Using SOLIDWORKS Simulation for Composites

SOLIDWORKS Simulation is a CAD-embedded finite element analysis (FEA) software that enables designers and engineers to perform structural analysis during the design phase. For predicting the performance of ductile metals such as steel and aluminum below their yield stress, the default “linear elastic isotropic” material model is generally suitable. Even brittle materials such as cast iron or unreinforced concrete are commonly modeled as linear elastic isotropic but may require an alternate failure criterion rather than the Von Mises yield criterion so commonly used. 

In past articles we’ve explored use cases for nonlinear analysis, including hyperelastic materials such as rubbers or plasticity models for loadings beyond the yield point of a material.

Something all the materials discussed so far share is that they are generally thought of as homogenous in nature or made up of a single constituent material.

Composite materials, on the other hand, are made up of multiple constituent materials and can be engineered to possess qualities such as stiffness, strength or toughness that exceeds the performance of most of the material.

In this article, we’ll explore a high-level overview of analysis techniques for composite materials within SOLIDWORKS and SIMULIA products.

Composites Applications

The domain of composites is quite broad. This article will attempt to focus on the “macro” scale composites commonly chosen by engineers and product designers for their rated properties. The constituent components of a composite are often classified as the matrix or binding medium, and the reinforcement which is added for additional strength or other physical characteristics.

Wood products such as common plywood are an example of this. Laminated veneer lumber (LVL) beams and other glue laminated or “glulam” construction are used to achieve open-concept floorplans that would only otherwise be possible with steel members.

Sandwich composites make use of an inner core layer such as foam or aluminum honeycomb, with encapsulating thin outer skins to carry shear forces.

Figure 1. Glulam beams (left) and aluminum honeycomb sandwich composite (right).

Reinforced concrete with embedded steel or carbon-fiber reinforced polymer is a mainstay of commercial and residential construction.

Injection molded plastic parts are commonly reinforced with chopped fiberglass or carbon fiber, with such strength that they can often replace aluminum castings or stamped steel components.

Fiberglass composites are commonly used in all sorts of commercial and recreational products, from boats to storage tanks and FR-4 is a fiberglass composite that also happens to be the base material for most printed circuit boards in use today. 

Figure 2. Fiberglass FR-4 PCB (left) and fiber-filled injection molded part (right).

Of course, the image most of us probably arrive at in our minds when we hear the word “composites” is carbon fiber, more specifically glass-reinforced polymer (GRP) and carbon-fiber reinforced polymer (CFRP), with the classical case being a rigid structure made up of multiple layers of woven continuous-strand textile bound together by an epoxy resin.

Depending on the application, engineers may choose to incorporate or modify pre-purchased composites or go into depth designing their own custom lay-ups.

This article will attempt to examine both approaches and the levels of simulation software required for performing structural analysis at various levels of fidelity.

Orthotropic Materials with SOLIDWORKS Simulation Standard

A key behavior for many composite materials is that due to their heterogenous makeup, they often exhibit different behaviors depending on the direction of loading. This behavior can be crudely approximated using the linear elastic orthotropic material definition available in the most basic levels of SOLIDWORKS Simulation – including the simulation included with SOLIDWORKS Premium and the SOLIDWORKS Simulation Standard license.

Figure 3. Linear elastic orthotropic material properties for a glass-reinforced polymer with reference geometry selection.

This material model is in contrast to the default linear elastic isotropic used for homogenous materials and allows definition of elastic modulus and shear modulus in the X, Y and Z directions. These directions must be defined by some reference geometry selection – either a plane, planar face, coordinate system or axis. The reference geometry selection maps the material properties to the appropriate axes so if there are multiple bodies with different orientations they must have a relevant individual reference geometry selection.

This necessitates some limitations – the geometry must either be planar, cylindrical or spherical in nature, depending on the reference geometry selection. If the end part cannot be defined as a single body while satisfying these rules, then it must be broken up into multiple more primitive bodies. Such a procedure is described in the help article Defining Orthotropic Properties.

It should be noted that this approach generally allows adequately representing the stiffness of a composite material for a structural analysis, allowing accurate predictions of the total displacement and any reaction or free body forces. As the stress information is not available per-ply, caution must be taken from drawing conclusions about failure of the composite material itself. 

Another benefit of this approach is that it is available for all study types in SOLIDWORKS Simulation, including thermal analysis.

Transverse Isotropy

It should be noted that most layered composites exhibit the behavior of transverse isotropy, meaning their behavior can be simplified to in-plane and through-plane behaviors. For this reason, you may find material might often be provided with only two components of elastic modulus (such as E1 and E2) and one component of shear modulus (G12).

