General multi-point constraints

You must specify whether the user subroutine will be coded in degree of freedom mode or in nodal mode.

MPC, USER, MODE=DOF
MPC, USER, MODE=NODE

Interaction module: Create Connector Section: select MPC as the Connection Category and User-defined as the MPC Type, choose DOF-by-DOF or Node-by-Node

Interaction module: Create Constraint: MPC Constraint: select User-defined as the MPC Type, choose DOF-by-DOF or Node-by-Node

The Abaqus/Standard shell elements S4R5, S8R5, S9R5, and STRI65 use a penalty method to enforce transverse shear constraints on the edges of the element. The use of mesh refinement MPCs LINEAR and QUADRATIC may, therefore, lead to overconstraining or “shear locking” of the bending behavior. Graded meshes, using the triangular elements as necessary to create a transition zone, are recommended for mesh refinement with these elements.

The shear flexible beam elements in Abaqus/Standard such as B31 or B32 will also “lock” if used as stiffeners along a mesh line where the mesh refinement MPCs are used.

For shell elements in Abaqus/Explicit the rotational degrees of freedom are not constrained by the LINEARMPC; therefore, a hinge is formed along the line defined by the constrained nodes.

MPC type LINEAR is a standard method for mesh refinement of first-order elements. However, in Abaqus/Explicit it might be preferable to use a surface-based tie constraint (see Mesh tie constraints) for mesh refinement, particularly when one or more of the meshes to be constrained involve shell elements with thickness.

This MPC constrains each degree of freedom at node p to be interpolated linearly from the corresponding degrees of freedom at nodes a and b (see Figure 1).

Figure 1. LINEAR type MPC.

MPC
LINEAR, p, a, b

MPC type QUADRATIC is a standard method for mesh refinement of second-order elements. This MPC type is available only in Abaqus/Standard.

This MPC constrains each degree of freedom at node p (where p is either $p_1$ or $p_2$) to be interpolated quadratically from the corresponding degrees of freedom at nodes a, b, and c (Figure 2). For coupled temperature-displacement, coupled thermal-electrical-structural, or pore pressure elements, only the displacement degrees of freedom are constrained.

Figure 2. QUADRATIC type MPC.

MPC
QUADRATIC, p, a, b, c

MPC type BILINEAR is a standard method for mesh refinement of first-order solid elements in three dimensions. This MPC type is available only in Abaqus/Standard.

This MPC constrains each degree of freedom at node p to be interpolated bilinearly from the corresponding degrees of freedom at nodes a, b, c, and d (Figure 3).

Figure 3. BILINEAR type MPC.

MPC
BILINEAR, p, a, b, c, d

MPC type C BIQUAD is a standard method for mesh refinement of second-order solid elements in three dimensions. This MPC type is available only in Abaqus/Standard.

This MPC constrains each degree of freedom at node p to be interpolated by a constrained biquadratic from the corresponding degrees of freedom at the eight nodes a, b, c, d, e, f, g, and h (Figure 4). For coupled temperature-displacement, coupled thermal-electrical-structural, or pore pressure elements, only the displacement degrees of freedom are constrained.

Figure 4. C BIQUAD type MPC.

MPC
C BIQUAD, p, a, b, c, d, e, f, g, h

The P LINEARMPC can be used in conjunction with the QUADRATICMPC for mesh refinement of second-order, fully coupled pore fluid flow-displacement elements.

The T LINEARMPC can be used in conjunction with the QUADRATICMPC for mesh refinement of second-order, fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements.

These MPC types are available only in Abaqus/Standard.

These MPCs constrain the pore pressure (P LINEAR) or temperature (T LINEAR) degree of freedom at node p to be interpolated linearly from the degrees of freedom at nodes a and b (Figure 5).

Figure 5. P LINEAR and T LINEARMPCs.

MPC
P LINEAR, p, a, b

MPC
T LINEAR, p, a, b

The P BILINEARMPC can be used in conjunction with the C BIQUADMPC for mesh refinement of pore fluid flow-displacement elements in three dimensions.

The T BILINEARMPC can be used in conjunction with the C BIQUADMPC for mesh refinement of fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements in three dimensions.

These MPC types are available only in Abaqus/Standard.

