# PFea Course Lesson 6- Local Region (Breakout) Analysis

Answer to problem from lesson 5

Zooming in closely to any of these nodal loads, they look like a point load applied to a boundary. This has finite load applied at a point, which has zero area, so the applied pressure is infinite. This is like the well-known Boussinesq problem in elasticity. Higher order elements will attempt to solve this singular problem.

In many stress analysis problems the maximum stress in the model is concentrated in a localized region, such as near a fillet, hole, or notch. It is much more economical to “break out” a local region for adaptive analysis rather than reanalyze the entire model. I’ve reviewed the theory behind this previously.

The first step for breakout analysis is determining the origin of the region of interest. This is usually the point of maximum stress in the model but can also be a user-specified point. Starting from that point, the next step is to identify how many elements are needed to retain in the breakout model to get an accurate answer from the adaptive stress analysis. The last step is to apply the displacements from the original solution as constraints at the interface between the break out model and the full model.

The intermediate step of determining how many elements to retain is the trickiest.  Ideally, at the interface between the breakout model and the full model, the stress should not be varying too rapidly, and should be much lower than the maximum stress. The elements in the model are sorted in ascending order of distance from their centroids to the origin point. This sorting is very fast if done with the quicksort (“qsort”) algorithm. A minimum number of elements is retained. Originally, additional elements were retained until the stress was low enough compared to the maximum stress or the stress gradient was low enough. Experience showed that both of these tests can often give “false positives” and cause an insufficient number of elements to be retained. Testing also showed that an accurate results is obtained if several thousand elements are retained in the breakout model. So now a very simple approach is used: after the sorting, the first several thousand elements are retained in the breakout model. The default is 5000. A model of this size can be adaptively solved very quickly, typically in a minute or less. This simple algorithm is carried out in postprocess.autoBreakoutSphere.

I refer to this approach of extracting a breakout model from a single large model as “ragged breakout” because the interface between the breakout model and the full model is not smooth. An example of this is shown in the figure below. This turns out not to be problematic, as long as all elements that touch the interface are marked as sacrificial.

Breakout by part from Assemblies

A different approach is used when analyzing assemblies. Here the breakout model is usually a single part. Working with codes that have application-programming interfaces, it is straightforward to determine which part the point of maximum stress is in. Alternatively, the user can select a part to use for the local region. The api can then provide the list of elements that belong to that part. This was done for the interface between SOLIDWORKS Simulation and stressRefine

This information is not available if working with an input file such as the Nastran bulk data file. However, the elements that belong to the part in which the point of maximum stress resides can be determined another way. In Nastran models, the interface conditions between adjacent parts in an assembly are often specified by “glued contacts”. These are “bsurfs” in Nastran, but other codes have a similar interface condition. The boundary of a part consists of element faces that only belong to a single element. These faces are either free (unloaded and unconstrained), loaded, constrained, or at the interface with another part, which means they have “bsurfs” on them. So for the purposes of identifying the part boundary, we just have to look for the faces owned by only one elements, or the faces that have bsurfs. In Nastran models, the faces with bsurfs should only have one element owner also, but checking for the bsurf is still necessary to determine the interface constraints to apply to the model, described below.

The mesh for the part is found by starting at an element in which the point of max stress is found, then searching the mesh topologically: All faces of the starting element are searched. If any are shared with adjacent elements, those elements then have their faces searched. This proceeds until no more faces shared by more than one elements are found. It is easiest to program this recursively, but that might lead to a large number of elements on the stack, so it is done in a loop, with candidate elements added to a list. This is carried out in stressRefine in postprocess. topoFilterSaveBreakoutElems. Here is an example:

Applying interface Conditions

Element faces that are at the interface between the breakout model and the full model have to be identified. The displacements from the FEA solution to the full model are applied as constraints on the nodes of these faces. For a “ragged” breakout model, these are faces that are only owned by one element in the breakout model but are owned by two in the full model. This is carried out in model.FindElemsAdjacentToBreakout. For breakout models that are parts from an assembly, the faces that need the interface condition are those with bsurfs.

Breakout Extraction Architecture

Currently extraction of breakout models is performed by the full stressRefine executable as a special type of run. This executable currently only works on Windows, as discussed previously. It requires the Intel Mkl pardiso solver which is not linking properly to stressRefine on Linux.

For that reason I am going to make a special executable that only does the breakout extraction and does not require an equation solver. This will work on both Linux and Windows. This will have an additional use. Breakout models can be extracted with this executable and then adaptively analyzed with a different program such as Sparselizard by simply providing a translator.

This concludes this PFEA short course. I hope it has been helpful in illustrating some of the issues involved in performing p-adaptive stress analysis, and how they have been handled in stressRefine.