3. 1. INTRODUCTION AND MOTIVATION
1.1 Challenge of Recording Drums
Capturing drum audio has long been regarded as a very difficult problem, particularly in a studio setting. To
record a drumset, one microphone is mounted on the rim of each drum, at least two microphones are placed
overhead, and several others may be positioned throughout the room. Of all the studio instruments, the drumset
is the only one that requires multiple microphones to record, and this introduces complications. While the mics
on each drum head are directional, there will always be bleed between tracks, meaning that the signal produced
by one drum will be picked up by the other mics. In addition to bleed, the overhead and room mics, which are
omnidirectional, are intended to pick up the signals produced by the entire drumset, in order to produce a fuller
sound. Add in the other instruments that may be in the room when doing a live recording, and the drum tracks
easily end up with a lot more than just drums. While there are many cases in which this is acceptable or even
desired, having the ability to produce truly isolated drum tracks opens the doors to a greater level of control in
which ambient noise can be added in by choice, and not by necessity.
When sound from a drum is picked up by multiple microphones at different distances from the source, the
problem of phasing is introduced. Phasing occurs when two or more waves of the same wavelength interfere
with each other due to their relative spatial relationship. When the peak of one wave occurs at the same point
as the valley of another, they will destructively interfere, resulting in a weaker overall signal produced by the
difference in amplitudes. Such waves are said to be out-of-phase. If instead the peaks of two waves occur at the
same point, they will constructively interfere, resulting in a stronger overall signal produced by the sum of their
amplitudes. Such waves are said to be in-phase. Because the signals recorded by each microphone are ultimately
added together in the overall mix, destructive interference can greatly diminish the sound quality of individual
drums.
In an effort to avoid the audio problems introduced by phasing, the process of miking a drumset is cumber-
some, delicate, and time consuming. Eliminating phasing involves positioning microphones very carefully with
respect to one another in order to ensure that the pressure wave that reaches each mic is in phase for every
drum. The human hearing range spans frequencies of 20 Hz to 20,000 Hz and wavelengths of about 17 m to 17
mm (assuming a speed of sound of 340 m/s), while drums typically span frequencies of 50 Hz to 600 Hz and
wavelengths of about 6.8 m to .56 m. Therefore in order to avoid destructive interference, adjustments as large
as a few meters may need to be made to mic positioning. Especially when space is limited, it can be difficult to
avoid phasing altogether when miking an entire drumset.
1.2 Recording Without Microphones
Some instruments, such as electric guitars, violins, and keyboards, do not require microphones to record, but
can instead be plugged in to extract the signal directly. This is very convenient as the sound is being extracted
from the mechanical vibrations of the instrument, eliminating the effects of external sound sources.
Using the electric guitar as an example, the vibrating metal string produces an oscillating magnetic field that
is converted to an electrical signal through its pickup. This signal can then be amplified for a live performance
or recorded directly. I would like to apply this same principle to drums, to analyze the feasibility of using the
vibrational motion of a drum head to produce an electrical signal. If such a system could be created, recording
drums would be as simple as plugging each drum into a recording studio without the complications introduced
by a multi-mic setup.
This report will serve to analyze the motion of a drum head using Finite Element Analysis through Abaqus
CAE, and analyze what would be required to use vibrational motion to replicate the sounds we hear.
1.3 Practical Considerations
While this report will not comment on the implementation of a sensor system to acquire the necessary data, there
are several things to keep in mind when evaluating such a system. First, it must be able to withstand motion of
the entire drum that occurs while playing. The impact of the drumsticks will cause the drum shells to vibrate,
and the entire drum to shift on its mount. The sensor system must be able to take accurate measurements and
must therefore have a sturdy mounting system. Second, the sensors cannot affect the motion of the drumhead
4. itself in any way. Third, the system should be capable of attaching to an existing drum. This implies that sensors
cannot be embedded in the drum heads, reflective coatings cannot be applied to the heads, and that nothing
should come into contact with the head during its motion.
2. THEORY OF DRUM HEADS
Before discussing the finite element implementation of a drum head, the theoretical background of drums must
be considered. Drums come in many different forms, with perhaps the most basic being a tom-tom drum used
in drumsets, as depicted in Figure 1.
Figure 1. A tom-tom drum used in drumsets has a very simple construction consisting of a cylindrical shell and tension
rods (left). These drums are fitted with drumheads on one or both of the shell ends (right). Both the drums and the
heads come in a variety of sizes and styles.
These drums consist of cylindrical shells usually made of finished wood, fitted with a circular membrane, or
drumhead, that is secured in place by a metal rim that attaches to the shell with adjustable tension rods. The
tension rods are adjusted with a drum key and used to control the tension in the head, and therefore affect the
pitch produced when struck.
Drumheads are made with many different styles in order to manipulate the sound they produced. Some
are double layered, coated with another material, or fitted with damping regions as shown in Figure 2. The
primary material is called Polyethylene Terephthalete (PET), more commonly referred to as Mylar R
, and is a
thermoplastic polymer with high tensile strength. It can exist in both an amorphous or semicrystalline state
depending on the manner in which it is processed, allowing for variation in appearance. Amorphous Mylar is
clear, while semicrystalline Mylar can be transparent, opaque, or white. In addition to being used in drumheads,
Mylar is also used for flexible packaging, as insulation for houses, or in the sails of high performance sailboats.
2.1 Drumheads as Membranes
From the perspective of structural theories, drumheads obey the membrane theory of shells, which is simplified
case of plate theory. Plate theory describes structural elements that have a small thickness relative to their planar
dimensions, and arbitrarily curved plates are referred to as shells. Thin shells are referred to as membranes,
in which shear and bending moments are small enough to be considered negligible. Membrane theory provides
the structural foundation for the drumhead FEA, and is discussed in much greater detail in a later section,
Membrane Theory.
5. Figure 2. Drumheads can be coated (left), lined with damping rings (center), or impact regions (right).
2.2 Vibrational Motion
A drumhead is a two-dimensional circular membrane that vibrates in three-dimensional space. In order to
understand the dynamics of a drumhead, it is useful to start with the simplified model of a one-dimensional
string vibrating in two-dimensional space, as is the case with a guitar string. In order for a string to oscillate,
it must be subjected to a tension, otherwise there will be no restoring force to cause vibrational motion. To
understand the behavior, consider tracking the motion of each particle that makes up the string. The slope
of the string at any given particle is assumed to be small enough that the displacement can be assumed to be
entirely vertical, such that displacement in the y-direction is defined as (all equations in this section from1
):
y = u(x, t) (1)
Several other important quantities are defined as:
Mass Density: λ(x) [mass/length]
Tensile Force: T(x, t) [force]
Body Force: B(x, t) [force/mass]
String angle: θ(x, t) [rad]
Slope:
dy
dx
= tan(θ) =
∂u
∂x
Consider a small segment of rope over the region x to x + ∆x. By using solving for force equilibrium in the
vertical direction:
ma = F (2)
[λ(x)∆x]
∂2
u
∂t2
= T(x + ∆x, t) sin(θ(x + ∆x, t)) − T(x, t) sin(θ(x, t)) + [λ(x)∆x] B(x, t) (3)
Taking the limit as ∆x → 0:
λ(x)
∂2
u
∂t2
=
∂
∂x
[T(x, t) sin(θ(x, t))] + λ(x)B(x, t) (4)
Using a small angle approximation:
λ(x)
∂2
u
∂t2
=
∂
∂x
T(x, t)
∂u
∂x
+ λ(x)B(x, t) (5)
Tension can usually be assumed to constant, in which case T → T0. If the body force (ie. gravity) is very small
compared to the tension force, which is usually the case, then it case be neglected:
λ(x)
∂2
u
∂t2
= T0
∂2
u
∂x2
(6)
6. By making the substitution c2
= T0/λ(x), the result is the one-dimensional wave equation:
∂2
u
∂t2
= c2 ∂2
u
∂x2
(7)
This represents a partial differential equation (PDE) that can be solved using separation of variables, such that
u(x, t) = φ(x)h(t). Plugging this into the wave equation, the system becomes:
φ(x)
d2
h
dt2
= c2
h(t)
d2
φ
dx2
(8)
1
c2h(t)
d2
h
dt2
=
1
φ(x)
d2
φ
dx2
= −k (9)
where k is a constant value.
By imposing the spatial boundary conditions that the string is clamped at both ends, φ(x) must take on the
shape of a sine wave, and k must take on discrete values:
φ(x) ∼ sin
nπx
L
, k =
nπ
L
2
; (n = 1, 2, 3...) (10)
The temporal function must take on the form:
h(t) = c1 cos(ct
√
k) + c2 sin(ct
√
k) (11)
Putting the two solutions together, the displacement is given by an infinite superposition of an orthogonal set
of solutions:
u(x, t) =
∞
n=1
sin
nπx
L
An cos
nπct
L
+ Bn sin
nπct
L
(12)
These solutions are called the normal modes (or harmonics) of vibration. The sound produced by the string
consists of the superpositions of the infinite number of natural frequencies:
ω = 2πf =
nπc
L
; c =
T0
λ
(13)
In the case that the string is fixed at both ends, these natural frequency produce standing waves, in which
the waves appear to be stationary with nodes at which there is no displacement, and antinodes at which there
is maximum displacement. The first 5 normal modes are displayed in Figure 3.
