Mesh Associated Data dialog box

Use the Mesh Associated Data dialog box to define attributes for all the elements in the selected mesh. The type of element attributes available depends on the solver you use. For a list of all element attributes supported by each solver, see Element and mesh attributes.

Note:

If you are overriding an element attribute in the Simulation file, click No Override next to the attribute to modify and select Apply Override from the list that appears. Then you can update the attribute. For more information, see Override element attributes.

Mesh
Select Mesh	Lets you select multiple meshes of the same type to edit the mesh associated data.
Element Properties
Shell Offset	Assigns an offset to a shell element. The offset is a distance to offset the element plane from the element’s connection points in the direction of the element coordinate system’s positive Z-axis.
Use Element Associated Data	Available only for the solvers and element types listed in Element and mesh attributes.If an element in this mesh has element-associated data defined, the software uses the element-associated data instead of the mesh-associated data. For example, this ability is useful when some elements in the mesh need a different material orientation than the rest of the elements.Note: With LS-DYNA, you can define element attributes at either the element level or the mesh level. If you select Use Element Associated Data for the mesh, and not all elements have material orientations defined, those elements are written to the keyword file as *ELEMENT_SHELL. This is the same as selecting None for the Keyword Option. With Nastran, for 1D meshes, the element-associated data always overrides the mesh-associated data.For Nastran RBE3 elements, there are special considerations. For more information, see Importing RBE2 and RBE3 elements.
Element Name	Available for Abaqus elements with alternative formulations.Displays the name of the selected element type. For a list of supported Abaqus elements and their formulations, see Abaqus elements.
Element Formulation	Available for Abaqus elements with alternative formulations.Lets you specify the alternative formulation for the element, such as its hybrid formulation. For a list of supported Abaqus elements and their formulations, see Abaqus elements.
Gap Thickness Source	Lets you specify the source of the data the software uses to assign the thickness values to the gaps between chocking elements in the Simcenter 3D Multiphysics environment.Physical Property Table — Use the Gap Thickness value defined in the Chocking Property dialog box to define the thickness of the gaps.Field — Use a table field to define a variable thickness for the gaps. This is useful when the thickness of the gap varies through the cross section.For more information, see Chocking elements.
Thickness SourceNote: This option may appear with a different label, depending on the selected solver.	Lets you specify the source of the data the software uses to assign the element thickness values. Physical Property Table — Use the Default Thickness value defined in the associated physical property table to define the thickness of the mesh.Midsurface — Use the thickness of the geometry from which you created the midsurface. For more information, see Creating midsurfaces before meshing.Field/Expression — Use a Table field or an expression to define the thickness value.Holes — Available for 2D plane stress elements. Calculates the thickness of the material minus a pattern of holes meshed with plane stress elements. Bolt — Available for 2D plane stress elements. Calculates the thickness of a pattern of bolts meshed with plane stress elements. Tip: Use the Thickness Evaluation Source customer default (Simulation→Meshing→General tab) to set the default for this option.For more information, see Shell thickness.
Centerline Definition	Available for 2D plane stress elements and when Thickness Source is set to Holes or Bolt.Controls the location of the centerline of the hole or bolt.Inferred — The software computes the centerline's location. This option works for four-sided meshes only. The software uses the edges from the sides to define the location of the centerline.Curve — Lets you select an existing curve as the centerline, including a curve that is offset from the mesh.Four Points — Lets you select four ordered points to define the centerline. The first two points define one direction on a material edge. The second two points define a second direction on the opposite material edge. The software averages the directions to define the centerline. Note: If the hole is conical, the software uses a special algorithm to compute the location of the centerline.Vector and Point— Lets you specify a direction vector and a through point to define the centerline. You can use the Centerpoint option to either specify the point that the centerline passes through or have the software infer the location of the centerpoint.
Exclude Edges that Intersect Centerline Exclude Edges Transverse to Centerline****Select Edge	Available when Centerline Definition is set to Curve, Four Points, or Vector and Point.Lets you select any edges or curves that you want the software to exclude from the thickness calculations. Typically, you should select edges that pass through the centerline.
Thickness Evaluation Type	Available when Midsurface is selected as the Thickness Source.Controls the location at which the software computes the thickness.At Every Node — Perform ray casting operations to compute the thickness at each node in the mesh associated with the midsurface. For example, at a triangular element, the software casts rays from each of the element’s nodes to determine the thickness values.At Element Centroid — Perform a single ray casting operation at the centroid of each element to determine the thickness value. With this option, the software then assigns the same thickness to all the element’s nodes. The At Element Centroid option offers slightly improved performance over the At Every Node option as the software performs fewer calculations.Average Feature Thickness — Extract the average thickness value for midsurface face pairs defined with the Midsurface by Face Pairs, Offset Midsurface, or the User Defined Midsurface commands. This option is the fastest way to evaluate the thickness as the software does not have to perform any ray casting calculations. It is the recommended option for constant thickness parts.Tip: Use the Thickness Evaluation Type customer default (Simulation→Meshing→General tab) to set the default for this option.
