Performing finite element analysis (FEA) on large models can be time consuming and frustrating due to the high number of elements and computer memory required. In general, any model that has more than 200,000 elements will begin to run slowly. Not everyone has access to a super-computer so it’s best to learn some tricks to reduce your FEA model size. One of the quickest ways to optimize your analysis is by taking advantage of model symmetry. This technique allows you to run a study on half or a quarter of your model without sacrificing quality.

Check out the model below. Using solid idealizations for the brackets and the base plate – the element count is already 132,000. It already takes about 1 minute to generate the mesh and about 10 minutes to run a simple linear static analysis. That time starts to add up if you’re running an iterative design optimization study with several load conditions. There’s certainly some room for improvement.

The first step to creating a symmetry model is to create a sectioned representation of your CAD model or assembly. For an assembly, this can be done by creating an extruded cut along each symmetry plane you’re using. For a part (or continuous model) this is usually created using Inventor’s “split” command to trim the solid.

This assembly is symmetric across two orthogonal planes. In the Assembly environment, I created a quarter section view using two extruded cuts. One along the XZ plane and one along the YZ plane. This creates a quarter sized model that will still provide the same level of accuracy.

When switching back to the Nastran environment, you’ll need to update your mesh, contacts, and connectors to coordinate with the new, simplified model. After making this change, the total element count (using the same mesh size) is only 33,000! That’s a reduction of 400%.

The second step to creating a symmetry model is applying Nastran “Symmetry” constraints. In other FEA software, this is also referred to as a “Frictionless” constraint. By applying a symmetry constraint, you’re creating a displacement condition in which the *displacement vector component perpendicular to the plane is zero *and the *rotational vector components parallel to the plane are zero*. This simulates the full model geometry being included.

Symmetry constraints are required on every model face that has been cut along a symmetry plane. For this example that means all faces lying on the YZ and XZ planes used to section the model.

The first symmetry constraint is applied by selecting the face cut by the YZ plane (shown below) and choosing “X” under Symmetry in the Constraint dialogue box. This will prevent translation along the X-axis and rotation about the Y and Z axes.

The second symmetry constraint is applied by selecting the face cut by the XZ plane (shown below) and choosing “Y” under Symmetry in the Constraint dialogue box. This will prevent translation along the Y-axis and rotation about the X and Z axes.

The last step to creating a symmetry model is to update the Load conditions to match the sectioned model. **If the applied load is cut by a symmetry plane, it needs to be reduced by 50%. **In this example, the Bearing Load is applied to a cylindrical face that lies on the XZ plane. In the full assembly, the magnitude of the load is 1000 lbf, so for the symmetry model it will be reduced to 500 lbf.

The linear static analysis only takes about 1 minute to complete now (instead of 10) and yields the same quality of result. The FEA model also loads in Nastran quicker.