Various types of multi-point constraints are tested. Simple geometries are
given displacements or loads that result in easily checked responses. These
responses confirm the proper functioning of the
MPCs being tested. Unless noted otherwise, the
static procedure is tested. All explicit dynamic tests have been performed so
that a quasi-static solution is obtained.
LINEARMPC
The LINEARMPC is tested in
Abaqus/Standard
and
Abaqus/Explicit.
A cantilevered bar is subjected to a uniform tensile loading on the free end.
Abaqus/Standard
analysis
Elements tested
C3D8
CPS4
Problem description
Model:
Two models (one consisting of CPS4 elements and the other consisting of C3D8 elements) were created within one input file.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio =
0.3.
Boundary conditions:
=0
at x=0, =0
at y=0, and =0
at z=0 for three-dimensional models.
Loading:
Step 1: A uniform pressure of 10000 in the
y-direction is applied to the top surface.
Step 2: The load that was applied in the first step is applied again,
this time using NLGEOM for large-displacement analysis.
Results and discussion
The results obtained agree with the analytical solution.
All displacement degrees of freedom are restrained throughout the analysis.
In Step 1 the pore pressure is set to zero at nodes 1 and 5. In Step 2 the pore
pressure is set to zero at nodes 5, 15, and 25.
Loading:
Step 1: A pore fluid velocity is specified along the top of the model.
Step 2: A pore fluid velocity is specified along the left edge of the
model.
Results and discussion
The results obtained agree with the analytical solution.
All displacement degrees of freedom are restrained throughout the analysis.
In Step 1 the temperature is set to zero at nodes 5, 15, and 25. In Step 2 the
temperature is set to zero at nodes 1 and 5.
Loading:
Step 1: A film coefficient and sink temperature are specified along the
left edge of the model.
Step 2: An emissivity and sink temperature are specified along the top
edge of the model.
Results and discussion
The results obtained agree with the analytical solution.
All displacement degrees of freedom are restrained throughout the analysis.
In Step 1 the pore pressure is set to zero on the front face of the model. In
Step 2 the pore pressure is set to zero on the right face of the model.
Loading:
Step 1: A pore fluid velocity is specified out of the back face of the
model.
Step 2: A pore fluid velocity is specified out of the left face of the
model.
Results and discussion
The results obtained agree with the analytical solution.
All displacement degrees of freedom are restrained throughout the analysis.
In Step 1 the temperature is set to zero on the left face of the model. In Step
2 the temperature is set to zero on the front face of the model.
Loading:
Step 1: An emissivity and sink temperature are given on the left face of
the model.
Step 2: A surface flux is specified on the back face of the model.
Results and discussion
The results obtained agree with the analytical solution.
The BEAMMPC is tested in
Abaqus/Standard
and
Abaqus/Explicit.
A cantilevered beam is subjected to a transverse tip load.
Abaqus/Standard
analysis
Elements tested
B22
B32
Problem description
Two-dimensional and three-dimensional beams are considered, with and without
the RIKS procedure (introduces a slight imperfection corresponding to
the first buckling mode).
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 1700.
Boundary conditions:
Node 1 is clamped.
Loading 1
Step 1: =−1000
at node 3.
Step 2: The first four buckling modes are extracted for a live load of
=−1000.
Step 3: The load that was applied in the first step is applied again,
this time using NLGEOM for large-displacement analysis.
Loading 2
Step 1: The first four buckling modes are extracted for a live load of
=−1.
Step 2: A RIKS procedure is adopted until a maximum load of
=−300
at node 6.
Results and discussion
The results agree with the theoretically expected results. The results of
the buckling analyses and the geometrically nonlinear analyses show that the
initial stress terms are accounted for correctly.
Nodes 2 and 3 are included in a rigid body tie-type node set.
Nodes 2 and 3 are connected by a beam element of type B31. This element is then included in a rigid body.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 0.03.
Boundary conditions:
Node 1 is clamped.
Loading:
=−1000
at node 3.
Beam section data
B31, 1 × 1 rectangle. PIPE31, pipe of radius 1 and thickness 0.1.
Results and discussion
To verify that the MPC is working
correctly, the rotation at node 3 should be the same as the rotation at node 2;
the vertical displacement at node 3 should be given by
.
