# Nonlinear buckling with no penetration contact support in 2017

One of my favorite feature in SOLIDWORKS Simulation 2017 is its ability to solve complex nonlinear buckling problems in an assembly environment. It enhances the existing nonlinear process whereas in buckling scenarios, only a single part could be analyzed or an assembly of parts where all parts had to literally bonded or glued together for analysis! I thought it would be beneficial to review some basic buckling concepts and common solving techniques before discussing this further!

** Buckling basics**:

In engineering mechanics 101, buckling is a type of mechanical failure mode characterized by sudden sideways deformation of a long slender member subjected to compression loads as illustrated here

.

Forces that act perpendicular to the “thin” direction of a slender structure are called **membrane forces. **Membrane forces can alter the bending stiffness of a structure. So tensile membrane forces increase lateral stiffness while compressive membrane forces decrease lateral stiffness. If the compressive forces are not perfectly aligned with the member axis, that can introduce an additional moment that can accelerate the buckling failure.

Buckling occurs when these compressive membrane forces are sufficiently high to cause the lateral stiffness to go to zero, as is seen in many real life scenarios like beam columns, vessels etc.

A long slender structure will fail mostly due to structural instability. Following assumptions can be made

- No material failure or non linearity prior to collapse
- Pre-buckling displacement is infinitesimal
- There is a critical load (
*P*) for which the structure is incapable of supporting any load at all. Any slight disturbance would make the structure unstable._{crit} - The load at which buckling initiates is called the
**Bifurcation point** - The buckling module calculates the
**Buckling Load Factor**which is a scale factor for the applied load to obtain the critical load

This is known as linear elastic buckling solved using an eigenvalue approach in SOLIDWORKS Simulation. Results of a sample linear elastic buckling analysis mode shapes and load factors are shown below.

__Linear Vs Nonlinear Buckling:__

The eigenvalue solution solves the equation (**[K] +****[Kg]){d} = {0}**

- [K] = structural stiffness matrix dependent on material
- eigenvalue for buckling mode. In other words, the critical load factor for a buckled mode shape[Kg] = geometric stiffness matrix independent of material properties. This matrix includes the effects of the

membrane loads on the stiffness of the structure. The stress stiffening matrix is assembled based on the results of a previous linear static analysis. - {d} = displacement vector corresponding to the buckling mode shape.

It uses an iterative algorithm that extracts the eigenvalues and the displacements that define the corresponding mode shape ({d}). Displacements here are not real but are normalized values used for visualization of the buckling model shapes! The shape the model takes while buckling is called the buckling mode shape and the loading is called the critical or buckling load. Buckling analysis calculates a number of modes as requested. Designers are usually interested in the lowest mode (mode 1) because it is associated with the lowest critical load. When buckling is the critical design factor, calculating multiple buckling modes helps in locating the weak areas of the model. The mode shapes can help you modify the model or the support system to prevent buckling in a certain mode

The critical buckling load factor calculated by the theory of elastic stability may over predict the critical load of the actual structure because of:

- Inelastic or nonlinear material behavior prior to instability
- Realignment / misalignment or eccentricity of the load or support conditions
- Finite displacements prior to buckling
- Initial imperfection in the structure
- Machining tolerance
- Material irregularities

Hence a more vigorous approach to study the behavior of engineering problems at and beyond buckling requires the use of nonlinear design analysis. Nonlinear buckling phenomenon includes a region of instability in the post-buckling region whereas linear buckling only involves linear, pre-buckling behavior up to the bifurcation (critical loading) point. See image below for an illustration.

The unstable region shown above is also known as the “snap through” region, where the structure “snaps through” from one stable region to another. To illustrate, consider the shallow arch loaded as shown below.

For nonlinear problems In general, the changing stiffness of the structure, material nonlinearity, the applied loads plus direction, and/or boundary conditions can be affected by the induced displacements. The equilibrium of the structure must be established for a deformed shape which is unknown and must be guessed. At each equilibrium state along the equilibrium path, the resulting set of simultaneous equations will be nonlinear. Therefore, a direct solution will not be possible and an iterative method such as Newton Raphson technique will be required. These are augmented by special load incremental control methods such as Force Control, Displacement Control and Arc Length Control. We will not dive into details on these. However the below illustrates the need to use Arc Length control methods for nonlinear buckling problems.

Both force control and displacement control will breakdown in the neighborhood of turning points (known as snap-through for force control and snap-back for displacement control) as shown in the figure above. These difficulties usually are encountered in buckling analysis of frames, rings, and shells. Arc – length control will successfully overcome these difficulties.

__Example Application:__

Now that we have some basic knowledge on buckling and using arc length control for predicting realistic buckling and post buckling behavior, I am going to jump straight into showing you an assembly analysis with contacts to illustrate this in 2017.

Let’s take a look at a remote control button assembly as shown below. The button is made out of silicone rubber and the contact plate is made out of polyethylene plastic materials. The button has to snap through the thin section in order to make contact with the plate.

A cross section of the geometry reveals the thin sections of interest on the button.

Appropriate material models are used in SOLIDWORKS Simulation nonlinear analysis for a realistic material response. The silicone is treated as a **Hyper elastic Mooney Rivlin** material with stress strain data obtained from tests.

Since the plate is much more rigid, a linear elastic material suffices for the polyethylene material.

Due to symmetry, an axisymmetric geometry of the assembly is automatically used in SOLIDWORKS Simulation for analysis. A load of 1 Newton is applied to the top edge of the button as shown below. Appropriate constraints are applied in axial and radial directions to restrain the geometry correctly.

While the loading direction is important, the magnitude is what the program will adjust during the solve to satisfy the equilibrium requirements for deformation using the Arc length control technique.

Appropriate **No Penetration** contact conditions are defined between the button and plate geometry as shown below.

A hollow section separates the top and bottom edges of the plate. These edges would eventually have to come into contact to either close an electrical circuit in the remote control to activate the function of the button! Thus its important that this behavior is accounted for through a second contact condition as below

Mesh controls are applied on the thin section areas to accurately capture the deformation response. The resulting mesh is shown below.

The Arc length control technique is selected from a list of supported control techniques in the nonlinear study setup properties.

__Results:__

Several points are probed along the thin section and their response is shown below

Zooming in one of the central locations on the thin section, the response plot is as below.

The response graph clearly shows the snap through response of the thin section. The sudden spike in the load factor towards the end indicates that the contacts in the plate are now taking on the bulk of the external force.

Here is a deformation video illustrating the function of this assembly.

Here are some other examples of the nonlinear buckling analysis for assemblies in 2017

In summary, SOLIDWORKS Simulation 2017 offers a powerful toolset to solve complex engineering problems, especially in the area of nonlinear buckling for assemblies. Hope you have enjoyed this read. If you have any questions or would like to learn more about SOLIDWORKS Simulation, please contact your local SOLIDWORKS reseller.