Figure 1
is a simple example that illustrates the concept of an assembly load.
Figure 1. Example of assembly load.
Container A is sealed by pre-tensioning the bolts that
hold the lid, which places the gasket under pressure. This pre-tensioning is
simulated in
Abaqus/Standard
by adding a “cutting surface,” or pre-tension section, in the bolt, as shown in
Figure 1,
and subjecting it to a tensile load. By modifying the elements on one side of
the surface,
Abaqus/Standard
can automatically adjust the length of the bolt at the pre-tension section to
achieve the prescribed amount of pre-tension. In later steps further length
changes can be prevented so that the bolt acts as a standard, deformable
component responding to other loadings on the assembly.
Modeling an Assembly Load
Abaqus/Standard
allows you to prescribe assembly loads across fasteners that are modeled by
continuum, truss, or beam elements. The steps needed to model an assembly load
vary slightly depending on the type of elements used to model the fasteners.
Modeling a Fastener with Continuum Elements
In continuum elements the pre-tension section is defined as a surface inside
the fastener that “cuts” it into two parts (see
Figure 2).
The pre-tension section can be a group of surfaces for cases where a fastener
is composed of several segments.
Figure 2. Pre-tension section defined using continuum elements.
The element-based surface contains the element and face information (see
Element-Based Surface Definition).
You must convert the surface into a pre-tension section across which
pre-tension loads can be applied and assign a controlling node to the
pre-tension section.
Input File Usage
Use the following options to model an assembly load across a
fastener that is modeled with continuum elements:
Assigning a Controlling Node to the Pre-Tension Section
The assembly load is transmitted across the pre-tension section by means
of the pre-tension node. The pre-tension node should not be attached to any
element in the model. It has only one degree of freedom (degree of freedom 1),
which represents the relative displacement at the two sides of the cut in the
direction of the normal (see
Figure 3).
The coordinates of this node are not important.
Figure 3. Normal to the pre-tension section; this normal should face away from
the underlying elements.
Defining the Normal to the Pre-Tension Section
Abaqus/Standard
computes an average normal to the section—in the positive surface direction,
facing away from the continuum elements used to generate the surface—to
determine the direction along which the pre-tension is applied. You may also
specify the normal directly (when the desired direction of loading is different
from the average normal to the pre-tension section). You can specify if the
normal is updated or fixed when performing a large-displacement analysis (see
Updating the Normal in a Large-Displacement Analysis).
Recognizing Elements on Either Side of the Pre-Tension Section
For all the elements that are connected to the pre-tension section by at
least one node,
Abaqus/Standard
must determine on which side of the pre-tension section each element is
located. This process is crucial for the prescribed assembly load to work
properly.
The elements used to define the section are referred to as “base elements”
in this discussion. All elements on the same side of the section as the base
elements are referred to as the “underlying elements.” All elements connected
to the section that share faces (or in two-dimensional problems, edges) with
the base elements are added to the list of underlying elements. This is a
repetitive process that enables
Abaqus/Standard
to find the underlying elements in almost all meshes—triangles; wedges;
tetrahedra; and embedded beams, trusses, shells, and membranes—that were not
used in the definition of the surface (see
Figure 4).
Figure 4. The base elements are used to find the underlying elements.
In most cases this process will group all of the elements that are
connected to the section into two regions, as shown in the figure. In rare
instances this process may group the elements in more than two regions, in
particular if line elements cross over element boundaries. An example is shown
in
Figure 5;
it has three regions, where region 1 is the underlying region.
Figure 5. An additional underlying element is found.
For each region other than region 1 an additional step is necessary to
determine on which side of the section the region is located.
Abaqus/Standard
computes an average normal, , for all the nodes of
the region that belong to the section; it also computes an average position
() of all these nodes.
In addition, it computes an average position () of the remaining
nodes of the region. If the dot product between the normal
and the vector
is negative, the region is assumed to be an underlying region and is added to
region 1. This additional step is illustrated in
Figure 5
for regions 2 and 3.
This additional step produces an incorrect separation for the beam element
shown in
Figure 6
since the beam is not found to be an underlying element.
Figure 6. An additional underlying element is not found.
If the pre-tension section has an odd shape and one or more line elements
that cross over element boundaries are connected to it, consult the list of the
underlying elements given in the data (.dat) file to make
sure that the underlying elements are listed correctly.
Elements that are connected only to the nodes on the pre-tension section,
including single-node elements (such as SPRING1, DASHPOT1, and MASS elements) are not included as underlying elements: they are
considered to be attached to the other side of the section.
Modeling a Fastener with Truss or Beam Elements
When a pre-tensioned component is modeled with truss or beam elements, the
pre-tension section is reduced to a point. The section is assumed to be located
at the last node of the element as defined by the element connectivity (see
Beam Element Library
and
Truss Element Library
for a definition of the node ordering for beam and truss elements,
respectively), with its normal along the element directed from the first to the
last node. As a result, the section is defined entirely by just specifying the
element to which an assembly load must be prescribed and associating it with a
pre-tension node.
As in the case of a surface-based pre-tension section, the node has only one
degree of freedom (degree of freedom 1), which represents the relative
displacement on the two sides of the cut in the direction of the normal (see
Figure 7).
The coordinates of the node are not important.
Figure 7. Pre-tension section defined using a truss or beam element.
Abaqus/Standard
computes the normal as the vector from the first to the last node in the
connectivity of the underlying element. Alternatively, you can specify the
normal to the section directly. You can specify if the normal is updated or
fixed when performing a large-displacement analysis (see
Updating the Normal in a Large-Displacement Analysis).