These MPCs constrain the pore pressure (P LINEAR) or temperature (T LINEAR) at node p to be interpolated bilinearly from the pore pressure or temperature at nodes a, b, c, and d (Figure 6).

Figure 6. P BILINEAR and T BILINEARMPCs.

MPC
P BILINEAR, p, a, b, c, d

MPC
T BILINEAR, p, a, b, c, d

MPC type BEAM provides a rigid beam between two nodes to constrain the displacement and rotation at the first node to the displacement and rotation at the second node, corresponding to the presence of a rigid beam between the two nodes.

Figure 7. BEAM type MPC.

MPC
BEAM, a, b

Interaction module: Create Connector Section: select MPC as the Connection Category and Beam as the MPC Type

Interaction module: Create Constraint: MPC Constraint; select Beam as the MPC Type

Constraining a beam stiffener to a shell

The general method of using a beam as a stiffener on a shell is to define the beam and shell elements with separate nodes. These nodes can then be constrained to each other using BEAM type MPCs.

A more economical way, when applicable, is to use the same node for the beam node and the shell node and then define the offset of the center of the cross-section of the beam in the beam section data. Figure 8 shows a T-shaped stiffener attached to a shell, using the I-beam cross-section. This is done by setting l (see Beam cross-section library) equal to the distance between the node and the underside of the lower flange and setting the thickness of the top flange to zero. This approach can be used with all beam elements that use TRAPEZOID, I, or ARBITRARY beam sections.

Figure 8. Stiffened shell.

MPC type CYCLSYM is used to enforce proper constraints on the radial faces bounding a segment of a cyclic symmetric structure (see Figure 9). This MPC type is available only in Abaqus/Standard.

MPC type CYCLSYM imposes the cyclic symmetry by equating radial, circumferential, and axial displacement components (and rotations, if active) at the two nodes (a and b). The symmetry axis can be defined by the original coordinates of two additional nodes (c and d) that do not need to be connected to any element in the structure. Scalar degrees of freedom (such as temperature) are made equal.

Figure 9. MPC type CYCLSYM.

MPC
CYCLSYM, a, b, c, d

MPC type ELBOW constrains two nodes of ELBOW31 or ELBOW32 elements together, where the cross-sectional direction, ${\mathbf{a}}_{\mathbf{2}}$, changes (see Pipes and pipebends with deforming cross-sections: elbow elements). This MPC type is available only in Abaqus/Standard.

Figure 10. ELBOW type MPC.

MPC
ELBOW, a, b

Interaction module: Create Connector Section: select MPC as the Connection Category and Elbow as the MPC Type

Interaction module: Create Constraint: MPC Constraint; select Elbow as the MPC Type

MPC type LINK provides a pinned rigid link between two nodes to keep the distance between the nodes constant, as shown in Figure 11. The displacements of the first node are modified to enforce this constraint. The rotations at the nodes, if they exist, are not involved in this constraint.

Figure 11. MPC type LINK.

MPC
LINK, a, b

Interaction module: Create Connector Section: select MPC as the Connection Category and Link as the MPC Type

Interaction module: Create Constraint: MPC Constraint; select Link as the MPC Type

MPC type PIN provides a pinned joint between two nodes. This MPC makes the global displacements equal but leaves the rotations, if they exist, independent of each other, as shown in Figure 12.

Figure 12. MPC type PIN.

MPC
PIN, a, b

Interaction module: Create Connector Section: select MPC as the Connection Category and Pin as the MPC Type

Interaction module: Create Constraint: MPC Constraint; select Pin as the MPC Type

This MPC type is available only in Abaqus/Standard.

A revolute joint is a joint in which relative rotation is allowed between two nodes about an axis that rotates during the motion (see Figure 13). The axis of the joint is defined in the initial configuration as the line from node b to node c. If these nodes are coincident, the axis is assumed to be the global z-axis. The rotation of the joint axis is that of node b.

The relative rotation in the joint is a single variable and is stored as degree of freedom 6 at node c. This degree of freedom can be used with other members in the model, but caution should be used because of the nonstandard use of degree of freedom 6. For example, a SPRING1 element (a spring to ground) might be attached to this degree of freedom. Since the degree of freedom measures a relative rotation, this spring would then be a torsional spring between nodes a and b.

