김경종
281 lines
20 KiB
Markdown
281 lines
20 KiB
Markdown
<!-- source-page: 571 -->
|
||
|
||
Abaqus/CAE Usage: Interaction module: Connector→Assignment→Create: select wires: Orientation 1, Orientation 2: Edit: select the orientations for the first and second points, respectively, of the selected wires
|
||
|
||
Degree of freedom activation and corotation of connection directions
|
||
|
||
Many connection types either require connection directions at the nodes on the element or allow optional directions to be defined. In cases where an orientation definition is permitted for defining connection directions (required or optional), connector elements activate the rotational degrees of freedom at the nodes to which they are attached, if they do not exist already. The only exception is connection type JOIN, for which connection directions are optional at the first node of the element, but rotation degrees of freedom are not activated.
|
||
|
||
The connector element’s orientation directions corotate with the rotational degrees of freedom at the corresponding node on the element. If there is no element with rotational degrees of freedom or rotation constraint (such as an equation or a multi-point constraint) attached to the node, you must ensure that sufficient rotational boundary conditions are provided to avoid numerical singularities associated with unconstrained rotational degrees of freedom. Connection type JOIN uses fixed directions when rotational degrees of freedom are not active at the nodes on the connector element.
|
||
|
||
# Example
|
||
|
||
Figure 31.1.2–1 illustrates the use of the CONN3D2 element to connect two bodies with a cylindricallike connector oriented at $6 0 ^ { \circ }$ from the global 1-axis. On the left is a schematic representation of the connection to be modeled; on the right is a representation of the equivalent finite element model. See “Connection-type library,” Section 31.1.5, for a list of connector type names.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
extensible
|
||
range
|
||
7.5
|
||
</details>
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
node 12
|
||
b
|
||
1 (local orientation)
|
||
node 11
|
||
a
|
||
2
|
||
</details>
|
||
|
||
Figure 31.1.2–1 Simplified connector model of a shock absorber.
|
||
|
||
The connection requires node b to remain on the line of the shock absorber, which is determined by the position and orientation directions of node a. Furthermore, the two rotation components perpendicular to the line of the shock absorber at node b must be the same as those at node a. Hence, the only relative motion components permitted in the connection are the displacement of node b relative to node a along the line of the shock absorber and the rotation of node b relative to node a about the line of the shock absorber. This displacement and this rotation are the available components of relative motion. The connector is defined using the following lines in the input file:
|
||
|
||
<!-- source-page: 572 -->
|
||
|
||
```txt
|
||
* ELEMENT, TYPE=CONN3D2, ELSET=shock
|
||
101, 11, 12
|
||
* CONNECTOR SECTION, ELSET=shock
|
||
slot, revolute
|
||
ori60,
|
||
* ORIENTATION, NAME=ori60
|
||
**Defines the local 1-direction along the slot (required)
|
||
**Also defines the rotation axis for the revolute (required)
|
||
0.5, 0.866025, 0.0, -0.866025, 0.5, 0.0
|
||
```
|
||
|
||
Alternatively, you could use the assembled connection type CYLINDRICAL instead of the two basic connection types SLOT and REVOLUTE.
|
||
|
||
# Defining additional connection type data
|
||
|
||
Some connection types allow additional data to define the kinematic behavior of the connector. For example, the connection type FLOW-CONVERTER allows you to specify a scaling factor for material flow at node b. See “Connection-type library,” Section 31.1.5, for more information.
|
||
|
||
# Defining the connector behavior
|
||
|
||
Abaqus provides comprehensive kinetic behavior modeling in the available components of relative motion. Defining connector behavior is optional and can be used to incorporate spring, dashpot, node-to-node contact, locking, friction, plasticity-like effects, and failure. The kinetic modeling capabilities in connectors are described in detail in “Connector behavior,” Section 31.2.1.
|
||
|
||
# Using connector elements in two-dimensional and axisymmetric analysis
|
||
|
||
Not all connection types can be used with element type CONN2D2. The connection-type library contains many connection types whose mechanics are valid for three-dimensional analyses only. In other cases the local directions required in the definition of the connection type conflict with the two-dimensional coordinate system. See “Connection-type library,” Section 31.1.5, for more information.
|
||
|
||
# Using multiple connector elements in parallel
|
||
|
||
Connector elements in Abaqus allow most physical connections to be modeled with a single connector element. However, in certain circumstances more complex connections or output considerations may require multiple connector elements to be used in parallel. This is accomplished by defining two or more connector elements between the same nodes. In this case you must ensure that a constrained component of relative motion in one connector element is not constrained (either by a kinematic constraint or through motion specified as described in “Connector actuation,” Section 31.1.3) by one of the other connector elements.
