김경종
270 lines
14 KiB
Markdown
270 lines
14 KiB
Markdown
<!-- source-page: 211 -->
|
||
|
||
# Prescribing surface-based seepage flow velocity
|
||
|
||
To prescribe a surface-based seepage flow velocity, specify a surface name, the seepage flow type, and the pore fluid velocity. The element-based surface (see “Element-based surface definition,” Section 2.3.2) contains the element and face information.
|
||
|
||
Input File Usage: \*DSFLOW surface name, S,
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Surface pore fluid for the Types for Selected Step: select region: Distribution: Uniform, Magnitude:
|
||
|
||
# Prescribing node-based seepage flow
|
||
|
||
To prescribe node-based seepage flow, specify the node or node set name and the magnitude of the flow per unit time.
|
||
|
||
Input File Usage: \*CFLOW node number or node set name, , magnitude
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Fluid for the Category and Concentrated pore fluid for the Types for Selected Step: select region: Magnitude: magnitude
|
||
|
||
# Prescribing seepage flow at phantom nodes for enriched elements
|
||
|
||
For an enriched element (see “Modeling discontinuities as an enriched feature using the extended finite element method,” Section 10.7.1), you can specify the seepage flow at a phantom node that is originally located coincident with the specified real node.
|
||
|
||
Alternatively, you can specify the seepage flow at a phantom node located at an element edge between two specified real corner nodes directly or indicate that the pore pressure applied to a phantom node located at an element edge is interpolated from the specified real corner nodes.
|
||
|
||
Input File Usage: Use the following option to specify the seepage flow at a phantom node originally located coincident with the specified real node:
|
||
|
||
\*CFLOW, PHANTOM=NODE node number, , magnitude
|
||
|
||
Use the following option to specify the seepage flow at a phantom node located at an element edge:
|
||
|
||
\*CFLOW, PHANTOM=EDGE first corner node number, second corner node number, magnitude
|
||
|
||
<!-- source-page: 212 -->
|
||
|
||
Use the following option to indicate that the pore pressure applied to a phantom node located at an element edge will be interpolated automatically from the specified real corner nodes when the enriched element is cracked:
|
||
|
||
\*CFLOW, PHANTOM=INCLUDED
|
||
|
||
node or node set name, , magnitude
|
||
|
||
Abaqus/CAE Usage: Prescribing seepage flow at phantom nodes for enriched elements is not supported in Abaqus/CAE
|
||
|
||
# Modifying or removing seepage flow velocities and seepage flow
|
||
|
||
Seepage flow velocities can be added, modified, or removed as described in “Applying loads: overview,” Section 34.4.1.
|
||
|
||
# Specifying time-dependent flow velocity and flow
|
||
|
||
The magnitude of the seepage velocity, $v _ { n } ,$ , can be controlled by referring to an amplitude curve. To specify different variations for different flows, repeat the seepage flow velocity or seepage flow definition with each referring to its own amplitude curve. See “Applying loads: overview,” Section 34.4.1, and “Amplitude curves,” Section 34.1.2, for details.
|
||
|
||
# Defining nonuniform flow velocities in a user subroutine
|
||
|
||
To define nonuniform element-based or surface-based flow, the variation of the seepage magnitude as a function of position, time, pore pressure, etc. can be defined in user subroutine DFLOW. If the optional seepage velocity, $v _ { n }$ , is specified directly, this value is passed into user subroutine DFLOW in the variable used to define the seepage magnitude.
|
||
|
||
<table><tr><td>Input File Usage:</td><td>Use the following option to define nonuniform element-based flow:*DFLOWelement number or element set name, SnNU, $v_{n}$ Use the following option to define nonuniform surface-based flow:*DSFLOWsurface name, SNU, $v_{n}$ </td></tr></table>
|
||
|
||
<table><tr><td>Abaqus/CAE Usage:</td><td>Use the following input to define nonuniform surface-based flow:Load module:Create Load: choose Fluid for the Category and Surface pore fluid for the Types for Selected Step: select region: Distribution: User-defined, Magnitude: $v_{n}$ Nonuniform element-based flow is not supported in Abaqus/CAE.</td></tr></table>
|
||
|
||
<!-- source-page: 213 -->
|
||
|
||
# 34.5 Prescribed assembly loads
|
||
|
||
• “Prescribed assembly loads,” Section 34.5.1
|
||
|
||
<!-- source-page: 214 -->
|
||
|
||
<!-- source-page: 215 -->
|
||
|
||
# 34.5.1 PRESCRIBED ASSEMBLY LOADS
|
||
|
||
Products: Abaqus/Standard Abaqus/CAE
|
||
|
||
# References
|
||
|
||
• “Prescribed conditions: overview,” Section 34.1.1
|
||
• \*BOUNDARY
|
||
• \*CLOAD
|
||
• \*PRE-TENSION SECTION
|
||
• \*SURFACE
|
||
• Chapter 22, “Bolt loads,” of the Abaqus/CAE User’s Guide
|
||
|
||
# Overview
|
||
|
||
# Assembly loads:
|
||
|
||
• can be used to simulate the loading of fasteners in a structure;
|
||
• are applied across user-defined pre-tension sections;
|
||
• are applied to pre-tension nodes that are associated with the pre-tension sections; and
|
||
• require the specification of pre-tension loads or tightening adjustments.
