Preparing a CAD model for FEA

When to simplify geometry and what can be simplified

Before you ever begin the simulation, determine which components of the assembly and which features of the parts are critical to the outcome of the simulation. Simplify your model down to these parts and features to save time in the setup and analysis.

For assemblies:

• Consider focusing on just the parts of an assembly that will produce the results you need and exclude parts that would not influence the results. 
• If it is a welded assembly, remove the welds and utilize contact (unless specifically studying the weld, of course).

For parts:

• Remove small/minor holes, grooves, chamfers, and fillets that are outside the area of high stress and other small features like cast-in part numbers. Recall that what ultimately will be analyzed are the elements. If you haven’t adequately meshed these small features, you are not simulating the appropriate representation of the geometry anyway.
• Some items, such as bolts, can often be replaced with idealizations. 

What to preserve in a model

While simplification is helpful, it is also possible to oversimplify – such that what you are left with is no longer representative of what needs simulated. While reducing model complexity reduces element count, resulting in a faster analysis, do so with consideration of the impact the removal is making (or not). 

If a feature, such as a fillet, is where the high stress is going to occur, you’ll want to preserve that and mesh it adequately so that the outcome is appropriate. 

Likewise, if the feature is a critical location to hold (constrain) or to apply a load – and you cannot determine any alternative method for doing so – you’ll probably need to retain it. 

If removing a hole or pocket alters the part enough such that the stiffness of the part is changed significantly, you may instead just want to remove any small details (fillets, chamfers, smaller holes within the pocket) in the feature and retain the larger hole or pocket.

Combining geometry in a model

Frequently, in assemblies, there are adjacent parts all of the same material. Using your CAD package to Boolean (join) these into a single body will reduce element count, reduce contact element count, simplify meshing, and reduce the number of parts you need to define items (such as material) for. Combining parts, when possible, can greatly simplify the setup and solve time. 

• Example: The region in the following image captured by the green oval encompasses no less than seven parts. If they were combined into a single body, that would greatly simplify setup and analysis. 

 

Excluding geometry to use boundary conditions

Sometimes, the only reason some parts are in an assembly is to prevent other parts from moving in a particular direction. The effect of these parts can be replaced by properly constraining the model. Focusing on just the portion of the assembly you need to analyze generally means terminating with boundary conditions at the disconnect from the rest of the assembly.

• Example: If our goal is to analyze the strength or modal frequency of the turn signal and light assembly shown in the following image, the steel plate it is attached to is sufficiently rigid that we could just analyze the light assembly. Use fixed constraints on the four bolt holes where it attaches to the steel plate and exclude the steel plate and the rest of the sub-assembly.

Using symmetry and anti-symmetry

One way to simplify is using symmetry or anti-symmetry, resulting in half (or less using quarter symmetry) of the number of parts or elements. Symmetry/anti-symmetry, when applicable, is a great and quick way to reduce the model to half, quarter, or even an eighth of the size – greatly reducing the size of the analysis. An added plus is that the symmetry constraints also help to add stabilization to the model – without artificially constraining. For example, a sphere (like a soccer ball) under uniform internal pressure could be modeled in 1/8 symmetry and the symmetry constraints required, alone, would be enough to make for a statically stable model. 

• When the loads, geometry, material, constraints, and results are symmetrical about a plane, only the part of the model on one side of that plane needs to be analyzed. 
• To get correct results, symmetry or anti-symmetry constraints need to be applied at the symmetry plane once the model is cut away to the reduced model. 
• With symmetry, the out-of-plane translation and two in-plane rotations are constrained as shown in the image on the left. 
• If the loads are in opposite directions (but equal), making for an anti-symmetric model, then the out-of-plane rotation is constrained along with the two in-plane translations – as shown in the image on the right.

When to split geometry

Many finite element analysis packages allow for the application of constraints and loads based on surfaces, edges, or points (corners) of the original CAD model. Take advantage of splitting geometry, when necessary, to apply constraints and loads exactly where you need them. 

• There are instances where you might want surfaces, edges, or points that didn’t exist in the original model.  
• Take advantage of split tools in the CAD package to generate new edges, points, or surfaces. 
  • Imagine you have a model of a tabletop surface. It is one large rectangular surface to begin with. Imagine someone has defined that you need to simulate a 100lbf being placed exactly center of the table, perhaps furthest from any supports. You could sketch an x pattern diagonally and split the surface so that now you have a point to add the force. Alternatively, to distribute it, you could use a circle or rectangle to intersect the surface and create a new surface region.

Example:

Initially, applying a pressure to the bottom lip of the bucket, it distributes to the entire surface.



Using a sketch of a circle, you can use the split tool to split the initial surface into shapes and sizes you would like to apply specific loads to. This likewise works for constraints.