Thickness Field	Available when Field is selected as the Thickness Source.Lets you select or create a field.
Scale Factor	Available when Field is selected as the Thickness Source.Defines a scale factor for the thickness.
Number of Instances	Available for plane stress elements only. Defines the number of instances of the plane stress mesh rotated about the rotational axis. You can use a plane stress mesh to model blades or holes in a gas turbine engine.
Transpose Centerline	Available for plane stress elements only.Rotates the centerline of a hole.If you model a hole with plane stress elements, the mesh must have four sides. When you select this option, the software rotates the centerline to align with the opposite pair of sides.Note: To display the centerline of a hole meshed with plane stress elements, select the Display Centerline check box in the Mesh Display dialog box.
Material Orientation Method/Set Material OrientationNote: This option may appear with a different label, depending on the selected solver.	Lets you define the material orientation for all elements in the mesh. For more information, see Material orientation.
Rotation 1, Rotation 2, Rotation 3	Available for 3D elements when Material Orientation Method is set to any option other than Physical Property Table.Lets you specify the axis about which to rotate the material orientation coordinate system.
Rotation Angle 1, Rotation Angle 2, Rotation Angle 3	Lets you specify the angle in degrees to rotate the material orientation coordinate system about the selected axis.
Element Section Controls****Hourglass Control	Available for Abaqus 2D shell and membrane elements.Lets you select a non-default hourglass control approach for reduced-integration elements and modified tetrahedral or triangular shell elements. Default — Uses the default values for hourglass control.Enhanced — Defines hourglass control that is based on the assumed enhanced strain method. This formulation provides improved coarse mesh accuracy with slightly higher computational cost and performs better for nonlinear material response at high strain levels when compared with the default total stiffness formulation.Stiffness — Defines hourglass control that is strictly elastic for all elements with reduced integration and for modified tetrahedral or triangular elements.For more information, see *SECTION CONTROLS in the Abaqus Keyword User’s Manual.
Scale Factor for Displacement DOFs****Scale Factor for Rotational DOFs	Available if Hourglass Control is set to Stiffness.Lets you specify scaling factors for the hourglass stiffness that Abaqus applies to the elements’ displacement and/or rotational degrees-of-freedom.The default scale factor for Abaqus is 1.0. Abaqus recommends a range of values between 0.2 and 3.0 for this option.
Section Orientation****Method	Lets you orient the 1D cross section on the beam mesh using one of these methods: Orientation Vector — Lets you orient the 1D element Y-axis or Z-axis (n1 or n2 axis for Abaqus) to an axis of the absolute coordinate system or to a vector you select on geometry.Orientation Node — Lets you orient the cross section using a node that, along with the first node of the element, defines the orientation vector for the section. The X-Y plane of the cross section orientation is defined by the vector from the first node in the 1D element to the orientation node you specify.For steps to define cross section orientation, see Define cross section orientation.
Select Element	The mesh orientation is defined with respect to the first element in the mesh, and then the software transforms it to the other elements in the mesh. In the dialog box, the Select Element (1) option is automatically set to the first element of the mesh for which you are editing the mesh associated data.
Element Axis	Specifies the axis of the element coordinate system to orient (Y-axis or Z-axis, or n1 or n2 axis for Abaqus).
Specify Vector	Lets you select the axis of the absolute coordinate system to which to orient the 1D cross section.For example, to orient the Y-axis of the 1D mesh to the X-axis of the absolute coordinate system, select XC-axis .Or, click Inferred Vector to infer the axis by selecting geometry in the graphics window.For more information, see Vector dialog box.
Reverse Direction	Reverses the direction of the vector.
Section Offsets****Offset End B = Offset End A	Lets you apply separate offsets to the two ends of the 1D cross section.If both ends of the cross section should use the same offset, leave the Offset End A = Offset End B check box selected.To apply a different offset to the two ends of the cross section, clear the Offset End B = Offset End A check box.
End A****Specify Point on Section	Lets you select a reference point for the offset on the 1D cross section. You offset the cross section from the beam mesh according to a reference point on the cross section. By default, this point is the section centroid (for ANSYS and LS-DYNA) or the section shear center (for Simcenter Nastran), but you can select a different reference point on the section. Note: If ANSYS is the selected solver, the default offset reference point is the section centroid. However, when you solve the model, the software adjusts the offset to be a distance from the section origin, which is how the ANSYS solver expects the offset. For steps to define 1D cross section offsets, see Offset a cross section.
Section Placement Method	Available only when Nastran is the selected solver.Select Language Specific to offset the cross section shear center to the beam mesh in terms of components of the nodal displacement coordinate system.
DOF1/ DOF2/ DOF3 Offset to Shear Center	Available when Section Placement Method is set to Language-Specific, for the Nastran solver.Enter displacement values in model units of length to offset the cross section in the X, Y, and Z directions of the nodal displacement coordinate system.Note: For models created in software versions prior to 2020.1, be sure to check and correct CBAR/CBEAM offsets that were defined with units other than length.
Specify Section Location	Available for solvers that support cross section offsets.Lets you select the point to which the 1D cross section should be offset. You can do this graphically by selecting curves, points, or other geometry. For information about the Point dialog box, see Point dialog box.
Offset to Point on Section	Available for solvers that support offsets.Lets you enter specific offset values in the X, Y, and Z directions (of the element coordinate system) from the specified point on the section. Offset Along Element refers to the X-axis.Note: The ANSYS solver does not support offsets along the X-axis.
