김경종
12 KiB
32.12.2 PIPE-SOIL INTERACTION ELEMENT LIBRARY
Product: Abaqus/Standard
References
• “Pipe-soil interaction elements,” Section 32.12.1
• *PIPE-SOIL INTERACTION
Overview
This section provides a reference to the pipe-soil interaction elements available in Abaqus/Standard.
Element types
2D elements
| PSI24 | Two-dimensional 4-node pipe-soil interaction element |
| PSI26 | Two-dimensional 6-node pipe-soil interaction element |
Active degrees of freedom
1, 2
Additional solution variables
None.
3D elements
| PSI34 | Three-dimensional 4-node pipe-soil interaction element |
| PSI36 | Three-dimensional 6-node pipe-soil interaction element |
Active degrees of freedom
1, 2, 3
Additional solution variables
None.
Nodal coordinates required
2D: X, Y
3D: X, Y, Z
Element property definition
Input File Usage: *PIPE-SOIL INTERACTION
Element-based loading
None.
Element output
The relative displacements corresponding to the forces below are chosen by requesting the corresponding “strains.” Elastic and plastic strains are available.
Two-dimensional elements
| S11 | Force per unit length in the first local direction. |
| S22 | Force per unit length in the second local direction. |
Three-dimensional elements
| S11 | Force per unit length in the first local direction. |
| S22 | Force per unit length in the second local direction. |
| S33 | Force per unit length in the third local direction. |
Node ordering and integration point numbering
text_image
4 far-field edge 1 pipeline edge 1 2 3
PSI24 and PSI34
text_image
4 6 3 far-field edge 1× × 3 × 2 pipeline edge 1 5 2
PSI26 and PSI36
32.13 Acoustic interface elements
• “Acoustic interface elements,” Section 32.13.1
• “Acoustic interface element library,” Section 32.13.2
32.13.1 ACOUSTIC INTERFACE ELEMENTS
Products: Abaqus/Standard Abaqus/CAE
References
• “Acoustic interface element library,” Section 32.13.2
• “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1
• *INTERFACE
• “Creating acoustic interface sections,” Section 12.13.18 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
Acoustic interface elements:
• can be used to couple a model of an acoustic fluid to a structural model containing continuum or structural elements;
• couple the accelerations of the surface of the structural model to the pressure in the acoustic medium;
• can be used in dynamic and steady-state dynamic procedures;
• must be defined with the nodes shared by the acoustic elements and the structural (or solid) elements;
• can be used only in small-displacement simulations and are not intended for use in nonlinear or hydrostatic fluid-structure interactions;
• are ignored in eigenfrequency extraction analyses if the subspace iteration eigensolver is used; and
• if necessary, can be degenerated into triangular elements.
For most problems the surface-based, structural-acoustic capabilities described in “Mesh tie constraints,” Section 35.3.1, and in “Defining tied contact in Abaqus/Standard,” Section 36.3.7, provide more general and easy to use methods for modeling the interaction between an acoustic fluid and a structure. Userspecified acoustic interface elements give you increased control over the coupling specification, at the expense of the convenience of the surface-based procedures.
Typical applications
The acoustic interface elements are used in simulations where the motion of a solid structure influences the pressure in the acoustic fluid, such as when the vibrations of a car frame produce noise in the passenger compartment; or where the pressure in the fluid affects a neighboring structure, such as when the smallamplitude sloshing of a fluid inside a container affects its response.
User-specified acoustic interface elements are also useful in problems involving only an acoustic medium because they allow you to specify displacement, velocity, or acceleration boundary conditions directly on the nodes of the acoustic interface elements. In this application, however, you must be aware that the tangential displacements are not coupled to the fluid. Therefore, zero-energy modes may
arise involving the displacement degrees of freedom if these nodes are not constrained in the tangential direction. When acoustic interface elements are used to couple fluid and solid elements, this problem does not arise because of the stiffness and inertia of the solid.
Choosing an appropriate element
The order of the underlying acoustic and structural elements usually dictates which acoustic interface element should be used. The general acoustic interface element, ASI1, can be used in any coupled acoustic-structural simulation; however, normally it is used only with the acoustic link elements (AC1D2 and AC1D3).