The displacements at node a are not constrained by the REVOLUTEMPC to be the same as the displacements at node b. Thus, the joint definition must usually be completed either by using a PIN type MPC between nodes a and b or by using suitable stiffness members between these two nodes.

An example of a revolute joint and application of the REVOLUTEMPC is provided in Revolute MPC verification: rotation of a crank. See Revolute joint for more details on revolute joints.

Figure 13. Revolute joint.

MPC
REVOLUTE, a, b, c

MPC type SLIDER keeps a node on a straight line defined by two other nodes but allows the possibility of moving along the line and allows the line to change length.

When transitioning from multiple layers of solid elements to shells, it is often desirable to constrain the nodes on the free edge of the solid elements to remain in a straight line. (This constraint is consistent with shell theory.) The SLIDERMPC can perform this function without restraining the “thinning” behavior of the solid layers. The SS LINEARMPC is then used to attach the shell element to this edge.

In Abaqus/Standard when a SLIDERMPC is used with one of the shell-solid MPCs—SS LINEAR, SS BILINEAR, or SSF BILINEAR—it must be given following the shell-solid MPCs.

Input data

For each node p shown in Figure 14 and Figure 15, give the nodes p, a, and b for each line of nodes that should remain straight. For each node q shown in Figure 14, give the nodes q, c, and d, and so on for each line of nodes that should remain straight.

Input File Usage

MPC
SLIDER, p, a, b 
SLIDER, q, c, d

Abaqus/CAE Usage

Slider multi-point constraints are not supported in Abaqus/CAE.

Figure 14. SLIDER type MPC used at a shell-solid intersection.

Figure 15. SLIDER type MPC used to model a telescoping beam.

MPC type TIE makes the global displacements and rotations as well as all other active degrees of freedom equal at two nodes. If there are different degrees of freedom active at the two nodes, only those in common will be constrained.

MPC type TIE is usually used to join two parts of a mesh when corresponding nodes on the two parts are to be fully connected (“zipping up” a mesh). For example, when a mesh is generated on a cylindrical body, the solution at the nodes at 0° and those at 360° must be the same. This can be done either by renumbering the nodes on one of the mesh extremes or by using this MPC for each pair of corresponding nodes, as shown in Figure 16.

Figure 16. Example of use of TIEMPC.

MPC
TIE, a, b

Interaction module: Create Connector Section: select MPC as the Connection Category and Tie as the MPC Type

Interaction module: Create Constraint: MPC Constraint; select Tie as the MPC Type

This MPC type is available only in Abaqus/Standard.

A universal joint is a joint in which relative rotation is allowed between two nodes, about two axes that are connected rigidly, and each of which rotates with the rotation of one end of the joint (see Figure 17). Such a joint might be used to couple two shafts that have an angular misalignment. The first axis of the joint, which is attached to node b, is defined in the initial configuration as the line from node b to node c. If these nodes are coincident, the axis is assumed to be the global z-axis. The second axis of the joint is at right angles to the first axis and is in the plane defined by the first axis and node d.

The relative rotations in the joint are stored as degree of freedom 6 at the nodes c and d. These degrees of freedom can be used with other members in the model, but caution should be used because of the nonstandard use of degree of freedom 6. For example, a SPRING1 element (a spring to ground) might be attached to one of these degrees of freedom. Since the degree of freedom measures a relative rotation, this spring would then be a torsional spring, restraining that component of relative rotation.

The displacements at node a are not constrained by the UNIVERSALMPC to be the same as the displacements at node b. Thus, the joint definition must usually be completed either by using a PIN type MPC between nodes a and b or by using suitable stiffness members between these two nodes.

See Universal joint for more details on universal joints.

Figure 17. Universal joint.

MPC
UNIVERSAL, a, b, c, d

This MPC type is available only in Abaqus/Standard.

As shown in Figure 18, MPC type V LOCAL constrains the velocity components associated with degrees of freedom 1, 2, and 3 at a first node (a) to be equal to the velocity components at a third node (c) along local, rotating directions. These local directions rotate according to the rotation at a second node (b). In the initial configuration the first local direction is from the second to the third node of the MPC (from b to c, as indicated by the arrows in Figure 18), or it is the global z-axis if these nodes coincide. The other local directions are then defined by the standard Abaqus convention for such directions (see Conventions). In Figure 18 this MPC is applied to nodes d, e, and f in the same manner.

