Working with ANSYS MESH200 elements

You define ANSYS MESH200 elements in Pre/Post by editing the mesh associated data of certain element types. MESH200 is a non-structural shell element that does not contribute to the solution. For example, you can use MESH200 elements:

• In multi-step meshing operations, such as extrusion, where you need a lower dimensionality mesh to create a higher dimensionality mesh.

• To temporarily represent discrete reinforcing fibers and smeared reinforcing layers, including their geometry, material, and orientation.

To create MESH200 elements in Pre/Post, edit the mesh associated data for an existing mesh. Then, select the new MESH200 option in the Element Type list in the Mesh Associated Data dialog box. The MESH200 option is available for all element types, except:

• MASS21

• CERIG,CP

• SOLID72

• CE (conductor)

You can use MESH200 elements in conjunction with any other ANSYS element types. You can delete these elements when you no longer need them or you can leave them in your model. These elements do not affect solution results.

Considerations for defining MESH200 elements

• When you export or solve an ANSYS input file that contains MESH200 elements:The software automatically defines the value for KEYOPT(1), which controls the topology of the MESH200 element and its number of nodes. The software uses the element type in the original mesh to set this value.Note: ANSYS does not document its support for solid wedge MESH200 elements. However, Pre/Post can create solid wedge MESH200 elements when the original element type is SOLID185(6) or SOLID70(6) (in Thermal analyses) and SOLID186(15) or SOLID90(15) (in Thermal analyses) by defining KEYOPT(1)=8 or 10, respectively,The software exports all loads, constraints, material, and material orientation settings that you define for MESH200 elements even though the elements are not used in the analysis.The software does not export any physical properties associated with MESH200 elements. When you import MESH200 elements, the software creates placeholder physical property tables.

• The software does not compute mass and mechanical properties for MESH200 elements.

• You cannot import MESH200 elements from a binary results file.

• For 2D MESH200 elements, the software does not display their thickness values.

• The software does not preserve the MESH200 element data if you export a file that contains MESH200 elements and then re-import the same file. When you import MESH200 elements into Pre/Post that you had previously exported, the software uses KEYOPT(1) to determine the element type as follows: KEYOPT(1) valueElement type in Pre/Post after import0 and 2 (beam element with 2 nodes)BEAM188 or LINK33 (Thermal analysis)1 and 3 (beam element with 3 nodes)Unsupported. The importer skips these elements.4 and 6 (triangle or quadrilateral shell with 3 or 4 nodes)SHELL181 or SHELL131 (Thermal analysis), or PLANE55 (Axisymmetric Thermal analysis) or PLANE182 (Axisymmetric Structural)5 and 7 (triangle or quadrilateral shell with 5 or 6 nodes)SHELL281 or SHELL132 (Thermal), or PLANE77 (Axisymmetric Thermal) or PLANE183 (Axisymmetric Structural)For example, if the original element type is LINK180 in Pre/Post, and you modify the mesh associated data to create MESH200 elements, the software sets KEYOPT(1) to 0 when you export the input file. If you later re-import the same file, the software creates BEAM188 elements.

How do I

Manually creating surface effect elements

Manually creating contact elements

Create an ANSYS KEYOPT table

Learn more

ANSYS environment

Working with ANSYS surface effect elements

Applying a flame temperature to SURF152 elements

Working with ANSYS FLUID116 elements

Working with ANSYS MASS21 elements

Working with ANSYS SOLID186 and SOLID187 elements

Working with ANSYS SOLID 272 and SOLID 273 elements

Working with ANSYS contact elements

Modeling cohesive zones with ANSYS interface elements

Specifying user defined KEYOPTs for ANSYS

Requesting output for ANSYS analyses

Previewing ANSYS solver syntax

Customizing ANSYS input files with user defined text

Look up more details

ANSYS elements

Using ANSYS high performance computing options

ANSYS boundary conditions

Working with ANSYS MESH200 elements, 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 } });