|
||
|
||
Multiple connector elements are sometimes used in parallel to obtain output in different coordinate systems. For a connector element between two bodies, the local directions at the nodes can be determined by the requirements of the connection type. However, output may be needed in a different, possibly
|
||
|
||
<!-- source-page: 573 -->
|
||
|
||
corotating, coordinate system. For example, the angular acceleration history could be reported in a local, body-fixed coordinate system (other than the one used to define the connector element) by using a second connector element (such as connection type CARDAN) that does not impose kinematic constraints or use connector behavior but aligns with the desired local output directions.
|
||
|
||
# Defining connectors in a model that contains parts and an assembly
|
||
|
||
An Abaqus model can be defined in terms of an assembly of part instances (see “Defining an assembly,” Section 2.10.1). Connector elements can be defined at either the part level or the assembly level in such a model.
|
||
|
||
# Using connector elements with nodal transformations
|
||
|
||
Nodal transformations (see “Transformed coordinate systems,” Section 2.1.5) can be defined for either node connected to the connector element. Since these transformations affect only the nodal degrees of freedom, their use does not affect the behavior of the connector element. Connector elements operate on components of motion local to the connection.
|
||
|
||
# Using nonlinear connections in geometrically linear analyses
|
||
|
||
If a connector element with a nonlinear kinematic constraint is used in a geometrically linear analysis, the kinematic constraint is linearized. For example, if connection type LINK is used in a geometrically linear analysis, the distance between the two nodes is held constant after projection onto the direction of the line between the original positions of the nodes. The difference should be noticeable only if the magnitudes of the rotations and displacements are not small.
|
||
|
||
# Mismatched masses at connector nodes in Abaqus/Explicit
|
||
|
||
If the nodes of a connector element in Abaqus/Explicit have masses that are highly mismatched, the implicit solver may encounter convergence problems due to the resulting ill-conditioned coefficient matrix. To prevent this from happening, if the nodal masses or rotary inertias of a connector element differ by more than three orders of magnitude, Abaqus/Explicit adds mass/rotary inertia to the connector element node that has the smaller mass/rotary inertia. The mass/rotary inertia added is negligibly small (less than three orders of magnitude smaller) compared to the larger of the connector element’s nodal inertias. This additional mass almost never affects the solution significantly. However, in certain situations (for example, for a strongly dynamic analysis that has connector elements with highly mismatched nodal masses) this adjustment may have a noticeable effect.
|
||
|
||
# Connector output
|
||
|
||
The connector element force, moment, and kinematic output is defined in “Connector element library,” Section 31.1.4. These output quantities include total, elastic, viscous, and friction forces and moments. In addition, reaction forces and moments caused by connector stops and locks are available as well as connector contact forces used for friction calculation.
|
||
|
||
<!-- source-page: 574 -->
|
||
|
||
To obtain accurate reaction force and moment output for connectors from Abaqus/Explicit, it may sometimes be necessary to run the analysis in double precision. In such situations a double precision run will also yield a better estimate of the work done by the reaction forces and moments, thereby providing a more accurate value of the energy due to the external work reported by Abaqus/Explicit.
|
||
|
||
Kinematic output includes relative position, relative displacement, relative velocity, relative acceleration, frictional slip, and constitutive displacements (the displacement used in the elastic force and hysteretic friction calculations defined as the difference between the current relative positions and the reference positions; see “Defining reference lengths and angles for constitutive response” in “Connector behavior,” Section 31.2.1). For relative rotations the Abaqus convention of reporting angles between and radians is not used with connector elements. Connector element output of angles and rotational components or relative motion includes accumulated multiple rotations whose magnitudes can be arbitrarily large. Energy output is available, as are output flags to identify whether a connector has failed (in Abaqus/Explicit only), locked, or reached a connector stop.
|
||
|
||
In a geometrically linear step in Abaqus/Standard the relative position output variable does not change (in the same fashion that the nodal coordinates are output). Therefore, care must be exercised in interpreting output for connector stops and locks since they use updated coordinates.
|
||
|
||
# Using connector elements for output only
|
||
|
||
Connector elements defined without kinematic constraints or constitutive behavior can be used to monitor kinematic output in local coordinate systems. Quantities of interest include relative position, displacement, velocity, and acceleration in local coordinate parametrization. Finite rotation parametrizations include Euler and Cardan angles, rotation vector, and flexion-torsion-sweep. For an example that uses a connector element to monitor Euler angles, see “Motion of a rigid body in Abaqus/Standard,” Section 1.3.6 of the Abaqus Benchmarks Guide.
