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:
Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step
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:
In Abaqus/CAE the normal of the pre-tension section is always fixed during the analysis.
Defining Multiple Pre-Tension Sections
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 .
Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and, if necessary, bolt axis: Method: Apply force
Prescribing a Tightening Adjustment
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).
Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step: select surface and, if necessary, bolt axis: Method: Adjust length
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 remains 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 issues 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.
When the pre-tension normal changes during a large displacement analysis, you need to
prescribe an initial pre-tension force to ensure the force in the fastener remains
constant during the rotation. If you prescribe an initial tightening adjustment by using a
boundary condition rather than prescribing a pre-tension force, the force in the fastener
may change during the rotation. To ensure the force remains constant when prescribing an
initial displacement during a large rotation analysis, you can use a small time increment
corresponding to a small incremental rotation.
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
