Mesh Associated Data dialog box (Simcenter Samcef)

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 analysis and elements you use. For a list of all element attributes supported by each solver, see Element and mesh attributes.

Mesh
Select Mesh	Lets you select multiple meshes.
Material Orientation
Material Orientation Method	Defines the material orientation method.You can choose between a Tangent Curve, a Vector or a Orientation Angle method.
Material Orientation Angle	Appears when Material Orientation Method is set to Orientation Angle.Defines the material orientation angle.
Primary Direction	Appears when Material Orientation Method is set to Tangent Curve.Lets you select the primary direction.
Specify Vector	Appears when you select Vector in the Material Orientation Method list.Lets you select the direction.
Rotation Angle	Appears when Material Orientation Method is set to Tangent Curve or Vector.Lets you define the rotation angle.
Thickness
Thickness Source	Lets you specify the source of the data the software uses to assign the element thickness values. Physical Property Table — Use the 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.Field — Use a Table field to define a variable thickness.
Use Element Associated Data	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.
Element Properties
EXCE****NXCE	Lets you choose the way that shell offsets are used: EXCE — Performs the integration over the thickness by taking the node positions as references.NEXCE — Performs the integration by simulating rigid bodies between the nodes and their projection on the mid-shell surface.For more information, see Shell offsets (Simcenter Samcef).
Shell Offset	Defines the offset value.
Constrained Dofs	Applies to the MeanInterpolation [MEAN] element.Lets you select how the degrees of freedom of the slave node and the master nodes are constrained.You can constrain the degrees of freedom by selecting All Translations and Rotations, All Translations, or All Rotations.
Options
MIND card	Lets you specify the flexural behavior and the geometrical stiffness of the Mindlin shells. For more information, see About the MIND Mesh Associated Data property (Simcenter Samcef).
Element Attributes
User Element Attributes (AEL card)	Lets you specify a free user text to be output as an .AEL command. This command is output after all the .AEL cards for the model's properties.Note: The software does not check if parameters defined in the free text string will overwrite .AEL parameters that are already defined in the model.Note: The added text must be compliant with the Samcef Command Language terminology. For more information, see the Samcef documentation.
Non-linearities (NLIS)	Determines whether Samcef ignores or processes geometrical nonlinearities. Use Taken Into Account to take them into account or use Ignore to ignore them.If you set proportional damping on the physical properties of the mesh (Solid dialog box), and the Geometric Nonlinearities Not Taken Into Account (.SAM NLIS) check box is cleared, select Ignore. Otherwise, when you export, a warning message is issued that stiffness damping (.AMO ALPHA) is not taken into account.
Incompressible Condition (BULK) (solid elements)	Determines the solid element's integration schemes for the deviatoric and volumetric parts of the constitutive law. You can choose the Linear, Bilinear/Trilinear, or Bilinear/Trilinear (log law) scheme. By default, no scheme is selected (None).
Samcef Mesh Attribute (.MAI ATT)	By default in the Samcef input file, an .MAI attribute is automatically defined for each mesh. You can override this default with this parameter.
*VolumeMass*Surface Flux (FLU)****Surface Convection (SCON)**Surface Radiation (SRAD)	Properties of the thermal nodal capacity element.For more information, see the Samcef online documentation.
Line Loads Apply On Shear Center (LSHR)	Applies to 1D beams.By default, loads on beams act on the section centroid. Select Line Loads Apply On Shear Center (LSHR) to apply the loads on the shear center instead.
Section Orientation
Applies to 1D beams.
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 to an axis of the absolute coordinate system or to a vector you select on the 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 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	Lets you select the 1D element to which the orientation and offsets will be applied.
Element Axis	Specifies the axis of the element coordinate system to orient (Y-axis or Z-axis).
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.
Reverse Direction	Reverses the direction of the vector.
Section Offsets
Applies to 1D beams.
Offset End B = Offset End A	Both ends of the cross section use the same offset.
End A****Specify Section Location	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 the section centroid. 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.
Offset to Point on Section	Lets you enter specific offset values in the Y and Z directions (of the element coordinate system) from the specified point on the section.
Pin Flags/End Releases – End A/End B	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.
Mesh Properties
Available for 2D meshes.
Export Mesh to Solver	Controls whether the software includes the 2D mesh data in your solver input file when you export or solve the model. If you plan to only use this 2D mesh as a seed mesh for a 3D mesh, clear this option.
Preview
Available when specifying the material orientation for 3D and 2D elements.
Preview	Temporarily displays the material orientation vector graphics on the elements. Lets you preview the vector graphics before you apply the material orientation changes to a mesh.

Note:

For the Mesh Associated Data for the Rigid Link element, see Rigid link mesh associated data properties (Simcenter Samcef).

For the Mesh Associated Data for the Bush element, see Bush mesh associated data properties (Simcenter Samcef).

For the Mesh Associated Data for the Concentrated Mass element, see Mesh Associated Data dialog box (Simcenter Samcef concentrated mass).

For the Mesh Associated Data for the Rigid element, see Rigid body RIGA element (Simcenter Samcef).

For the Mesh Associated Data for the Spring Damper element, see Mesh Associated Data dialog box (Simcenter Samcef spring damper).

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 Samcef), 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 } });