is reasonable to estimate this wavelength using the highest frequency present in the loads or prescribed boundary conditions. An “internodal interval” is defined as the distance from a node to its nearest neighbor in an element; that is, the element size for a linear element or half of the element size for a quadratic element. At a fixed internodal interval, quadratic elements are more accurate than linear elements. The level of refinement chosen for the acoustic medium should be reflected in the solid medium as well: the solid mesh should be sufficiently refined to accurately model flexural, compressional, and shear waves. The level of mesh refinement required depends on the application. Any finite element discretization of a domain in which waves propagate introduces a certain amount of error per wavelength. In meshes that are small in terms of wavelengths, relatively coarse (for example, six internodal intervals per wavelength) meshes may be adequate. For meshes that contain many wavelengths at the frequency of interest, the per-wavelength finite element discretization error accumulates, generally necessitating greater levels of refinement. In these larger meshes the accumulated per-wavelength error may be present throughout the mesh if refinement is inadequate. The acoustic wavelength decreases with increasing frequency, so there is an upper frequency limit for a given mesh. Let $L _ { m a x }$ represent the maximum internodal interval of an element in a mesh, $n _ { m i n }$ the number of internodal intervals we desire per acoustic wavelength $( n _ { m i n } ~ \ge ~ 1 0$ is recommended), $f _ { m a x }$ the cyclical frequency of excitation, and $c = \sqrt { \mathrm { K } _ { f } / \rho _ { f } }$ the speed of sound, where $K _ { f }$ is the bulk modulus of the acoustic medium and $\rho _ { f }$ is its density. The requirements are then expressed as $$ L _ {m a x} < \frac {c}{n _ {m i n} f _ {m a x}} \qquad \mathrm{or} \qquad f _ {m a x} < \frac {c}{n _ {m i n} L _ {m a x}}. $$ The above expressions can be used to estimate the maximum allowable element length if the frequency is given or the maximum frequency for which a given mesh size is valid. For example, in air at room temperature, $c \approx 3 4 3$ meters per second. The following table gives some values for maximum internodal distances to model given maximum frequencies $f _ { m a x }$ accurately:
Maximum Frequency of Interest, $f_{max}$ Maximum Internodal Interval, $L_{max}$ , $n_{min} \equiv 8$ Maximum Internodal Interval, $L_{max}$ , $n_{min} \equiv 12$
100 Hz< 430 mm< 286 mm
500 Hz< 86 mm< 57 mm
1000 Hz< 43 mm<29mm
20 kHz< 2.1 mm< 1.4mm
For exterior problems the accuracy of an analysis also depends on the accuracy of the absorbing boundary condition. As mentioned above, the absorbing boundary impedance conditions implemented in Abaqus are used with a standoff thickness $r _ { 1 }$ of acoustic finite elements between the acoustic sources and the radiating boundary. Since the approximate radiation conditions converge to the exact condition in the limit of infinite standoff, a greater standoff thickness improves the accuracy of the solution. The standoff thickness $r _ { 1 }$ is expressed as $m _ { m i n }$ wavelengths at the minimum frequency to be analyzed: $$ r _ {1} > \frac {c m _ {m i n}}{f _ {m i n}} \qquad \mathrm{or} \qquad f _ {m i n} > \frac {c m _ {m i n}}{r _ {1}}. $$ Continuing the example using the properties of air, we can calculate the recommended minimum standoff thicknesses corresponding to a specified minimum frequency of interest, using $m _ { m i n } = 1 / 3$ :
Minimum Frequency of Interest, $f_{min}$ Radiation Boundary Standoff, $r_1$
100 Hz>1140 mm
500 Hz>230 mm
1000 Hz>114 mm
20 kHz>5.7 mm
