Assembly Definition

1. Placeholder for glosslist element

A hinge can be modeled using two flanges and a pin, as shown in Figure 1. The flange geometry is defined by creating a part, which is instanced twice inside the hinge assembly. Another part, the pin, is created and instanced once. The pin is modeled as a rigid body created from an analytical surface (see Analytical Rigid Surface Definition).

Figure 1. The hinge assembly.

This hinge example is used throughout this section to illustrate the keyword interface for parts and assemblies.

A part definition must appear outside the assembly definition. Multiple parts can be defined in a model; each part must have a unique name.

PART, NAME=PartName
  Node, element, section, set, and surface definitions
END PART

A part instance definition must appear within the assembly definition. If the part instance is not imported from a previous analysis, each part instance must have a unique name and refer to a part name. A part instance name of Assembly is not allowed. In addition, you can specify data that are used to position the instance within the assembly. Give a translation and rotation for the part instance relative to the origin of the assembly (global) coordinate system.

If the part instance is to be imported from a previous analysis, each part instance must specify the name of the instance to be imported. For more information on defining part instances for use with the import capability, see About Transferring Results between Abaqus Analyses.

Additional sets and surfaces can be defined at the instance level, as explained later in this section.

INSTANCE, NAME=InstanceName, PART=PartName
 <positioning data>
 Additional set and surface definitions (optional)
END INSTANCE

INSTANCE, INSTANCE=instance-name
 Additional set and surface definitions (optional)
IMPORT
END INSTANCE

Only one assembly can be defined in a model. All part instance definitions must appear within the assembly definition.

Sets and surfaces can be defined at the assembly level by including the appropriate definitions within the assembly definition.

ASSEMBLY, NAME=name
  Part instance definitions
  Set and surface definitions
  Connector and constraint definitions
  Rigid body definitions
END ASSEMBLY

The hinge assembly shown in Figure 1 can be defined using the following syntax in the input file:

PART, NAME=Flange
   NODE, NSET=Flange
    1, ...
    2, ...
    ...
    360, ...
   ELEMENT, ELSET=Flange
    1, ...
    2, ...
    ...
    200, ...
   SOLID SECTION, ELSET=Flange, MATERIAL=Steel
   ELSET, ELSET=Flat, GENERATE
    176, 200, 1
   SURFACE, NAME=Flat
    Flat, S1
END PART
PART, NAME=Pin
   NODE, NSET=RefPt
    1, ...
   SURFACE, TYPE=REVOLUTION, NAME=Pin
    ...
   RIGID BODY, REF NODE=1, ANALYTICAL SURFACE=Pin
END PART
ASSEMBLY, NAME=Hinge
   INSTANCE, NAME=Flange-1, PART=Flange
    <positioning data>
   END INSTANCE
   INSTANCE, NAME=Flange-2, PART=Flange
    <positioning data>
   END INSTANCE
   INSTANCE, NAME=Pin-1, PART=Pin
    <positioning data>
   END INSTANCE
   ELSET, ELSET=Top
    ...
   NSET, NSET=Output
    ...
END ASSEMBLY
MATERIAL, NAME=Steel
 ...

When creating a model, it is often necessary to refer to something outside of the current level; for example, a section definition within a part must refer to a material, which is defined at the model level. Loads defined within a step must refer to sets within the assembly. But some references between levels are not allowed; for example, a set in one part instance cannot refer to nodes in another part instance. The following references are allowed:

These rules are illustrated in Figure 4.

Figure 4. Allowable references between levels.

The Abaqus naming conventions allow for a model that contains an assembly. When something is defined within a part, instance, or the assembly and is referred to from outside its level, the complete name must be used to identify it (set Flat of instance Flange-2 in assembly Hinge, for example). A complete name is given in the input file using “dot” notation: each name in the hierarchy is separated by a “.” (period). For example, some complete names in the Hinge assembly are

Such names would be used to refer to the sets from outside the assembly. The same syntax is used to refer to individual nodes or elements.

As always, the context determines whether a node or element is being referred to. The “.” has special meaning; it is used to separate the individual names in a complete name. Therefore, the “.” cannot be used in labels such as set and surface names. For example,

Complete names are limited to 80 characters, including the periods.

However, when referring to a name in an input file that is not defined in terms of an assembly of part instances, the “.” in the name should be replaced by underscores. Such a situation can occur, for example, when an element set from a previous analysis is referred to by the current analysis but the current input file is not defined in terms of an assembly of part instances.

PART, NAME=Flange
 ...
ELSET, ELSET="Set 1"
 ...
END PART
 ...
ELEMENT OUTPUT, ELSET=Hinge.Flange-1."Set 1"

ASSEMBLY, NAME=Hinge
   ...
   NSET, NSET=Top
    Flange-1.2, Flange-1.5, ...
    Flange-2.1, Flange-2.4, ...
END ASSEMBLY

STEP
     ...
     NODE OUTPUT, NSET=Hinge.Top
END STEP

STEP
     ...
     BOUNDARY
      Hinge.Flange-2.FixedEnd, 1, 3
END STEP

• The mesh can be defined either on a part or on an instance of that part (not both). Typically, parts are meshed and instances inherit that mesh, but it is not required. If, for example, you want to use fully integrated elements for one part instance and reduced-integration elements for another, or if you want to define a more refined mesh on one part instance than on another, you must mesh the instances separately.

