Shell thickness

Video: Define shell mesh and element thickness

You can define the thickness of 2D shell elements as a constant value, an expression (for more information about expressions, see Expressions), or as a field. You can define it in several places, depending on your solver and your needs.

Property	Where defined	Priority	Notes
Corner Node Thickness	Element Associated Data dialog box	Overrides the midsurface thickness and the Default Thickness defined at physical property level.	Available only for Simcenter Nastran, ANSYS, Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal.For ANSYS, this value is stored in the R or RMORE command in the ANSYS input file. If you import an input file, R commands will be translated to the physical property table rather than element-associated data. For Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal, this property is available only for 2D shell collectors with Type set to Thin Shell or Multi-Layer Shell Uniform.Defines the thickness at all corners of the element or at selected nodes.Is stored with the element. You can view the thickness value using the Element Associated Data→List command. Is not used when you clear the Use Element Associated Data check boxIn the Mesh Associated Data dialog box for Simcenter Nastran or ANSYS.In the Mesh Collector dialog box for Thermal/Flow, Electronic Systems Cooling, or Space Systems Thermal.
Midsurface thickness	Geometry	Overrides the Default Thickness specified in the physical properties. Is used if no thickness is defined in the element-associated data.	Is calculated from the geometry from which the midsurface was generated. Is used when Midsurface is selected as the Thickness Source in the Mesh Associated Data dialog box. Is written out to the solver input file when you solve the model. In Pre/Post, you can create special displays to view the distribution of midsurface thickness values across the mesh. For more information, see Creating displays to validate element thickness.
Default Thickness	Physical property table (for example, the PSHELL dialog box if you are using Simcenter Nastran)	Is used when no thickness is defined in the element-associated data.	A Default Thickness value is required regardless of whether you are using the midsurface thickness or element-associated data. Is used when Physical Property Table is selected as the Thickness Source in the Mesh Associated Data dialog box. For Simcenter Nastran, is written out on the PSHELL bulk data entry.For ANSYS, is written out using the SHELL command. For Abaqus, is written out using the *SHELL SECTION keyword. For Simcenter Samcef, is written out on the .PHP THICK input file entry.
Thickness	Physical property table	Is used when no thickness is defined in the element-associated data.

Setting default options for mesh associated data thickness

You can use customer defaults to control the default settings for thickness options in the Mesh Associated Data dialog box.

• Use the Thickness Source option to set the default source for the thickness data for the elements in the mesh, such as Midsurface or Physical Property Table.

• Use the Thickness Evaluation Type default to set the default location at which the software evaluates midsurface thickness data, such as At Element Centroid or At Every Node.

To set these Shell Thickness Data defaults, in the Customer Defaults dialog box, select Simulation→Pre/Post→Meshing→General tab.

Learn more

Physical properties and element attributes

Editing mesh and element properties

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Shell thickness, 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 } });