This solution is obtained. The results for Cases 2 and 3 match the results for
Case 1.
The ELBOWMPC is tested in both static and
dynamic analyses in
Abaqus/Standard.
Four cases are tested with each element type in the static analyses (see
Figure 1).
Figure 1. ELBOWMPC geometry.
In addition to the differences shown in the figure, there are the following
differences:
Case 1: Control model. No ELBOWMPC. Otherwise the same as Case 4.
Case 2: 16 integration points around the pipe; 3 section points through
the thickness; 5 Fourier ovalization modes.
Case 3: 12 integration points around the pipe; 5 section points through
the thickness; 4 Fourier ovalization modes.
Case 4: 20 integration points around the pipe; 5 section points through
the thickness; 6 Fourier ovalization modes.
The following data apply to the four cases in each file:
Boundary conditions:
Node 1 has degrees of freedom 1–6 fixed. All nodes have
NODEFORM condition.
Loading:
Step 1: =1
× 106 at node 4.
Step 2: =2
× 106 at node 4.
Step 3: The load that was applied in the first step is applied again,
this time using NLGEOM for large-displacement analysis.
Step 4: The load that was applied in the second step is applied again,
this time using NLGEOM for large-displacement analysis.
General:
Two straight pipes, each discretized with two elements,
are considered in the dynamic analysis. In the first case the second
cross-sectional directions of both elements are identical and the ELBOWMPC is not used. In the second case
the second cross-sectional directions are different and the ELBOWMPC is used to ensure continuity of
displacements. The analysis consists of two steps. In the static step the pipes
are subjected to bending by applying a concentrated force. In the
direct-integration implicit dynamic step the force is removed and the pipes
vibrate freely.
Results and discussion
For the static analyses Cases 2–4 give the same answer as Case 1;
at points A and B match. In the dynamic case the results for both pipes (with
and without the ELBOWMPC) are identical.
The LINKMPC is tested in
Abaqus/Standard
and
Abaqus/Explicit.
Two cantilevered beams are subjected to transverse loading.
Abaqus/Standard
analyses
Elements tested
B23
B33
Problem description
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 7800.0.
Boundary conditions:
Nodes 1 and 6 are clamped.
Loading:
Step 1: The first four natural frequencies are extracted.
Step 2: =−250
at node 2, =250
at node 5.
Step 3: The loads that were applied in the previous step are applied
again, this time using NLGEOM for large-displacement analysis.
Results and discussion
The LINKMPC provides a pinned, rigid link
between two nodes. For this example this means that the translational degrees
of freedom should have equal magnitudes but opposite sense and the rotational
degree of freedom should be the same for the nodes that are joined by the
MPC. This solution is obtained.
Nodes 3 and 4 are included in a rigid body pin-type node set.
Nodes 3 and 4 are connected by a truss element of type T3D2. This element is then included in a rigid body.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 0.03.
Boundary conditions:
Nodes 1 and 6 are clamped.
Loading:
=−250
at node 2, =250
at node 5.
Beam section data
B31, 1 × 1 rectangle. PIPE31, pipe of radius 1 and thickness 0.1.
Results and discussion
The LINKMPC provides a pinned, rigid link
between two nodes. For this example this means that the translational degrees
of freedom should have equal magnitudes but opposite sense and the rotational
degree of freedom should be the same for the nodes that are joined by the
MPC. This solution is obtained. The results
for Cases 2 and 3 match the results for Case 1.
The PINMPC is tested in
Abaqus/Standard
and
Abaqus/Explicit.
A beam structure that is cantilevered at both ends has a pressure loading
applied to one-half of the model.
Abaqus/Standard
analysis
Elements tested
B23
Problem description
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0.
Boundary conditions:
Nodes 1 and 4 are clamped.
Loading:
Step 1: The left half of the beam is loaded by a force per unit length, PY=−1000.
Step 2: The load that was applied in the first step is applied again,
this time using NLGEOM for large-displacement analysis.
Beam section data
B23, 1 × 1 rectangle.
Results and discussion
The PINMPC provides a pinned joint between
two nodes by making the translational degrees of freedom equal. The
displacements of nodes 2 and 3 are identical.