|
||
|
||
# Concept of an assembly load
|
||
|
||
Figure 34.5.1–1 is a simple example that illustrates the concept of an assembly load.
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
pre-tension
|
||
section
|
||
gasket
|
||
bolt
|
||
A
|
||
</details>
|
||
|
||
Figure 34.5.1–1 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 34.5.1–1, and subjecting it to a tensile load. By modifying the elements on
|
||
|
||
<!-- source-page: 216 -->
|
||
|
||
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 34.5.1–2). The pre-tension section can be a group of surfaces for cases where a fastener is composed of several segments.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
pre-tension
|
||
section
|
||
elements chosen by
|
||
user to describe
|
||
the pre-tension section
|
||
</details>
|
||
|
||
Figure 34.5.1–2 Pre-tension section defined using continuum elements.
|
||
|
||
The element-based surface contains the element and face information (see “Element-based surface definition,” Section 2.3.2). You must convert the surface into a pre-tension section across which pretension loads can be applied and assign a controlling node to the pre-tension section.
|
||
|
||
<!-- source-page: 217 -->
|
||
|
||
Input File Usage: Use the following options to model an assembly load across a fastener that is modeled with continuum elements:
|
||
|
||
\*SURFACE, TYPE=ELEMENT, NAME=surface\_name
|
||
|
||
\*PRE-TENSION SECTION, SURFACE=surface\_name, NODE=n
|
||
|
||
Abaqus/CAE Usage: 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 34.5.1–3). The coordinates of this node are not important.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
n
|
||
pre-tension
|
||
section
|
||
pre-tension
|
||
node
|
||
</details>
|
||
|
||
Figure 34.5.1–3 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). The normal is not updated when performing large-displacement analysis.
|
||
|
||
<!-- source-page: 218 -->
|
||
|
||
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 34.5.1–4).
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
pre-tension
|
||
section
|
||
embedded
|
||
beam
|
||
element
|
||
region 1 { base elements
|
||
underlying elements
|
||
that share facets with the
|
||
base elements
|
||
region 2
|
||
</details>
|
||
|
||
Figure 34.5.1–4 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 34.5.1–5; it has three regions, where region 1 is the underlying region. 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 34.5.1–5 for regions 2 and 3.
|
||
|
||
This additional step produces an incorrect separation for the beam element shown in Figure 34.5.1–6 since the beam is not found to be an underlying element. 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.
|
||
|
||
<!-- source-page: 219 -->
|
||
|
||
|
||
pre-tension
|
||
section
|
||
region 1
|
||
region 2
|
||
beam element (region 3)
|
||
position of A, B, and n for region 2
|
||
position of A, B, and n for region 3
|
||
|
||
Figure 34.5.1–5 An additional underlying element is found.
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
pre-tension
|
||
section
|
||
B
|
||
n
|
||
A
|
||
beam element
|
||
region 1
|
||
</details>
|
||
|
||
Figure 34.5.1–6 An additional underlying element is not found.
|
||
|
||
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.
|
||
|
||
<!-- source-page: 220 -->
|
||
|
||
# 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,” Section 29.3.8, and “Truss element library,” Section 29.2.2, 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.
|
||
|
||
Input File Usage: Use the following option to model an assembly load across fasteners modeled with beam or truss elements:
|
||
|
||
\*PRE-TENSION SECTION, ELEMENT=element\_number, NODE=n
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Bolt load for the Types for Selected Step
|
||
|
||
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 34.5.1–7). The coordinates of the node are not important.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
pre-tension
|
||
node
|
||
n
|
||
2
|
||
pre-tension
|
||
section
|
||
beam or truss
|
||
element
|
||
1
|
||
</details>
|
||
|
||
Figure 34.5.1–7 Pre-tension section defined using a truss or beam element.
|
||
|
||
Defining the normal to the pre-tension section
|
||
|
||
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. This normal is not updated during large-displacement 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.
|