2.2.1 Vibration of Circular Membrane
Now, consider a circular membrane of radius a. The wave equation defined in equation 7 can be generalized to
two dimensions as:
∂2
u
∂t2
= c2 ∂2
u
∂x2
+
∂2
u
∂y2
= c2 2
u (14)
where c2
= T/σ.
Again, assume that the slope of the membrane at any point is small enough that displacement is entirely
vertical, allowing displacement to be defined in cylindrical coordinates as:
z = u(r, φ, t) (15)
Other important quantities are defined as:
Mass Density: σ(r, φ) [mass/area]
Tensile Force: T(r, φ, t) = T0 [force/length]
7. Figure 3. The first five normal modes of vibration for a string of length L.
By assuming a clamped rim, such that u(a, φ, t) = 0, the wave equation can be solved in the same manner is in
one dimension, but the solution takes on a slightly different form. The circular symmetry about the origin and
the conditions this imposes requires the use of Bessel functions in the solution:
u(r, φ, t) =
∞
m,n
Jm ηmn
r
a
cos(mφ) [Amn cos (ηmnωt) + Bmn sin (ηmnωt)] (16)
where ω = c/a, Jm is the mth
Bessel function of the first kind, and ηmn is the nth
root of Jm.
Assume that the membrane starts entirely in the xy plane with no vertical displacement, and that the initial
velocity is determined by the location of an impact on the membrane surface:
u(r, φ, 0) = 0, ˙u(r, φ, 0) ∼
1
r
δ(r − d)δ(φ) (17)
where d is the distance of the impact point from the center and δ(·) is the Dirac-delta function. Using these
initial conditions, the constant coefficients Amn and Bmn can be written as:
Amn = 0, Bmn =
D
ηmn
Jm ηmn
d
a
[Jm+1 (ηmn)]
2 (18)
where D is an arbitrary constant that determines the overall amplitude.
2.2.2 Normal Modes of Circular Membrane
The normal modes of a circular membrane are characterized by a pair of indices (m, n), where m represents the
number of nodal diameters through the center, and n represents the number of nodal circles about the center
8. Figure 4. The first 12 normal modes for an ideal circular membrane. The lines represent nodal diameters and circles, and
the decimal below each shape represents the frequency ratio of the mode relative to the fundamental frequency for mode
(0, 1).3
(including the rim). Nodal diameters and circles are analogous to nodes in one dimension, and represent paths
along which there is no displacement. The first 12 modes are displayed in Figure 4.
The frequency for each mode is given by:
fmn =
ηmnc
2πa
=
ηmn
2πa
T
σ
(19)
where ηmn is the nth
root of Jm, c is the wave speed, and a is the radius of the membrane. Using this expression,
the fundamental frequency is given by:
f01 =
2.405
2πa
T
σ
=
2.405
2πa
c (20)
The frequency ratios shown below each mode in Figure 4 are defined relative to frequency f01.
If there is any irregularity in the membrane, such as an uneven coating, or a damping ring of mylar, the mode
shapes and frequencies will all change. This irregularities are often added intentionally in order to manipulate
9. the sound in a particular way. Furthermore, a real drumhead will provide some resistance to shear and bending
that will in general raise the modal frequencies, while membrane theory assumes no such resistance.
The membrane model is clearly an idealized one, but it will certainly serve the purpose of displaying the
general behavior of a standard drumhead.
2.3 Drumsticks and Impact
Drumheads are generally struck by drumsticks, such as those depicted in Figure 5. Like drumheads, drumsticks
come in many different styles, and even materials. Generally, the sticks are made out of wood, but the tips (also
called “beads”), are sometimes made of Nylon to provide different sound and feel.
Figure 5. Drumsticks are used to hit drumheads, and come in many styles. Top left shows a standard set of all-wood
drumsticks. Top right shows a variety of stick and tip styles. Bottom shows a pair of sticks with nylon tips.
Perhaps the most crucial component of the analysis is the contact of the stick with the head, as this is the
driver for all vibrational motion that follows. A study was conducted in which the tip of a drumstick was fitted
with an accelerometer and a piezoelectric crystal as shown in Figure 6 in order to measure the contact time,
force, and acceleration of the drumstick during a stroke.3
The results are shown in Figure 7.
The primary results of interest from the data shown in Figure 7 are the initial contact time of approximately
3 ms and peak force of about 100 N.
The dynamics of membrane vibration, as well as the geometry and loading conditions of the problem have
been defined. This provides a foundational understanding of the problem to be modeled using finite element
analysis.
10. Figure 6. Drumstick fitted with an accelerometer and piezoelectric crystal in order to measure force and acceleration
during impact with the drumhead.
Figure 7. Measured force, contact time, and acceleration during a stroke and impact with the drumhead. The horizontal
lines below the force signal indicate contact between the stick and head. Letters A and D mark an influence of the
drumstick vibration on force and acceleration. Letters B, C, E, and F mark the interaction of the drumstick with a
traveling wave on the drumhead.
11. 3. THEORY OF FINITE ELEMENT ANALYSIS
In order to understand the workings of an Abaqus analysis, we must first understand the concepts of finite
element analysis (FEA) and the building blocks that make it possible. Then the equations and derivations of the
fundamental quantities that lay the foundation for FEA can be described in detail. This section was extracted
from a report that I wrote for MAE 261B.2
3.1 Finite Elements
In order to analyze the behavior of body, we must discretize the domain into finite elements. These elements
can in general have any number of sides, but triangles and quadrilaterals provide more than enough flexibility
and are much simpler to work with. In this analysis, we will focus on the use of triangular elements. When a
domain in broken up into triangular elements, each triangle will in general have different dimensions and different
orientations. For this reason it becomes very useful to map each general element into an isoparametric element.
Isoparametric elements are standard elements defined in a natural coordinate system for which we can use
shape functions to interpolate the behavior of the element between nodes. An example of an isoparametric
triangular element is shown in Figure 8. The element is bounded by nodes, and the shape functions relate the
coordinates of every point in the element to the positions of the nodes, allowing for interpolation of values such
as displacement within the element.
Figure 8. A general triangular element is mapped to an isoparametric triangular element by the Jacobian matrix. A linear
triangular element uses only nodes 1-3, removing the midpoint nodes. A quadratic triangular element uses all 6 nodes.
The finite element analysis is driven by nodal positions, as the behavior of each element is dependent entirely
on the behavior of the nodes. Depending on the desired accuracy or geometry of the body, 3-node or 6-node
triangular elements may be used. A 3-node triangular element is considered linear, as there is no information
between the nodes to allow for curving. Thus the 6-node triangular element is considered quadratic, as the
midpoint nodes along the edge allow for nonlinear behavior. For each of these element types, there are a number
of shape functions equal to the number of nodes, and every isoparametric element is characterized by these same
functions.
3.2 Shape Functions
The shape functions for triangular elements are defined as follows:
12. Linear Triangular Element:
N1(r, s) = 1 − r − s
N2(r, s) = r
N3(r, s) = s (21)
Quadratic Triangular Element:
N1(r, s) = 2(1 − r − s)(0.5 − r − s)
N2(r, s) = 2r(r − 0.5)
N3(r, s) = 2s(s − 0.5)
N4(r, s) = 4r(1 − r − s)
N5(r, s) = 4rs
N6(r, s) = 4s(1 − r − s) (22)
A location in the natural coordinate system (r, x) can be interpolated from the lab frame nodal positions
(x, y) by the shape functions:
x(r, s) =
a
xaNa(r, s) (23)
where a is indexing the nodes.
3.3 Jacobian Matrix
The general element is mapped from the lab frame to the isoparametric domain by the Jacobian matrix. In
other words, the Jacobian provides means for moving between the isoparametric and physical domains. It is
based on the reference nodal positions and the shape functions, and can be expressed as:
JIα =
a
XiaNa,α (24)
where Xia are the components of the reference nodal position vectors. The Jacobian matrix has dimensions of
(lab frame dimensions) × (element dimensions). In a two dimensional lab frame, the Jacobian matrix will be 2
× 2, and in a three dimensional lab frame it will be 3 × 2.
When working in two dimensions, the Jacobian is very useful because it is a square matrix, and is therefore
invertible. The inverse Jacobian is used in a simple formulation of the element response to deformation in two
dimensions. But a two dimensional formulation has limited flexibility, as it implies no out of plane deformation
and no curved surfaces. However, in three dimensions, the Jacobian is not invertible, which necessitates an
alternative formulation that makes use of curvilinear coordinates for calculating to behavior of curved surfaces
(see Element Response).
3.4 Curvilinear Coordinates and Configurations
To describe the deformation of an arbitrarily curved body, it is useful to introduce a curvilinear coordinate
system that allows us to define a basis in such a way that is natural or convenient for the body. For example,
it is easy to describe the deformation of a cylindrical body in cylindrical coordinates, or a spherical body in
spherical coordinates. These are idealized examples, but illustrate the point that coordinate axes can be chosen
to work well with the geometry of the body undergoing deformation.
In curvilinear coordinates, we refer to the curved coordinate axes as θi
, where i ranges from 1 to 3 to represent
the three axes. These coordinates are used to describe positions in the body, which will ultimately be expressed
in the lab frame. The lab frame can be thought of as the frame of an observer outside of the body, in which
positions are described in terms of Cartesian coordinates x, y, and z, or Ei. For a given body, we will use
curvilinear axes θi
in such a way that we can write expressions for θi
in terms of Ei, and vice versa.