  • If the mesh is defined on a part, it is inherited by every instance of that part.

  • If the mesh is defined on a part, it cannot be redefined (overridden) on an instance of that part. In other words, if the node and element definitions appear within the part definition, they cannot appear within the instance definition for that part.

  • If a mesh is not defined on a part, it must be defined on every instance of that part.

• A part definition is required even if no mesh is defined on it. In such cases the empty part definition is used only to relate various instances to each other via the instance definitions. This allows the Visualization module to group information by part.

• Rebar must be defined within a part along with the elements that are being reinforced.

• Reference nodes can be created at the assembly level.

• Only mass, rotary inertia, capacitance, connector, spring, and dashpot elements can be created at the part or the assembly level. All other element types must be defined within a part (or part instance). To define assembly-level elements that refer to part-level nodes, include the part instance name when defining the element connectivity. For example:

  ELEMENT, TYPE=MASS
  1, Instance-1.10

• Sections must be assigned where the mesh is defined (either within a part definition or within each instance of the part).

• If a part is meshed, all instances of that part have the same element types and are made of the same materials.

• The set referred to by a section definition must be created at the same level as the mesh and section definition.

• If the part is meshed, the section assignment cannot be overridden at the instance level.

• Sets and surfaces (rigid or deformable) can be created within a part, part instance, or the assembly.

  • Sets and surfaces can be created on a part if a mesh is defined on the part.

  • Sets and surfaces defined on a part are inherited by each instance of that part.

  • Assembly-level sets and, in Abaqus/Standard, secondary surfaces can span part instances.

• If an element set or node set definition with the same name appears more than once at the same level, the new members are appended to the set.

• A surface definition cannot appear more than once with the same surface name within the same level.

• New sets and surfaces can be created on a part instance. If a set or surface is defined on a part instance and a set or surface with that name was not defined on the part, the set or surface is added to the instance.

• Sets and surfaces cannot be redefined on a part instance. If a set or surface is defined on a part instance and a set or surface with that name was also defined on the part, an error will be generated.

• Sets and surfaces are not step dependent. All sets and surfaces must be defined within a part, part instance, or the assembly.

NSET, NSET=NsetName, INSTANCE=InstanceName
ELSET, ELSET=ElsetName, INSTANCE=InstanceName

Rigid bodies can be defined at the part or assembly level.

• To define a rigid body at the part level, include the rigid body and rigid body reference node definitions within the part definition.

  • Rigid elements, deformable elements, and analytical surfaces cannot be combined within a part.

  • If a rigid body is defined within a part, all deformable, rigid, or connector elements in the part must belong to the rigid body.

  • Mass, rotary inertia, spring, dashpot, and heat capacitance elements can be included in a part that contains a rigid body definition, but these elements cannot belong to the rigid body.

  • To create a part-level rigid body from an analytical surface, include the surface definition within the part definition. Only one analytical surface is allowed per part.

• To define a rigid body at the assembly level, include the rigid body and reference node definitions within the assembly definition.

  • A rigid body can be created at the assembly level from any combination of rigid elements, deformable elements, and up to one analytical surface.

  • The rigid body definition can refer to assembly-level or part-level sets.

  • A part that contains a rigid body definition cannot be included in an assembly-level rigid body.

• You can define a discrete surface at the part or assembly level independent from the rigid body definition.

• An analytical surface definition can appear only within a part definition, even if the rigid body is defined at the assembly level.

• Materials are defined at the model level so that they can be reused. The material definition cannot appear within a part, part instance, or the assembly.

• All materials in a model must have unique names.

An interaction is a relationship between surfaces or between a surface and its environment. Interactions in Abaqus include contact, radiation, film conditions, and element foundations.

• Interactions are defined at the model level in Abaqus/Standard and at the model level or within steps in Abaqus/Explicit; they cannot be defined within a part, assembly, or instance.

Constraints are inflexible coupling mechanisms such as MPCs and equations (see About Kinematic Constraints).

• Constraints can be defined within a part or the assembly. They can be defined within a part instance if the mesh is defined within the part instance. Constraints should be defined at the assembly level if they constrain the motion of one part instance relative to another.

• Constraints are translated and rotated according to the positioning data given for a part instance.

Distributions are used to specify arbitrary spatial variations of selected element properties, material properties, local coordinate systems, and spatial variations of initial contact clearances (see Distribution Definition).

• Distributions should be defined at the level at which they are used. For example, if a distribution is used to define shell thicknesses, the distribution should be defined at the same level as the section definition that refers to it. If a distribution is used to define a material property, it should be defined at the model level with the material definition.

In the following examples most parameters and data lines are omitted for clarity.

In the second example the instances are meshed.

The assembly's coordinate system is the global coordinate system. You can position part instances within the assembly by giving a translation and/or rotation relative to the global origin. Specify a translation by giving a translation vector. Specify a rotation by giving two points, a and b, to define a rotation axis plus a right-handed angular rotation around that axis.

Local coordinate systems defined within a part or part instance will be translated and rotated according to the specified positioning data, as shown in Figure 5. (In this figure details such as element and section definitions are omitted for clarity.) Results given in a local coordinate system are output in the transformed local system. Equations will also be translated and rotated according to the positioning data for an instance. All data within a part (or part instance) definition are defined relative to the part's local coordinate system; positioning data are applied to a part instance after everything within that instance is defined.

Figure 5. Defining local coordinate systems.