Working with ANSYS SOLID186 and SOLID187 elements

There are special considerations for working with ANSYS SOLID185 and SOLID186 elements in Pre/Post.

Creating degenerative SOLID186 tetrahedron elements

You can create a special degenerative tetrahedral type of SOLID186 element in Pre/Post. In ANSYS structural analyses, SOLID186 elements are hexahedral elements, but their nodes can be combined to degenerate them into tetrahedral, pyramids, or wedge elements. The degenerative tetrahedral type of SOLID186 elements is an alternative to SOLID187 tetrahedral elements.

To create the degenerative tetrahedral type of SOLID186 elements in Pre/Post:

1. Use the 3D Tetrahedral Mesh command to create a mesh of SOLID187 parabolic tetrahedral elements.

2. Edit the mesh associated data for the mesh of SOLID187 elements. In the Mesh Associated Data dialog box, use the Element Type list to select SOLID186 (Degenerative)

Note:

The Element Type list also includes the SOLID95 (Legacy, degenerative) option. This option is listed to support the import of legacy ANSYS input files that may include degenerative SOLID95 elements.

Support for SOLID185/186 hexahedral element connections

In ANSYS, SOLID186 elements (parabolic hexahedral element with 20 nodes) and SOLID185 elements (linear hexahedral element with 8 nodes) can be connected through a shared element face and four shared corner nodes. When these elements are connected, ANSYS typically removes the four midside nodes of the SOLID186 element to create a hexahedral element with 16 nodes.

When you model includes SOLID186 elements that are connected to SOLID185 elements through a shared element face, you can use the Remove midside nodes on export option in the Mesh Collector dialog box to control whether the software automatically removes the midside nodes of the SOLID186 elements during the export process. Select this option to remove the midside nodes and create a hexahedral element with 16 nodes. You should store the SOLID186 and SOLID185 meshes in the same mesh collector in the Simulation Navigator.

• You can connect up to three faces of a single SOLID186 element to adjacent SOLID185 elements. However, as a best practice, you should generally only connect a single face of a SOLID186 element to a single, adjacent SOLID185 element.

• If you select the Remove midside nodes on export option in the Mesh Collector dialog box for a selected Solid collector, the software checks all meshes in that collector for SOLID186 and SOLID185 elements that share faces. Note: You should store only meshes that have SOLID186 and SOLID185 elements that share faces in the Solid mesh collector. You should not store other types of meshes in this collector

• When you export the ANSYS input file, the software merges the corner nodes of the shared face between the SOLID186 and SOLID185 elements if the nodes are coincident.

• When you import SOLID186 and SOLID185 elements that share faces, Pre/Post uses linear interpolation to create midside nodes for the SOLID186 elements. This changes each SOLID186 element to a 20 node hexahedral element.

• The software does not preserve the SOLID186 and SOLID185 mesh collector data when you export an ANSYS input file and then re-import the same file. When you re-import the file, Pre/Post does not always place the associated SOLID186 and SOLID185 meshes in the same mesh collector, even if the corner nodes at the shared face between the elements are coincident. When this occurs, you must manually place the appropriate SOLID186 and SOLID185 mesh pairs in the same mesh collector.

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 SOLID 272 and SOLID 273 elements

Working with ANSYS contact elements

Working with ANSYS MESH200 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 SOLID186 and SOLID187 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 } });