The computational requirements for an exterior problem thus depend on both the radiation boundary standoff and the internodal distance. The number of nodes N in a model depends on the volume of the mesh, controlled by $r _ { 1 }$ and the spatial dimension $d ,$ and the mesh density, controlled by $L _ { m a x }$ . The exact number of nodes depends on the details of the model, but the expression $$ N \sim \left(\frac {r _ {1}}{L _ {m a x}}\right) ^ {d} \sim \left(\frac {f _ {m a x}}{f _ {m i n}} m _ {m i n} n _ {m i n}\right) ^ {d} $$ indicates the size of the model with respect to the ratio of the maximum to minimum frequencies in a given analysis. Because the mesh size for an exterior problem exhibits such strong dependence on the bandwidth, $f _ { m a x } - f _ { m i n }$ , you can control the size of an analysis by splitting the band. For example, if the overall frequency range of interest is 100 to 10000 Hz, a single spherical mesh covering this band in three dimensions has size $$ N \sim (1 0 0 m _ {m i n} n _ {m i n}) ^ {3} \sim 1 e 6 (m _ {m i n} n _ {m i n}) ^ {3}. $$ However, splitting the problem into two bands, and , and creating an exterior mesh for each band, results in two analyses of size $$ N \sim (1 0 m _ {m i n} n _ {m i n}) ^ {3} \sim 1 0 0 0 (m _ {m i n} n _ {m i n}) ^ {3}. $$ In coupled acoustic-structural systems there usually exist different wave speeds for the fluid and solid media. In the region of the acoustic-structural interface, the wave phenomena in both media may exhibit length scales characteristic of the slower medium; that is, the length scale of the wave dynamics may be as short as the shorter wavelength, corresponding to the lower wave speed. This result follows from the fact that the two media are coupled at the boundary. The region near the acoustic-structural interface where these effects are important is usually no thicker than the shorter wavelength. For example, in an analysis involving water interacting with rubber, the wave speed in the rubber may be much lower than that of water. A finite element mesh used to model this problem in detail would require refinement down to six (or more) nodes per shorter wavelength, on both sides of the interface. On the water side (faster, longer wavelength) accuracy will probably not be compromised significantly if this region of high refinement extends no further into the water than one short wavelength. Of course, in some analyses the effects in the vicinity of the interface may be unimportant. Then, the two meshes can be refined only so far as to represent their own characteristic wavelengths accurately. # Output Nodal output variable POR (pressure magnitude at the nodes of the acoustic elements) is available for an acoustic medium (in Abaqus/CAE this output variable is called PAC). When the scattered wave formulation (default) is used with incident wave loading, output variable POR represents only the scattered pressure response of the model and does not include the incident wave loading itself. When the total wave formulation is used, output variable POR represents the total dynamic acoustic pressure, which includes contributions from both incident and scattered waves as well as the dynamic effects of fluid cavitation. For either formulation output variable POR does not include the acoustic static pressure. In Abaqus/Explicit an additional nodal output variable PABS (the absolute pressure, equal to the sum of POR and the acoustic static pressure) is available. When the dynamic effects of fluid cavitation are of interest, you can specify the acoustic static pressure in an acoustic analysis that uses the total wave formulation. If the acoustic static pressure is not specified in an acoustic region, it is assumed to be large; thus precluding cavitation in that region. For general steps, including implicit and explicit dynamic steps, no energy quantities are computed for acoustic elements. Consequently, these elements will not contribute to the total energy balance. # Steady-state dynamic output For steady-state dynamic analysis POR is complex and can be displayed in several forms in the Visualization module of Abaqus/CAE. The phase angle (PPOR) is available as output to the data (.dat) and results (.fil) files. Several additional