Checking for duplicate elements and nodes

Use the Duplicate Nodes and Duplicate Elements commands to check whether your model contains any coincident elements or nodes. Coincident elements or nodes are considered duplicates.

Checking for duplicate nodes

Use options in the Duplicate Nodes dialog box to detect and merge duplicate nodes. The software only merges nodes of identical types. For example, the software does not merge a midnode with an end node.

The following graphic shows an example of how the Duplicate Nodes command graphically indicates the location of duplicate nodes.

The ability to detect and merge duplicate nodes is particularly useful when you are working with:

• Assembly models.

• Models that contain multiple meshes.

If you try to solve a model that contains coincident nodes, singularities or other rigid body motion errors can occur during the solve.

You can also use the Duplicate Nodes command to merge coincident nodes to join adjacent component FEMs in an assembly FEM. For more information, see Merging component nodes with the Duplicate Nodes model check command.

Understanding how the software merges duplicate nodes

When the software merges nodes, it uses the following set of rules to determine which node to merge and which node to retain.

Note:

The software cannot merge nodes that are connected to superelements.

• In an assembly FEM, an occurrence of a node takes precedence over a node at the assembly-level.

• A node that is defined on geometry takes precedence over a node that was either created manually or is associated with a manually created element.

• A node that is defined on polygon geometry takes precedence over a node that is defined on wireframe geometry.

• A node that is created at a Mesh Point location takes precedence over a node that is related to the Mesh Point geometry.

Checking for duplicate elements

Use options in the Duplicate Elements dialog box to detect and delete duplicate elements. The software evaluates all elements that have the same topology (for example, 1D, 2D, 3D). This means, for example, that the software considers a Nastran CBEAM element and a 2-noded RBE2 element to be duplicates when they exist at the same location and uses the same pair of nodes to define their connectivity.

Depending on the Display Settings you select in the Duplicate Elements dialog box, if your model contains duplicate elements, the software:

• Temporarily highlights the duplicate elements in magenta in the graphics window.

• Lists the labels of all duplicate elements and the shared (vertex) nodes in the Information window.

• Places all duplicate elements into an output group in the Simulation Navigator.

The Duplicate Elements command is helpful when, for example, your model contains multiple 1D connections. You can validate that those 1D connections are defined appropriately before you solve.

For example, in the Nastran environment, a CELAS1 element is defined with two nodes, each with one DOF. If you connect two different components that are meshed with solid elements with CELAS1 elements, you need three CELAS1 elements defined on the same set of nodes to fully define the connection. In the following graphic, the Duplicate Elements option was used to identify multiple, coincident CELAS1 elements in a larger assembly FEM.

If the software identifies any duplicate elements, you can optionally choose to delete one of those elements. In the Duplicate Elements dialog box, you can use the Preference list in the Deletion Settings group to specify, for example, whether you want the software to retain the element with the higher or lower label (ID).

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM file active
Command Finder	Duplicate Elements or Duplicate Nodes

Learn more

Checking your finite element model

Checking for free and non-manifold element edges

Aligning the first edges of 2D elements

Checking and orienting the directions of 1D elements

Checking and orienting the normals of 2D elements

Checking and orienting the normals of 3D element faces

Checking aerodynamic panel meshes

Detecting interference and clearance issues between faces

Checking CAE model consistency

Checking the association of nodes to geometry

Checking the completeness of your model prior to a solve

Computing mechanical loads

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Checking for duplicate elements and nodes, 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 } });