress should be below the material yield stress.
Moreover, a recommendation of 5 grid points per half sine size is also made for Nastran to capture the stiffness of the structure with enough accuracy. Compare this case below where a 4 m column is analysed with 250 mm mesh size and 1250 mm mesh size (in the red boxed image). For the first mode the shape is similar, but the load multiplier differs significantly (boxed in black). For higher order modes the shapes differ as well.
Defining a linear buckling solution – SOL105
As we will see in the video below what we require to set up a linear buckling solution in SC3D is first of all a FEM. Having a complete .fem file we can create a new .sim and define a SOL105 solution. When defining the SOL105 we can choose what subcase it should be using for calculating the differential stiffness and if we have any pretension subcase. For the SOL105 definition of the eigenvalue extraction method is also set. In the Simcenter Nastran User’s Guide they recommend the subspace iteration or the implicitly restarted Arnoldi method since “…when compared to the enhanced inverse power and the Lanczos methods they are: Computationally more efficient when you want to calculate a small number of eigenvalues, which is typical in a linear buckling analysis because only the lowest buckling loads are of any practical interest.”
Having created the solution we need to define boundary conditions after which we can solve.
As can be seen in the video the resulting eigenvalues are written out as load multipliers to give answer to when the system loads will trigger instability in the structure. The lowest eigenvalue provides a multiple of 200.67 which is to be multiplied with the applied load of 1.00 kN which results in a critical load of 201 kN. Just in the middle of the values predicted by Euler’s formula.
Use Modal Displacements to Create Initial Imperfections
Having an answer to when the structure will buckle under these linear assumptions we can take it one step further. This first analysis tells us how the structure likely will deform (buckle) under high enough load. We can impose the buckled shape on the structure as initial imperfections to “guide” it into the that specific instability mode. One can think this justified as we found out from the linear case that this is the lowest eigenmode and therefore buckling failure in any other shape is not feasible. Having eigenvalues close to each other could change this reasoning, and usually this is handled by norms when dimensioning for instability.
To impose initial imperfections the easiest way is to create a Field from the SOL105 analysis results
- Load the result from which displacements are to be saved
- Tools → Create Field From Results
- When creating the field you can choose either Node ID or Cartesian as independent domain. Using Cartesian enables you to use a different mesh when applying the imperfections. For the dependent domain Cartesian should be used.
Tired of Going Simple – Post Buckling Behaviour
Now having a obtained a field for initial imperfections it is time to define a new solution to look at the post-buckling behaviour. SOL401 provides excellent functionality to do so. This way we can obtain a more realistic value of when the structure is likely to buckle, and we can also see the shape of the buckling failure.
By adding a nonlinear buckling subcase we gain the opportunity to control both the loading and the displacement increment to traverse our intended equilibrium path. -Fancy word, but it means that we are trying to find combinations in space where the external loads, F, will be in equilibrium with the internal forces originating from displacements, u, of the continuum. What the Arc-Length parameters in the nonlinear buckling subcase provides are means of tweaking the allowable load and displacement increment in the step such that our simulation follows the intended load path in F-u space. For a single degree of freedom you could think of it as shown below where we want to follow the line (the equilibrium path) but due to e.g. buckling we reach so called limit points. If we use a force-controlled simulation reaching x will pose great risk of snapping through to x’. Trying to handle this situation we might revert to a displacement-controlled simulation to reach y, but doing so will risk that we end up in y’ skipping the path in-between.
To solve this, arc-length methods provide bounds for the solution much like the striped circles (need not be circles, but it provides a relatable example) in the plot so that the load and displacement cannot take too large increments per each step (cannot reach outside of the circle). This avoids the snap-back behaviour. Additionally, these methods provide means for the solution not to start going backwards as the circle will certainly intersect the equilibrium path at least twice. This is explained in greater detail in Simcenter Nastran Multi-Step Nonlinear User’s Guide (SOL 401 and SOL 402) or in textbooks such as Nonlinear Solid Mechanics for Finite Element Analysis: Statics by J Bonet, A. J. Gil and R. D. Wood.
In the video below you can see how a nonlinear buckling subcase is set up in SOL401 using SC3D:
The nonlinear buckling case needs to have large displacements enabled and it is required for it to have the end time of the last preceding subcase (or 0 if it is first). One can think that the nonlinear buckling subcase is happening during a single time period where you are enabled to see the collapse of the structure. In this example material nonlinearity was not activated and likely the structure would collapse slightly sooner due to the high stress in the flanges. However, the graph of the load factor (ratio of the maximum load applied) vs. displacement of the top node of the column shows buckling initiating around 95 % of the maximum load, i.e. at 191 kN. So, including initial imperfections we get a strikingly similar result as to the hand calculation with an effective length factor of 2.1, which is recommended to be used in dimensioning of the column. Pretty neat for a formula which fit on the back of a napkin.
This post was made using SC3D version 2506 and I hope it was helpful for you. If you have questions related to the content reach out to us at support@volupe.com.
Viktor Hultgren, M.Sc.
Contact: support@volupe.com
+46 704 21 06 61