Nodes 2 and 3 are included in a rigid body pin-type node set.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 0.03.
Boundary conditions:
Nodes 1 and 4 are clamped.
Loading:
The left half of the beam is loaded by a force per unit length,
PY=−1000.
Beam section data
B21, 1 × 1 rectangle.
PIPE21, pipe of radius 1 and thickness 0.1.
Results and discussion
The PINMPC provides a pinned joint between
two nodes by making the translational degrees of freedom equal. The
displacements of nodes 2 and 3 are identical. The results for Case 2 match the
results for Case 1.
All degrees of freedom are restrained at node 10 throughout the analysis.
Nodes 5 and 6 are initially constrained in degree of freedom 6.
Loading:
Step 1: A concentrated follower force is applied at node 20 to pull the
joint.
Step 2: The joint is rotated by 45° about the 3–4 joint axis by
prescribing degree of freedom 6 at node 4.
Step 3: The joint is rotated by 45° about the current 3–5 axis by
prescribing degree of freedom 6 at node 5.
Results and discussion
The axial follower force of Step 1 couples with the rotations in subsequent steps to cause a
lateral deflection of node 1 despite a very high material modulus.
The SLIDERMPC is tested in
Abaqus/Standard
for a truss and a beam structure and in
Abaqus/Explicit
for a truss structure.
Abaqus/Standard
truss analyses
Elements tested
T2D2
Problem description
A truss structure has a SLIDERMPC connecting node 2 to nodes 1 and
3.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0.
Boundary conditions:
==0
at node 1, =0
at node 3.
Load case 1
Step 1: =−500
at node 2, =−1000
at node 2.
Step 2: The loads that were applied in the first step are applied again,
this time using NLGEOM for large-displacement analysis.
Load case 2
=−500
at node 2, =−1000
at node 2. A static Riks step is adopted.
Truss section data
T2D2, cross-sectional area = 1.
Results and discussion
The SLIDERMPC keeps a node on a straight line
between two nodes but allows it to slide along the line and the line to change
length. This solution is obtained. The geometrically nonlinear analyses show
that the initial stress terms are accounted for correctly.
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0.
Boundary conditions:
====0
at node 4. All displacements and rotations are fixed at node 1. A
transformation at node 1 places the local x-axis along the
direction from node 1 to node 3.
Loading:
Step 1: =10
at node 3. Node 1 is rotated about the transformed z-axis.
(=0.3.)
Step 2: The load and displacement that were applied in the first step
are applied again, this time using NLGEOM for large-displacement analysis.
Beam section data
B31, cross-sectional area = 1.
Results and discussion
The SLIDERMPC keeps a node on a straight line
between two nodes but allows it to slide along the line and the line to change
length. This solution is obtained. The geometrically nonlinear analyses show
that the initial stress terms are accounted for correctly.
A truss structure has a SLIDERMPC connecting node 2 to nodes 1 and
3.
Material:
Linear elastic, Young's modulus = 3.0 × 106, Poisson's ratio = 0,
density = 0.03.
Boundary conditions:
==0
at node 1, =0
at node 3.
Loading:
=−500
at node 2, =−1000
at node 2.
Truss section data
T2D2, cross-sectional area = 1.
Results and discussion
The SLIDERMPC keeps a node on a straight line
between two nodes but allows it to slide along the line and the line to change
length. This solution is obtained.
All degrees of freedom are restrained at node 10 throughout the analysis.
Nodes 3 and 4 are initially constrained in degree of freedom 6.
Loading:
Step 1: A concentrated follower force is applied at node 20 to pull the
joint.
Step 2: The joint is rotated by 45° about the 1–3 joint axis by
prescribing degree of freedom 6 at node 3.
Step 3: The joint is rotated by 45° about the current 1–4 axis by
prescribing degree of freedom 6 at node 4.
Results and discussion
The axial follower force of Step 1 couples with the rotations in subsequent steps to cause
lateral deflection of node 1 despite a very high material modulus.
The SS LINEAR and SLIDERMPCs are tested in
Abaqus/Standard
and
Abaqus/Explicit.
A cantilever beam consisting of solid and shell elements connected by SS LINEAR and SLIDERMPCs is subjected to a transverse
tip loading.
Initial
Abaqus/Standard
analysis
Elements tested
C3D8
S4R
Problem description
Loading:
Step 1: =−15
at nodes 105 and 125, =−30
at node 115.
Step 2: The loads that were applied in the first step are applied again,
this time using NLGEOM for large-displacement analysis.
Step 3: The loads that were applied in the second step are removed.
Step 4: The boundary conditions are changed, and a rotation of
around the z-axis is prescribed at
x=0.
Initial boundary conditions
===0
at x=0, ===0
at z=0 (except at nodes 19 and 121).
Boundary conditions in Step 4
===0
and
prescribed at x=10.
Results and discussion
The SLIDERMPC is used to keep a node on a
straight line between two nodes, but it allows the node to slide along the line
and the line to change length. This enforces the assumption that plane sections
remain plane. The SS LINEARMPC constrains a shell node to a
line of solid element nodes. This ties the translation and rotation of the
shell node to the displacement and rotation of the solid nodes. Continuity of
displacements and rotations is achieved at the shell-solid boundary.
Note:
The poor performance of the first-order brick element, C3D8, in bending is demonstrated by an excessively stiff response in
Step 1 and Step 2.
===0
at x=0, ===0
at z=0 (except at nodes 19 and 121).
Loading:
=−15
at nodes 105 and 125, =−30
at node 115. A static Riks step is adopted.
Results and discussion
The SLIDERMPC is used to keep a node on a
straight line between two nodes, but it allows the node to slide along the line
and the line to change length. This enforces the assumption that plane sections
remain plane. The SS LINEARMPC constrains a shell node to a
line of solid element nodes. This ties the translation and rotation of the
shell node to the displacement and rotation of the solid nodes. Continuity of
displacements and rotations is achieved at the shell-solid boundary.
SS LINEAR and SLIDERMPCs with RIKS and transforms.
Dynamic
Abaqus/Standard
analysis
Elements tested
C3D8
S4R
Problem description
Boundary conditions:
The edge at x=10 is fixed.
Loading:
Step 1: The first four natural frequencies are extracted.
Step 2: =−30
at all nodes along x=0. A large-displacement analysis is
performed.
Step 3: The load applied in Step 2 is removed. A dynamic analysis is
performed.
Results and discussion
The SLIDERMPC is used to keep a node on a
straight line between two nodes, but it allows the node to slide along the line
and the line to change length. This enforces the assumption that plane sections
remain plane. The SS LINEARMPC constrains a shell node to a
line of solid element nodes. This ties the translation and rotation of the
shell node to the displacement and rotation of the solid nodes. Continuity of
displacements and rotations is achieved at the shell-solid boundary.
SS LINEAR and SLIDERMPCs with
DYNAMIC and transforms.
Abaqus/Explicit
analysis
Elements tested
C3D8R
S4R
Problem description
Material:
Linear elastic, Young's modulus = 30.0 × 106, Poisson's ratio =
0.3, density = 0.3.
Boundary conditions:
0 at
0,
0 at
0.
Loading:
−15 at nodes 105 and 125,
−30 at node 115.
Results and discussion
The SLIDERMPC is used to keep a node on a
straight line between two nodes, but it allows the node to slide along the line
and the line to change length. This enforces the assumption that plane sections
remain plane. The SS LINEARMPC constrains a shell node to a
line of solid element nodes. This ties the translation and rotation of the
shell node to the displacement and rotation of the solid nodes. Continuity of
displacements and rotations is achieved at the shell-solid boundary.
SS LINEAR, SSF BILINEAR, and SLIDERMPCs with
DYNAMIC.
TIEMPC
The TIEMPC is tested in
Abaqus/Standard
and
Abaqus/Explicit.
A cantilevered beam is subjected to a transverse tip load.
Initial
Abaqus/Standard
analysis
Elements tested
B22
Problem description
Material:
Linear elastic, Young's modulus = 28.1 × 106, Poisson's ratio =
0.3, density = 1700.
Boundary conditions:
Nodes 1 and 11 are clamped.
Loading:
Step 1: =−300
at nodes 6 and 15. A linear perturbation analysis is performed.
Step 2: The natural frequencies and mode shapes for the continuous
cantilever beam are extracted.
