Composites Design and FEA Analysis with CATIA and SIMULIA¶
Summary. This example utilizes the CATIA Composites Design workbench and the Elfini workbench to create a composite part with material properties, ply stacking, and ply orientation and perform a ply level stress analysis to determine at which pressure and location failure is expected.
Defining the Composite Panel¶
The panel (figure) is a composite laminate composed of two seperate materials. The panel is clamped on all four edges, eliminating the rotational and translational degrees of freedom, and a pressure is applied normal to the undeformed surface. It is expected that the elongated hole will likely be a stress concentration of the panel, but it is not clear what pressure the laminate is capable of supporting. However, this information will be ascertained by performing the analysis using the Elfini Finite Element workbench in CATIA. From these results, the location and plies that are at highest risk of failure will be identified using the tsai-hill composite failure criterion, and with that information, design changes can be implemented to reduce the stress and risk of failure.
Panel Used in this Example
In CATIA, the Composites Design Workbench allows us to create surfaces and assign the parameters defining the composite (figure), as well as easily validating the producibility of the part based on the curvature of the part. All the material properties, and composite parameters, such as ply thickness, orientation, material type, weight, etc are stored in the CATPart file created in the CPD workbench (figure).
Composite Parameters
The choice of material can be changed in the CATMaterial file if multiple materials are used, such as carbon fiber, fiberglass, epoxy, etc.
One of the challenges when designing with composites is that, due to the typical complexity of a composite part, the part design and simulation results can be difficult to visualize, and choosing the correct design parameters required to properly define the part is often unclear. A ply table is a simple way to understand how the composite is constructed. The table shown in (figure) shows how the composite is organized with ply number, material, and orientation. The ply table can be used interactively with the 3D model to look at the ply properties. The plys of interest for this example are highlighted in orange. These plys are on the top and bottom and cover the entire composite and make up the elongated hole, which is the expected maximum stress of the laminate. There are a total of 5 plies that make up the elongated hole, 3 on top (Ply.37,35,36) and 2 on the bottom (Ply.33,34)
Ply Table
If we want to see the actual shape and stacking of a ply, we can navigate to the CATIA tree in Stacking Engineering (figure), and we see Ply.37 is glass and Ply.35 is S1454-G803
Ply 1 and 2
Another useful visualization is the ply exploder. The ply exploder generates a 3D visual of the individual ply stacks based on the color defined for that ply.
Ply Exploder
Simulation Pre-Processing¶
In the CATIA CPD (Composites Part Design) workbench, we define many of the properties that we need for a finite element simulation. The material properties and orientation can be time-consuming when pre-processing models, but in Simulia, the process is streamlined due to the workbenches being well-integrated, eg the interactive ply table.
Loads and Boundary Conditions¶
The boundary conditions are clamped edges, which constrains all 6 degrees of freedom for the surface edge (rotation and translation). The load applied is initially a $10\ KPa$ pressure applied normal to the undeformed panel surface, indicated by the yellow arrows (figure).
FEA Setup
Within the Elfini workbench, additional visualization tools are available. This allows the engineer/designer to confirm designs are correct as well as making communication much easier for assembly or if modifications are necessary. One of such tools is the thickness fringe plot (figure) and the ply angle plot (figure).
Thickness Fringe
Lamina 4 angle plot
Once we have the boundary conditions and loads applied, we can compute the model. After about 20 seconds, we have our displacement, strain, and stress calculations for each ply.
Post-Processing¶
The simulation generates a large amount of data that can be cumbersome to digest, but using tools, such as specialized composites failure criteria, can make the analysis much easier and more robust. A summary of the important material properties (modulus of elasticity and material ultimate strength in compression and tension) are shown as a reference to the calculations. The complete material properties are shown in the Appendix in section (Appendix).
Property S1454-G803 Glass
$E_{x}$ 60 GPa 4 GPa
$E_{y}$ 60 GPa 4 GPa
$\sigma_{x-comp-ult}$ 500 MPa 40 MPa
$\sigma_{y-comp-ult}$ 500 MPa 40 MPa
$\sigma_{x-ten-ult}$ 700 MPa 60 MPa
$\sigma_{y-ten-ult}$ 700 MPa 60 MPa The availability of the field outputs is based on what the user requested in the pre-processing step. This example shows contour plots of stress, displacement, and the tsai-hill failure criterion. The mesh has been created relatively coarse for speedy calculations, but an actual engineering application should have a higher element density. Some examples of displacement visualizations are shown in figure and . In the figure , the displacement contour lines are overlaid on a deformed model mesh based on the the 3-dimensional displacement values.