SOLIDWORKS Simulation has no transverse isotropic definition, so the missing properties for a full orthotropic material may be back-calculated (e.g., E1 = E3 assuming plane 1-3 is the plane of isotropy). Poisson’s ratio may also be back-calculated from the elastic modulus and shear modulus.

Materials may also behave differently based on the physics in question. For instance, PCBs are sometimes approximated as isotropic materials for structural analysis but generally must be represented as orthotropic materials for thermal analysis where the conductivity of the copper plays a more significant role.

Analysis of a Quadcopter Frame

For an example of using this approach, we’ll apply a linear orthotropic material to a frame for a quadcopter. This is an ideal case for these assumptions since the frame will be routed out of a pre-purchased CFRP sheet and the geometry is planar in nature.

Figure 4. Quadcopter CAD assembly (top) and same assembly prepared for analysis (bottom).

The analysis is a static study with a 5 g downward acceleration applied. Restraints are applied at the motor mounting locations using the Remote Load tool acting as a remote displacement and representing a ball joint style pivot.

It should be noted that this fixture scheme was arrived at after comparing against the naïve approach of “fixed geometry,” as visualized in the exaggerated displacement plot below.

Figure 5. Fixed geometry restraints (top) and remote load pivot fixture (bottom).

It can be seen from above that the response with the pivot restraints appears much more natural and represents the facts that the propellers will apply thrust force normal to their current direction, rather than the global vertical direction. The fixed geometry fixtures appear to have a severe and artificial stiffening effect which reduces the overall displacement. The lower image also shows that the quadcopter must be somewhat tail heavy with the rear end dipping down lower than the front. I’ll have to check with the designer to make sure the mass of the battery is correct.

A true-scale animation plot is presented in the following figure.

Figure 6. True scale displacement animation.

As no per-ply stress information is available, we really shouldn’t use stress components to predict factor-of-safety for the frame.

One potential alternative is to use strain as a predictor for failure.

Figure 7. Strain plot for CFRP sheet.

The figure above shows a strain plot for the frame, with the plot scaled for a strain design limit. This is about the best we can do without having access to more detailed composites information, but may suffice for many users looking to work with pre-purchased composite sheet or tube.

Composites Analysis with SOLIDWORKS Simulation Premium

The next step up in realism is to utilize the composites analysis available in SOLIDWORKS Simulation Premium. This requires using a shell mesh definition for the composite in question, and so requires a constant wall thickness region. This type of composite definition is possible in the linear static, frequency and buckling study types.

Material properties are defined in the same fashion as the linear orthotropic material, except there is no reference geometry selection and they can vary per ply. The ply orientation is mapped by default to the U-V coordinates of the surface, allowing truly orthotropic behavior for compound surfaces that is not restricted to specific geometry primitives.

Figure 8. Composite shell definition.

Composite shell definition for a fixed-wing drone fuselage is pictured above. To simplify the shell definition, a surface was extracted from solid body using the Offset Surface command. If you’re unfamiliar with shell definition in SOLIDWORKS Simulation, I’d recommend the tutorial on SOLIDWORKS Simulation Shell Definition.

The ability to align orthotropic material properties with arbitrary compound surfaces is really one of the biggest features of this composite shell definition. It allows analysis of things that aren’t just plates and tubes.

Note though that the orientation of the coordinate mapping should be verified and can be altered or corrected per face if there is an alignment discontinuity or mismatch. This can be a daunting process for geometry with many distinct faces/fillets as pictured above. For geometry with a low number of faces or with smooth continuous compound surfaces very little correction should be required.

Individual plies can be specified with their own thickness, angle and material properties during the shell definition allowing room for substantial experimentation from the designer.

As far as the simulation setup is concerned, the drone is subjected to a combination of torsion and gravitational acceleration that is intended to represent a very rough landing. Contact sets were defined to locally bond the composite shell to the other components in the load path, including the front and rear injection-molded housings and the tail boom.

Figure 9. Simulation setup with contact definitions.

The response is pictured below using Von Mises stress for the first ply, but note the additional options to plot stress for other plies, maximum across all plies and also interlaminar shear. 

Figure 10. Stress visualization.

Failure Theories

As mentioned, the composites functionality in SOLIDWORKS Simulation Premium adds the capability to track and interpret per -ply stresses as well as interlaminar shear stress.

This enables additional failure criteria in the factor of safety plot, including the Maximum Stress, Tsai-Hill and Tsai-Wu failure criterion.

Figure 11. Predicted factor of safety using Tsai-Wu criterion.

