김경종
21 KiB
Note: Equation constraints cannot be defined at the part (or part instance) level in Abaqus/CAE.
Prescribing a nonhomogeneous constraint
It is sometimes necessary to impose a constraint in the form
A _ {1} u _ {i} ^ {P} + A _ {2} u _ {j} ^ {Q} + \dots + A _ {N} u _ {k} ^ {R} = \hat {u},
where { \hat { u } } ( t ) is a prescribed value that may vary with time, t. This is easily done by rewriting the equation as
A _ {1} u _ {i} ^ {P} + A _ {2} u _ {j} ^ {Q} + \dots + A _ {N} u _ {k} ^ {R} - \hat {u} _ {m} ^ {Z} = 0
and introducing a node, Z, that is not attached to any element in the model. Choosing \hat { u } _ { m } ^ { Z } to be some convenient degree of freedom m at node Z allows the prescribed value { \hat { u } } ( t ) to be imposed through a boundary condition specification. If necessary, an amplitude reference can be provided to give the variation with time (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1); such an amplitude reference is required in Abaqus/Explicit for prescribed displacements.
For example, assume that node 1000 in the example above is a “dummy” node that appears only in this equation and is not attached to any other part of the model. Defining a boundary condition to constrain degree of freedom 3 at node 1000 to −12.5 would impose the constraint
u _ {3} ^ {5} - u _ {1} ^ {6} = 1 2. 5.
Constraint forces and global equilibrium
Linear constraint equations introduce constraint forces at all degrees of freedom appearing in the equations. These forces are considered external, but they are not included in reaction force output. Therefore, the totals provided at the end of the reaction force output tables may reflect an incomplete measure of global equilibrium.
To illustrate this behavior, consider a spring-supported beam subjected to a concentrated load as shown in Figure 35.2.1–1. The static reaction forces are R _ { y } ^ { C } = - 3 and R _ { \prime \prime } ^ { D } = - 6 . In Figure 35.2.1–2 the same structure is subjected to the additional linear constraint equation u _ { y } ^ { \check { A } } - u _ { y } ^ { B } = 0 , which constrains the beam to remain horizontal. This introduces constraint forces F _ { y } ^ { A } = \mathrm { { 1 . 5 } } and F _ { y } ^ { B } = - 1 . 5 . , and the new reaction forces are R _ { y } ^ { C } = R _ { y } ^ { D } = - 4 . 5 . These reaction forces produce a global force balance in the Y-direction, but since the constraint forces are not included in reaction force output, the global moment balance about point A cannot be verified.
text_image
P_y = 9 A 2 1 B C D R_y^C = -3 R_y^D = -6 y x
Figure 35.2.1–1 Beam with no linear constraints.
text_image
Fy^A = 1.5 Py = 9 Fy^B = -1.5 A 2 1 B C D Ry^C = -4.5 Ry^D = -4.5 y x
Figure 35.2.1–2 Beam with linear constraint u _ { y } ^ { A } - u _ { y } ^ { B } = 0
Constraint force s F _ { y } ^ { A } and F _ { y } ^ { B } are not included in reaction force output.
The global force balance can also be incomplete. This is demonstrated in Figure 35.2.1–3, where a pulley connection between nodes A and B is represented by the linear constraint equation u _ { y } ^ { A } - u _ { x } ^ { B } = 0 . The constraint forces at the pulley, F _ { x } and F _ { y } , are not included in the reaction force output, producing incomplete global force balances in both the X- and Y-directions.
text_image
P_y = 9 y A F_x = -9 F_y = -9 B C R_x^C = 9 x
Figure 35.2.1–3 Pulley connection represented by the linear constraint u _ { y } ^ { A } - u _ { x } ^ { B } = 0 . Constraint forces F _ { x } and F _ { y } are not included in reaction force output.