13. The curvilinear coordinates are often chose to match the geometry of the body in an idealized configura-
tion. For example, if our body has a shape close to that of a sphere, we would use a sphere as the idealized
configuration and spherical coordinates as our curvilinear coordinates. We then define two mappings from the
idealized configuration: one to the reference configuration and another to the deformed/current configuration.
The reference configuration represents the initial geometry of the body, prior to deformation, and will be
represented by capital letter symbols. The deformed configuration represents the geometry of the body at
some point in time during deformation, and will be represented with lowercase symbols. This geometry will in
general change with time, and thus is often referred to as the current configuration. We can define functions to
represent these two mappings in terms of the curvilinear coordinates of the system:
Reference Configuration (Ω0):
X = φ0(θi
) = f1(θi
)eθ1
+ f2(θi
)eθ2
+ f3(θi
)eθ3
(25)
Deformed Configuration (Ω):
x = φ(θi
) = g1(θi
)eθ1
+ g2(θi
)eθ2
+ g3(θi
)eθ3
(26)
3.4.1 Covariant and Contravariant Basis Vectors
In order to express our reference and deformed configurations, we need to construct bases. Because we are using
curvilinear coordinates, we can do this in two ways. The first is to construct the tangent basis vectors, which
are tangent to the coordinates axes θi
. These are referred to as covariant basis vectors, and are denoted with
a subscript index as gi. The second is to construct the dual basis vectors, which are normal to the θi
-surfaces.
These surfaces are formed by the plane containing two coordinate axes. For example, the θ1
surface is the plane
containing the θ2
and θ3
axes, and the first dual vector will be normal to this surface. These vectors are referred
to as contravariant basis vectors, and are denoted with a superscript index as gi
. Note that covariant and
contravariant basis vector do not in general point in the same direction.
The covariant and contravariant basis vectors are defined as follows (keeping in mind that capital symbols
are used for the reference configuration and lowercase symbols are used for the deformed configuration):
Gi =
∂φ0
∂θi
, Gi
= Gij
Gj, gi =
∂φ
∂θi
, gi
= gij
gj, (27)
where Gij
and gij
represent metric tensors, and are described in more detail below. The covariant and con-
travariant metric tensors are related by the inverse:
Gij
= [Gij]−1
, gij
= [gij]−1
(28)
Properties Because each basis is defined based on three curved axes defined by the geometry of the body, the
basis will not in general be orthonormal. In other words, the dot product of two basis vectors will not yield the
Kronecker Delta, but will instead give a tensor called the metric tensor.
gi · gj = gij = δij, gi
· gj
= gij
= δij (29)
The elements of the metric tensor gij describe the length of the tangent vectors (diagonal elements) and the
angles between them (off-diagonal elements). Because the bases arises from the curvilinear coordinate axes, it
makes sense that the metric tensor does not generally equal the identity matrix. However, the identity matrix is
used to describe the relationship between covariant and contravariant basis vectors:
gi
· gj = δi
j (30)
3.5 Membrane Theory
This code is based on a structural theory called membrane theory. Membranes are shells that are considered
to be very thin, and this leads to several assumptions. This theory provides the governing equations that we will
be solving to determine the equilibrium state of the system in the presence of prescribed load or displacements.
14. 3.5.1 Assumptions
Like any structural theory, membrane theory makes certain assumptions and imposes constraints to simplify the
problem. These are:
1. Shell is very thin (thickness length)
2. Fibers initially perpendicular to the midsurface remain perpendicular after deformation
3. No bending, which implies that there is no moment
4. No transverse shear, which implies that there is no stress resultant in the transverse direction
3.5.2 Plane Stress
Membrane theory will enforce plane stress on the structure, which will require that the stress in the transverse
direction be zero. This has numerous consequences in the formulation of the constitutive law equations (discussed
further in Constitutive Law), but here it is important to note that this will cause a stretching effect through the
thickness. This is characterized by a thickness stretch ratio λ, which gives the ratio of the deformed thickness
to the original thickness. As stresses are applied in the plane that cause the structure deform, λ > 1 indicates
compressive loads causing the membrane to become thicker, and λ < 1 indicates tensile loads causing the
membrane to become thinner.
3.5.3 Midsurface
In membrane theory, because the structure is so thin, the midsurface is chosen as the surface of interest for defining
the deformation of the body. The midsurface basis vectors for the undeformed and deformed configurations are
defined as Ai and ai, respectively. These are equal to the standard basis vectors defined previously, Gi and
gi, in all cases except for the deformed midsurface vector in the transverse direction, a3 = g3. This vector is
normalized by the magnitude of the area enclosed by the in-plane deformed basis vectors, a1 and a2, which are
referred to as aα. The result is than a3 and g3 are related by the thickness stretch ratio. The midsurface basis
vectors and their relationship to the standard basis vectors are summarized here:
Aα = X,α =
a
XaNa,α aα = x,α =
a
xaNa,α
A3 =
A1 × A2
√
A
a3 =
a1 × a2
√
a
Ai = Gi Ai
= Gi
aα = gα aα
= gα
λa3 = g3
1
λ
a3
= g3
√
A = det(Aαβ)
√
a = det(aαβ)
Aαβ = Aα · Aβ aαβ = aα · aβ (31)
3.5.4 Weak Form
In order to make a nonlinear structural problem solvable by a finite element code, we will utilize the principle
of virtual work and turn this into an energy minimization problem. This principle states that the internal
virtual work is equal to the internal virtual work for a system in equilibrium, which can be expressed as:
δΠ[x] = δWint − δWext = 0 (32)
where x is the midsurface position.
The internal virtual work is defined by the stress resultants nα
in the body:
δWint[x] =
Ω0
nα
· δx,αdA (33)
15. nα
=
H
P Gα
µdθ ≈ P · Gα
µH = ταi
giH (34)
where µ =
√
G/
√
A = 1 because Gi = Ai, and the stress is constant across the thickness H.
The external virtual work due to an applied load f is given by:
δWext[x] =
Ω0
f · δxdA (35)
The virtual displacement can be rewritten using shape function interpolation by taking the variation of equation
23, allowing the PVW to be rewritten as:
δΠ[x] =
Ω0
nα
·
a
δxaNa,α − f ·
a
δxNa dA (36)
=
a
fint
a − fext
a = 0 (37)
where the internal and external forces are given by:
fint
a =
Ω0
nα
Na,αdA (38)
fext
a =
Ω0
f NadA (39)
We then define the residual force as the difference between these two forces:
ra(x) = fint
a − fext
a (40)
By taking the derivative of the residual we can obtain a relationship to the stiffness matrix by noting that the
external force is not a function of x:
∂ria
∂xkb
=
∂fint
ia
∂xkb
−
∂fext
ia
∂xkb
=
∂fint
ia
∂xkb
= Kiakb (41)
In order to bring the system into equilibrium, the residual force will need to equal 0, which means that the
internal force will have to balance the external force. If the system is not in equilibrium, we must determine
a displacement to x such that the internal force will change to match the external force. This equation is in
general nonlinear however, so we can linearize it using a Taylor expansion to determine an update for x:
ria(x + dx) = 0 = ria(x) +
∂ria
∂xkb
dxkb (42)
But ∂ria
∂xkb
is equal to the stiffness matrix Kiakb, so we can express the update to x as:
dxkb = −K−1
iakbria(x) (43)
This can be rewritten in the following way:
K · u = fint
− fext
= r → 0 (44)
Because this equation is nonlinear, it will be solved iteratively until the residual is equal to 0. This will be
done by calculating the stiffness matrix and the internal force for the current nodal positions and solving for the
displacements that correspond to the residual. Then those displacements will be applied to update the nodal
positions, which will again be used to compute the stiffness matrix and the internal force array. This process
will continue until the nodal displacements give an internal force that balances out the external force, and the
residual goes to 0, indicating that the body has been deformed to a state of equilibrium.
16. 3.6 Deformation Gradient
The deformation gradient is a matrix that describes the manner in which the body is deformed at a point in
space. The diagonal elements represent stretching and the off-diagonal elements represent twisting of the body.
It is computed from the outer product of basis vectors in the undeformed and deformed configurations:
F = gi ⊗ Gi
(45)
For membrane theory, this can be expressed as:
F = aα ⊗ Aα
+ λ a3 ⊗ A3
(46)
Notice that the thickness stretch ratio scales the outer product between the transverse midsurface basis vectors.
These expressions can be used in the general case for three dimensions.
For analysis in two dimensions, the deformation gradient can be computed in alternative manner that doesn’t
require basis vectors. Using the nodal positions in the current configuration xia, and the information about the
current configuration carried by the Jacobian matrix, the deformation gradient can be expressed as:
FiJ =
a
xiaNa,αJ−1
αJ (47)
This expression is usable only two dimensions when the Jacobian matrix is invertible.