Input File Usage
Use the following option to model an assembly load across
fasteners modeled with beam or truss elements:
You can define multiple pre-tension sections by repeating the pre-tension
section definition input. Each pre-tension section should have its own
pre-tension node.
Use with Nodal Transformations
A local coordinate system (see
Transformed Coordinate Systems)
cannot be used at a pre-tension node. It can be used at nodes located on
pre-tension sections.
Applying the Prescribed Assembly Load
The pre-tension load is transmitted across the pre-tension section by means
of the pre-tension node.
Prescribing the Pre-Tension Force
You can apply a concentrated load to the pre-tension node. This load is the
self-equilibrating force carried across the pre-tension section, acting in the
direction of the normal on the part of the fastener underlying the pre-tension
section (the part that contains the elements that were used in the definition
of the pre-tension section; see
Figure 8).
Figure 8. The prescribed assembly load is given at the pre-tension node and
applied in direction .
You can prescribe a tightening adjustment of the pre-tension section by
using a nonzero boundary condition at the pre-tension node (which corresponds
to a prescribed change in the length of the component cut by the pre-tension
section in the direction of the normal).
Controlling the Pre-Tension Node during the Analysis
You can maintain the initial adjustment of the pre-tension section by using
a boundary condition fixing the degrees of freedom at their current values at
the start of the step once an initial pre-tension is applied in the fastener;
this technique enables the load across the pre-tension section to change
according to the externally applied loads to maintain equilibrium. If the
initial adjustment of a section is not maintained, the force in the fastener
will remain constant.
When a pre-tension node is not controlled by a boundary condition, make sure
that the components of the structure are kinematically constrained; otherwise,
the structure could fall apart due to the presence of rigid body modes.
Abaqus/Standard
will issue a warning message if it does not find any boundary condition or load
on a pre-tension node during the first step of the analysis.
Display of Results
Abaqus/Standard
automatically adjusts the length of the component at the pre-tension section to
achieve the prescribed amount of pre-tension. This adjustment is done by moving
the nodes of the underlying elements that lie on the pre-tension section
relative to the same nodes when they appear in the other elements connected to
the pre-tension section. As a result, the underlying elements will appear
shrunk, even though they carry tensile stresses when a pre-tension is applied.
Limitations When Using Assembly Loads
Assembly loads are subject to the following limitations:
An assembly load cannot be specified within a substructure.
If a submodeling analysis is performed (About Submodeling),
any pre-tension section should not cross regions where driven nodes are
specified. In other words, a pre-tension section should appear either entirely
in the region of the global model that is not part of a submodel or entirely in
the region of the global model that is part of a submodel. In the latter case,
a pre-tension section must also appear in the submodel when the submodel
analysis is performed.
Nodes of a pre-tension section should not be connected to other parts of
the body through multi-point constraints (General Multi-Point Constraints).
These nodes can be connected to other parts of the body through equations
(Linear Constraint Equations).
However, an equation connecting a node on the pre-tension section to a node
located on the underlying side of the section introduces a constraint that
spans across the pre-tension cut and, therefore, interacts directly with the
application of the pre-tension load. On the other hand, an equation connecting
a node on the pre-tension section to a node on the other side of the section
does not influence the application of the pre-tension load.
Procedures
Any of the
Abaqus/Standard
procedures that use element types with displacement degrees of freedom can be
used. Static analysis is the most likely procedure type to be used when
prescribing the initial pre-tension (Static Stress Analysis).
Other analysis types such as coupled temperature-displacement (Sequentially Coupled Thermal-Stress Analysis)
or coupled thermal-electrical-structural (Fully Coupled Thermal-Electrical-Structural Analysis)
can also be used. Once the initial pre-tension is applied, a static or dynamic
analysis (About Dynamic Analysis Procedures)
may, for instance, be used to apply additional loads while maintaining the
tightening adjustment.
Output
The total force across the pre-tension section is the sum of the reaction
force at the pre-tension node plus any concentrated load specified at that
node. The total force across the pre-tension section is available as output
using the output variable identifier TF (see
Abaqus/Standard Output Variable Identifiers).
The forces are along the normal direction. The shear force across the
pre-tension section is not available for output.
The tightening adjustment of the pre-tension section is available as the
displacement of the pre-tension node. The output of displacement is requested
using output identifier U. Only the adjustment normal to the pre-tension section is
output since there is no adjustment in any other direction.
The stress distribution across the pre-tension section is not available
directly; however, the stresses in the underlying elements can be displayed
readily. Alternatively, a tied contact pair can be inserted at the location of
the pre-tension section to enable stress distribution output by means of output
identifiers CPRESS and CSHEAR. See
Defining Tied Contact in Abaqus/Standard
for details on defining tied contact.
Input File Template
HEADINGPrescribed assembly load; example using continuum elements
…
NODEOptionally define the pre-tension nodeSURFACE, NAME=nameData lines that specify the elements and their associated faces to define the pre-tension sectionPRE-TENSION SECTION, SURFACE=name, NODE=pre-tension_node
**
STEP
** Application of the pre-tension across the section
STATICData line to control time incrementationCLOADpre-tension_node, 1, pre-tension_valueorBOUNDARY,AMPLITUDE=amplitudepre-tension_node, 1, 1, tightening adjustmentEND STEPSTEP
** maintain the tightening adjustment and apply new loads
STATICorDYNAMICData line to control time incrementationBOUNDARY,FIXEDpre-tension_node, 1, 1
BOUNDARYData lines to prescribe other boundary conditionsCLOADorDLOADData lines to prescribe other loading conditions
…
END STEP
