Analysis of Composite Aerospace Structures

Finite Elements Professor Kelly

John Middendorf #3049731

Assignment #3

I hereby certify that this is my own and original work.

Signed,

John Middendorf

Analysis Objective

Using a composite material, an airfoil is to be analyzed in Patran/Nastran with the

following dimensions and design requirements.

Loads and Boundary Conditions

The airfoil is subjected to a upward pressure load of

10kPa on the top surface, and fixed by six points on

the rear spar.

Composite Material

The composite consists of

8 layers of 0.2mm thick

pre-preg composite fabric

modeled as a 2D

orthotropic material with

the properties as shown

on the right:

The layup of a single layer of the composite is modeled as a laminate in Patran and has

the following properties:

Shell Modeling

Finite Element modeling offers the ability to model thin walled structures as 2D shells.

Because the surface area to wall thickness for this airfoil is less than the rule of thumb

10:1 ratio, 2D shell modeling, which assumes transverse normal and shear stresses are

small, is appropriate. Some sources the 10:1 ratio is based on element area, while other

sources, part area; both will be considered in the following analysis. Shell elements need

to model both axial (membrane) stresses and bending moments. Quadratic Quadrilateral

(Quad 8) elements were chosen for this problem, which are more accurate in cases which

involve bending, than triangular or Quad 4 elements.

Orientation is an important consideration when using shell elements. When properties are

assigned to a element in Patran, the program uses the element’s specific coordinate

system to apply the properties. The x and y axes are oriented in the plane of the shell,

and the z axis is normal to it. Therefore, when creating the geometry and mesh for this

2D shell analysis, it is important to be aware of each individual element coordinate

system to ensure proper modeling, and to make sure the z axis is coming out of plane for

each shell surface modeled.

Model Geometry

Three groups were created in Patran, one for the spars and ribs, one for the top surface

and one for the bottom surface. Each segment was modeled as an individual surface to

ensure proper meshing at each junction (as opposed to joining adjacent co-planar

surfaces). Surface normals were verified for each surface in each group:

Elements

Quad 8 elements were used, and

consistent XY orientation was

attained by the sequence of the

selection of curves to create each

surface. This wasn’t completely

necessary, since our material has

equal properties in the x and y

directions. I verified this by running

some simple tests with varying

configurations on the sample shown

(below right), and compared the

results with the property-equivalent

isotropic material (this sample was fixed

on one corner and a pressure load applied

on the top surface). The important

consideration for correct property

association is the element normals, which

follow the surface normals.

Note: comparison runs were made with Quad 4

and Tria elements, both of which produced stiffer

result(i.e. less flexural deformation). It was important for this model to err on the side of less stiffness,

rather than more. See Appendix.

Mesh Creation

Two meshes were studied for the

final results, one with a nominal

40mm global edge length, the

other with a nominal 20mm

global edge length. The default

isomesh was used as shown on

the right. Nodes were of course

equivalenced after each complete

mesh creation of each group.

Because the results were similar,

and also because a finer mesh

would have exceeded the rule of

thumb element area to thickness

ratio of 10:1, the two (40mm and

20mm) meshes were considered

adequate for the results.

Fixing the Mesh

The default mesh created quite a few elements that were out of range in terms of aspect

ratio and skew. These were all located at the trailing edge of the rib surfaces, where a

overly stiff model could give poor results. Therefore I went through a process to mend

each mesh to model more

accurately using the following

steps:

1. Create the mesh for the

ribs

and spars.

2. Fix the bad elements by

splitting them along the

longer edge, until all

passed the verification

test.

3. Mesh the top and

bottom surfaces

separately with the global

edge length.

4. Equivalence the nodes and

check to ensure proper

mesh connections.

5. Assign properties and run

model.