Obtaining the constraint force
The linear constraint generates constraint forces at all the degrees of freedom involved in the equation. For a given constraint equation these forces are proportional to their respective coefficients. To find the constraint forces, introduce a node Z that is not attached to any element in the model; rewrite the constraint equation as
A _ {1} u _ {i} ^ {P} + A _ {2} u _ {j} ^ {Q} + \dots + A _ {N} u _ {k} ^ {R} - A _ {1} \hat {u} _ {m} ^ {Z} = 0;
and specify a zero displacement boundary condition at degree of freedom m of node Z. The reaction force obtained at node Z will be equal to the constraint force acting at node P in degree of freedom i. The constraint force in any term with coefficient A _ { K } in the constraint equation is obtained by multiplying the constraint force at node P in degree of freedom i with the ratio A _ { K } / A _ { 1 } . For example, if the equation is
u _ {3} ^ {5} - u _ {3} ^ {6} = 0
and the forces in the constraint are needed, the equation can be rewritten as
u _ {3} ^ {5} - u _ {3} ^ {6} - u _ {3} ^ {1 0 0 0} = 0,
where node 1000 is the fixed “dummy” node. Since the coefficient of u _ { 3 } ^ { 5 } is the opposite of the coefficient of u _ { 3 } ^ { 1 0 0 0 } , the constraint force at node 5 is the same as the reaction force at node 1000. Since the coefficient of u _ { 3 } ^ { 6 } is the same as the coefficient of u _ { 3 } ^ { 1 0 0 0 } , the constraint force at node 6 is the opposite of the reaction force at node 1000.
Defining a constraint in a deformed state
Sometimes we may wish to impose an equation starting at a certain point in the analysis:
A _ {1} \Delta u _ {i} ^ {P} + A _ {2} \Delta u _ {j} ^ {Q} + \ldots + A _ {N} \Delta u _ {k} ^ {R} = 0,
where \Delta u represents the change in displacement after time t _ { 0 } . The equation can be rewritten as
A _ {1} u _ {i} ^ {P} + A _ {2} u _ {j} ^ {Q} + \ldots + A _ {N} u _ {k} ^ {R} - \hat {u} _ {m} ^ {Z} = 0,
where, again, node Z is not attached to any element in the model. Prior to time t _ { 0 } (which is assumed to be at the end of a step), degree of freedom m of node Z is left unrestrained. After time t _ { 0 } further changes in \hat { u } _ { m } ^ { Z } are restrained in Abaqus/Standard by applying a boundary condition fixing the degree of freedom at its current values at the start of the step.
Reading the data from an alternate input file
The input for a linear constraint equation can be contained in a separate input file.
Input File Usage: *EQUATION, INPUT=file_name
If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line.
Abaqus/CAE Usage: Interaction module: Create Constraint: Equation: click mouse button 3 while holding the cursor over the data table, and select Read from File
35.2.2 GENERAL MULTI-POINT CONSTRAINTS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Kinematic constraints: overview,” Section 35.1.1
• *MPC
• “Defining MPC constraints,” Section 15.15.6 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• Chapter 24, “Connectors,” of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
Multi-point constraints (MPCs):
• allow constraints to be imposed between different degrees of freedom of the model; and
• can be quite general (nonlinear and nonhomogeneous).
The most commonly required constraints are available directly by choosing an MPC type and giving the associated data. The available MPC types are described below; MPCs that are available only in Abaqus/Standard are designated with an (S) .
In Abaqus/Standard the constraints can also be given by user subroutine MPC.
Linear constraints can be given directly by defining a linear constraint equation (see “Linear constraint equations,” Section 35.2.1).
In Abaqus/Explicit some multi-point constraints can be modeled more effectively using rigid bodies (see “Rigid body definition,” Section 2.4.1).
Several MPC types are also available with connector elements (“Connector elements,” Section 31.1.2). Although the connector elements impose the same kinematic constraint, connectors do not eliminate degrees of freedom.
MPC constraint forces are not available as output quantities. Therefore, to output the forces required to enforce the constraint specified in an MPC, you should use an equivalent connector element. Connector element force, moment, and kinematic output is readily available and is defined in “Connector element library,” Section 31.1.4.
Identifying the nodes involved in the MPC
For any MPC type, either node sets or individual nodes can be given as input. If the first entry is a node, subsequent entries must be nodes. If the first entry is a node set, subsequent entries can be either node sets or single nodes. The latter option is useful if a degree of freedom at each of a set of nodes depends on a degree of freedom of a single node, such as may occur in certain symmetry conditions or in the simulation of a rigid body.
