Skip to content

Bent Lines Structure

The Structure tab in the Bent Line properties window is composed of three main areas: Sections, Primary points of section, and Composition of segments.

Sections

Any Bent Line is always composed of a single Line section. The shape of the section is defined through the Shape Definition tab.

Note

On the contrary of Generic Lines, Bent Lines cannot be split into several sections.

Reference unstressed configuration

The reference unstressed configuration defines the shape of the line at rest, i.e. when the line is not submitted to any external or internal loadings.

The option defaults to as-defined shape for Bent Lines, which sets the shape of the line at rest similar to the shape shown in the 3D View window of your model. Note that considering the as-defined shape is suitable only for lines representing rigid spools or similar applications.

The reference unstressed configuration may be turned back to straight pipe if needed, as with the Generic Lines. Note however that bends will not be kept during the calculation in this case.

Primary points of section

In the Primary points of section area, enter the positions (in the global coordinate system) of the two section end points. Different linked to connections can be defined: free, anchored, or connected (to existing structures, including the Sea & ground); in this last case, the attach point field allows the user to link the line end to one of the existing points on a structure.

Unless the free option is selected, different connection type can be imposed: Pin, Clamp, User defined (with the six degrees of freedom independently chosen free or constraint or clamped), Flexjoint or Spring .

Unless the pin option is selected, elevation and azimuth departure angles must be specified in the impose neutral axis direction fields. Carefully check these imposed departure angles (ENCASD & PSID) at the connected point, to ensure the direction matches the line. See more details...

Warning

Clamp connections may be defined at line ends by specifying the departure angle through its azimuth and elevation. This determines the departure direction only (i.e. tangent direction only but not the 2 principal bending directions associated with the cross-section at the connection point), and the FE engine automatically sets-up the local reference frame associated with the line at the initial stages of the calculation. Initial torsion in the line may arise from inappropriate initial torsion constraints at line ends.

An improved initialization technique is used by default for torsional degrees of freedom along the line which avoids inducing some fictitious torsion in the line.

Another initialization technique allowing prescribing the directions of the principal bending axes (and therefore initial torsion) at line ends can be invoked by ticking the checkbox beside the edit boxes used to input the azimuth and elevation angle.

This makes no difference for the vast majority of cases. By default, it is recommended not to check the "Also impose bending axes" option when defining clamp connections.

Composition of segments

In this part of the window, each selected section can be further divided into segments, and the properties of each segment are defined through Line segment type.

Unlike Generic Line components, the number of segments and the associated length cannot be directly defined in this panel. Initially there is a single segment defined. New segments can be generated through the Shape Definition panel. The new segments will be added in the list as a succession of straight sections and bends. New segments are assigned a name automatically but this can be edited directly in the table.

Segment data are listed below:

  • Name: This is the name that is used to refer to the line segment. Segment names may be used to specify regions along the line when post-processing partial results envelopes graphs. These names are also used to fine tune numerical contact parameters along specific regions of a line (e.g. to request contact being circumscribed to selected regions of a line, or to set optimum density of contact elements along segments).

  • Length: This is the unstretched length of the line segment. The length is not editable, but is calculated directly by the GUI , taking into account the geometry defined into the Shape Definition tab. As you modify the shape, the section and line lengths are automatically updated..

  • Partition: Within segments between defined end points, partitioning of the segment is possible. The partition number defines the number of FE element for load, displacement and stress calculations, and thus must be set by the user to achieve optimum balance between run-time (calculation resources) and analysis accuracy. The interest in results at particular regions in the model may require more partition points (and hence smaller elements). This may be a primary reason to split the model up into segments, apart from structural property changes and connections. Beware that the ratio between the element length set for adjacent sections should never exceed 2. This may mean you need to add intermediate segments simply to create a gradual transition of element length throughout the model.

  • Segment property: Each segment must be assigned an existing Line segment type which defines the structural properties to be considered for the line segment. The line segment type must already exist before it is assigned to a line segment. Therefore two short cut buttons are provided to create new segment type or to edit segment types.

  • Property type: The last column property type is not editable but is an echo of the type associated with the line type you have selected to act as a reminder.