3.7 Kinematic Quantities
With the basis vectors defined for both the reference, and deformed configurations, we can now compute the
kinematic quantities that describe the deformation of the body. There are three tensor that describe the strains
in the body at a point in space, the right Cauchy-Green deformation tensor, the left Cauchy-Green
deformation tensor, and the Green-Lagrange Strain:
Right Cauchy-Green Deformation Tensor: C = F T
F (48)
Left Cauchy-Green Deformation Tensor: B = F F T
(49)
Green-Lagrange Strain: E =
1
2
(C − I) (50)
3.8 Constitutive Law
The stress-strain relationship for a body is defined by model called a constitutive law. There a various consti-
tutive laws that make different assumptions about the response of a body, such as a material being compressible
or incompressible, or behaving elastically or inelastically. In this analysis, we will use the Neo-Hookean model,
which assumes hyperelastic material behavior and allows for compression. The law is expressed as an equation
for the strain energy density of the body as a function of strain, from which we can derive expression for the
first Piola-Kirchhoff Stress and tangent moduli.
In the expressions in this section, notice the use of capitalization in the subscripts. The lowercase subscripts
indicate components in the deformed configuration, while the uppercase subscripts indicate components in the
lab frame.
The Neo-Hookean model expresses strain energy density as:
w(C) =
λ0
2
[ln(J)]2
− µ0ln(J) +
µ0
2
(tr(C) − 3), (51)
17. where J = det(F ) is referred to as the Jacobian, and λ0 and µ0 are the first lam´e parameter and shear
modulus of the material, respectively. The strain energy density can be rewritten entirely as a function of the
deformation gradient F by expressing tr(C) in terms of F :
tr(C) = Ckk = Cklδkl
Ckl = (Fkm)T
(Fml) = FmkFml
=⇒ tr(C) = FmkFmlδkl
Now we can derive an expression for the first Piola-Kirchhoff stress PiJ :
PiJ =
∂w
∂FiJ
=
∂
∂FiJ
λ0
2
ln2
(J) − µ0ln(J) +
µ0
2
(FmkFmlδkl − 3) (52)
= λ0ln(J)
1
J
∂J
∂FiJ
− µ0
1
J
∂J
∂FiJ
+
µ0
2
∂Fmk
∂FiJ
Fmlδkl + Fmk
∂Fml
∂FiJ
δkl (53)
Using the identity ∂J
∂FiJ
= JF−1
Ji :
PiJ = λ0ln(J)
1
J
(JF−1
Ji ) − µ0
1
J
(JF−1
Ji ) +
µ0
2
[δmiδkjFmlδkl + Fmkδmiδljδkl] (54)
= λ0ln(J)F−1
Ji − µ0F−1
Ji +
µ0
2
[δmiδkjFmk + Fmlδmiδlj] (55)
= λ0ln(J)F−1
Ji − µ0F−1
Ji +
µ0
2
[FiJ + FiJ ] (56)
= [λ0ln(J) − µ0] F−1
Ji + µ0FiJ (57)
We can take another derivative with respect to the deformation gradient to find the tangent moduli CiJkL:
CiJkL =
∂PiJ
∂FkL
(58)
=
∂
∂FkL
[λ0ln(J) − µ0] F−1
Ji + µ0FiJ (59)
= λ0
1
J
∂J
∂FkL
F−1
Ji + [λ0ln(J) − µ0]
∂F−1
Ji
∂FkL
+ µ0
∂FiJ
∂FkL
(60)
Using the identity
∂F −1
Ji
∂FkL
= −F−1
Jk F−1
li :
CiJkL = λ0
1
J
(JF−1
lk )F−1
Ji + [λ0ln(J) − µ0] −F−1
Jk F−1
li + µ0δikδjl (61)
= λ0F−1
lk F−1
Ji − [λ0ln(J) − µ0] F−1
Jk F−1
li + µ0δikδjl (62)
In computing the element response, the contravariant components of the tangent moduli Cijkl
will be needed.
In order to find these, the tangent moduli needs to be expressed in the lab frame as CIJKL, and then converted
to its contravariant components. This can be accomplished by computing an additional stress quantity called
the second Piola-Kirchhoff stress, S which is given by:
S = F −1
P (63)
The contravariant components of the tangent moduli can then be computed using the following two expres-
sions:
CIJKL =
1
2
F−1
Ii F−1
Kk (CiJkL − δikSJL) (lab frame) (64)
Cijkl
= CIJKL Gi
I
Gj
J
Gk
K
GL
L
(contravariant) (65)
18. An additional stress quantity that will be useful in this analysis is called the Kirchhoff stress. It is given
by:
τ = P F T
(66)
τij
= gi
I
[τ]IJ gj
J
(67)
To summarize, we now have the following key expressions for the Neo-Hookean constitutive law:
Strain Energy Density: w(F ) =
λ0
2
[ln(J)]2
− µ0ln(J) +
µ0
2
(tr(F T
F ) − 3) (68)
First Piola-Kirchhoff Stress: PiJ = [λ0ln(J) − µ0] F−1
Ji + µ0FiJ (69)
Second Piola-Kirchhoff Stress: S = F −1
P (70)
Kirchhoff Stress: τ = P F T
(71)
Tangent Moduli: CiJkL = λ0F−1
lk F−1
Ji − [λ0ln(J) − µ0] F−1
Jk F−1
li + µ0δikδjl (72)
Tangent Moduli Lab: CIJKL =
1
2
F−1
Ii F−1
Kk (CiJkL − δikSJL) (73)
Tangent Moduli Contravariant: Cijkl
= CIJKL Gi
I
Gj
J
Gk
K
GL
L
(74)
3.8.1 Plane Stress
The assumption of plane stress places a constraint on the structure of the deformation gradient and requires the
stress through the thickness to be zero. This has different consequences in two and three dimensions, which are
discussed here.
Two Dimensions In two dimensions, the deformation gradient is constrained to take the following form:
F =
F11 F12 0
F21 F22 0
0 0 λ
(75)
Because there is no stress through the thickness, the first Piola-Kirchhoff stress tensor should have a value of 0
for P33. Since the only arbitrary or prescribed quantities of F are the 2 × 2 matrix of in-plane elements, we say
that P33 is a function only of Fαβ (where α and β each run from 1 to 2) and the stretch ratio λ.
P33(Fαβ, λ) = 0 (76)
Because Fαβ is prescribed, we must solve this equation by finding the value of λ that makes it true. P (F )
is nonlinear, and therefore must be solved iteratively using Newton’s Method, discussed later (see Newton’s
Method).
In two dimensions, the plane stress assumptions serves to simplify the problem by reducing dimension from
3D to 2D. Once we have solved for lambda using Newton’s method, we can now proceed with the analysis using
reduced matrices containing only the in-plane components. First, note that 2D and 3D strain energy density are
defined to be equal. For the first Piola-Kirchhoff stress, the transition to 2D is simple, because all components in
the 3-direction have been forced to zero under the assumption of plane stress. Therefore, the in-plane components
of P are nothing more than the 2 × 2 matrix containing the non-zero elements. In other words, Pαβ is a subset
of PiJ . For the tangent moduli however, the transition is not that simple. Despite imposing plane stress, there
will in general be non-zero elements in the 3-directions, and we cannot simply reduce to 2D by taking a subset
of this tensor. Instead, we want to capture the contributions of these non-zero elements by created an adjusted
2D 4th order tensor from the full 3D tangent moduli. The components of the 2D tangent moduli can be found
in the following way:
P2D
αβ ≡
∂w2D
∂Fαβ
=
∂
∂Fαβ
[w(F, λ)] =
∂w
∂Fαβ
+
∂w
∂λ
∂λ
∂Fαβ
(77)
19. We know that ∂w
∂Fαβ
= Pαβ and ∂w
∂λ = 0, so we can write:
Pαβ =
∂w(Fαβ, λ)
∂Fαβ
, P2D
αβ = Pαβ (78)
This shows, as stated previously, that the 2D form of the first Piola-Kirchhoff stress is just a subset of the 3D
form. Now we can use this to compute the tangent moduli:
C2D
αβδγ ≡
∂P2D
αβ
∂Fδγ
=
∂2
w2D
∂FαβFδγ
=
∂
∂Fδγ
[Pαβ(Fαβ, λ)] =
∂Pαβ
∂Fδγ
+
∂Pαβ
∂λ
∂λ
∂Fδγ
(79)
We know that
∂Pαβ
∂Fδγ
= Cαβδγ and
∂Pαβ
∂λ =
∂Pαβ
∂F33
= Cαβ33, so we can write:
C2D
αβδγ = Cαβδγ + Cαβ33
∂λ
∂Fδγ
(80)
Now we can find ∂λ
∂Fδγ
by enforcing the plane stress assumption that P33(Fαβ, λ) = 0.
P33(Fαβ, λ) = 0 =⇒ dP33 = 0 =
∂P33
∂Fαβ
dFαβ +
∂P33
∂F33
dλ (81)
0 = C33αβdFαβ + C3333dλ (82)
0 = C33αβdFαβ + C3333
∂λ
∂Fαβ
dFαβ (83)
0 = C33αβ + C3333
∂λ
∂Fαβ
dFαβ (84)
=⇒
∂λ
∂Fαβ
= −
C33αβ
C3333
(85)
Now we can use this value to solve for the components of the 2D tangent moduli:
C2D
αβδγ =
∂
∂Fδγ
[Pαβ(Fαβ, λ)] = Cαβδγ + Cαβ33
∂λ
∂Fδγ
(86)
=⇒ C2D
αβδγ = Cαβδγ − Cαβ33C33δγ
1
C3333
(87)
Using this equation we can compute the adjusted 2D tangent moduli under the assumption of plane stress from
the components of the full 3D tangent moduli.