Step 3: The natural frequencies and modes shapes are extracted for the
cantilever beam that uses MPCTIE.
Step 4: The loads that were applied in the first step are applied again,
this time using NLGEOM for large-displacement analysis.
Results and discussion
MPCTIE makes all active degrees of freedom equal between two nodes (both
translational and rotational degrees of freedom). The results of a cantilever
beam that uses MPCTIE are the same as those of a continuous cantilever beam under the same
loading.
A cantilever beam with MPC type TIE, subject to a slight imperfection corresponding to the first buckling
mode.
Material:
Linear elastic, Young's modulus = 28.1 × 106, Poisson's ratio =
0.3, density = 1700.
Boundary conditions:
Node 1 is clamped.
Loading:
Step 1: The first four buckling modes are extracted for a perturbation
load =−300
at node 6.
Step 2: A RIKS analysis (with NLGEOM) is conducted until a maximum load of =−600
at node 6.
Results and discussion
MPCTIE makes all active degrees of freedom equal between two nodes (both
translational and rotational degrees of freedom). The results of a cantilever
beam that uses MPCTIE are the same as those of a continuous cantilever beam under the same
loading.
Nodes 3 and 4 are included in a rigid body tie-type node set.
The results from the above two cases are compared to the solution of a
continuous cantilever beam under the same transverse tip loading.
Material:
Linear elastic, Young's modulus = 28.1 × 106, Poisson's ratio =
0.3, density = 0.3.
Boundary conditions:
Nodes 1 and 11 are clamped.
Loading:
−300 at nodes 6 and 15.
Beam section data
B21, 0.5 × 0.5 rectangle.
PIPE21, pipe with radius 0.5 and thickness 0.05.
Results and discussion
MPCTIE makes all active degrees of freedom equal between two nodes (both
translational and rotational degrees of freedom). The results of a cantilever
beam that uses MPCTIE are the same as those of a continuous cantilever beam under the same
loading. The results from Case 2 match the results from Case 1.
The CYCLSYMMPC is tested in
Abaqus/Standard.
A disk is subjected to cyclic symmetric force loading in the first analysis; in
the second analysis the disk is subjected to both cyclic symmetric force
loading and cyclic temperature boundary conditions. The problem is modeled
using a quarter of the disk with the appropriate CYCLSYMMPC.
Boundary conditions:
Nodes 6 and 11 are clamped. The reference node for the CPEG4T model is also clamped. Node 1 also has all displacement and
rotation degrees of freedom restrained because of the CYCLSYMMPC. Nodes 6, 11, and 1 have their
temperatures set to zero for the second analysis.
Loading:
=100
at node 106. For the second analysis the temperature of nodes 101 and 111 is
set to 100, and the temperature of node 106 is set to 200.
The first analysis uses the direct-integration implicit dynamic procedure;
the second analysis uses the fully coupled thermal-stress steady-state
procedure.
Results and discussion
The results obtained from the quarter disk model that uses
MPC type CYCLSYM are the same as the results obtained from an analysis of a complete
disk under cyclic symmetric loading and subjected to cyclic temperature
boundary conditions.
Internal MPC types
BEAMRIGID and
BEAMTIE with transforms
These files test the use of the internally generated
MPCs (MPC
types BEAMRIGID and
BEAMTIE) with transforms in
Abaqus/Standard.
Transformations are applied to the reference node as well as to the nodes of
the rigid element (or rigid beam). The boundary conditions and loadings,
mentioned below, are given in the local transformed system.
Rigid elements
Elements tested
R2D2
R3D4
Problem description
Boundary conditions:
=0
and =1.5
at node 5.
Loading:
Step 1: =10.0
at node 3.
Step 2: Same as above, but a large-displacement analysis is performed.
Results and discussion
The results agree with the theoretically expected results. The results of
the geometrically nonlinear analyses show that the initial stress terms are
accounted for correctly.
=1.5
at node 5. All other displacements are fixed.
Loading:
Step 1: =10.0
at node 1.
Step 2: Same as above, but a large-displacement analysis is performed.
Results and discussion
The results agree with the theoretically expected results. The results of
the geometrically nonlinear analyses show that the initial stress terms are
accounted for correctly.
