Problems xcouplingk_std_beam.inp, xcouplingk_xpl_beam2d.inp, xcouplingk_std_bem3.inp and xcouplingk_xpl_beam3d.inp impose rigid beam constraints using the *COUPLING option.

Problems xcouplingk_std_revolute.inp and xcouplingk_xpl_revolute.inp test the finite rotation revolute behavior of the kinematic coupling constraint when only two rotational degrees of freedom are constrained.

Problems xcouplingk_std_universal.inp and xcouplingk_xpl_universal.inp test the finite rotation universal behavior of the kinematic coupling constraint when only one rotational degree of freedom is constrained.

Figure 5.1.6–1 shows the geometry for these problems .

In these tests the center node is the reference node, and the perimeter nodes are the coupling nodes. Four separate coupling definitions that share the same reference node are defined. Each coupling definition defines the local coordinate system using a different orientation system: cylindrical, rectangular, spherical, and, for the ABAQUS/Standard analyses, a system defined by user subroutine ORIENT. In all cases the resulting local constraint basis directions coincide with the local directions of a cylindrical coordinate system whose axis is normal to the plane containing the nodes and passes through the reference node.

In problems xcouplingk_std_orient_1.inp and xcouplingk_xpl_orient_1.inp the kinematic coupling constrains all but the radial degree of freedom at the coupling nodes. Linear springs to ground (SPRING1) for the ABAQUS/Standard analyses and connector elements to ground (CONN3D2) with linear elastic connector behavior for the ABAQUS/Explicit analyses are attached to all coupling nodes and act in the - and -directions. The reference node is then rotated radians about the -axis.

In problems xcouplingk_std_orient_2.inp and xcouplingk_xpl_orient_2.inp the kinematic coupling constrains the circumferential degree of freedom only. Linear springs to ground (SPRING1) for the ABAQUS/Standard analyses and connector elements to ground (CONN3D2) with linear elastic connector behavior for the ABAQUS/Explicit analyses are attached to all coupling nodes and act in the -, -, and -directions. The reference node is then rotated about -axis.

The model consists of an axial arrangement of 20 shell elements. These elements are tied together using a combination of kinematic coupling constraints as well as MPCs. The constraints are defined such that the kinematic coupling reference node appears after the constraint definitions that are eliminated degrees of freedom on that node; thus, constraint sorting is required. The structure is clamped on one end, and a concentrated axial load is applied on the other end.

The initial starting geometry for each test is shown in Figure 1.10.3–1. For the geometric linear test, for ABAQUS/Standard, each coupling node is connected by a spring to ground (SPRING1) in each direction. In the geometrically nonlinear test in ABAQUS/Standard, each coupling node is connected by a dashpot to ground (DASHPOT1) in each direction, and an axial spring element (SPRINGA) connects each pair of coupling nodes. In the geometrically nonlinear test in ABAQUS/Explicit, each coupling node is connected by a connector to ground (CONN3D2) with damping behavior specified in each direction, and a connector element with specified elasitic behavior connects each pair of coupling nodes. The reference node for the *COUPLING option is node 10.

Linear behavior

Properties:

The spring stiffnesses are 100, 200, and 300 for degrees of freedom 1, 2, and 3, respectively, for the springs connected to all coupling nodes. The distributing weight factors are 1, 2, and 3 for nodes 1, 2, and 3, respectively.

Loading:

Step 1	The force at the reference node is 1.0 in the -direction. The moment at the reference node is 2.0 about the -axis.
Step 2	The force at the reference node is 1.0 in the -direction. The moment at the reference node is 2.0 about the -axis.
Step 3	The force at the reference node is 1.0 in the -direction. The moment at the reference node is 2.0 about the -axis.
Step 4	Frequency extraction.
Step 5	Transient modal dynamic step with a load, 1.0, applied to the reference node.
Step 6	Mode-based steady-state dynamic step with a load, 1.0, applied to the reference node.

Nonlinear behavior

Properties:

The dashpot damping coefficients are 100, 200, and 300 for degrees of freedom 1, 2, and 3, respectively, for the dashpots connected to all coupling nodes. The axial springs connecting the coupling nodes each have a spring constant of 1.0 × 10⁸. The distributing weight factors are 1, 2, and 3 for nodes 1, 2, and 3, respectively.

