Managing elements in Coupled Thermal-Structural analyses

Use the following information to help you manage elements in Coupled Thermal-Structural and Dynamic Coupled Thermal-Structural analyses.

Using conventional shell elements in both Coupled Thermal-Structural and Dynamic Coupled Thermal-Structural analysis

• Both homogenous and composite shells are supported. Use the Shell Section Physical Property Table to define properties of homogenous shells. Use the Basic Laminate Physical Property Table or Laminate Physical Property Table to define multilayer shells.

• Shell section controls are supported for S4RT elements in Coupled Thermal-Structural analysis.

• Specify the material orientation coordinate system for material calculations in the Shell Section Physical Property Table or in the Mesh Associated Data dialog box. In the Mesh Associated Data dialog box, tangent curve and vector are also available.

• Specify constant shell thickness in the Shell Section Physical Property Table. In the Mesh Associated Data dialog box, you can activate midsurface thickness (*NODAL THICKNESS keyword). You can plot the thickness contours.

• Shell mass properties are computed and can be viewed in the Solid Properties data.

Using plane strain elements

In a Coupled Thermal-Structural analysis

For all 4-node bilinear elements (CPE4T, CPE4HT, and CPE4RT, and CPE4RHT), the software exports hybrid meshes (in the 2D Mesh dialog box, the option Attempt Quad Only is set to On-Single triangle) with transition element CPE3T.The software exports 8-node biquadratic elements CPE8T and CPE8RT with transition element CPE6MT, and CPE8RHT with CPE6MHT.   Mesh information displays the Pre/Post topology: The Quad8 Plane Strain XXY elements corresponds to CPE8xT Abaqus elements.The Tri6 Plane Strain XXY elements correspond to CPE6xT Abaqus elements.    Specify the material orientation coordinate system for material calculations in the Solid 2D Plane Physical Property Table. In the Mesh Associated Data dialog box, tangent curve and vector are also available. Abaqus requires the x and y directions to lie on the surface formed by the plane strain elements; otherwise, the solver issues an error message. For more information, see Material orientation. Specify constant thickness in the Solid 2D Plane Physical Property Table or derive it from the midsurface. If the midsurface does not have a constant thickness, the software does not export the thickness data. Abaqus does not support variable thickness on a nodal basis for plane strain elements.

In a Dynamic Coupled Thermal-Structural analysis

CPE4RT is exported with CPE3T in hybrid meshes. Specify the material orientation coordinate system for material calculations in the Solid 2D Plane Physical Property table or in the Mesh Associated Data dialog box. In the Mesh Associated Data dialog box, tangent curve and vector are also available. Abaqus requires the x and y directions to lie on the surface formed by the plane strain elements; otherwise, the solver issues an error message. For more information, see Material orientation. Specify constant thickness in the Solid 2D Plane Physical Property Table or derive it from the midsurface. If the midsurface does not have a constant thickness, however, the software does not export the thickness data. Abaqus does not support variable thickness on a nodal basis for plane strain elements.

Using plane stress elements

In a Coupled Thermal-Structural analysis

For hybrid meshes, the software exports element CPS4T and CPS4RT with CPS3T as the transition element. The software exports elements CPS8T and CPS8RT with CPS6MT as the transition element.

In a Dynamic Coupled Thermal-Structural analysis

The software exports element CPS4RT with CPS3T as a transition element.

Generalized plane strain elements in a Coupled Thermal-Structural analysis

• The following table provides a summary of the export behavior for hybrid meshes. The parent element refers to the element selected (including element formulation option when meshing with Set Attempt Quad Only set to On-Single triangle):  Parent elementTransition elementCPEG4TCPEG3TCPEG4HTCPEG3HTCPEG4RTCPEG3TCPEG4RHTCPEG3HTCPEG8TCPEG6TCPEG8HTCPEG6MHTCPEG8RHT****CPEG6MHT

• Mass property calculation is not supported for generalized plane strain elements.

• A Coupled Thermal-Structural analysis requires additional attributes in the Generalized Plane Strain Physical Property Table:Length of Fiber Passing Through Ref. NodeLength of the axial material fiber connecting the node and its image in the other bounding plane.Angle Between Bounding Planes, X-axis****Angle Between Bounding Planes, Y-axis

Axisymmetric solid elements

• In hybrid meshes, the software exports CAX4RT with CAX3T as the transition element.

3D solid elements

In a Coupled Thermal-Structural analysis

For hybrid meshes, the software exports all 8-node trilinear elements (C3D8T, C3D8HT, C3D8RT, and C3D8RHT) with transition element C3D6T. In coupled thermal-structural solutions, 3D solid laminates are not allowed; therefore, Solid Section is the only physical property table available. Specify the material orientation coordinate system for material calculations in the Solid Section Physical Property Table or in the Mesh Associated Data dialog box. In the Mesh Associated Data dialog box, tangent curve and vector are also available. If you select Spatial Field, you can select the *Use Distribution to Define Local CSYS check box so the software exports material orientation vector (MOV) data in a compact way using the *DISTRIBUTION keyword.

In a Dynamic Coupled Thermal-Structural analysis

No hybrid meshes are available in an explicit analysis (C3D6T is not available). Therefore, the software cannot export C3D8T and C3D8RT with transition element C3D6T).In coupled thermal-structural solutions, 3D solid laminates are not allowed; therefore, Solid Section is the only physical property table available. Specify the material orientation coordinate system for material calculations in the Solid Section Physical Property Table or in the Mesh Associated Data dialog box. In the Mesh Associated Data dialog box, tangent curve and vector are also available. If you select Spatial Field, you can select the *Use Distribution to Define Local CSYS check box so the software exports material orientation vector (MOV) data in a compact way using the *DISTRIBUTION keyword.

Continuum shell elements in a Coupled Thermal-Structural or Dynamic Coupled Thermal-Structural analysis

• Homogenous continuum shells are supported.

• Use the Continuum Shell Section Physical Property Table to specify shell cross-section properties.

• Specify the material orientation coordinate system for material calculations in the Continuum Shell Section Physical Property Table or in the Mesh Associated Data dialog box. In the Mesh Associated Data dialog box, tangent curve and vector are also available.

Learn more

Types of coupled thermal-structural analyses (Abaqus)

Coupled thermal-structural analysis (Abaqus)

Dynamic coupled thermal-structural analysis (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Managing elements in Coupled Thermal-Structural analyses, 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 } });