Three Dimensions In three dimensions, the deformation gradient takes the form given by equation 46, which
in general will be a fully populated matrix. To enforce plane stress, the transverse component of the Kirchhoff
stress defined in equation 67 will be forced to 0:
τ33
(P , λ) = 0 (88)
Just as was the case with the first Piola-Kirchhoff stress in two dimensions, this equation is nonlinear, and must
be solved iteratively using Newton’s method (see Newton’s Method).
In order to compute the stiffness matrix, the contravariant tangent moduli defined in equation 65 must be
condensed to an effective 2D tensor. The effective contravariant tangent moduli is given by:
˜Cαβγδ
= Cαβγδ
−
Cαβ33
− C33γδ
C3333
(89)
where Cαβγδ
are the 2D components of the full 3D contravariant tangent moduli.
20. 3.9 Quadrature Points
Every element contains quadrature points, which define specific locations in the isoparametric domain at which
the material response quantities governed by the constitutive law are evaluated. The deformation gradient
is evaluated at each quadrature point and used to calculated the strain energy density, the stresses, and the
tangent moduli. With these quantities sampled at the quadrature point, the element response can be evaluated
by numerically integrating over the isoparametric domain using Gauss Quadrature.
3.10 Gauss Quadrature
This analysis requires the evaluation of integrals, and it would be costly to perform integration explicitly. For
this reason, we will use Gauss quadrature to perform numerical integration. Gauss quadrature works by using a
weighted sum of function values at specific quadrature points within a domain. It is constructed to yield exact
results for polynomial functions of degree 2n − 1 or lower for n-point quadrature, provided that the polynomial
is well-approximated at the quadrature points. In this analysis, we will make use of 1-point quadrature, which
will evaluate a linear polynomial exactly, and 3-point quadrature, which will evaluate a fifth order polynomial
exactly.
Whether or not the function is well-approximated at the quadrature points will be determined by whether the
interpolated shape function values at these points can capture the element behavior. For example, for a 3-node
isoparametric triangular element, 1-point quadrature will provide exact integration results, as the element can
only display linear behavior, which will be exactly interpolated by the shape functions. In order to accurately
capture quadratic behavior, a 6-node element must be used to pick up the behavior between corner nodes. We
must also use 3-point quadrature to ensure accuracy, because the accuracy 1-point quadrature is limited to linear
functions.
The computational cost will be lowest for the lowest order to quadrature, therefore the analysis will make
use of the lowest order quadrature possible to ensure accurate results. There are applications for intentionally
using lower-order quadrature, but these will not be discussed here.
The general expression for Gauss quadrature of a function g(ζ) is:
1
−1
g(ζ)dζ =
n
i=1
g(˜ζi)wi (90)
where n is the number of quadrature points, ˜ζi is the coordinate of the ith quadrature point, and wi is the weight
of the ith quadrature point.
3.11 Element Response
With the deformation gradient and material response quantities from the constitutive model, three quantities
can be computed: strain energy, internal nodal force array, and the stiffness matrix. These quantities describe
the behavior of the entire element by integrating the material response quantities over the element domain.
Here the isoparametric formulation comes in handy because the integral can be performed in the isoparametric
domain and then transformed back to the physical domain using the inverse Jacobian matrix. These integrals
are computed using Gauss Quadrature in both two and three dimensions.
3.11.1 Two Dimensions
The strain energy of the element is determined by integrating the strain energy density over the physical
element domain Ω0:
W =
Ω0
wdV =
Ω0
wdA ∗ H (91)
21. The internal nodal force array is the representation of a distributed force over the element at the nodes.
In other words, the distributed load is converted to a set of equivalent forces acting only on the nodes of the
element. The force array is determined by integrating the first Piola-Kirchhoff stress:
fint
ia =
Ω0
PiJ Na,αJ−1
αj dV =
Ω0
PiJ Na,αJ−1
αj dA ∗ H, i, J ∈ {1, 2} (92)
The stiffness matrix represents the resistance of the element to deformation in various directions. It is
determined by integrating the two dimensional tangent moduli that has been adjusted for plane stress:
Kiakb =
Ω0
C2D
iJkLNa,αNb,βJ−1
αj J−1
βl dV =
Ω0
C2D
iJkLNa,αNb,βJ−1
αj J−1
βl dA ∗ H, i, J, k, L ∈ {1, 2} (93)
Notice that the integrals through the constant thickness yield a constant value H.
3.11.2 Three Dimensions
In three dimensions, the Jacobian matrix that was utilized in two dimensions must be replaced because it is a
3 × 2 matrix and is not invertible. To this, we will make use of the deformed basis vectors, and the differential
area
√
A, which relates the element area in the isoparametric domain to the area in the physical domain. The
strain energy is determined by integrating over the isoparametric domain ˆΩ as:
W =
ˆΩ
w
√
A dθ1
dθ2
∗ H (94)
With the stress resultant defined from membrane theory by equation 34, the internal nodal force defined in
equation 92 can be expressed as:
fint
ia =
ˆΩ
ταj
(gj)iNa,α
√
A dθ1
dθ2
∗ H, i, j ∈ {1, 2, 3} (95)
Because the internal nodal is a nonlinear function of the stress resultant, we can linearize nα
to produce:
δnα
= 2 ˜Cαβγδ
(aβ ⊗ aδ) +
ταγ
2
I · δaγ ∗ µH (96)
The quantity inside the brackets is a tensor that maps differential changes in tangent basis vectors to differential
changes in the stress resultant. From this expression we can determine the equation for the stiffness matrix:
Kiakb =
ˆΩ
2 ˜Cαβγδ
(aβ ⊗ aδ)ik +
ταβ
2
δγ
βδik Na,αNb,γ
√
A dθ1
dθ2
∗ H, i, k ∈ {1, 2, 3} (97)
The first term is called the material stiffness, as it depends on the effective two dimensional tangent moduli, and
the second term is called the geometric stiffness because it depends on the Kirchhoff stress, which is a function
of the deformation gradient and first Piola-Kirchhoff stress.
3.12 Property Levels
It is important to distinguish the level at which certain key quantities in the analysis are defined. There are
three levels we are concerned with: model-level, element-level, and quadrature point-level. At each of these
levels, some quantities are defined or computed one time, and others are updated with every deformation step.
This information is summarized here:
22. Model:
• material
• constitutive model
• quadrature class
• element type
Element:
One-time:
• reference configuration
• Jacobian matrix
Every step:
• strain energy
• internal nodal force array
• external nodal force array
• stiffness matrix
Quadrature Point:
One-time:
• position
• weight
Every step:
• current configuration
• deformation gradient
• Jacobian
• stretch ratio
• strain energy density
• first Piola-Kirchhoff stress
• Kirchhoff stress
• tangent moduli
• effective 2D tangent moduli
3.13 Nonlinear Solving
Solving nonlinear equations is not a straightforward process, and is often done using iterative techniques. Two
such methods implemented in this code are Newton’s Method, and the Newton-Raphson Method.
23. 3.13.1 Newton’s Method
Newton’s Method is an iterative technique for solving a nonlinear equation f(λ). To use it, we must start by
choosing a reasonable initial value for λ for which f(λ) likely does not equal zero.
f(λ0) = 0 (98)
Then we will perturb λ by some small quantity, and use a first order Taylor approximation to solve for the value
of the perturbation that will make f(λ) equal to zero.
f(λ + dλ) = f(λ) +
df(λ)
dλ
dλ = 0 =⇒ dλ = −
df(λ)
dλ
−1
f(λ) (99)
We then use this perturbation to compute a new value of λ and repeat the process. This loop will continue until
f(λ) is within some tolerance of 0, at which point we say the loop converges. It is very important to note that
if λ0 is far enough from the final value of λ, this loop will diverge.
For the plane stress application in two dimensions, the function we are attempting to solve iteratively is
P33(Fαβ, λ) = 0. Therefore we can express equation 99 in terms of the quantities of our problem as:
dλ = −
P33(Fαβ, λ)
C3333
(100)
In three dimensions, we are attempting to iteratively solve τ33
(P , λ) = 0. The Newton update can be expressed
as:
dλ = −
τ33
(P , λ)
2λC3333
(101)
where τ33
can be expressed as
τ33
=
1
λ
a3
[P ] A3 T
(102)
This expression is convenient because it does not require the use of g3
, which is dependent on the yet to be
determined stretch ratio.
The Newton’s method solver is a loop that iteratively solves for the stretch ratio beginning with an initial
guess. If the initial guess is bad enough, it is possible for the lambda update dλ, computed in equations 100 and
101, to cause the value of the stretch ratio to go negative. This will produce a negative Jacobian, and therefore
an unphysical deformation gradient. If this is the case, the stretch ratio is set to a small negative value, 10−6
,
to give the solver another chance to converge rather than simply raising a Jacobian error. In many cases, the
solver will still fail to converge and will raise a convergence error if the maximum number of iterations (set to
15) is exceeded.