Prescribed reference node motion for ABAQUS/Standard:

Step 1	Total rotation of about the -axis. Translation .
Step 2	Total rotation of about the -axis. Translation .
Step 3	Total rotation of about the -axis. Translation .
Step 4	Direct-integration dynamic step with a total rotation of about the -axis. Translation .

Prescribed reference node motion for ABAQUS/Explicit:

Step 1	Total rotation of about the -axis. Translation .
Step 2	Total rotation of about the -axis. Translation .
Step 3	Total rotation of about the -axis. Translation .
Step 4	Total rotation of about the -axis. Translation .

Various models consisting of either continuum, beam, or shell elements are used in this test. In all models a uniform surface load is applied via a reference node and a distributing coupling constraint. A non-uniform mesh density is used to verify that the proper tributary area is calculated. The reference node is located at the center of the loaded surface, offset in the normal direction.

A part is defined consisting of two rows of 20 CPE4R elements. Each element is a unit square. The coupling nodes are defined along the top surface. A reference node is created at the center of the top surface. The part is then instanced three times in the assembly definition. For each part instance a coupling constraint with a different influence region is defined. The first part instance has an infinite influence radius; i.e., all nodes defined on the surface will be included in the coupling definition. The second part instance uses an influence radius of 5.5, and the third part instance uses an influence radius of 0.5. A concentrated load is applied to each reference node. Input files are provided for each weighting scheme: uniform, linear, quadratic, and cubic.

The geometry is shown in Figure 5.1.6–3.

This example consists of both a two-dimensional and three-dimensional test.

In the two-dimensional test, two separate models are defined. Each model consists of a single CPE4 element with one face coupled to a reference node with a distributing constraint. The opposite face of the CPE4 element is fixed. Beam elements are attached to the reference nodes for visualization purposes only. The first model uses the default coupling in which the rotation degree of freedom of the reference node is coupled to the solid surface (the displacement degrees of freedom of the reference are always coupled to the surface with distributing constraints). The second model releases the rotation constraint. A series of boundary condtions are applied to the reference nodes simulating shear, tension, and bending (in various linear and nonlinear steps).

In the three-dimensional test, eight separate models are defined. Each model consists of a single C3D8 element with one face coupled to a reference node with a distributing constraint. The opposite faces of the C3D8 elements are fixed. Beam elements are attached to the reference nodes for visualization purposes only. The first model uses the default coupling in which all three rotation degrees of freedom of the reference node are coupled to the solid surface. The next three models respectively release the rotation constraint in the 1, 2, and 3 directions. The final four models are identical to the first four, except that the rotation constraint directions are specified using the ORIENTATION parameter on the *COUPLING option. A series of boundary conditions are applied to the reference nodes simulating shear, tension, and bending (in linear and nonlinear steps).

This example consists of two sets of tests in which a pipe is modeled with beam and shell elements and with beam and continuum elements.

The pipe analyzed with beam and shell elements has a length of 0.8 m, an outside radius of 0.1 m, and a thickness of 0.01 m. The material has a Young's modulus of 200 GPa and a Poisson's ratio of 0.3. Half of the pipe is modeled with beam elements and the other half is modeled with shell elements (see Figure 5.1.6–4(a)). The beam node closest to the shell model is defined as the reference node for the distributing coupling constraint. An element-based edge surface is defined on the shell model, which is coupled to the reference node. The coupled model is subjected to four linear loading conditions simulating: (1) twist about the pipe axis, (2) axial stretch along the pipe axis, (3) pure bending about the x-axis, and (4) shear loading. The four load conditons are applied in a single linear step using the *LOAD CASE option. Two models are analyzed: one with linear beam and shell elements and one with quadratic beam and shell elements.

The pipe analyzed with beam and continuum elements has a length of 0.8 m, an outside radius of 0.1 m, and a thickness of 0.04 m. The material has a Young's modulus of 200 GPa and a Poisson's ratio of 0.3. Half of the pipe is modeled with beam elements and the other half is modeled with continuum elements (see Figure 5.1.6–4(b)). The beam node closest to the continuum model is defined as the reference node for the distributing coupling constraint. An element-based surface is defined on the continuum model, which is coupled to the reference node. The coupled model is subjected to four linear loading conditions simulating: (1) twist about the pipe axis, (2) axial stretch along the pipe axis, (3) pure bending about the x-axis, and (4) shear loading. The four load conditons are applied in a single linear step using the *LOAD CASE option. Two models are analyzed: one with linear beam and continuum elements and one with quadratic beam and continuum elements.