secondary quantities are available for multidimensional acoustic finite elements in direct-solution steady-state dynamic or subspace-based steady-state dynamic analysis. The “sound pressure level” is defined as: $$ S P L \equiv 2 0 \log_ {1 0} p _ {R M S} - 2 0 \log_ {1 0} p _ {R E F}, $$ where $p _ { R E F }$ is defined as a physical constant in the model (see “Defining the reference pressure” below), and the $p _ { R M S }$ is computed from the complex-valued acoustic pressure at any point using the formula: $$ 2 p _ {R M S} ^ {2} = \Re (\tilde {p}) ^ {2} + \Im (\tilde {p}) ^ {2}. $$ The acoustic particle velocity at any material point is $$ \tilde {\mathbf {v}} = \frac {i}{\tilde {\rho} \omega} \frac {\partial \tilde {p}}{\partial \mathbf {x}}. $$ The acoustic intensity vector, a measure of the rate of flow of energy at a material point, is $$ \tilde {\mathbf {I}} = - \frac {1}{2} \sigma \hat {\tilde {\mathbf {v}}}. $$ In an acoustic medium the stress tensor is simply the acoustic pressure times the identity tensor, so this expression simplifies to $$ \tilde {\mathbf {I}} = \frac {- 1}{2 i \hat {\tilde {\rho}} \omega} \left[ \tilde {p} \frac {\partial \hat {\tilde {p}}}{\partial \mathbf {x}} \right]. $$ The hats denote complex conjugation. The real part of the intensity is referred to as the “active intensity,” and the imaginary part is the “reactive intensity.” The acoustic pressure gradient is also available for acoustic finite elements in steady-state dynamic analysis. In steady-state dynamic analysis, additional nodal output quantities are available for acoustic infinite elements. PINF denotes the complex pressure coefficients of the infinite element shape functions. These coefficients can be used to visualize the exterior acoustic field (i.e., within the volume of the acoustic infinite elements) using scripting in the Visualization module of Abaqus/CAE; see “Using infinite elements to compute and view the results of an acoustic far-field analysis,” Section 9.10.11 of the Abaqus Scripting User’s Guide. INFN is the normal vector used by the acoustic infinite element to define the element volume. INFR denotes the radius used for the element at that node, and INFC denotes the element cosine; that is, the minimum dot product between the nodal normal vector and the acoustic infinite element facet normal vectors attached to that node. See “Acoustic infinite elements,” Section 3.3.2 of the Abaqus Theory Guide, for more complete descriptions of these quantities. INFN, INFR, INFC are useful in debugging a model using acoustic infinite elements; consequently, it is sometimes valuable to perform a steady-state dynamics, direct analysis on a model to visualize this information. For steady-state dynamic steps, energy quantities are available for acoustic elements. These elements contribute to the total energy balance in steady-state dynamics. # Defining the reference pressure You must define the reference pressure, , used to compute the sound pressure level; there is no default value for the reference pressure. Input File Usage: \*PHYSICAL CONSTANTS, SPL REFERENCE PRESSURE= Abaqus/CAE Usage: You cannot define a reference pressure in Abaqus/CAE. # Input file template The following is an example of the step definition for a direct-solution steady-state dynamic acoustic analysis that looks for the response of a model at six frequencies ranging linearly from $f = 1 0 \mathrm { t o } f =$ cycles/time. The pressure at node set INPUT (nodes at the boundary) is prescribed to have an inphase component of 3.0 and an out-of-phase component of −4.0 (i.e., a complex value of ). An in-phase inward volume acceleration of 40.0 is specified at node 10. On the surface LINER1 an impedance is defined based on the impedance property named CARPET1. On the second face of all of the elements in element set PAD, another surface impedance based on CARPET1 is defined. On the fourth face of all of the elements in element set END, the default plane wave boundary condition