A breakout model is an analysis model created to represent a portion of a large structure in order to get more specific information.

NOTE: Breakout models are a term used in the Femap community, but they are also commonly known as **submodels**. We will be using the terms interchangeably in this article.

For example, in this orthogrid pressure plate, you can use a breakout model (or submodel) to access the stress concentration in the specific joint shown below.

If you have a large model, it is impractical (and perhaps impossible) to apply a high-fidelity mesh to the entire model. However, without a high-fidelity mesh, we will miss detailed information on what is happening in the fillet region shown in the submodel on the right. A breakout model can help you look at the subsection and see where the stresses are, see if that fillet is structurally sufficient, and generally give you more information.

- When a small portion of a large design needs to be iteratively designed - You don’t want to have to run your large analysis model over and over again. Instead, you can iterate the submodel and save computation time on the solution
- When a feature is added to an existing part - In our first example, we will look at a scenario where avionics wants to add a pass-through to a wing-rib. It will be computationally expensive to run the entire model just to analyze the new mesh on the rib, so a breakout model would be useful.

- When the size of a model does not allow for the fidelity needed in specific locations
- When stress information is needed for a fillet or pad-up in a plate model

Let’s look at some examples of situations where breakout modeling can be used.

In this first example, assume that avionics asked you to add a pass-through to a wing rib.

Here is our full wing model:

And here is the rib that we want to add a pass-through to:

In Femap we can easily isolate the rib, add the pass-through, and interactively apply a new mesh to the rib:

Now that we have our breakout model, we can analyze the rib to see how adding the pass-through has affected the structure.

As a control, here is the submodel without the hole:

and here is the submodel with the hole:

It is a very similar stress layout, but you can see the hole is affecting it with the stress risers around the hole.

This second example demonstrates a local stress riser on a large orthogrid plate with bolted exterior supports.

Let’s say that you originally modeled the bosses on the plate with a CBUSH and RBE. However, later you need to find more information around the boss area.

Some common options are:

- Hex-mesh the area of the model
- No element doubling
- Element penetration
- Element skins

- Pull nodal displacements and rotations from the analysis and create SPCD’s to apply on solid mesh breakout.
- Integrate solid meshed breakout into full model.

Let’s explore the pros and cons of each of these methods.

Here is the control that we will be comparing our experiments to. The control is the model as it would be run if it was a large model.

It is at 132-133 ksi Von Mises which shows artificially high stress compared to the “accurate model.

This is the “accurate model” which is a tet mesh of the plate.

This model shows 96 ksi. It shows artificially hard results, as expected.

This is no element doubling:

The boss has been hex meshed and butt jointed with the plate elements, providing accurate stiffness and mass. However, solid elements are not able to support moments at their nodes. Therefore, you have a hinge condition anytime you have a plate butting up against a solid element.

This could lead to an artificial load path or, if you’re not fully constrained, it could give you excessive pivot ratios.

In this case we are well constrained. There is a nice connection to the boss and the model is fairly accurate with a max stress of 92 ksi compared to the 96 ksi on the solid model.

• Accurate stiffness

• Accurate mass

• No moment supported at junction

• Potentially unconservative

• Potentially incorrect load path

• Solid Elements cannot resolve moments at its nodes so all plate-solid interactions are hinges

In the applications where it can’t run or you don’t know if it will run, you have to solve your hinge condition.

This is element penetration:

The rib elements are going into the solid and all the nodes are coincident & merged. You will not get excessive pivot ratios because the moment at the hinge has been solved. However, we’ve added material and therefore added stiffness, mass, and strength.

We can expect to find a lower stress, which is what we find at 82 ksi. It also pushed the stress concentrations further out.

• Can support moment at junction

• Heightened mass

• Artificially stiff

• Artificially strong

• Unconservative

Element skins is another option.

In this scenario we take a skin around the solid and butt the ribs into it. It solves the same problems and has the same limitations.

This example has similar results at 82 ksi.

NOTE: A thinner skin can be used to lessen this effect, but thin skins behave like no element doubling, leading to a potentially incorrect load path.

• Can support moment at junction

• Heightened mass

• Artificially stiff

• Artificially strong

• Unconservative

This is a small section of the large model that has been tet-meshed. There are many nodes, elements, and high fidelity.

The RBEs from the source model have been spidered out.

Enforced displacements have been applied and so the model is contorted as if you just had plates.

As with all enforced displacements, this submodel is sensitive to stiffness. We’ve added a large boss in the center and increased the stiffness of this small submodel.

There will be a high force/stress moving through the model when the displacements are applied, as shown with a stress of 234 ksi. Notice that for this method, we removed a border of 3 elements from the outside because the RBE elements tend to push artificial stress risers into the model because they are perfectly rigid. If they were not removed the model would look like this:

As you can see there are high stress areas where the rigids connect with a stress of 437 ksi.

For this application, this method does not provide an accurate representation of the model behavior.

• Quick to model

• Accurate mass

• Potentially incorrect stress

• Artificially high stress if stiffness increased

• Artificially low stress if stiffness decreased

• Accurate stress if stiffness is not significantly changed

In this method we take the same tet-meshed model from the last example and zipped it into the full plate model.

It does not have to be the entire model, but make sure you go out far enough where the changes you’re making to the stiffness are a small percentage (close to 0%). In this case we used the entire model and applied the original loads (not enforced displacements). The method provided us good results with a peak stress of 95 ksi compared to the 96 from the control model.

• Accurate stress

• Accurate mass

• Slower to model

• Requires more solution time

- “Map output from model” is a quick way to set up loads on a breakout
- Try to keep nodes in original location (use mesh refine, not remesh)
- Try to keep breakout stiffness similar to original model if using enforced displacements

- Plate to solid transitions can work in some instances, but have limitations

- “Dummy elements” can be used for ballpark estimates if needed, but will often give inaccurate results

- “Zipped in” breakout models will give the most consistently accurate results
- Grow breakout model by at least three elements lengths from the point of interest

# Related Articles

## Developing Breakout Models in Femap

What is in this webinar? This webinar will explain how to create efficient and accurate breakout models from large structure in order to obtain detailed information of a small detail or interface. It will also explain when breakout models are needed ...## Analyzing Composites using FEA (Femap)

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 to Composite FEA

What is in this webinar? An Introduction to Composite Finite Element Analysis Theory and Modeling. Femap Details and Licensing Advanced Support Services## FEA Modeling from Start to Finish

What is in this webinar? This webinar will cover the entire finite element modeling process from pre-processing to post-processing. In this two part series, Dr. David Cross and Ryan Tatman cover the entire finite element modeling process for ...## The Post-processing Toolbox - Tools to Analyze and Interpret Your FEA Results

What is in this webinar? Femap has a variety of tools that enable access, visualization, and manipulation of the solver data. This webinar will focus on the Postprocessing Toolbox. Russ Hilley will introduce the tools within the toolbox, including ...