3.13.2 Newton-Raphson Method
The Newton-Raphson Method is a strategy for solving nonlinear equations that is based on the method of
continuation. The idea is that if we are trying to solve for the displacement that results from an applied load,
we can do so by solving the problem in increments. Assume a value xn is known, then increment the load to
fext
n+1 and compute xn+1 by using xn as an initial guess. Compute xn+1 will be an iterative process that will
converge given that the load step is small enough to be within the radius of convergence of the loop. After the
loop converges, the load is incremented again and the process continues until the load has been incremented to
its final value.
24. Process The equation we are trying to solve is given by:
fint
(x) − fext
= 0 (103)
Denote xk
n+1 as the value of the next position for the kth iteration of the loop, where k = 0, 1, 2...
Displace the position by some amount u and set: xk+1
n+1 = xk
n+1 + u
Linearize equation 103:
< Dfint
(xk
n+1), u > +fint
(xk
n+1) − fext
n+1 = 0 (104)
K(xk
n+1)u = fext
n+1 − fint
(xk
n+1) = −r(xk
n+1) (105)
If |r(xk
n+1)| < TOLERANCE then the residual has been forced to 0 and the solution has converged. If not,
then solve for the displacement:
u = −K−1
(xk
n+1)r(xk
n+1) (106)
Now set xk+1
n+1 = xk
n+1 + u and repeat the process until the residual is within tolerance of zero.
This is the exact process implemented in the solver method of the model. The applied external load is
incremented in small steps and the displacement of the nodes is solved for each time, and their current positions
are updated. After the loop converges, the load incremented and the process continues until the external load
reaches its final value and the final deformed positions of the nodes are determined.
With a full understanding of the theory of finite element analysis for membrane problems, we are ready to
set up the model in Abaqus CAE.
4. ABAQUS MODEL
Setting up a finite element model requires simplifying a physical model such that the analysis converges while still
providing an accurate representation of the original system. This allows for meaningful results to be determined
in a reasonable amount of time. One such assumption is that a drumhead can be represented by a membrane.
This allows for the use of membrane elements, which neglect shear and bending resistance, simplifying the
material response and allowing for faster computation than using plate elements intended for thicker structures.
The objective of this analysis is to model a drumhead subjected to an impact load from a drumstick at the
center, and observe the free response of the head that follows. In particular, the model should be refined enough
such that the transmission of waves through the head is clearly visible, allowing for an accurate displacement
mapping of the entire head over time. This data represents the signals that would hypothetically be recorded
by a sensing system attached to the drum for the purposes of micless recording.
A step-by-step guide to setting up the Abaqus model for a dynamic membrane system subject to an impact
load is presented in Appendix A. Key considerations and modeling choices will be explained here.
Geometry The drumhead is represented by a circular membrane of diameter 16” (.4064 m), and a thickness
of .01 in (.254 mm).
Material The drumhead is made of single-ply sheet of Mylar, with material properties given by:
• Young’s Modulus: E = 0.62 − 1.4 GPa → 1.0 GPa
• Poisson’s Ratio: ν = 0.35 − 0.45 → 0.4
• Density: ρ = 900 − 930 kg/m3
→ 900 kg/m3
The values after the arrows represent those chosen for use in the model.
25. Partitioning Partitions were created to divide the membrane into 8 slices as shown in Figure 9. This allowed
for the creation of a symmetric mesh and therefore made the results more uniform.
Boundary Conditions In order to add tension to the membrane, a prescribed radial displacement of 0.5”
(0.0127 mm) is applied to the rim of the drumhead. After the stretch is applied, the rim is clamped to restrict
further movement. The boundary conditions are displayed in Figure 10.
Loading The stick impact is modeled as a concentrated force of 100 N applied at the center of the head. It is
applied as a step function with a period of 3 ms.
Steps There are three steps in the model:
1. Pre-stretch: A static step during which the prescribed radial displacement is applied. This places the
head under tension.
2. Stick impact: A dynamic, implicit step during which the stick impact force is applied as a step function
with a period of 3 ms. This step incorporates non-linear geometry. During this step, the rim is fully
clamped.
3. Free response: A dynamic, implicit step during which the load is removed and the drumhead is allowed
to vibrating freely with a clamped rim. This step incorporates non-linear geometry.
Wave Speed Because the load is applied at the center, it is expected that the fundamental mode will be
dominant. A 16” tom drum (radius a = .2032 m) generally has a fundamental frequency of about 250 Hz. From
equation 20, the wave speed can be determined as:
(250 Hz) =
2.405
2π(.2032 m)
c =⇒ c = 132.7 m/s (107)
Figure 9. Membrane partitioned into 8 slices (left), and symmetric mesh (right).
26. Figure 10. Prescribed radial displacement applied during the Pre-stretch, and clamped boundary conditions applied during
the stick impact.
Tension The wave speed, along with the mass density, can be used to compute the tension in the head. σ is
the area mass density, and can be computed by multiplying the density of the material by the thickness:
σ = ρt = (900 kg/m3
)(0.000254 m) = 0.2286 kg/m2
(108)
The tension can now be determined:
c =
T
σ
=⇒ T = c2
σ = (132.7 m/s)2
(0.2286 kg/m2
) = 4025.5 N/m (109)
Stress The tension corresponds to a stress in the membrane that can be determined by dividing the tension
by the thickness:
Smises =
T
t
=
4025.5 N/m
0.000254 m
= 1.58 × 107
Pa (110)
By applying a prescribed radial displacement of 0.5”, a stress of 1.04 × 108
Pa forms in the head as shown in
Figure 11. This is within an order of magnitude of the calculated result, and is good enough for the analysis.
Element Size The element size must be determine such that it is smaller than the smallest wavelength
considered by the model. In this model, only the first few modes will contribute to the vibration, resulting in
frequencies less than 3 times fundamental frequency according to the ratios given in Figure 4. To be conservative,
the fundamental frequency will be multiplied by 10 to give a maximum frequency of 2,500 Hz. The corresponding
wavelength is given by:
λmin =
c
fmax
=
132.7 m/s
2, 500 Hz
= 0.053 m (111)
To determine element size, the minimum wavelength will by divided by 10 to ensure that the smallest wave can
be represented across multiple elements. Therefore the element size is:
Element size: h =
1
10
λmin = 0.0053 m (112)
27. Timestep The timestep, or increment size of the dynamic steps, must be set such that a wave cannot propagate
over more than one element. This is referred to as the Courant-Friedrichs-Lewy condition. Given the element
size determined above, the time it will take to travel over one element is:
∆telement =
h
c
=
0.0056 m
132.7 m/s
= 4 × 10−5
s (113)
As with the element size, this quantity will be divided by 10 to be conservative:
Timestep: ∆t =
1
10
∆telement = 4 × 10−6
s (114)
Note: Due to runtime constraints, I was not able to perform the entire simulation at this timestep. I was
only able to use the Hoffman cluster for a couple days, and the first run with the above timestep ended up
causing a memory error. As a result, I had to let Abaqus scale the timestep on its own, but set the initial step
size to be 4 × 10−6
s as defined above.
Mesh The element type is specified as M3D6: 6-node triangular membrane elements. The circular shape of
the head lends itself well to triangular elements as opposed to quadrilaterals, and quadratic order is utilized to
increase accuracy by better capturing bending behavior. The mesh with the element size specified above, and
type defined here is displayed in Figure 9.
4.1 Results
These results represent what I was able to obtain from my best run on the Hoffman cluster. In observing the
results, I am observing how well the simulation represents the expected behavior of a vibrating membrane by
analyzing wave propagation and the presence of the dominant modes. The ultimate (and future) goal would be
to utilize displacement data for various drumstick impact locations on the head to determine the sound signal
that would be produced in each case, and compare to the signal recorded with a microphone for a real drum.
That is beyond the scope of this project.
The results will be reported and discussed for each of the three simulation steps.
4.1.1 Pre-stretch
In this static step, the drumhead is subjected to a uniform prescribed radial displacement in order to place
the head under tension. Tension is required for the membrane to support vibrational motion. The stretched
membrane is shown in Figure 11.
Figure 11. Stretched membrane at the end of the Pre-stretch step with color mapping representing the Von Mises stress.
28. As expected, the drumhead reaches equilibrium in a state of constant stress, which implies constant tension,
and therefore constant wave speed throughout the membrane. The Von Mises stress in the head is 1.042×108
Pa,
which corresponds to a tension of 24, 466.8 N/m.
4.1.2 Stick Impact
The Stick Impact step is a dynamic, implicit step during which the drumstick applies a point load at the center
for the entire 3 ms period. The load ramps up from 0 to 100 N instantaneously as a step function. The initial
impact causes a wave to propagate outwards from the center as shown in the series of images in Figure 12.
The tension that results from the pre-stretch gives a wave speed of c = 340.3 m/s. At this speed, the
wave should travel a total distance of 1.02 m over the course of the 3 ms impact period. This means that the
Figure 12. Wave propagation from center to edge following initial stick impact. The color mapping represents transverse
displacement.
29. wave should travel center-to-edge-to-center (a distance of 0.4064 m) about 2.5 times by the time the impact has
finished.
In observing the simulation data, the wave makes the trip twice before the impact period ends. This provides
reasonable agreement and seems to approximately validate the wave speed derived from the stress in the head.