Deformed mesh displacement plot of ply.37
The discontinuous contour plot in figure with deformation is a simple-to-interpret visual to the analyst on the validity of the results as well seeing the large deformation areas of the structure due to the various locality of plies with the relative cumulative thickness.
Deformed contour displacement plot of ply.37
Stress is the measurement that is most important because our failure metric is defined as a experimentally pre-determine stress. To properly investigate this composite, each ply should be reviewed after the simulation is complete.
After a load of $P_{applied}=10\ kPa$ is applied to the panel, the von-mises stress ($\sigma_{v}$) with the fiber orientation shows that, in figure ply.34 has the largest von-mises stress.
Since this is a linear FEA problem, the results are only likely valid for small deformations, and so, the relationship between applied load and stress should be linear. Also, a common assumption in composite analysis is assuming that out-of-plane stress is 0, known as plane stress ($\sigma_{3}=0$). With these assumption, we can assume that ply.34 will be the highest risk ply, and by inspection, ply.34 does indeed have the highest stress of all the plies. The von-mises stress is a handy scalar stress equivalent due to its ease to interpret results. (although other stresses, such as principal stresses should be observed to confirm validity of results). The plots here show the mean ply stress as well as the fiber orientation of the ply.
Von-Mises Stress
The stress state of Ply.34 is show in an undeformed state with a contour plot of von-mises stress . When looking at the entire composite, the stress concentration is where it was expected to be, in the elongated hole.
Exploded plys with von-mises ply stress of ply.34
When performing a stress analysis of a composite, iterations of the calculation of stiffness must be made to calculate the global structure stiffness. Once the global stiffness is calculated, the global displacement, strain and stress is determined. However, failure of a composite often occurs first to a ply, and since plies can have various stresses due to potentially differing material properties and loading states, the local ply stress must be determined and corroborated to the material strength to determine if ply failure is anticipated. The failure criterion commonly used for composites is the tsai-hill [Daniel2006]. The tsai-hill criterion is adapted from the von-mises criterion, which is defined as failure when the material yields. Typically, long-fiber composites are transversely isotropic. With this assumption, we can write the tsai-Hill criterion here (2). Once this value exceeds 1, the ply is expected to fail
The tsai-hill criterion is easily accessible in Simulia to determine if failure is expected. The contour plots in figure is for our initial loading case of $10\ KPa$, which is well below 1, indicating that our composite part is not likely to fail. Also of importance is ply.34, which has the largest tsai-hill parameter, or nearest to failure, which agrees with our linear stress-load assumption.
Tsai-Hill Failure Criterion
For this component, the pressure it must withstand is 125 kPa, so if we increase the pressure load, the tsai-hill failure criterion exceeds 1.0 and failure is expected in ply.34. The principal local stress were observed to be:
An example calculation of the von-mises stress agrees well with what the model
If we use these values with the strength values defined previously, we find that the hand calculation of the tsai-hill parameter is near $1.0$, and the Simulia tsai-hill parameter exceeds 1 at 1.05 as shown in the image below. Also, we provided the failure stress in the material properties as $\sigma_{ut}=700 Mpa$ and $\sigma_{uc}=500 MPa$
This discrepancy is difficult to prescribe, but it is likely due to the coarseness of the mesh. The hand-calculation versus the Simulia value is a considerable difference, so a finer mesh should be used. But, no failure criterion is deterministic, so the value being relatively close to 1 would indicate that failure is probable and a redesign should be implemented.
Final Failure of the composite is ply 34
Summary¶
An example of a composite stress analysis using CATIA-Simulia was shown. The composite properties were defined in CATIA's composite part design (CPD) workbench, and imported into Simulia FEA and solved prednisone using the Elfini FEA workbench as a 2D, plane stress surface. The tsai-hill criterion was used to evaluate each ply and it's severity of stress relative to the strength. Ply.34 was found to be at the highest risk of failure and future designs of this panel should use this information to improve the strength, minimize the deformation, utilize different materials and layups. The files to execute this example can be freely obtained from the author if requested.
References¶
- I. M. Daniel and O. Ishai. Engineering Mechanics of Composite Materials, 2nd edition, Oxford University Press, 2006.
Appendix¶
The glass material properties, which refers to an epoxy, with $E=4\ GPA$, and $\sigma_{ult}=60 MPa$
Glass Properties
and the fiber material, with $E=60\ GPA$ and a $\sigma_{ult}=700 MPa$. This is the strength that we will use for our failure criteria. The constitutive properties are isotropic, however the tensile/compressive strength vary, which will ultimately determine the maximum pressure that can be applied.
Lamina Properties
Comments
comments powered by Disqus