How to assess postbuckled condition for aerospace structures using advanced nonlinear
Post Buckling Behavior Analysis in Femap using NX Nastran Advanced Nonlinear
What is Advanced Nonlinear
Advanced Nonlinear is an add-on solver to the basic FEMAP suite of tools. It does not come standard but is an added package that you can buy. It runs the ADINA Solver through NASTRAN. You can find it in the FEMAP Analysis manager allowing quick and easy set up for your solutions.
Advanced Nonlinear gives you additional capabilities beyond the basic nonlinear package with NASTRAN, and there are a few different solution types you can choose:
That can be in a geometric sense when the small displacement assumption no longer holds true, or when there are large displacements and large strains.
For material non-linearity, you can use Advanced Nonlinear to look at things when you move out of elastic, into the plastic regime. You can also use nonlinear to analyze contact and contact regions.
This tutorial will specifically cover pre- and post-buckling behavior that can be captured using Advanced Nonlinear. This captures both deformations that occur before buckles that can lead to buckling, and capturing and exploring post buckling behavior.
Thin Wall Cylinder Demonstration
The first demonstration is a thin-walled cylinder that is 40’ long, fixed 6’ at the base, and has a 1900 tip force two feet from the tip.
As we will see, the advanced nonlinear solution is able to capture deformation that will lead to a buckle that isn’t captured by a linear buckling solution. Our linear buckling solution is going to predict buckling at ~7400 lb pounds, while the advanced nonlinear shows instability at ~4800 lbs.
First, let’s look at our load. As seen below, there is a 1900-pound load as well as a time-frequency dependence.
Looking at the function, the load corresponds to the function. At the time 400, we have hit four times the load. As we go up, we’re saying what percentage of load is happening along this curve.
We use the time function to bring the load into the time domain. The load will “follow” and scale according to the time function. The curve below is scaled by 1% of load for every second (1x Load @ 100 s, 2x load @ 200s, 4x load @ 400 seconds) We utilize that function in the analysis manager.
Solver Parameters (Analysis Manager)
When we solve this, we’re going to have 400 steps, and we’re going to increment each step by 1. That means that as it solves at times step 1 is going to be applied 1 percent of load, and if we get to time step 400, we’re applying 400 percent of the load. This is due to the time function applied to the load that we saw above.
We set the “Output Every Nth Step” as 2, so we get information every other time step.
Iteration and Convergence Parameters (Analysis Manager)
Next, we’re going to look at the iteration and convergence parameters. The auto increment option is normally off. We turn it on so we can get the options for the auto time stepping.
We also turned on “Low Speed Dynamic Analysis”. If you have this on, you want to make sure that you have given your model mass, as it will use the mass matrix to help with the convergence. The mass is defined through the density (defined on the material card).
Linear Buckling Solution Results
We will first look at the results of the linear buckling solution. The number 3.9 at the bottom represents at 3.9 times our load, there will be buckling, as seen by the pattern.
Nonlinear Buckling Solution Results
With the nonlinear run, starting at 100% of the load, you can see that deflection is starting and we see some stress. Here we are deformed a little more than 31 inches.
In a linear solution, at two times the load we would expect to have a little under 63 inches of deformation (2x the 100% load case). But as you can see, the nonlinear run (at time step 200) jumps up to more than two times the deformation at time step 100.
When we are no longer assuming a linear solution, we can’t expect exactly proportional loading displacement.
Cross Section Deformation
Looking at the cross-section, you’ll notice that it is a little bit thinner than what we started with.
We started with a perfect circle. Placing a clipping Plane (with an exaggerated deformation three times to give us a better idea of what is happening) on the cross-section allows us to see that it has started to warp. It has lost the original shape of a circle to more of an ellipse.
Ramping up the load, you’ll notice the cross-section starts to get thinner and thinner. As it gets thinner, there is more stress concentrating in the region pictured below. Around time step 254 you can see buckles form.
We wanted to go to time step 400 but we lost convergence at time step 254 which indicates that the structure is no longer able to carry a load. It has buckled much earlier than what was predicted in the linear buckling solution.
As seen in this demonstration, Advanced Nonlinear can help you find buckling in your model analysis with more accuracy and even find buckles that are not found in the classic linear buckling system.
Box Beam Structure Demonstration
Our next demonstration is on a box beam/wing-like structure.
We have an exterior skin and on the inside, we have ribs, spars, a fore and aft spar, and stringers.
Looking at the thickness, the inboard region is much more supported than the outboard region.
The forepart of the wing has more support in the stringers than the aft part, which has no stringers.
One thing to point out about this model is that it is completely made from aluminum.
Inspecting the Model
This model was built using nonlinear materials. We have found that “Nonlinear Plastic” is the best option for material non-linearity in Advanced Nonlinear.
If you’re going to use nonlinear plastic you need to make sure you have two things:
You need the yield criteria and an initial yield stress that corresponds to that. We set this as von Mises
You need a function dependence. We used Stress v. Strain.
Looking at the Function
This is a stress vs. strain graph. In the elastic regime we’ve gone all the way up to 65 KSI and in the plastic regime we have extended it pretty far.
One tip for convergence: If you are going with nonlinear plastic material, you should try and extend the curve out as long as you can. Try to make sure that your model isn’t going to have to solve for anything outside the stress-strain curve.
We’re going to jump right to the end, to the final time step.
As you can see, there are multiple skin buckles at multiple bays of this wing.
When you look at the back, not only has the skin started to buckle and shed its load, but it has started to affect other parts of the structure.
On the aft spar there is a buckle on the web and we have an aft spar that has exceeded yield stress over 50% of its area. (Making it likely to fail).
Looking at the inside, we see more activity.
The stringers have started to wave. There is out of plane motion and it is likely to unload.
Next lets start at an earlier time frame and see what happens when we ramp up the load.
As we can see, more and more skin buckles form and it eventually gets pushed into the spar.
The nice thing about Nonlinear is that even with all the buckling and non-linearity in our model, we’re still able to get a converging run and able to see what happens with a planned or unplanned buckle.
When you are running Nonlinear, this Analysis Manager will pop-up.
It charts how long it is taking for your solution to converge. It’s not a straight line. The blips show where the model is having trouble converging.
If we recall our model, between time steps 20 and 30 is where our first skin buckle began to form.
You could use this to troubleshoot and figure out where you want to add more time steps or change your convergence parameters to push your solution to converge.
Advanced Nonlinear can be used to show a more realistic solution when geometric or material non-linearities exist. It’s able to capture buckles and continue to solve in order to investigate post buckling behavior.
What is in this webinar? This two-part series will detail the role that composites can play in Finite Element Analysis. Running on consecutive Wednesday afternoons, this series will show the use and value of composites in two separate Finite Element ...
Introduction This guide provides an in-depth overview of freebodies in Femap. If you would like to see the breakdown of each particular step and get a better understanding of freebodies, view the accompanying webinar hosted by Russ Hilley. What is a ...
Introduction Welcome to the introduction to FEMAP video series. In the previous video we set up the material and element properties on the machined arm components and defined loads and boundary conditions. In this video we will continue the ...
Welcome to the Getting Started with Femap tutorial series In this tutorial, we'll use Femap to go through the steps of creating and setting up a finite element model, analyzing it with NX Nastran, and reviewing the results. Why did we create this ...
What is in this webinar? This webinar will explain how to spread loads on your model using data surfaces through the Data Surface Editor. The following topics will be covered: What is load spreading? How external data, such as a pressure map, can be ...