4.1.3 Free Response
The Free Response is a dynamic, implicit step during which the drumstick load is removed and the drumhead is
allowed to oscillate freely for 1 s. The load is removed instantaneously from 100 to 0 N, which effectively acts as
Figure 13. The central node rebounds upwards when the impact load is removed at the beginning of the free response
step. A new wave forms at the center and begins to propagate outward, followed by several additional waves as the central
node continues to oscillate with high frequency.
30. Figure 14. The same frame displayed with the full membrane and with a cross-section cut. Note that the shape clearly
resembles the (0,2) for a circular membrane.
a second impact that causes a wave to propagate as the head rebounds upwards due to the internal strain energy,
as shown in Figure 13. Because the central node is now allowed to move freely, it quickly oscillates several times
at the beginning of the step, causing the formation of several smaller wave fronts.
These wave fronts that form from the small oscillations of the middle node following the rebound represent
small disturbances that quickly die off. The initial rebound wave however, excites some higher order modes and
creates a distinct second wave the propagates and interferes with the wave produced from the initial impact.
The (0,2) mode is displayed from two different angles in Figure 14.
In the steps that follow, the (0,1) mode quickly becomes dominant, and is the only visible remaining mode.
The drumhead simply oscillates between the two states shown in Figure 15. While it makes sense that the
free response would ultimately collapse to the fundamental mode, the manner it which it happens is clearly
missing some information. As mentioned previously, due to runtime constraints, Abaqus was allowed to select
Figure 15. The free response is ultimately dominated by the fundamental mode (0,1), oscillating between the down and
up positions.
31. the timestep by making the largest jumps possible while still allowing the nonlinear solvers to converge. Despite
setting an initial timestep of 4 × 10−6
, the timestep quickly grows to the order of 1 × 10−3
. Given that a wave
can travel center-to-edge-to-center 2 times in 3 × 10−3
, the data is really just showing a random sampling of
the free response as it moves further away from the beginning of the step. The result is that the dominant
fundamental mode is the only mode that remains visible and the smaller oscillations are aliased such that they
become invisible. It is interesting to note however, that Abaqus increasing the timestep is an indication that the
fundamental mode is dominant. If the displacement contributions due to higher order modes were significant
relative to the fundamental, the solver would not converge and therefore not elect to increase the timestep in the
next increment. The repeated decision to do so indicates that higher order mode contributions to displacement
are relatively insignificant, but does not mean that they aren’t present in the vibrational motion of the drumhead.
4.1.4 Conclusions
Overall, the Abaqus model provided a very good representation of the expected behavior. The waves propa-
gated as expected, though it was somewhat surprising to see the waves produced at the beginning of the free
response step after the impact load was released. The fundamental mode dominated, as expected, but there
were contributions of some higher order modes, in particular the radially symmetric (0,2) mode.
The wave propagation speed provided validation for the membrane equations of motion, as the relationship
between wave speed and tension was well-represented in the model. The wave produced from initial impact was
expected to travel center-to-edge-to-center 2.5 times during the impact period, and did so just over 2 times.
To investigate further into the wave speed, an additional analysis was done through a brief experiment
described in the next section.
32. 5. EXPERIMENT: WAVE SPEED IN DRUMHEAD
An ultrasound experiment was conducted in an effort to determine the speed of an acoustic wave traveling through
the head of a 12” tom tuned to relatively high frequency and provide further validation to the theoretical and
finite element model.
The principle behind the experiment is to send guided waves from a source located at the center of the
drumhead to a receiver placed at known distances and measure the time of transmission. By using the distance
between the source and receiver transducers and the transmission time, the speed of the wave can be determined.
Waveform data was recorded at 100 kHz (optimum for the given equipment) at distances ranging from 1 to 5 in
in 1 in increments.
5.1 Experimental Setup
The following equipment was used in the experiment
(images shown in order at right):
1. Function Generator: 5-cycle Hanning Window
100 kHz, 5Vp−p
2. Signal Amplifier: 20 dB gain on receiving signal
3. Source and receiving transducers
4. Oscilloscope
5. Computer with Vallen Wavelet Transform, and
LabVIEW DAQ software (not pictured)
A diagram of the experimental setup is shown in
Figure 16.
5.2 Procedure
1. Connect computer, signal generator, signal mod-
ifier, oscilloscope, and transducer with BNC ca-
bles
2. Turn on all electronic equipment connected in
the previous step
3. Select 5 Vp−p voltage and frequency 100 kHz on
the signal generator
4. Apply gel to the ends of the source and receiver
transducer to increase sensitivity
5. Place holder containing holes spaced at 1 in on
the head, insert the source transducer at the cen-
ter of the head, and insert the receiver in an ad-
jacent hole
6. Adjust scope to read the source and receiving
signal
7. Save waveform data on computer
8. Repeat 5-7 for various receiver locations
33. Figure 16. Experimental setup for wave speed measurement of a drumhead.
9. Analyze waveform data using waveform plot
10. Analyze waveform data using Vallen Wavelet (explained in more detail below)
5.3 Vallen Wavelet Data Processing
Vallen Wavelet transform calculates the arrival time for an energy packet corresponding to 100 kHz, the frequency
produced by the signal generator, as the source transducers can excite modes close to this frequency. Vallen
Wavelet computes arrival time by transforming data from the time domain to the frequency domain as shown
in Figure 18 and operating on this data.
5.4 Results and Discussion
The travel time was measured at four separation distances between the source and receiver transducers, and the
velocity was computed for each based on the waveform plots. The results are summarized in Table 1.
Table 1. Experimental results for wave speed.
Distance (in) Travel Time (µs) Velocity (m/s)
1 42 604.8
2 91 558.2
3 141 540.5
4 20 503.0
34. Figure 17. Recorded waveform data.
Figure 18. Recorded Vallen Wavelet transform data used to calculate wave packet arrival time.
35. The average wave speed is 551.6 ± 36.6 m/s, where the standard deviation represents 6.64% of the average,
indicating consistent experimental procedure.
The Vallen Wavelet result for the velocity of the energy packet is 742.5 m/s, which does not provide good
agreement with the data produced by the waveform plots, which should be considered to be more reliable.
The finite element model indicated a wave speed of approximately 340 m/s based on the stress in the head,
and this was well-validated by the behavior of the membrane during the simulation. The waveform plot data,
which produced an average speed of 551.6 m/s cannot be compared directly against this number because the
two numbers are not representative of equivalent physical systems. The finite element model represents a 16”
drum subjected to a tension of 24,466.8 N/m, which translates to a frequency of about 640 Hz, which is rather
high for a drum of that size. The drum used for the experiment is 12” in diameter with relatively high tension,
though neither this value or its frequency can be determined directly. It is reasonable to expect that the tension
of the 12” drum is comparable to that of the FEA model, though it is very unlikely that they are the same. The
difference in tension and the 4” difference in diameter will both contribute towards discrepancies in wave speed.
For the purposes of validation, it is encouraging to once again see wave speeds that are within a factor of 2 of
each other.
6. CONCLUSIONS AND FUTURE CONSIDERATIONS
When I started this project, I had originally hoped to come up with a preliminary design for a sensor system
that could record displacement data that could be used to reconstruct the sound signal being produced by a
drumhead to allow for the micless recording of drums. Unfortunately, I had to settle with performing an almost
entirely software-based analysis. However, what this project was able to do was combine a passion of mine
(drumming) with the most prominent skill I developed during my Master’s program: finite element analysis. I
have a deep understanding of the theory behind it, have written my own code for membrane theory, and have
now implemented my first large-scale simulation to analyze the vibrational response of a drumhead, which I find
to be incredibly exciting and fulfilling. This report represents a comprehensive overview of the knowledge and
skills that I have acquired, and I am proud to present it.
The next step with this model would be to run it for a variety of impact locations with a finer timestep by
setting the maximum increment size to the order of 1 × 10−6
s in order to allow for the clear observation of
higher order modes throughout the free response. These would become increasingly important as the impact
location moves off-center, which is the reality of the system being modeled. A drummer will never hit the drum
exactly in the center, and that is precisely what gives the drum such a unique and varied sound. Every stroke
is different because the changing impact location provides a different set of initial conditions to the equations of
motion for a circular membrane, resulting in the excitation of different vibrational modes each time.
I would love to create a model using Abaqus that would produce displacement data over time for various
impact scenarios at select nodes on the head, positioned to capture the contributions of the most prominent
vibrational modes. Next, a Python model would utilize the displacement data to compute the Fourier coefficients
for the dominant modes and determine a resultant output signal that could be fed into a signal generator to play
the sound that was produced by the drumhead model.
7. ACKNOWLEDGMENTS
I would like to thank all of the UCLA Professors that I had the great opportunity to learn from, either through
a course or a simple conversation, during my time here. In particular, I would like to thank Professor Klug
for sending me down the path to Finite Element Analysis and helping me discover a passion in mechanical
engineering that I will take with me into my career. Finally, I would like to thank Professor Nasr Ghoniem,
my advisor, for his support and guidance over the last year to plan my Master’s program and make this report
possible.
36. APPENDIX A. ABAQUS MODEL SETUP GUIDE
Part
1. Use the Module dropdown selector to choose the
Part module
2. Select Create Part
3. Create Part
• Name > Drumhead
• Modeling Space > 3D
• Type > Deformable
• Shape > Shell
• Type > Planar
• Press Continue...
4. Sketch geometry
• Select Center circle tool
• Set center point: (0,0), Press enter
• Set perimeter point: (.2032, 0), Press enter
• Press esc to exit tool
• Press Done
Figure 19. Part geometry.