is specified. Printed output of pressure magnitude and phase is requested for node set OUTPUT. Acoustic pressure and displacement are written to the output database. All output is written once for each of the six excitation frequencies. ```txt *HEADING ... *SURFACE, NAME=LINER1 10, S3 *IMPEDANCE PROPERTY, NAME=CARPET1 Data describing impedance properties as a function of frequency ** *STEP *STEADY STATE DYNAMICS, DIRECT 10, 100, 6 *SIMPEDANCE, PROPERTY=CARPET1 LINER1, ** *IMPEDANCE, PROPERTY=CARPET1 PAD, I2 *IMPEDANCE END, I4 ** Apply complex pressure at node set INPUT *BOUNDARY, REAL INPUT, 8, 8, 3. *BOUNDARY, IMAGINARY INPUT, 8, 8, -4. ** Apply an in-phase inward volume acceleration at node 10 *CLOAD 10, 8, 40. ** Output requests *NODE PRINT, NSET=OUTPUT, TOTALS=YES POR, PPOR *OUTPUT, FIELD *NODE OUTPUT U, PU, POR *END STEP ``` The following is a template of the step definition for an Abaqus/Explicit acoustic analysis. On the surface SURF an impedance is defined based on the impedance property named IPROP. In addition, impedance is defined on elements or element sets. ```txt *HEADING ... *ELEMENT, TYPE=AC2D4R ... ** *SURFACE, NAME=SURF Data line to define surface *IMPEDANCE PROPERTY, NAME=IPROP Data describing impedance properties ** *STEP *DYNAMIC, EXPLICIT or *DYNAMIC TEMPERATURE-DISPLACEMENT, EXPLICIT Data line to define incrementation *SIMPEDANCE, PROPERTY=IPROP SURF, ** *IMPEDANCE Data lines to define impedance on elements or element sets *CLOAD Data line to define acoustic loads *FIELD Data line to define field variable values *END STEP ``` The following template is representative of a coupled acoustic-structural shock problem using the preferred interface for applying incident wave loading (see “Incident wave loading due to external sources” in “Acoustic and shock loads,” Section 34.4.6): ```txt *HEADING ... *ELEMENT, TYPE=..., ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=..., ELSET=SOLID Data lines to define solid elements *ELEMENT, TYPE=..., ELSET=BEAM Data lines to define beam elements *BEAM SECTION, ELSET=BEAM, MATERIAL=... Data lines to define the beam stiffness section properties *BEAM FLUID INERTIA Data line to define the beam virtual mass property ``` ```txt *SURFACE, NAME=IW_LOAD_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_SOLID Data lines to define the solid surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_BEAM Data lines to define the beam surface loaded by the incident wave *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *INCIDENT WAVE INTERACTION PROPERTY, NAME=IWPROP, TYPE=SPHERE Data lines to define a spherical incident wave field *UNDEX CHARGE PROPERTY Data lines to define the underwater explosion parameters ** Tie the acoustic mesh to the solid mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID *STEP *DYNAMIC, EXPLICIT or *DYNAMIC ** Load the acoustic surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_ACOUSTIC, source node, standoff node, reference magnitude ** Load the solid surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_SOLID, source node, standoff node, reference magnitude ** Load the beam surface *INCIDENT WAVE INTERACTION, PROPERTY=IWPROP IW_LOAD_BEAM, source node, standoff node, reference magnitude *END STEP ``` The following template is representative of a coupled acoustic-structural shock problem using the alternative interface for applying incident wave loading: ```txt *HEADING ... *ELEMENT, TYPE=..., ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=..., ELSET=SOLID Data lines to define solid elements *ELEMENT, TYPE=..., ELSET=BEAM Data lines to define beam elements *BEAM SECTION, ELSET=BEAM, MATERIAL=... Data lines to define the beam stiffness section properties ``` ```txt *BEAM FLUID INERTIA Data line to define the beam virtual mass property *SURFACE, NAME=IW_LOAD_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_SOLID Data lines to define the solid surface loaded by the incident wave *SURFACE, NAME=IW_LOAD_BEAM Data lines to define the beam