MPC type V LOCAL can be useful for defining a complex motion within a model. For example, the MPC can be used to model the steering of an automobile in a dynamic analysis for which the resulting inertial effects are of interest. See Local velocity constraint for more details on the local velocity constraint.

Figure 18. Local velocity constraint.

MPC
V LOCAL, a, b, c 
V LOCAL, d, e, f

The SLIDER, SS LINEAR, SS BILINEAR, and SSF BILINEARMPCs allow for a transition from shell element modeling to solid element modeling on a shell surface. This modeling technique can be used to obtain solutions at shell-solid intersections or other discontinuities, where the local modeling should use full three-dimensional theory but the other parts of the structure can be modeled as shells. The shell-to-solid submodeling capability (About submodeling) and the surface-based shell-to-solid coupling constraint (Shell-to-solid coupling) can also be used to obtain more accurate solutions in such cases, with considerably less modeling effort.

In Abaqus/Standard the MPC usage assumes that the interface between the shell and solid elements is a surface containing the normals to the shell along the line of intersection of the meshes, so that the lines of nodes on the solid mesh side of the interface in the normal direction to the surface are straight lines. (Line a, $p^1$, $p^2$, …, b in Figure 14 and lines $p^1$, $p^2$, …, $p^n$ in Figure 19 to Figure 20 should be straight lines.) It also assumes that the nodes of the solid elements are spaced uniformly on the interface surface as indicated in Figure 14 and Figure 19 to Figure 20. For each shell node on the edge use MPC type SS LINEAR, SS BILINEAR, or SSF BILINEAR, as appropriate, to constrain the shell node to the corresponding line or face of solid element nodes through the thickness. Then, use a SLIDERMPC to constrain each interior node on the line through the thickness to remain on the straight line defined by the bottom and top nodes of that line. For an example, see Multi-point constraints.

The SS BILINEAR and SSF BILINEARMPCs are not intended for use with the variable node solid elements (C3D27, C3D27H, C3D27R, and C3D27RH).

In Abaqus/StandardMPCs SS LINEAR, SS BILINEAR, and SSF BILINEAR eliminate all displacement components and two of the rotation components at the shell node, and the SLIDERMPC eliminates two displacement components at each interior solid element node in the interface. Therefore, any boundary conditions needed at the interface (such as those required when the shell/solid interface intersects a symmetry plane) should be applied only to the top and bottom nodes on the solid element side of the interface.

MPC type SS LINEAR constrains a shell corner node to a line of edge nodes on solid elements for linear elements (S4, S4R, or S4R5; C3D8, C3D8R; SAX1; CAX4; etc.).

The constrained nodes need not lie exactly on these lines, but it is suggested that they be in close proximity to the lines for meaningful results.

Figure 19. SS LINEAR type MPC. 4-node shells to 8-node bricks.

MPC
 SS LINEAR, S, $p^1$, $p^2$, …, $p^n$

MPC
 SS LINEAR, S, $p^1$, $p^n$

MPC type SS BILINEAR constrains a corner node of a quadratic shell element (S8R, S8R5) to a line of edge nodes on 20-node bricks. This MPC type is available only in Abaqus/Standard.

The constrained node need not lie exactly on the line, but it is suggested that it be in close proximity to the line for meaningful results.

Figure 20. SS BILINEAR type MPC. Corner of 8-node shell to edge of 20-node bricks.

MPC
SS BILINEAR, S, $p^1$, $p^2$, …, $p^n$

MPC type SSF BILINEAR constrains a midside node on a quadratic shell element (S8R, S8R5) to a line of midface nodes on solid 20-node bricks. This MPC type is available only in Abaqus/Standard.

The constrained node need not lie exactly on the line, but it is suggested that it be in close proximity to the line for meaningful results.

Figure 21. SSF BILINEAR type MPC. Midside of 8-node shell to surface of 20-node bricks.

MPC
SSF BILINEAR, S, $p^1$, $p^2$, …, $p^n$