 |
|
| |
|
Simulation
Details:
Simulation was performed using
ABAQUS 6.5, a commercial FE software package capable of simulating
highly nonlinear behavior. The 3D geometry of the FE model was defined
in Solid Works (CAD system) and read into the ABAQUS/CAE preprocessor.
The filter (Figure 1) consists of two functional parts: the Trans-catheter
Intravascular Ring Platform [TIRP], or "cage", and the filter element.
The parts are connected by fixation rings (also shown in Figure 1),
so that no relative motion between parts is possible at the connection
points.
All parts and rings are made of Shape Memory Alloy (SMA). The SMA
constitutive model available in ABAQUS is able to represent the super-elastic
behavior of this material. An example of a typical stress-strain curve,
based on material constants obtained from a uniaxial physical experiment,
is shown in Figure 2.
Each part of the filter (cage, filter element and fixation ring) was
analyzed separately. To test fracture risks due to high strain, the
cage and filter element were axially stretched to a nearly straight
configuration. At this stretch level, they can fit into the delivery
catheter (1.7mm diameter). At the end of that stage the strain level
is at its peak.
Due to the high aspect ratio of the structure, the element that best
expresses the physical situation is a first-order shear-deformable
(Timoshenko) beam element (B31 in ABAQUS). This element is adequate
for structures in which one dimension is significantly greater than
the other two dimensions, as is clearly the case at hand. It allows
for axial, bending and torsional deformation, as well as transverse
shear deformation. In addition, B31 is formulated so that its cross
section can change as a function of axial deformation in geometrically
nonlinear simulation. |
|
Figures 3, 4 and 5 show the resulting deformations at various stages of stretching in the cage and filter element respectively. The original undeformed geometry is shown in green.
In order to calculate
the strain field at the fixation rings, a detailed 3D model was built
of a ring and the wires it holds. The initial configuration of the
model is shown in Figure 6.
|
 |
Taking into account an overlap between the inner surface of the ring
and the outer surfaces of the wires as they are brought together,
the final geometry was obtained by solving the interference fit problem.
This was achieved in ABAQUS by a special contact solution option,
which allows the initial interference to be gradually eliminated over
several solution increments. In this configuration the wires were
compressed against each other and the initial ring shape was deformed
so that no interference existed between the ring's inner surface and
the wires' outer surfaces. The resulting strain field at the ring
is shown in Figure 7.
In order to calculate the fatigue factor and life of the device, the
alternating strain from the pulsating pressure inside the blood vessel
needed to be determined. To that end, two analysis steps were defined
to obtain the worst-case load conditions that the device can encounter
while in operation:
Step 1: Deployed configuration.
The cage was pressed between two rigid plates to a distance of a nominal
blood-vessel diameter. The strain field at the end of this step was
the base state for the fatigue-strain calculation.
Step
2: Obtaining the alternating strain. The
plates were moved toward each other to reflect the maximum diameter
change of the blood vessel. This step yielded the alternating strain
amplitude (change of strain from base state to final state).
|
|
| The FE model that was used for the cage is described above. In addition,
two rigid plates were defined to represent the blood vessel walls.
Figures 8 and 9 show side views of the device configuration in the
base and final states respectively. |
 |
|
|
|
Home
Shmulik Keidar Ltd