Multiphysics > Meshing for Pre/Post Multiphysics analyses

Cohesive elements

Cohesive elements are specialized 3D elements with zero thickness that you can use to model specific types of damage and failure. You can create cohesive elements between pairs of geometric surfaces in the Simcenter 3D Multiphysics and Simcenter Samcef environments. You can also create cohesive elements when modeling laminates in the Simcenter Samcef environment. For more information, see Cohesive layers.

For example, you can use cohesive elements to:

Model phenomena such as delamination between plies in a laminate composite.
Join two surfaces, such as adhesively bonded surfaces. Cohesive elements offer several advantages over traditional glue-type connections. For example, with cohesive elements, you can account for compliance in the connection as well as damage in the cohesive material.

You can create cohesive elements as a thin layer between two coincident or nearly coincident surfaces, as shown in this graphic. This model includes one layer of cohesive elements between two meshes of solid elements that represent a double cantilever beam. This model includes loading conditions that are designed to pull the beams apart and cause cohesive failure.

Supported element types

In the Simcenter 3D Multiphysics environment, you can create linear and parabolic hexahedral cohesive elements that have a thickness of zero or close to zero. In the Simcenter Samcef environment, you can create cohesive elements with a real thickness value.

Simcenter 3D Multiphysics	Simcenter Samcef environment
Linear cohesive hexahedron (Simcenter Nastran CHEXCZ bulk data entry)	Cohesive (T147)(8)
Parabolic cohesive hexahedron (Simcenter Nastran CHEXCZ bulk data entry)	Cohesive (T147)(20)

Additionally, the software may also create linear or parabolic pentahedral cohesive elements (CPENTCZ) as needed for transition areas. You cannot manually create pentahedral cohesive elements.

Creating cohesive elements

Typically, you create a single layer of cohesive elements between two sets of 2D elements or between the faces of two sets of 3D elements. You can create the cohesive elements in several ways:

You can use the 3D Swept Mesh command with the Type list set to Manual Between to create one layer of cohesive elements between specified source and target faces. If the source and target faces are coincident, the software generates cohesive elements that have a thickness value of zero.Note: The software does not check the generated cohesive elements for possible degenerative elements.
You can use the Element Extrude command with the Type list set to Element Faces to create cohesive elements manually.Note: The software does not check the generated cohesive elements for elements that have a length of zero.
You can use the Layup Modeler dialog box to create cohesive layers between plies in a global layup.
You can use the Laminate Modeler dialog box to create cohesive layers between plies in a laminate physical property.

Defining material and physical properties for cohesive elements

Use the Cohesive Property dialog box to define the properties for the cohesive elements. You can specify:

The material to use for the elements. You can use an Isotropic, Orthotropic, or the Damage Interface type of material for cohesive elements. Use a Damage Interface material to obtain estimates of material damage during the solve. You can use options in the Damage Interface Material dialog box to specify, for example, the damage estimation model to use as well as specify the threshold.For more information, see Multiphysics Damage Interface material and Damage Interface material (Simcenter Samcef).
The material orientation for the elements.
The thickness of the elements.

In the Multiphysics environment, the options in the Cohesive Property dialog box correspond to the fields on the PSOLCZ bulk data entry for Simcenter Nastran.

Cohesive element support in the Multiphysics thermal solver

The thermal solver treats cohesive elements as solid elements. When the thickness is zero or the material is set to Damage Interface, the thermal solver assumes perfect contact between the upper- and lower-face boundary elements. Cohesive elements do not participate in radiation calculations.

Obtaining results for cohesive elements

During the solve, the software calculates results for cohesive elements at the corner nodes. For example, you can calculate:

Damage values, if you use a Damage Interface material.
Surface tractions.
Relative displacements.

To request results output for cohesive element results:

In the Simcenter 3D Multiphysics environment, select the Cohesive Element Results page in the Structural Output Requests dialog box and then select Enable CZRESULTS Request.
In the Simcenter Samcef environment, in the Structural Linear Output Requests and Structural Nonlinear Output Requests dialog boxes: Use options on the Composite Stress and Composite Strain pages to request that the software calculate interlaminar stress tensors as well as mechanical and total strain tensors.Use options on the Damage page to request that the software calculate damage values, provided that you use a Damage Interface material.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed partSimcenter 3D Multiphysics as the specified solver and the analysis type set to Structural, Coupled, or ThermalorSimcenter Samcef as the specified solver and the analysis type set to Structural

Learn more

2D meshes for Multiphysics structural solutions

Chocking elements

Look up more details

Multiphysics elements

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area