|
||
|
||
In Abaqus/Explicit all such connectors are solved without invoking the implicit solver, which leads to better performance in domain parallel mode (particularly when such connectors nodes overlap with other constraints such as slave nodes of tie constraints).
|
||
|
||
<!-- source-page: 575 -->
|
||
|
||
# 31.1.3 CONNECTOR ACTUATION
|
||
|
||
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Connectors: overview,” Section 31.1.1
|
||
• \*CONNECTOR LOAD
|
||
• \*CONNECTOR MOTION
|
||
• “Defining a connector force,” Section 16.9.13 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining a connector moment,” Section 16.9.14 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining a connector displacement boundary condition,” Section 16.10.5 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining a connector velocity boundary condition,” Section 16.10.6 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
• “Defining a connector acceleration boundary condition,” Section 16.10.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
|
||
|
||
# Overview
|
||
|
||
# Connector actuation:
|
||
|
||
• is meant to model situations, such as deployment maneuvers, where a motor attached to the body loads the connection with an internal force or moment history or a hydraulic system imposes a known motion;
|
||
• can be used to fix available components of relative motion; and
|
||
• consists of driving an available component of relative motion by a prescribed displacement (rotation) or by a specified force (moment).
|
||
|
||
The prescribed relative motions and loads are in the local directions associated with the available components of relative motion for the connector.
|
||
|
||
Prescribing displacements/rotations for available components of relative motion that also include connector stop or connector lock behaviors may lead to overconstraints. Abaqus will issue a warning message if an overconstraint occurs.
|
||
|
||
# Fixing available components of relative motion
|
||
|
||
A common practice is to fix available components of motion. Such fixed motion conditions can be used to customize connection types for specific applications. As an example, the REVOLUTE connection type uses the local 1-direction as the shared revolute axis and, hence, the available component of relative
|
||
|
||
<!-- source-page: 576 -->
|
||
|
||
motion. If, for convenience, a revolute connection about the local 3-direction were needed, you could fix the relative rotations about the local 1- and 2-directions in a CARDAN connection type. In doing so, a connection type identical to the REVOLUTE connection type would be created; however, the shared axis would be the local 3-direction instead of the local 1-direction.
|
||
|
||
An example is provided later in this section in which the pin part of a pin-in-slot connection is modeled with a CARDAN connection type with fixed rotations.
|
||
|
||
Input File Usage: Use the following option in the model portion of the input file to fix available connector components of relative motion:
|
||
|
||
\*CONNECTOR MOTION
|
||
|
||
Abaqus/CAE Usage: Load module: Create Boundary Condition: Step: Initial: Mechanical: Connector displacement
|
||
|
||
# Displacement-controlled actuation
|
||
|
||
You can specify a relative displacement, velocity, or acceleration between two parts in the connector’s local directions in a manner similar to defining a boundary condition (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). You specify the connector element set name or connector element number; the component number identifying the available component of relative motion being actuated; and the value of the relative displacement, velocity, or acceleration.
|
||
|
||
The penalty used for enforcing connector motion may lead to a noisy solution, particularly in single precision for some models. Use of double precision is, therefore, preferable in such situations. If performance is a concern for double precision, you can run the constraint packaging and constraint solver in double precision (see “Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD execution,” Section 3.2.2).
|
||
|
||
You cannot specify the motion of connectors in a subspace dynamic analysis.
|
||
|
||
Input File Usage: Use the following option in the history portion of the input file to specify a relative displacement for a connector:
|
||
|
||
\*CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=DISPLACEMENT
|
||
|
||
Use the following option in the history portion of the input file to specify a relative velocity for a connector:
|
||
|
||
\*CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=VELOCITY
|
||
|
||
Use the following option in the history portion of the input file to specify a relative acceleration for a connector:
|
||
|
||
\*CONNECTOR MOTION, AMPLITUDE=name, OP=MOD or NEW, TYPE=ACCELERATION
|
||
|
||
Abaqus/CAE Usage: Load module: Create Boundary Condition: Mechanical: Connector displacement, Connector velocity, or Connector acceleration
|
||
|
||
<!-- source-page: 577 -->
|
||
|
||
# Example
|
||
|
||
Figure 31.1.3–1 illustrates a pin-in-slot connection oriented at $4 5 ^ { \circ }$ from the global 1-axis modeled with element type CONN3D2.
