How to set up geometrically nonlinear analysis

Have you ever performed an analysis that did not converge, or that ended with the result you did not expect? Many of such problems are resolved with correct solver settings, and today I will discuss how to set an arc-length geometrically nonlinear analysis of a shell. This means we will do a nonlinear buckling problem from scratch!

Before we start a checklist of things worth knowing before starting this tutorial:

• I will perform a geometrically nonlinear analysis (commonly refereed to as “nonlinear buckling”).
• Nonlinear buckling is a completely different procedure than linear buckling as described here.
• Model I will use is described here (with all geometry data and needed informations and Femap video-guide).
• I already did a mesh optimization study.
• Here is a guide on how to interpret results from such analysis with stability path.
• I shared with you the most common mistakes in such analysis.

Since I have already decided that I want to use the arc-length method to trace the stability path now it is time to set things up. Arc-length methods in most solvers require few parameters in order to work properly.

Arc length method parameters

• Initial step definition – in many solvers this is organised differently but goal is simple: define how big step should be done in the first increment of the analysis, since solver won’t have any history to base on.
• What are the convergence tolerances for each iteration (usually default settings of your solver suffice)
• Rules for analysis termination (since you want to trace failure most of the time, reaching target load is rarely an option, as model will be destroyed before that load)
• Rules about increasing and decreasing load increments

How to Reasonably do Nonlinear FEA Join me for free on October 20th

Join my 2h FREE Live Event and learn all that you need to know to start using Nonlinear FEA as an Expert! I will talk about:

• How Nonlinear FEA really works
• What to pay attention to during Analysis Setup
• How to Analyze and Understand Outcomes
• … and much more!

Sign up now!

Nonlinear FEA Training

Join me for Free on October 14th!

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

Sign up!

In NX Nastran parameters described above have the following names and meanings:

• NINC – this is the “initial step definition” parameter. It divides the implemented load by it’s value, and the outcome of the division is the target first increment. In other words if the load is 50kN/m and I pick NINC = 50, first increment will be 50kN/m / 50 = 1kN/m.
• MAXITER – is a parameter on the border between “rules for analysis termination” and “convergence tolerances”. This is the number of iterations for one increment that are “allowed” before analysis terminates with “no convergence” message.
• EPSU, EPSP, EPEW – values of tolerances for displacements, forces and work. This are the “convergence tolerances” parameters and I usually use the default values.
• MXINC – maximal increments – this is the main “analysis termination” tool in NX Nastran. Unfortunately in most cases if you terminate analysis manually you do not have an access to outcome in NX Nastran. Since we wish our analysis to end, the easiest way is to limit maximal number of increments (if enforcing certain deformation is not possible as load). After the amount of increments is reached analysis “cleanly” terminates.
• MINALR, MAXALR – those parameters control “increasing and decreasing” of load increments. In many cases I do not like to increase increments in my analysis, so I set those as 1.0.

The above parameters are not all of course but are the most important. Also, there are certain things to those parameters I did not mention (like the fact that some of them may have negative values which will be interpreted somehow by the solver). For now, I assume this is enough to perform simple nonlinear analysis. In Femap, those parameters are set in two windows of the “nonlinear analysis options” tab. Those windows are shown below:

Apart from the parameters I described above, I marked a few others. KMETHOD and KSTEP are responsible for stiffness matrix updates during calculation run, and TYPE defines different arc-length strategies (modified Riks is the most popular, but I also use Crisfield). MAXR is a parameter that steers the process of increasing/decreasing load increments – you can limit how big an increase/decrease is acceptable. With [2] I have marked a box that must be checked – otherwise Femap won’t generate the NLPCI keyword and all parameters defined in “Advanced Options” will be ignored (resulting in non Arc-length analysis).

There are of course other parameters but for now, let’s leave them at default values in order to avoid long theoretical discussions. For the same reason I am avoiding going into the NX Nastran input file (the instructions generated in Femap for NX Nastran solver), but with a more complex design, it is actually worth learning the NX Nastran code to some extent (to be honest this is how I learn things – I learn NX Nastran code and when I know what I want I simply search which field in Femap are responsible for parameters I wish to set).

Below parameter values, I used in geometrically nonlinear analysis (note that leaving something “blanc” will use default NX Nastran value, even though most things are already filled in with default values in Femap just in case!). Important thing: the default value of MXINC is only 20 so you almost always want to fill that field since 20 is not enough in most cases).

The outcome of this analysis was already shown previously. I used the vertical displacement of the node on the shell top on a horizontal axis, and a force multiplier multiplied by the load I imputed (50kN/m), meaning that when the “set value” is 0.500 this means the current load is 0.5 x 50kN/m = 25kN/m. Obtained results are below.

As written here results differ from those obtained in LBA.

And finally a video tutorial – I already ordered new gear to play with so there is a chance that the next tutorial will be recorded with my commentary that won’t sound like broken radio 🙂

Have a good one!

Łukasz