(844) 825-5971 Contact Us SimuTech Group’s YouTube Channel

Get Our Latest Tips & Tricks

Receive the latest updates to our popular Tips & Tricks articles and videos by subscribing to our Monthly Newsletter and Subscribe to the SimuTech Group YouTube channel channel.
For even more advanced ANSYS instruction, check out our consulting and training services. Or simply contact us to discuss any of your ANSYS needs.

ANSYS Workbench Nonlinear Buckling with Pre-Buckled Shape Distortion

BucklingANSYS Workbench Nonlinear Buckling with Pre-Buckled Shape Distortion

In some symmetrical structures, the most likely shape for buckling may be ambiguous. In FEA models, some nonlinear large-displacement models may not buckle in an expected shape, because nothing initiates an expected buckling deformation. Success with such models can be aided if either a small load initiates the failed shape deformation, or if the "perfect" unloaded shape is slightly deformed in the pattern of a typical linear eigenvalue buckling shape.

The following image shows a thin part subject to a pressure on the thin top face, and simply supported at the ends. The support is from Remote Displacement objects that prevent UX, UY, ROTY and ROTZ. The far end also prevents UZ. The part will bend like a simply supported beam. When sufficiently loaded, the part will buckle out of plane, in the UX direction.

 

Buckling 2a

Note that the applied loading is a pressure on the thin upper face. In the large-displacement analysis, this pressure will act as a follower load, changing the direction in which it pushes as the face rotates. Users may prefer to apply a force to the face, so that the direction is not modified during large-displacement analysis.

The buckled shape can be seen further below. In a nonlinear large-displacement analysis, this example fails to buckle because of the perfect symmetry of the model and load. To trigger nonlinear buckling, some sort of UX offset loading or geometric imperfection needs to be applied. An often-preferred technique is to perform a linear eigenvalue buckling analysis based on the applied loads, and use a buckling mode deformation to apply a slight distortion to the unloaded mesh employed in the nonlinear large-displacement buckling analysis. This can be facilitated via the UPGEOM command of ANSYS. In Workbench, the deformation can be applied by APDL Commands Objects.

The following image shows a deformation plot for a large-displacement nonlinear analysis with the above loading. Deformation is in the YZ plane, without buckling in the UX direction. To trigger buckling in the UX direction, either a load in X is required, or a slight deformation of the unloaded mesh from a linear eigenvalue buckling analysis. (Note that the very slight UX movement is due to Poisson's Ratio effects, but the significant movement is restricted to the YZ plane.)

Buckling 3a

Application of deformation of the unloaded mesh in a shape based on the result of a linear eigenvalue buckling analysis can be applied with UPGEOM, which adds displacements from a previous analysis (in this case a linear eigenvalue buckling analysis) and updates the geometry (node positions) of the finite element model mesh to the deformed configuration. The command includes selection of a load step/substep from a previous analysis, and a node displacement amplitude scaling factor. It is typical in pre-deformed nonlinear large displacement buckling analysis to apply a maximum displacement magnitude on the order of maximum manufacturing variation. The user must be aware of the units employed in solving to get the scaling factor to be appropriate.

This article illustrates nonlinear buckling with a pre-buckled linear buckling shape applied, using the Workbench Mechanical interface. Two small APDL Commands Object snippets are included in the model Outline that convey the result of a linear eigenvalue buckling analysis to the shape of the unloaded mesh in the nonlinear large-displacement buckling analysis.

The following image shows a Project Schematic for a model that is to undergo nonlinear buckling analysis. The schematic starts with a Linear Static Structural Analysis for the chosen model. The full intended load can be applied, as long as it is suitable for providing pre-stress to a Linear Eigenvalue Buckling Analysis. The linear static analysis would use small displacement, linear material properties, and contact pairs that were all linear in their behavior—either bonded or no-separation.

Buckling 4a

Below the Linear Eigenvalue Buckling Analysis, there is a schematic for a Nonlinear Buckling Analysis. Note that it shares "Model" taken from the Static Linear Structural Analysis. This means that all settings prior to the loading on the environment will be shared, and the analyses will be part of the same Outline in Workbench Mechanical.

There is a second Nonlinear Buckling Analysis schematic in the lower right corner of the Project Schematic image. This last analysis shares the same model. This final schematic was used to examine the result of applying a larger amplitude deformation by a linear eigenvalue buckling shape to the same model and loading.

The next image shows the Workbench Mechanical Outline resulting from the above Project Schematic. The static structural linear analysis environment automatically sends its loads into the linked linear buckling analysis environment. Below that are the two large-displacement nonlinear buckling analyses.

Buckling 5

Note the presence of a Commands Object in the linear buckling postprocessing area. It makes a copy of the RST results file from the Linear Buckling analysis. There is another Commands Object in each nonlinear buckling environment, which applies a distortion taken from a chosen linear buckling mode shape in the RST file copy, using it to slightly distort the unloaded mesh in a nonlinear buckling run.

This model has been meshed with Solid Shell elements, requiring only one element through the thickness. Mapped meshing was employed.

 

Buckling 6a

The following image shows deformation for the first buckling mode as calculated in a Linear Eigenvalue Buckling model. Note that the ―Time‖ is 0.89028 – this is the Load Factor, a factor indicating the fraction of the applied load that would cause buckling of the elastic structure. Note also that the largest displacement in this plot has been normalized to a value of 1.0.

Buckling 7a

This shape can be chosen to drive a mesh deformation for the non-loaded mesh in the nonlinear buckling analysis that follows. The deformation is intended to help initiate this buckling shape in the nonlinear analysis.

In the postprocessing area of the Linear Eigenvalue Buckling analysis, an APDL Commands Object is inserted to write copy of RST file. It is placed two levels up in the file system subdirectories. This is at the same level as the Workbench project file, and should act as a ―neutral‖ location. Users may prefer a location of their own choosing, but it should be able to be reached via relative directory references.

Here is the APDL Commands Object contents:


Buckling 8b