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
2.0
|
||
15.0
|
||
body 2
|
||
node 120
|
||
node 110
|
||
body 1
|
||
45°
|
||
Rightarrow
|
||
node 120
|
||
2
|
||
1 (local orientation)
|
||
node 110
|
||
2
|
||
1
|
||
global directions
|
||
</details>
|
||
|
||
Figure 31.1.3–1 A pin-in-slot connection modeled with SLOT and CARDAN connection types.
|
||
|
||
The figure on the left is a schematic representation of the connection to be modeled, while the figure on the right is the finite element mesh. Displacements in the slot are allowed only along the line of the slot, and connection type SLOT is appropriate for enforcing these kinematics. Assume the pin and slot are constructed in such a way that the only rotation of the pin relative to the slot is along the local 3-direction. This is a revolute constraint; however, basic rotation connection type REVOLUTE uses the local 1-direction as the revolute axis. In this case connection type CARDAN combined with a specified constraint can be used to define a revolute-type connection with the appropriate revolute axis.
|
||
|
||
For illustrative purposes assume the connection is actuated by a rotational velocity of radians per second around the pin’s axis. Using input parametrization for convenience, the following lines are used:
|
||
|
||
```txt
|
||
*PARAMETER
|
||
PI = 3.141592
|
||
rotangvel = PI/4
|
||
...
|
||
*ELEMENT, TYPE=CONN3D2, ELSET=pininslot
|
||
101, 110, 120
|
||
*CONNECTOR SECTION, ELSET=pininslot
|
||
cardan, slot
|
||
ori45,
|
||
*CONNECTOR MOTION
|
||
pininslot, 4
|
||
```
|
||
|
||
<!-- source-page: 578 -->
|
||
|
||
```txt
|
||
pininslot, 5
|
||
*ORIENTATION, NAME=ori45
|
||
0.707, 0.707, 0.0, -0.707, 0.707, 0.0
|
||
...
|
||
*STEP
|
||
...
|
||
*CONNECTOR MOTION, TYPE=VELOCITY
|
||
pininslot, 6, <rotangvel>
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
# Force-controlled actuation
|
||
|
||
You can specify concentrated loads applied to the available components of relative motion in a manner similar to defining concentrated loads for other elements in Abaqus (see “Concentrated loads,” Section 34.4.2). However, connector loads are always follower loads that rotate with the rotation of the available components of relative motion as the connector element moves. You specify the connector element set name or connector element number, the component number identifying the available component of relative motion being loaded, and the value of the actuation force or moment.
|
||
|
||
Input File Usage: Use the following option in the history portion of the input file to specify a concentrated load for a connector:
|
||
|
||
```txt
|
||
*CONNECTOR LOAD, AMPLITUDE=name, OP=MOD
|
||
```
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: Mechanical: Connector force or Connector moment
|
||
|
||
# Example
|
||
|
||
Returning to the example in Figure 31.1.3–1, assume that the pin is pushed along the slot by a constant force of 1000.0 units (for example, through a hydraulic system). The following lines should be added to the input file:
|
||
|
||
```batch
|
||
*STEP
|
||
...
|
||
*CONNECTOR LOAD
|
||
pininslot, 1, 1000.0
|
||
...
|
||
*END STEP
|
||
```
|
||
|
||
# Connector actuation in linear perturbation procedures
|
||
|
||
Nonzero magnitude connector motions are allowed only in the eigenvalue buckling, direct-solution steady-state dynamic, and linear static perturbation procedures. Any nonzero magnitude specified during an eigenfrequency extraction procedure is ignored, and the specified available component of relative motion is held fixed. Connector motions cannot be used in any modal-based procedure.
|
||
|
||
<!-- source-page: 579 -->
|
||
|
||
In direct-solution steady-state dynamic analyses the real and imaginary parts of any available connector component of relative motion are either restrained or unrestrained simultaneously; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will automatically restrain both the real and the imaginary parts of a component of relative motion even when only one part is prescribed specifically. The unspecified part will be assumed to have a perturbation magnitude of zero.
|
||
|
||
A nonzero prescribed connector motion in an eigenvalue buckling step will contribute to the incremental stress and, thus, will contribute to the differential initial stress stiffness. When prescribing nonzero connector motions, you must interpret the resulting eigenproblem carefully. See the discussion for boundary conditions in “Eigenvalue buckling prediction,” Section 6.2.3, for more details.
|
||
|
||
In steady-state dynamic analyses both real and imaginary connector loads can be applied in a manner similar to concentrated loads (see “Mode-based steady-state dynamic analysis,” Section 6.3.8; “Direct-solution steady-state dynamic analysis,” Section 6.3.4; and “Subspace-based steady-state dynamic analysis,” Section 6.3.9). Multiple connector load cases can be defined in random response analyses (see “Random response analysis,” Section 6.3.11) in the same manner as concentrated loads. Connector loads are ignored during an eigenfrequency extraction analysis.
|
||
|
||
<!-- source-page: 580 -->
|