Watch out — You can get different results depending on how you mesh the model.

Paul M. Kurowski
Design Generator Inc.
pkurowski@rogers.com

 The process of creating a mathematical model consists of idealizing CAD geometry (here removing external rounds), defining loads, supports, material properties, and the type of analysis (here structural static). The mathematical model is discretized into a finite-element model. This completes the preprocessing. The model is then solved and the analysis of results concludes the FEA. First and secondorder tetrahedral elements are shown before and after deformation. Note that the deformed faces of the second-order element may assume either concave or convex shape. The mesh is made with firstorder tetrahedral elements. Notice the imprecise element mapping to the hole. Flat face segments represent the face of the cylindrical hole. Second-order elements map precisely to curvilinear geometry. First-order sheel elements: The mesh was created with firstorder shell elements. Notice the imprecise mapping to curvilinear geometry. Second-order shell elements: Meshing the thin band with secondorder-shell elements produces precise curvilinear geometry. The plate can be modeled with either solid (left) or shell elements. The actual choice depends on the particular requirements of analysis and, sometimes, on personal preferences. A degree of freedom (DOF) is the ability of a node to translate or rotate. Three DOF means a node can only translate (along X, Y, and Z axes) while six DOF means it can also rotate about the axes. The three meshes have one, two, and four layers of elements across the thickness. Adding more layers results in uniform mesh refinement. Note that the denser themesh, the greater the displacement.

There was a time when the task of building a model for finite-element analysis (FEA) was long and tedious. Those days are over. Modern CAD and FEA programs work together so closely that CAD geometry becomes a starting point for FEA. But what really happens after CAD geometry goes into an FEA program for meshing? And how does meshing affect FEA results? The answers call for examining the properties of finite elements and finite-element meshes and seeing how they alter results. It's also useful to review how fundamental assumptions made in element formulation affect global behavior of the analyzed model.

WHAT GETS MESHED?
Geometry from CAD used for analysis must be meshable into correct and reasonably small finite elements. But the process of defining these elements often necessitates making changes to the CAD geometry. Typical modifications include defeaturing (removing unnecessary details), idealization (for example, representing thin wall with a surface), and geometry cleanup.

Having prepared meshable, but not yet meshed geometry, we define material properties, loads, supports and restraints, and select a type of analysis, such as structural, thermal, or some other. This procedure creates a mathematical model on which an FEA solver can work.

The mathematical model now must be split into finite elements through a process of discretization, more commonly called meshing. However, loads and supports are also discretized by applying them to nodes of the finite-element mesh.

Continuous CAD geometry and discrete FEA geometry are only superficially similar. While CAD geometry has solids, surfaces, faces, lines, and vertexes, no such entities exist in FEA geometry. No part of CAD geometry becomes FEA geometry. FEA geometry only has nodes. Mathematical formulations define element behavior and element connectivity to nodes. Displaying a mesh as lines connecting nodes helps us visualize element locations and it makes FEA geometry look almost like a CAD model which adds to the confusion in distinguishing between the two.

What elements does meshing make? The meshing process splits continuous geometry into finite elements. The type of elements created in this process depends on the type of geometry meshed, the type of analysis, and sometimes on the preferences of theperson doing the modeling. For brevity, we'll discuss the two most-frequently used elements: solids and shells.

It's important to clarify terminology here. For instance, "solid" has different meanings when referring to "solid geometry" and a "solid element." In a nutshell, solid CAD geometry is an FEA volume, and solid elements are created by meshing those volumes.

Automatic meshing of solid CAD geometry takes place most often with tetrahedral solid elements, or just tets. This is because present day automeshers can't reliably mesh complex geometries with anything but tets. Tetrahedral solid elements can either be first or second-order elements. The user decides which to use. However, we will show that only second-order elements should be used for an analysis of any importance.

First-order tetrahedral elements have four nodes, straight edges, and flat faces. Those edges and faces remain straight and flat after the element has experienced deformation under the applied load. First-order elements model the linear-displacement field inside their volume, on faces, and along edges. The linear or first-order displacement field gives these elements their name. Recall from mechanics of materials that strain is the first derivative of displacement. Therefore strain, and consequently stress, are both constant throughout first-order tetrahedrons. The situation imposes a severe limitation on the capability of meshes constructed with first-order elements to model stress distributions of any real complexity. To make matters worse, straight edges and flat faces of the elements do not map properly to curvilinear geometry.

Second-order tetrahedral elements have 10 nodes and model the secondorder displacement field in their volume, along faces, and edges. The edges and faces before and after deformation can be curved. Therefore, these elements map precisely to curved surfaces. Second-order tetrahedral elements model the second-order (parabolic) distribution of displacements inside their volume, on faces, and along edges. Consequently, they model the linear distribution of strains and stresses. Though they are more computationally demanding than first-order elements, secondorder-tetrahedral elements are used for most analyses. They represent a "happy middle" between numerical complexityand the ability to model real-life displacements and stresses.

What is the role played by shell elements? While solid-tetrahedral elements can mesh volumes derived from solid CAD geometry, use shell elements to mesh surfaces and when analyzing thinwalled structures. Because surface geometry does not carry information about thickness, the user must provide it.

Similar to solid elements, shell elements also come as first and second order. There are analogical consequences to mapping their curvilinear geometry to model displacement and stress fields. Again, only second-order shell elements should be used for analyses of importance.