Apply Pin Flags/End Releases On	Available for solvers that support end releases.Lets you model hinged or pinned ends on the 1D mesh. End releases (also called pin flags) remove connections between a node and selected degrees of freedom. The degrees of freedom are defined in the element coordinate system. Each Element — Apply the end release to the end node of each element.End Nodes of Chain — In a mesh, apply the end release only to the end node of the last element.
Pin Flags/End Releases – End A/End B (End I/End J for Ansys)	Available for solvers that support end releases.Lets you set DOF1 – DOF6 to On to disconnect the forces for end A and/or end B of the element. For more information, see End releases for 1D elements.
Element Orientation****Specify Vector	Available when the selected solver is Simcenter Nastran, for spring-damper and gap elements.Lets you use the standard vector tools to define the element orientation by specifying a vector. For more information about the Vector dialog box, see Vector dialog box.In the example below, the orientation is defined in the Z direction of the nodal displacement coordinate system (which, in this case, is the same as the absolute coordinate system). The arrow indicates the orientation vector.
Reverse Direction	Available when the definition method is set to Vector.Reverses the direction of the vector.
Element Orientation****Uniaxial	Available when the selected solver is Simcenter Nastran, for spring-damper elements.Specifies that the stiffness and damping physical properties will be defined in a single direction (parallel with the element line), and therefore no orientation is necessary.
Spring Damper****Offset Definition	Available when the selected solver is Simcenter Nastran, for spring-damper elements.You can offset the stiffness and damping properties of the spring-damper axially (along the element line) or in the components of a coordinate system.GA-GB Line — Offset the stiffness and damping properties along the element line. You can enter a value from 0–1. Leaving the value blank results in the default value of 0.5, which places the properties at the center of the element. Coordinate System — Offset the stiffness and damping properties in terms of the components of the coordinate system you select or create. This can be the Absolute coordinate system, or you can use the CSYS tools to define a Cartesian, Cylindrical, or Spherical coordinate system.
Distribute Mass	Available for CONM2 0D elements.Distributes the total Mass value, divided by the number of elements in the mesh collector, to each element in the mesh.
Description	Available for 1D joint elements (CJOINT).Sets a description of the joint that appears in the Information window and in post-processing for time history curves. If you omit the description, the joint is identified by the element ID and the joint type.Note: The description applies to all joint elements within the mesh.
Enable CSYS Override	Available for 1D joint elements (CJOINT).Lets you select a coordinate system for the joint.
CSYS Type	Available for 1D joint elements (CJOINT). Appears when the Enable CSYS Override check box is selected.Specifies the type of coordinate system you want to use for the orientation of joint.
Local	Available for 1D joint elements (CJOINT).Appears when CSYS Type is set to Cartesian, Cylindrical, or Spherical.Lets you select the method for creating the coordinate system.
Control Node	Available for 1D joint elements (CJOINT).The control node applies to revolute, inline, cylindrical, slider, and slider-universal joints. For more information, see Control nodes.If you did not create a control node yet, see Create and assign control nodes.Lets you select an independent node that internally allows the solver to drive joints and/or store results. For joints with a rotational DOF, drives the joint with rotation or torque.For joints with a translational DOF, drives the joint with displacement or force.
Control Node Degrees of Freedom	Available for RBE3 elements used in kinematic joints (CJOINT).Specifies the degrees of freedom for the control node.Note: When you realize a kinematic joint universal connection with CJOINT+RBE3, the six degrees of freedom of the leg nodes drive only the translation of the core node. This can lead to problems when you connect shell elements to a joint using RBE3. To avoid the problems, set the three rotational degrees of freedom to On.
Leg Node Degrees of Freedom	Available for RBE3 elements used in kinematic joints (CJOINT).Specifies the degrees of freedom for the legs of the RBE3 spider.
Fourier Connection Option	Available for FOU3 1D connection elements.Specifies how to connect the 2D axisymmetric mesh to a 3D node.3 Kinematic ConstraintsThe connection point on the 3D mesh shares the same axial and radial location as the 2D multi-harmonic node.3 Node Linked to Mean DisplacementThe connection point on the 3D mesh lies along the axis of symmetry.To reset the connection option for the selected meshes to the same value, select the default value from the table and click Reset .
CSYS	Available for CBUSH2 1D connection elements.Specifies the coordinate system to use for the orientation of the bushing.To reset the coordinate systems for the selected meshes to the same coordinate system, select the default value from the table and click Reset .
Link Option	Available for CLINK 1D connection elements.Specifies the type of misalignment to use in the CLINK connection.Misalignment in Translation and RotationSelect when parallel and angular misalignments are applied.Misalignment in TranslationSelect when only parallel misalignment is defined. This option reduces the degrees of freedom.To reset the connection option for the selected meshes to the same value, select the default value from the table and click Reset .
Mesh Properties
Available for 1D and 2D meshes.
Export Mesh to Solver	Controls whether the software includes the mesh data in your solver input file when you export or solve the model. Note: If you plan to only use this 2D mesh as a seed mesh for a 3D mesh, clear this check box.
Preview
Available when specifying the material orientation for 3D and 2D elements.
Automatic	Select Automatic to have the software automatically preview the material orientation vector graphics for the method and parameters you specify.
Preview	Temporarily displays the material orientation vector graphics on the elements. This button lets you preview the vector graphics before you apply the material orientation changes to a mesh.