Fixing the mesh (continued)

The final triangular elements in the rib isomesh mesh

also had very poor aspect and skew ratios. After some

trial and error of producing proper tip triangular

elements, I decided that I could eliminate these

elements, and model the tip without them, on the

assumption that in reality the final sharp edge of the

ribs probably gives little overall strength to the

structure, and the ill-conditioned elements in the model

could overestimate the stiffness. When the nodes of the

top and bottom surface were equivalenced with the

nodes of the ribs and spars, the resulting nodes describe

a model that is bonded to the upper and lower surfaces

at key element points, essentially modeling a series of

riveted joints for the final section of the rib/top and

bottom surface connection. This is in keeping with

making only assumptions that will under-stiffen the structure, since we want to be

conservative in our deformation analysis. Typical results shown below right indicate no

undue deformation due to the lack of final tip elements.

Results: Single Layer of Composite Material

Above: One layer of composite deformation fringe.

Below: Trailing edge tip deflection XY plot.

Even with one layer of composite, the design meets the tip deflection requirement of

25mm. The 2mm panel deflection relative to the edge is another story. Here the “bubble”

dimension it is clearly greater than 2mm.

Results: Two Layers of Composite

For two layers, a composite of composites was created in the material database, and

applied to all surfaces:

Results: Two layers (continued)

On the right is the tip deflection

for the solution with two layers

of the composite laminate, with

the 40mm mesh.

The bubble dimension is not as

easy to determine as the tip

deflection. Because of the

deflected angle of the airfoil, the

maximum height of the bubble

does not correspond to the

maximum displacement given by

the deformation fringe result.

The actual distance of the height of the bubble form the edge is relative to the deformed

edge profile. In the XY graph below left, it is relative to the difference between the upper

curve, which is plotting the y values for deformation along the line that goes through the

point of maximum deformation, and the lower curve, which is the deformation plot of the

edge of the airfoil (measured at the top edge of an end rib). The actual value of the height

of the bubble can be found by multiplying the difference between the two curves by the

cosine of the deflection angle. The deflection angle is approximately 0.27 (the arctan of

3.3/700), the cosine of which is essentially 1 (0.9999). After going through the

mathematics of how to calculate the equivalent edge deformation in the deflected state

from the XY values of the original state, it was decided to approximate maximum bubble

deformation. Here, for the two ply, reading off the XY plot below, it is about 5.3mm-

1.5mm= 3.8 mm.

Bubble Estimation

In order to estimate the bubble, I also tried fixing the bottom surface of the ribs, which

gave the following results:

Above: Fixed bottom center spar edges. Above right: tip deflection for fixed spar run.

These results seem to underestimate the actual bubble height, in addition, the center top

surface panel is pulled up by the upward pressure, rather than deflecting downward as in

the normal run with only the control surfaces fixed.

In any case, two layers of composite layup does not meet the 2mm bubble deflection

requirement. On to three layers, next.

Results: Three layers of composite.

Above: Deformation Fringe plot with three

layers of composite.

Left: Tip deformation XY plot.

Three Layer Analysis

Again, fixing the bottom spars gives us a rough idea of the bubble deflection:

But more accurate numbers come from reading the graph plotting the end rib top edge

deflection and the center line of the maximum deflection curve:

Here, the maximum value of the bubble height to be around 2.65-0.9=1.75mm, which

meets the 2mm requirement. Therefore, 3 layers of laminate material are required.

Results: 20 mm mesh run to confirm result of coarse mesh:

The finer mesh confirms the coarse mesh results (where max deformation was 2.56).

Maximum bubble is again around 2.65-0.9 = 1.75mm. This is a conservative estimate,

but three layers of composite layup meets all requirements for the problem.

ANSWER: Three layers of composite required.

Bonus Pages

Shape of Final Deformation (three layers of laminate)

Four Layer Solution:

Appendix: Comparison of element types

All runs below run with default 40mm global length isomesh, and 2 layer laminate

properties assigned to each element.

Above: Default unmodified isomesh (with 48 elements not meeting default Patran

Reliability Threshold). Max deformation= 5.10mm. Quad 8 elements.

Above: Quad 4 elements. Max deformation= 5.01mm. Stiffer than Quad 8 elements.

Above: Tria elements. Max. Deformation =4.62mm. The stiffest of the lot.