surface loaded by the incident wave *SURFACE, NAME=TIE_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh *SURFACE, NAME=TIE_SOLID Data lines to define the solid surface interface with the acoustic mesh *INCIDENT WAVE PROPERTY, NAME=IWPROP, TYPE=SPHERE Data lines to define a spherical incident wave field *INCIDENT WAVE FLUID PROPERTY Data lines to define the fluid properties for the incident wave field *AMPLITUDE, DEFINITION=BUBBLE, NAME=PRESSUREVTIME Data lines to define the underwater explosion parameters ** Tie the acoustic mesh to the solid mesh *TIE, NAME=COUPLING TIE_ACOUSTIC, TIE_SOLID *STEP *DYNAMIC or *DYNAMIC, EXPLICIT ** Load the acoustic surface *INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP IW_LOAD_ACOUSTIC, {amplitude} ** Load the solid surface and the beam surface *INCIDENT WAVE, PRESSURE AMPLITUDE=PRESSUREVTIME, PROPERTY=IWPROP IW_LOAD_SOLID, {amplitude} IW_LOAD_BEAM, {amplitude} *END STEP ``` The following template is representative of a coupled acoustic-structural sound transmission problem using the preferred interface for applying incident wave loading (see “Incident wave loading due to external sources” in “Acoustic and shock loads,” Section 34.4.6): ```txt *HEADING ... *ELEMENT, TYPE=..., ELSET=ACOUSTIC Data lines to define acoustic elements *ELEMENT, TYPE=..., ELSET=SOLID ``` Data lines to define solid elements \*SURFACE, NAME=IW\_LOAD\_ACOUSTIC Data lines to define the acoustic surface loaded by the incident wave \*SURFACE, NAME=IW\_LOAD\_SOLID Data lines to define the solid surface loaded by the incident wave \*SURFACE, NAME=TIE\_ACOUSTIC Data lines to define the acoustic surface interface with the solid mesh \*SURFACE, NAME=TIE\_SOLID Data lines to define the solid surface interface with the acoustic mesh \*INCIDENT WAVE INTERACTION PROPERTY, NAME=FIRST, TYPE=SPHERE Data lines to define a spherical incident wave field \*INCIDENT WAVE INTERACTION PROPERTY, NAME=SECOND, TYPE=PLANE Data lines to define a planar incident wave field \*\* Tie the acoustic mesh to the solid mesh \*TIE, NAME=COUPLING TIE\_ACOUSTIC, TIE\_SOLID \*STEP \*STEADY STATE DYNAMICS, DIRECT or SUBSPACE PROJECTION \*\* Define the load on the acoustic and solid surfaces due to \*\* the first loading case: \*LOAD CASE, NAME=FIRST\_SOURCE \*\* Load the acoustic surface: define the real part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL IW\_LOAD\_ACOUSTIC, first source node, first standoff node, reference magnitude \*\* Load the acoustic surface: define the imaginary part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY IW\_LOAD\_ACOUSTIC, first source node, first standoff node, reference magnitude \*\* Load the solid surface: define the real part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=FIRST, REAL IW\_LOAD\_SOLID, first source node, first standoff node, reference magnitude \*\* Load the solid surface: define the imaginary part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=FIRST, IMAGINARY IW\_LOAD\_SOLID, first source node, first standoff node, reference magnitude \*END LOAD CASE \*\* Define the load on the acoustic and solid surfaces due to \*\* the next loading case: \*LOAD CASE, NAME=SECOND\_SOURCE \*\* Load the acoustic surface: define the real part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL IW\_LOAD\_ACOUSTIC, second source node, second standoff node, reference magnitude \*\* Load the acoustic surface: define the imaginary part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY IW\_LOAD\_ACOUSTIC, second source node, second standoff node, reference magnitude \*\* Load the solid surface: define the real part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=SECOND, REAL IW\_LOAD\_SOLID, second source node, second standoff node, reference magnitude \*\* Load the solid surface: define the imaginary part at the \*\* standoff point \*INCIDENT WAVE INTERACTION, PROPERTY=SECOND, IMAGINARY IW\_LOAD\_SOLID, second source node, second standoff node, reference magnitude \*END LOAD CASE \*END STEP