Linear static analysis of laminated composites in Abaqus (Structures module of aerospace program at University of the West of England)

1. Aircraft underbelly composite structure
(fairing) modelling in Abaqus CAE
By
Dr Mahdi Damghani
24/03/2019 1

2. Introduction
• Underbelly structure/fairing (yellow highlighted in
below figure) is regarded as a secondary structure
and hence does not carry significant and critical
load.
• It is riveted to the surrounding structure so can be
conservatively idealised as being simply supported
on all edges.
• The total pressure on the panel including both
aerodynamic and internal pressure are 0.02MPa.
• It is made of uni-directional Carbon Fibre
Reinforced Polymer (CFRP) with stacking
sequence [45/-45/02/45/-45/902/02]s giving 40%
0deg, 40% 45deg and 20% 90deg plies.
24/03/2019 2

3. Introduction
• The material mechanical properties for the CFRP are given as
below:
• Some of the values mentioned above are assumed values.
• We intend to obtain:
• Stresses and strains under static loading.
E11
(MPa)
E22
(MPa)
G12
(MPa)
G13
(MPa)
G23
(MPa)
ν12 ν13 ν13 t (mm)
117333 10544.5 5582 5582 3538.2 0.3 0.3 0.49 0.187
24/03/2019 3

4. Introduction
• The structure is a single curvature panel and
is assumed to have geometrical dimensions
(in millimetres) as the opposite figure;
• The geometries mentioned here do not
represent those of a real aircraft and are given
for demonstration purpose only.
• Material direction, i.e. 0deg orientation, is also
given as opposite.
24/03/2019 4
4000 mm
R=8000 mm
0
90

5. GEOMETRY GENERATION
24/03/2019 5

6. Step 1
• Create a deformable 3D shell
extrusion of the panel as
illustrated in the opposite
figure.
24/03/2019 6

7. Step 2
• Create the 2D arc profile
using “Thru 3 points”
approach;
• Dimension the arc giving it
radius of 8000 mm using
dimensioning tool
24/03/2019 7

8. Step 3
• Extrude the arc profile to
the amount of 4000 mm
until you get the final shape
of the structure as shown in
the opposite figure.
24/03/2019 8

9. MATERIAL, SECTION & ORIENTATION
DEFINITION
24/03/2019 9

10. Step 1
• Create Elastic material;
• Give it a name such as
CFRP;
• The type of material should
be selected as Lamina.
24/03/2019 10

11. Step 2
• Enter the material
mechanical
properties as shown.
• Bear in mind that we
are using mm and N
as the consistent
unit.
24/03/2019 11

12. Step 3
• Create a shell
composite section
as shown and then
PRESS Continue…
.
• Go to Steps 4 & 5.
24/03/2019 12

13. Note
• There is another way of assigning composite section to your
structure which is also provided in this tutorial regarded as Steps
3’a, Step 3’b and Step 3’c shown in the next two slides.
• It is your choice to adopt one of the two approaches.
• If you adopt for step 3’a, 3’b & 3’c instead of Step 3 then steps 4
and 5 are not required.
24/03/2019 13

14. Step 3’a
• Go to composite
menu and create a
stacking sequence
as shown
24/03/2019 14

15. Step 3’b
• Populate the
stacking sequence
information as
shown in the
opposite figure.
24/03/2019 15
For each ply select the CSYS
we defined previously as the
The entire panel is picked for
the region for each ply.
Symmetric lay-up is chosen so
only half of the lay-up is defined.
For each ply select the CSYS
we defined previously as the

16. Step 3’c
• Plot a visualisation of
your stack.
• Since we used CSYS
for material orientation
definition we cannot
see ply directions
visually.
24/03/2019 16

17. Step 3’c note
• As opposed to previous
slide, using the global
coordinate system to be
projected onto the panel
for material orientation
determination will allow
the visualisation to show
you ply orientation better
as shown in the
opposite figure.
However, we have
assigned a CSYS
ourselves so previous
slide is how it shows the
orientation.
24/03/2019 17
If a CSYS was not chosen then
the global coordinate system will
be project onto the panel for
material orientation determination.
Projection of x and y axes will be 1
& 2 directions, respectively.