If node sets are used, corresponding set entries will be constrained to each other. If sorted node sets are given as input, you must ensure that the nodes are numbered such that they will match up correctly when sorted. The nodes in an unsorted node set (see “Node definition,” Section 2.1.1) will be used in the order that they are given in defining the set.
In Abaqus/Standard multi-point constraints cannot be used to connect two rigid bodies at nodes other than the reference nodes, since multi-point constraints use degree-of-freedom elimination and the other nodes on a rigid body do not have independent degrees of freedom. In Abaqus/Explicit a rigid body reference node or any other node on a rigid body can be used in a multi-point constraint definition.
Abaqus/CAE uses connectors to define multi-point constraints between two points and constraints to define multi-point constraints between a point and slave nodes in a region. Set-to-set multi-point constraints and unsorted node sets are not supported in Abaqus/CAE.
Input File Usage: *MPC
Abaqus/CAE Usage: Use the following options to define a multi-point constraint between two points:
Interaction module:
Connector→Geometry→Create Wire Feature
Connector→Section→Create: Connection Category: MPC,
MPC type: select type
Connector→Assignment→Create: select wires: Section:
select MPC connector section
Use the following options to define a multi-point constraint between a point and slave nodes in a region:
Interaction module:
Constraint→Create: MPC Constraint: select control point
and region; MPC type: select type
Use with transformed coordinate systems
Local coordinate systems (see “Transformed coordinate systems,” Section 2.1.5) can be defined for any nodes connected to MPCs. Some special considerations apply for user-defined MPCs, as described in “MPC,” Section 1.1.14 of the Abaqus User Subroutines Reference Guide.
Defining multiple multi-point constraints at a point
See “Kinematic constraints: overview,” Section 35.1.1, for details on how multiple kinematic constraints at a point are treated in Abaqus/Standard and Abaqus/Explicit.
In Abaqus/Standard MPCs are usually imposed by eliminating the degree of freedom at the first node given (the dependent degree of freedom). MPC types BEAM, CYCLSYM, LINK, PIN, REVOLUTE, TIE, and UNIVERSAL are sorted internally by Abaqus/Standard so that the MPC in which a node is used as a dependent node is the last MPC that uses this node. Therefore, groups of these MPCs can be given in any order. However, even for these MPCs, a node can be used only once as a dependent node. In other cases dependent degrees of freedom should not be used subsequently to impose kinematic constraints; this generally precludes the use of the first node in an MPC definition as an independent node in any
subsequent multi-point constraint, equation constraint, kinematic coupling constraint, or tie constraint definition.
Using MPCs in implicit dynamic analysis
In implicit dynamic analysis Abaqus/Standard enforces MPCs rigorously for the displacements. The velocities and accelerations are derived from the displacements with the relations defined by the dynamic integration operator (see “Implicit dynamic analysis,” Section 2.4.1 of the Abaqus Theory Guide). For linear MPCs (such as PIN, TIE, and mesh refinement MPCs) and geometrically linear analysis the velocities obtained in this way satisfy the constraint exactly. However, the accelerations satisfy the constraint only approximately. If nonlinear MPCs (such as BEAM, LINK, and SLIDER) are used in geometrically nonlinear analysis, both the velocities and accelerations satisfy the constraint only approximately. In most cases the approximation is quite accurate, but in some cases high frequency oscillations may occur in the accelerations of the nodes involved in the MPC.
Using nonlinear MPCs in geometrically linear Abaqus/Standard analysis
If a nonlinear MPC is used in a geometrically linear Abaqus/Standard analysis (see “General and linear perturbation procedures,” Section 6.1.3), the MPC is linearized. For example, if MPC LINK is used in a geometrically nonlinear Abaqus/Standard analysis, the distance between the two nodes of the link remains constant. If it is used in a geometrically linear Abaqus/Standard 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.
Defining MPCs in a user subroutine
In Abaqus/Standard you can define multi-point constraints in user subroutine MPC.
Constraints defined in user subroutine MPC can only use degrees of freedom that also exist on an element somewhere in the same model. For example, if a model contains no elements with rotational degrees of freedom, user subroutine MPC cannot use degrees of freedom 4, 5, or 6. This limitation can be overcome by adding a suitable element somewhere in the model to introduce the required degrees of freedom. This element can be added so that it does not affect the response of the model.