37. Property
1. Use the Module dropdown selector to choose the
Property module
2. Select Create Material
3. Edit Material
Name > Mylar
•• Select General > Density
• Mass Density > 900
• Select Mechanical > Elasticity > Elastic
• Young’s Modulus > 1e9
• Poisson’s Ratio > 0.4
• Press OK
4. Select Create Section
5. Create Section
• Name > Head (Membrane)
• Category > Shell
• Type > Membrane
• Press Continue...
38. 6. Edit section
• Material > Mylar
• Membrane thickness > .000254
• Section Poisson’s Ratio > Specify value >
.0.4
• Press OK
7. Select Assign Section
8. Click on the part to highlight it (part will be red
when selected)
9. Press Done at the bottom of the viewport
10. Edit Section Assginment
• Section > Head (Membrane)
• Assignment > From section
• Press OK
11. Part should be highlighted turquoise, indicating
that the section has been assigned
Figure 20. Successfully assigned section to part.
39. Assembly
1. Use the Module dropdown selector to choose the
Assembly module
2. Select Create Instance
3. Create Instance
• Create instances from > Parts
• Parts > Drumhead
• Instance Type > Independent (mesh on in-
stance)
• Press OK
4. Part is colored blue, indicating part instance has
been created
Figure 21. Successfully created part instance.
40. Step
1. Use the Module dropdown selector to choose the
Step module
2. Select Create Step
3. Create Step
• Name > Pre-stretch
• Insert new step after > Initial
• Procedure type > General
• Select from box: Static, General
• Press Continue...
4. Edit Step
• (Optional) Description > Add tension to
the membrane through uniform radial dis-
placement
• Press OK
5. Select Create Step
6. Create Step
• Name > Stick impact
• Insert new step after > Pre-stretch
• Procedure type > General
• Select from box: Dynamic, Implicit
• Press Continue...
7. Edit Step
• (Optional) Description > Stick impact with
drumhead
• Time period > 0.003
• Nlgeom > On
• Switch to Incrementation tab
• Maximum number of increments > 100000
• Increment size, Initial > 4e-6
• Increment size, Minimum > 3e-8
• Maximum increment size > Analysis appli-
cation default
• Press OK
41. 8. Select Create Step
9. Create Step
• Name > Free response
• Insert new step after > Stick impact
• Procedure type > General
• Select from box: Dynamic, Implicit
• Press Continue...
10. Edit Step
• (Optional) Description > Free vibrations of
the membrane after impact
• Time period > 1
• Nlgeom > On
• Switch to Incrementation tab
• Maximum number of increments > 100000
• Increment size, Initial > 4e-6
• Increment size, Minimum > 3e-8
• Maximum increment size > Analysis appli-
cation default
• Press OK
11. Select Create Field Output
12. Create Field
• Name > Pre-stretch output
• Step > Pre-stretch
• Press Continue...
13. Edit Field Output Request
• In the Output Variables box, type: S, U,
RF, NFORC
• (Alternative) Select the above quantities
using the dropdowns below the text box
• Press OK
14. Repeat 11-13 for Stick impact and Free response
steps, naming accordingly and selecting the ap-
propriate step.
42. Load
1. Use the Module dropdown selector to choose the
Load module
2. Use the Step dropdown selector to choose the
Pre-stretch step
3. Select Create Boundary Condition
4. Create Boundary Condition
• Name > Clamped Rim
• Step > Pre-stretch
• Category > Mechanical
• Types for Selected Step > Displace-
ment/Rotation
• Press Continue...
5. Select the rim of the drumhead by hovering over
it (highlight orange) and then clicking (highlight
red when selected)
6. Press Done at the bottom of the viewport
7. Select Create Datum CSYS to create a new co-
ordinate system
8. Create Datum CSYS
• Name > Cylindrical
• Coordinate System Type > Cylindrical
• Press Continue...
• Select (0,0,0) as the origin by clicking or
by typing in the box at the bottom of the
viewport
• Type (1,0,0) or select the point at the right
edge of the circle to be on the R-axis
• Type (0,1,0) to be in the R-Theta plane
• Press Cancel when the Create Datum
CSYS window pops back up
43. 9. Edit Boundary Condition
• Select the Mouse icon next to CSYS:
(Global) to edit the coordinate system se-
lection
• Press Datum CSYS List... at the bottom
of the viewport
• Names > Cylindrical to select the coordi-
nate system that was just created
• Press OK
• Cylindrical will now be selected
• Check the box next to U1:, and the box will
fill with a 0
• Change the U1: to be 0.0127
• Press OK
10. The assembly will show orange arrow pointing
radially outward to indicate the prescribed ra-
dial displacement
11. Use the Step dropdown selector to choose the
Stick impact step
12. Select the Clamped Rim boundary condition
that was just created from the Model tree by
double clicking on it
13. Constrain all other degrees of freedom by check-
ing the boxes for U2, U3, UR1, UR2, UR3 (note
the asterisks that appears next to them to indi-
cate that they are modified for this step)
14. Press OK
15. The assembly will show blue and orange trian-
gles around the rim to indicate the fixed degrees
of freedom
44. 15. From the menu at the top, select Tools > Parti-
tion...
16. Create Partition
• Type > Face
• Method > Use shortest path between 2
points
• Select the start point as the point on the
left edge of the circle
• Select the end point as the point on the
right edge of the circle
• Press Create Partition at the bottom of the
viewport
• A horizontal line will be drawn connecting
the two points through the center of the
drumhead
• The Create Partition window should still
be open. Change Type > Edge
• Method > Select midpoint/datum point
• Select the partition line that was just cre-
ated
• Select the midpoint of the line, which
should be at the center of the circle
• Press Create Partition at the bottom of the
viewport
• Close the Create Partition window
• Press esc to exit the tool
17. The drumhead should now appear with both a
horizontal partition line and yellow point at the
center (though it may be hard to see) as shown
below. Check that the center point is there by
hovering over it with the mouse, and it should
turn orange.
45. 18. Select Create Load
19. Create Load
• Name > Stick impact load
• Step > Stick impact
• Category > Mechanical
• Types for Selected Step > Concentrated
force
• Press Continue...
20. Select the point at the origin (highlighted in red
when selected)
21. Edit Load
• CF3 > -100
• Press OK
22. Rotate the viewport by holding cntrl + alt, then
clicking and dragging the view, such that the yel-
low arrow representing the load is visible. Note
that the load is pointing in the -z direction.
46. Mesh
1. Use the Module dropdown selector to choose the
Mesh module
2. Select Seed Part Instance
3. Global Seeds
• Approximate global size > 0.0053
• Important note: This simulation was
run on the UCLA Hoffman supercomputer
cluster and took about an hour to run. I
do not recommend running the model with
this element size on a personal computer, or
even a school computer, as it will take far
too long, and will likely not finish due to
a memory error. If you wish to run this
model on a personal computer, I recom-
mend returning to the mesh and seeding
the global seed size to 0.05. This analysis
should complete in a reasonable amount of
time, though the coarse mesh will lead to
somewhat inaccurate results.
• Press OK
• The part will be shown many white circles
around the rim, indicating the nodal loca-
tions for the mesh
• Press Done at the bottom of the viewport
4. Select Assign Element Type
5. Click on the part to select it (highlighted in red
when selected)
6. Press Done at the bottom of the viewport
7. Element Type
• Element Library > Standard
• Family > Membrane
• Geometric Order > Quadratic
• Select Tri tab
• At bottom, it should read: “M3D6: a 6-
node triangular membrane”
• Press OK
• Press Done at the bottom of the viewport
8. Select Assign Mesh Controls
47. 9. Mesh Controls
• Element Shape > Tri
• Technique > Free
• Algorithm > Checked
• Press OK
10. Select Mesh Part Instance
11. Select Yes at the bottom of the viewport
12. The part will turn light blue and display a trian-
gular mesh as shown below. Note the symmetry
of the mesh about the partition line.
Figure 22. Meshed membrane.
48. Job
1. Use the Module dropdown selector to choose the
Job module
2. Select Create Job
3. Create Job
• Name > Vibration-Analysis
• Press Continue...
4. Edit Job
• (Optional) Description > Vibrational anal-
ysis of a drumhead subject to an impact
load at center
• Press OK
49. 5. Select Job Manager
6. Job Manager
• Make sure that Vibration-Analysis is high-
lighted and Press Submit along the right
side of the window to run the analysis. The
status of the job should change to Running
• Select Monitor while the analysis is run-
ning to monitor progress and view warning
and error messages
• Select Results when the status of the job
has changed to Completed to view the results in the Visualization module. Data analysis will not be
further discussed here.
Figure 23. Job Manager window.
50. REFERENCES
1. Haberman, Richard. “Applied partial differential equations with Fourier series and boundary value problems.”
AMC 10 (2004): 12.
2. Ryan, Tyler. “Nonlinear Finite Element Analysis Code for Membrane Theory”. UCLA MAE 261B.
3. Wagner, Andreas. “Analysis of drumbeats-interaction between drummer, drumstick
and instrument.” KTH Computer Science and Communication. [Online]. Available:
http://www.speech.kth.se/publications/masterprojects/2006/AndreasWagner.pdf (2006).