18. Step 4
• Define the stacking
sequence for the
structure and give the
thickness, material
type and orientation
for each ply as
shown.
• Bear in mind that
since the lay-up is
symmetric, I defined
only half of the
thickness (10 plies
only) and checked the
symmetric option.
24/03/2019 18

19. Step 5
• PRESS Assign
Section button (see
red rectangle
opposite).
• Select the fairing
structure and press
Done for the section
to be assigned.
• Then your fairing get
green colour
suggesting it has the
section assigned to it.
24/03/2019 19

20. Note
• So far, Abaqus does not understand what direction is 0deg, 90deg
or even 45deg.
• We need to create a coordinate system.
• The created coordinate system will be projected onto the structure.
• The projected directions will be named in Abaqus as 1, 2 and 3
directions on which E11, E22 would to be acting upon.
• For example E11 will be modulus of elasticity in direction 1 and
similarly E22 is for direction 2. G12 suggests shear modulus in plane
12.
24/03/2019 20

21. Step 7
• Create a rectangular
coordinate system
for material
orientation.
• Use 3 Points
method as shown.
24/03/2019 21

22. Step 8
• Select the points as
shown for various
axes of the
coordinate system
to be defined and
PRESS Done.
24/03/2019 22
Origin of CSYS
Point lying on x
axis
Point lying on y
axis

23. Step 9a
• Go to Material
orientation menu
and give the defined
coordinate system
as the material
orientation.
24/03/2019 23

24. Step 9b
• Once you assign the
coordinate system the
opposite figure
appears showing the
direction of 1, i.e.
0deg, 2, i.e. 90deg and
n, i.e. stack direction.
• PRESS OK.
24/03/2019 24

25. CREATING AN ASSEMBLY/INSTANCE OF
THE GEOMETRY
24/03/2019 25

26. Step 1
• Create dependant
instance of the
geometry as shown
in the opposite figure.
24/03/2019 26

27. CREATING ANALYSIS STEPS
24/03/2019 27

28. Step 1
• Create a static load
step as shown.
24/03/2019 28

29. CREATING FIELD OUTPUT FOR
COMPOSITE
24/03/2019 29

30. Step 1
• For the Domain click
on Composite Lay-
Up.
• For output variables
select all stresses.
• This will allow you to
have stresses in
each individual ply
for post-processing.
24/03/2019 30

31. CREATING BOUNDARYCONDITIONS AND
LOADING
24/03/2019 31

32. Step 1a
• Create pressure
loading for static step
as shown
24/03/2019 32

33. Step 1b
• Select the brow side
as the internal side.
• After pressing the
brown side you will
be prompted to input
pressure value.
• Give pressure value
of 0.02 MPa.
24/03/2019 33

34. Step 2a
• Go to BCs and apply
boundary condition
for “Initial” step at all
edges of the panel.
• This will make sure
that all other steps
will inherit this BCs.
24/03/2019 34

35. Step 2b
• Constrain displacement
degrees of freedom
only as we are
conservatively
assuming a simply
supported boundary
condition.
24/03/2019 35

36. SEEDING AND MESHING THE PANEL
24/03/2019 36

37. Step 1
• Seed the part using
approximate global size of
250.
• Bear in mind that the
choice of seeding density
is subject to mesh
sensitivity study and the
current value is chosen for
demonstration purpose
only. Evidently, the lower
the global size the more
accurate are the results.
24/03/2019 37

38. Step 2
• Go to mesh control
menu and choose
structured meshing
algorithm.
• Make sure Quad
elements are chosen
as the use of Tri
elements is best
avoided since they
give constant strain
across the element
and are not accurate.
24/03/2019 38

39. Step 3
• Go to element type
and select Quad
element Reduced
integration type for
the panel.
24/03/2019 39

40. Step 4
• Mesh the part as
shown.
24/03/2019 40

41. CREATING ANALYSIS JOB
24/03/2019 41

42. Step 1
• Create a full
analysis job and
submit the job for
analysis.
24/03/2019 42

43. EXPLORE THE RESULTS
24/03/2019 43

44. Step 1
• Go to Field Output
to select the kind of
output required for
further processing.
24/03/2019 44

45. Step 2
• Select stress
components and
maximum in-plane
stress invariant.
• Go to Section Points
and from there you
can request stress in
each ply.
24/03/2019 45

46. Step 3
• Contour of maximum
in-plane principal
strain.
• In practice these
values are compared
against maximum
strain allowable that
are obtained from
experimental test to
make sure the panel
does not fail. Principal
strains must be below
allowable strain.
24/03/2019 46

47. Step 4
• Contour plot of total
quantity of displacement
on the panel.
24/03/2019 47