Constraints defined in the user subroutine are applied to the transformed degrees of freedom. A boundary nonlinearity occurs in Abaqus/Standard when MPCs are activated/deactivated in a user subroutine.
Input File Usage: *MPC, USER
Abaqus/CAE Usage: Use one of the following options:
Interaction module: Create Connector Section: select MPC as the Connection Category and User-defined as the MPC Type
Interaction module: Create Constraint: MPC Constraint; select User-defined as the MPC Type
Specifying the version of user subroutine MPC
You must specify whether the user subroutine will be coded in degree of freedom mode or in nodal mode.
Input File Usage: Use one of the following options:
*MPC, USER, MODE=DOF
*MPC, USER, MODE=NODE
Abaqus/CAE Usage: Use one of the following options:
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
Reading the data from an alternate input file
The input for an MPC definition can be contained in a separate input file.
Input File Usage: *MPC, INPUT=file_name
If the INPUT parameter is omitted, it is assumed that the data lines follow the keyword line.
Abaqus/CAE Usage: Reading data from an alternate input file is not supported in Abaqus/CAE.
MPCs for mesh refinement
| LINEAR | This MPC is a standard method for mesh refinement of first-order elements. It applies to all active degrees of freedom at the involved nodes including temperature, pressure, and electrical potential.In Abaqus/Explicit it might be preferable to use a surface-based tie constraint (see “Mesh tie constraints,” Section 35.3.1) for mesh refinement, particularly when one or more of the meshes to be constrained involve shell elements with thickness. |
| QUADRATIC(S) | This MPC is a standard method for mesh refinement of second-order elements. It applies to all active degrees of freedom at the involved nodes with the exception of temperature degrees of freedom in coupled temperature-displacement analysis and coupled thermal-electrical-structural analysis and to pressure degrees of freedom in coupled pore pressure analysis. For refinement using second-order pore pressure or coupled-temperature displacement elements, the P LINEAR or T LINEAR MPC must be used in conjunction with this MPC. |
| BILINEAR(S) | This MPC is a standard method for mesh refinement of first-order solid elements in three dimensions. It applies to all active degrees of freedom at the involved nodes including temperature, pressure, and electrical potential. |
| C BIQUAD(S) | This MPC is a standard method for mesh refinement of second-order solid elements in three dimensions. It applies to all active degrees of freedom at the |
| involved nodes with the exception of temperature degrees of freedom in coupled temperature-displacement analysis and coupled thermal-electrical-structural analysis and to pressure degrees of freedom in coupled pore pressure analysis. For refinement using pore pressure or coupled-temperature displacement elements in three dimensions, the P BILINEAR or T BILINEAR MPC must be used in conjunction with this MPC. | |
| P LINEAR(S) | This MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled pore fluid flow-displacement elements. It applies to pressure degrees of freedom only. For acoustic analysis it applies the same constraint as the LINEAR MPC. |
| T LINEAR(S) | This MPC can be used in conjunction with the QUADRATIC MPC for mesh refinement of second-order, fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements. It applies to temperature degrees of freedom only. For heat transfer analysis it applies the same constraint as the LINEAR MPC. |
| P BILINEAR(S) | This MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of pore fluid flow-displacement elements in three dimensions. It applies to pressure degrees of freedom only. For acoustic analysis it applies the same constraint as the BILINEAR MPC. |
| T BILINEAR(S) | This MPC can be used in conjunction with the C BIQUAD MPC for mesh refinement of fully coupled temperature-displacement and fully coupled thermal-electrical-structural elements in three dimensions. It applies to temperature degrees of freedom only. For heat transfer analysis it applies the same constraint as the BILINEAR MPC. |
Using mesh refinement MPCs with shell or beam elements
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 LINEAR MPC; therefore, a hinge is formed along the line defined by the constrained nodes.
Using MPC type LINEAR
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,” Section 35.3.1) 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 35.2.2–1).
text_image
a p b a b p a
Figure 35.2.2–1 LINEAR type MPC.
Input data
Give the nodes p, a, and b as shown in Figure 35.2.2–1.
Input File Usage: *MPC LINEAR, p, a, b
Abaqus/CAE Usage: Mesh refinement multi-point constraints are not supported in Abaqus/CAE.