Defining the normal direction of the acoustic-structural interface
The connectivity of the acoustic interface elements and the right-hand rule define the normal direction of the acoustic-structural interface, as shown in “Acoustic interface element library,” Section 32.13.2. It is very important that this normal point into the acoustic fluid, as shown in Figure 32.13.1–1 and Figure 32.13.1–2. The one exception is the ASI1 acoustic interface element, where you must define the normal direction.
text_image
fluid 1 solid 2 ASI2D2 ASIAX2
text_image
fluid 1 2 solid ASI2D3 ASIAX3 3
Figure 32.13.1–1 Normal directions for two-dimensional and axisymmetric acoustic-structural interface elements.
Defining the acoustic interface element’s section properties
You must associate the acoustic interface section definition with a set of acoustic interface elements. This section definition must be used with three-dimensional and axisymmetric acoustic interface elements, even though there are no user-defined geometric properties for these elements.
Input File Usage: *INTERFACE, ELSET=element_set_name
Abaqus/CAE Usage: Property module:
Create Section: select Other as the section Category and
Acoustic interface as the section Type
Assign→Section: select regions
text_image
fluid 1 3 solid 2 ASI3D3
text_image
fluid 1 4 3 solid 2 ASI3D4
flowchart
graph TD
1["1"] -->|solid| 2["2"]
1 -->|fluid| 3["3"]
2 -->|fluid| 4["4"]
3 -->|fluid| 5["5"]
4 -->|fluid| 6["6"]
text_image
fluid 4 7 3 8 6 1 5 2 solid ASI3D8
Figure 32.13.1–2 Normal directions for three-dimensional acoustic-structural interface elements.
Defining the geometric properties associated with ASI1 elements
The ASI1 elements consist of a single node. Abaqus/Standard cannot calculate the surface area associated with these elements, so you must supply this information. If accurate surface areas are not given, Abaqus/Standard may calculate incorrect accelerations or acoustic fluid pressure at the acoustic-structural interface.
In addition, Abaqus/Standard cannot calculate the direction of the interface normal associated with these elements. You must provide the direction cosines, in the global Cartesian coordinate system, of the interface normal for these elements.
Input File Usage: *INTERFACE
surface area, X-direction cosine, Y-direction cosine, Z-direction cosine
Abaqus/CAE Usage: General-use acoustic interface sections are not supported in Abaqus/CAE.
Defining the thickness for planar acoustic interface elements
You can specify the thickness of planar acoustic interface elements. The default value is unit thickness.
Input File Usage: *INTERFACE thickness
Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Acoustic interface as the section Type: Plane stress/strain thickness: thickness
Using acoustic interface elements when elements with different interpolation orders form the acoustic-structural interface
It is normally assumed that the same order of interpolation will be used for both the acoustic fluid mesh and the structural mesh (at least at the interface surfaces). If this is not the case, suitable MPCs must be applied to the nodes along the acoustic-structural interface to maintain the compatibility in the pressure (MPC type P LINEAR) or displacement fields (MPC type LINEAR).
32.13.2 ACOUSTIC INTERFACE ELEMENT LIBRARY
Products: Abaqus/Standard Abaqus/CAE
References
• “Acoustic interface elements,” Section 32.13.1
• *INTERFACE
Overview
This section provides a reference to the acoustic interface elements available in Abaqus/Standard.
Element types
Element for general use
ASI1 1-node
Active degrees of freedom
1, 2, 3, 8
Additional solution variables
None.
Elements for use in planar models
ASI2D2 2-node linear
ASI2D3 3-node quadratic
Active degrees of freedom
1, 2, 8
Additional solution variables
None.
Elements for use in 3D models
ASI3D3 3-node linear
ASI3D4 4-node linear
ASI3D6 6-node quadratic
ASI3D8 8-node quadratic
Active degrees of freedom
1, 2, 3, 8
Additional solution variables
None.
Elements for use in axisymmetric models
| ASIAX2 | 2-node linear |
| ASIAX3 | 3-node quadratic |
Active degrees of freedom
1, 2, 8
Additional solution variables
None.
Nodal coordinates required
| General use element: None. |
| Planar: X, Y |
| 3D: X, Y, Z |
| Axisymmetric: r, z |
Element property definition
For general-use elements, you must define the element’s surface area and the direction cosines of the normal to the acoustic fluid-structural interface, pointing into the fluid. For elements for use in planar models, you must specify the thickness (out-of-plane) of the element. The default is unit thickness if no thickness is specified. For elements for use in three-dimensional and axisymmetric models, no additional data are required.
Input File Usage: *INTERFACE
Abaqus/CAE Usage: Property module: Create Section: select Other as the section Category and Acoustic interface as the section Type
General-use acoustic interface sections are not supported in Abaqus/CAE.
Element-based loading
Distributed impedances cannot be applied.
Element output
None.