A helpful SOLIDWORKS article discusses selecting a composites failure criterion can be found here.

In short, Tsai-Hill and Tsai-Wu take into account the interactions between stress components and thus are capable of predicting failure of plies due interlaminar shear stresses (failure modes such as delamination) but aren’t intended for predicting failure in the matrix. Maximum stress criterion looks only at maximal values and can be useful for predicting failure in the composite matrix but isn’t intended for predicting failure due to delamination. 

It should be noted that the method used by SOLIDWORKS Simulation Premium is first ply failure (FPF) and will never show or describe delamination visually or allow simulating behavior past the initial failure. The “rule of mixtures” assumption utilized by SOLIDWORKS Simulation also approximates the bulk behavior of the composite from its makeup information, potentially neglecting localized failure modes.

Additionally, the way the ply information is mapped to the shell mesh means that we can’t easily analyze the relatively common case of composites with variable wall thickness or tapering sections.

Composites Analysis in SIMULIA

The desktop software package SIMULIA Abaqus/CAE and the cloud-connected equivalent 3DEXPERIENCE SIMULIA structural simulation roles both provide in-depth composites modeling and analysis, adding several major capabilities that span across many domains such as fatigue and durability, fracture mechanics and vibrations.

Composites in SIMULIA structural tools may be defined at various levels of detail and represented by either “composite shells” or “composite continuum shells” as in the case for many layups or with high-detail solid mesh. This means it is possible to analyze both the performance of something like a complex vehicle body or other large-scale structure or zoom in to analyze specific failure modes at connections or joints in very high detail.

Composite Ply Definitions

Composite shell sections function similarly to the composites functionality module in SOLIDWORKS Simulation Premium, mapping over ply stack information to surfaces, except that they support variable wall thickness and so can easily represent tapered or variable wall thickness.

Figure 12. Composite lay-up example from Abaqus CAE user guide.

Composite continuum shell sections combine many of the benefits of shell and solid mesh by incorporating a 3D nodal representation of the thickness. The user guide for Composite Continuum Shell describes in further detail:

“Like a shell section, a composite continuum section has one dimension (the thickness) that is significantly smaller than the other two dimensions. However, composite continuum shell sections are modeled in three dimensions; therefore, the model defines the thickness and stresses in the thickness direction are not negligible.”

Ply information can be defined directly in the analysis tool or, if product design is being performed in CATIA or the associated 3DEXPERIENCE roles, the ply information can be imported for analysis providing a tight coupling between design and analysis for faster iteration.

Delamination and Crack Propagation

The SIMULIA structural tools also support simulating behavior such as crack initiation and propagation. Cohesive elements within the software can be applied. These cohesive elements may be assigned to fail at certain magnitudes of strain or shear stress, allowing visualization of the beginning of crack formation or delamination. The virtual crack closure technique (VCCT) is an alternative approach that can be applied to further simulate crack propagation from some existing flaw or defect, as visible in the figure below from the Abaqus user guide example: Post buckling and growth of delamination in composite panels.

Figure 13. Composite panel in post-buckled state with SIMULIA Abaqus.

The two techniques utilized together can provide a robust overview of resistance of composites to delamination or failure of any bonded connections.

Additional damage models combined with the available Explicit solver also allow representing brittle fracture for modeling detailed behavior of impacts, crashes and other high speed dynamic events.

Figure 14. Ballistic impact of fiber composite.

Embedded Reinforcement Elements

In some cases, it makes sense to directly represent the reinforcing material rather than represent it by its bulk properties. A common example is reinforced concrete, where for concrete damage modeling the concrete aggregate serves as the matrix and is meshed with solid elements. The rebar is represented by 1D elements defined as an “embedded region” within the concrete.

As a thorough example, I would highly recommend checking out this tutorial on analysis of a reinforced concrete beam in Abaqus/CAE by Dr. Clayton Petit: 2D Concrete Beam (Concrete Damage Plasticity).

Figure 15. Reinforced concrete beam damage modeling in Abaqus/CAE.

Summary & Conclusion

Composites are increasingly common as manufacturing costs decrease and designers seek to optimize structures for weight and efficiency. This article examined several approaches to analysis at various levels of detail, beginning with analysis of simple orthotropic materials in any package of SOLIDWORKS Simulation, to analyzing composites with various ply stacks in SOLIDWORKS Simulation Premium and ultimately the possibilities for analyzing failure modes such as delamination in detail with either desktop SIMULIA Abaqus/CAE or the cloud-connected 3DEXPERIENCE SIMULIA structural simulation roles.

Recent Articles

Related Stories

Enews Subscribe