These options are available when the magnitude is defined as Field.
Select Existing Field from List	Lets you select an existing field.
Formula Constructor	Lets you use a formula to construct a field. For more information, see Define a boundary condition using a formula field.
Table Constructor	Lets you use a table to construct a field.For more information, see Define a boundary condition using a table field and Define a material property using a table field.
Link Constructor	Lets you reference an existing field. You can override the field's spatial map to use the field in another location.For more information, see Linked Field dialog box.
Plot(XY)	Plots the field as an XY graph.For more information, see: Plot functions, Graph overview, and Edit display properties of graph objects.

How do I

Add element-associated data

Edit the mesh associated data for multiple meshes

Remove element-associated data

List and show element-associated data for a mesh

Add mesh-associated data

Create an ANSYS KEYOPT table

Override element attributes

View material orientation graphically

Define Nastran 2D element material orientation

Define Nastran 3D element material orientation

Define Abaqus 2D element material orientation

Define Abaqus 3D element material orientation

Define ANSYS 2D element material orientation

Define ANSYS 3D element material orientation

Define LS-DYNA 2D element material orientation

Define LS-DYNA 3D element material orientation

Define 2D element material orientation (Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal)

Define 3D element material orientation (Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal)

Learn more

Mesh-associated data

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Mesh Associated Data dialog box, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });