Line Mesh Panel

Use the Line Mesh panel to create a chain of one-dimensional elements such as beams along a line.

Location: 1D page

The Line Mesh panel is used for creating beam models or beam representations of structural models. Line mesh can be created from lines or node lists. Once the selection is complete, click mesh to preview the node seeding of the mesh. It also invokes the density and biasing subpanels, similar to those in the automeshing module, allowing you to interactively modify the element density and biasing.

Line mesh (continuous chain of one-dimensional elements) can be created for a selection of lines or list of nodes (node list).

Panel Options

Option Action
Lines / Node List Choose where to create the mesh.
If the selection contains more than one line, each line is individually meshed with the global element size (set in the Mesh subpanel of the Options panel). Therefore, they are not considered as a continuous line if the lines are connected. For example, for three lines that are continuous, each having a length of three units: when line meshed global element size is five units, one element is created for each line (total three elements) rather than two elements for all three lines together.
If the lines being meshed are connected, meaning their ends are within node tolerance (set in the mesh Options panel) of each other, the line mesh created is connected. It also means that the 1D elements created share common nodes.
Node List
Each pair of sequential nodes in the node list is considered as a segment to line mesh. Therefore, a minimum of one 1D element is seeded for each pair. The number of 1D elements between each pair of nodes is determined by global element size.
The 1D element created maintains connectivity with the selected nodes in the node list. If the nodes of the node list belong to an existing FE mesh, the new 1D elements created share common nodes with them.
segment is whole line / breakangle =
segment is whole line
Treat the entire line as a single segment and seed your mesh nodes accordingly, ignoring break angles.
Specify an angle to determine points at which to split the line into segments that can be individually controlled.
element size = Specify a size for the 1D elements.
element config Select a configuration of 1D elements to be created.
Note: Each 1D element can have different types depending on the solver template. Use the Elem Types panel to set the necessary element type for the intended 1D element. For example, a spring element can be used to create a CELAS1, CELAS2, CBUSH, CDAMP1, or CDAMP2 type of element in Nastran. Line mesh is created with the current element type set in the Elem Types panel.
For the bars element configuration, additional options for defining offsets and orientation are available.
Offsets Specify the required x, y and z offsets for a and b locations.
Note: Only available for bar type element configurations.
Orientation Choose a cross section orientation for which the bar properties are defined.
Automatically determine orientation using the Frenet frame. The orientation for each bar element varies based on the curvature of each line being meshed.
Define orientation via a vector (N1,N2,N3) or along global axes.
Define orientation as X, Y and Z components of the global axes.
Define orientation using a chosen orientation node and an the y or z direction.
Note: Only available for bar type element configurations.
property = Select an optional property collector. The 1D elements created (such as bars or springs) automatically get assigned to these property collectors.
Note: Only valid for solver templates that define a property directly to 1D elements. Some solvers such as Abaqus and LS-DYNA allow properties to be defined only to the components and not directly to the elements.
add elems to current component / add elems to line component Specify where to organize the 1D line mesh elements after they are created.

Command Buttons

Button Action
mesh Create a 1D line mesh. Secondary panels which can be used to change the density and biasing of the 1D elements are displayed upon clicking mesh. You can interactively adjust the density (and biasing) of 1D elements along a line segment, set the element densities of one or more segments to a specified value, and so on using these secondary panels.
reject Undo the most recent meshing action.
return Exit the panel.