Certain classes of shapes can be modeled using either solid or shell elements. The type of element used for modeling tetrahedral solids or shells sometimes depends on the objective of the analysis. The nature of the geometry often dictates what type of element should be used for meshing. For example, parts produced by casting lend themselves to meshing with solid elements, while sheet-metal structures are best meshed with shell elements.

How does the meshed model's behavior differ from the original? Suppose we want to model displacements in the bracket with a hole on the first page. Having settled on a certain mesh density, we mesh the part with second-order tets. Will the finite-element model return the same displacement field as in the continuous model? No, it will not. Second-order tetrahedral elements can only return a displacement field which is piecewise parabolic. Of course, if elements are sufficiently small complex displacement fields can be well approximated by piecewise parabolic distribution of displacements. This is the essence of finite-element approximation.

Now, let's make an important observation: By meshing a part with a certain type of element and using a certain size and shape, we impose additional constraints on the part. The meshed part must conform to applied loads and restraints. But being meshed, it must also conform to constraints imposed by meshing. In other words, deformation must satisfy loads and restraints and be piecewise parabolic. Because the meshed part has the additional constraints, the process of meshing makes it stiffer.

The amount of additional stiffness depends on the element and their size. First-order elements require that the displacement field be piecewise linear. This is more restrictive than in second-order elements where the displacement field must be piecewise parabolic. Larger elements add more stiffness than small ones. However, the effect of added stiffness (call it artificial stiffness) always accompanies finite-element models. The effect of artificial stiffness is small but demonstrable in most cases, even with a reasonably well-refined mesh.

How does artificial stiffness affect results? Two examples from structural static analysis can show the effect of artificial stiffness introduced by meshing. We will then extend conclusions to modal and buckling analyses. All geometry, material, load, and support information is presented for readers who would like to reproduce results in their own FEA programs.

Consider a cantilever beam meshed with three different densities to see how the maximum deflection changes. To make this comparison fair, even the first mesh (the rough one) must be able to model bending stiffness.

The beam deflects further with finer meshing. This proves that the finite-element model becomes "softer" with a rise in element density. The effect arises because artificial constraints become less imposing with mesh refinement. Notice, too, that the deflection differences between the three models are small. Thus even the first rough mesh can model beam-bending stiffness correctly. Indeed, one layer of second-or-der elements produces linear-stress distribution across the thickness and, therefore, can correctly model bending stiffness in a regular shape such as the beam where stresses change linearly from tensile to compressive. The difference in results between the first and second models is 0.07 mm, while between the second and third it is only 0.02 mm. This proves that displacement results converge, as they should, to the solution offered by a continuous mathematical model.

How do stress results change with mesh refinements? Select any location on the beam surface to examine stresses and you will see they increase with more refined mesh. This effect arises from two contributing factors. First is that stresses are calculated based on displacement results, so larger displacements lead to larger stresses. This contribution, however, is usually small. The second and more important factor is that smaller elements collect stress information closer to the beam surface where higher stresses reside. How easy this effect is to visualize depends on if and what stress averaging technique has been used to plot results. Finally, with mesh refinement you will notice high-stress concentrations in all four corners of supported faces (Not illustrated. Do this one on your own). This arises because stresses in those corners are singular and diverge to infinity with mesh refinements.

A second example is that of a thin flat steel strip (2503 103 2 mm) with supports on both sides. The strip has a 5-mm-thick block attached to the middle of its span. A load displaces the top face down 3.37 mm. The objective is to find reaction forces on both ends of the strip. Notice that though the deflection is small (1.3% of the length), the problem requires nonlinear deformation analysis to account for membrane stiffness that develops during the deformation.

Suppose we now mesh and solve the model three times, with one, two, and four layers of elements across the thickness. We'll notice that the reaction forces drop.

Why does the reaction force drop with mesh refinement? As before, the strip "softens" as the mesh is refined. Therefore, lower reactions develop after application of the same displacement.

The effect of artificial constraints also shows in modal analysis. By simple reasoning we can see that a modal analysis will overestimate the frequencies of a continuous model. This is because the finite-element model has the artificial stiffness mentioned earlier and stiffer models mean higher frequencies of vibration. Mesh refinement lets the frequencies converge from above to the exact solution.

 HOW THE REACTIONS COMPARE Thickness Horizontal, N Vertical, N One element 1,937 102.5 Two elements 1,935 102.3 Four elements 1,934 102.1 Horizontal is along the length on the strip and vertical is across the beam thickness. Prescribed displacements are applied in this vertical direction.

STIFFENING WITH BUCKLING
The effect of artificial constraints on results of buckling analyses resembles that in modal analyses. The added stiffness results in an overly optimistic magnitude of buckling load which converges from above to the exact solution of the mathematical model. And that on top of the fact that buckling analysis overestimates buckling loads because it disregards details such as geometric and material imperfections and load offsets. We must be careful when interpreting results of a linear buckling analysis which produces nonconservative results. Often, calculating a buckling load factor will require a nonlinear buckling analysis.

We have demonstrated the stiffening effect of a mesh using correctly shaped elements and correct meshes that can properly model structural behavior (bending, for the example presented). The stiffening effect is more pronounced when the mesh contains many degenerated elements or when a mesh just can't correctly model the stiffness, or both.