Engineering analysis + design software

User Area > Advice

Connectivity - How to Spot Problems and Fix Them

Connectivity problems are a common type of modelling error in finite element analyses, often leading to unintended structural behaviour in a model and causing warnings and errors in the solution regarding the condition of the stiffness matrix.

In finite element analysis, elements are principally connected by sharing common nodes at their boundaries or corners. Each matching nodal degree of freedom for compatible elements at a shared node is rigidly linked. Whilst there are other valid methods of connecting elements (such as slidelines and constraint equations), this page summarises the different methods of checking a model for fundamental connectivity in terms of shared nodes between adjacent elements and then how to fix them.  There is also a more comprehensive Technical Note (number 1036, "Connectivity - How to Spot Problems and Fix Them?" ) that compliments this page, which can be downloaded from the following page:

LUSAS Technical Notes

This gives further details of these approaches and is illustrated with some examples to demonstrate them.

LUSAS is a feature based Modeller; meaning that we define the geometry of the structure first and then allow LUSAS to create a mesh of elements and nodes within the enveloped form that the geometry defines. Therefore to ensure connectivity of the underlying mesh, the following principles apply to the geometry features:

  • For volumes to be fully connected they must share a common surface
  • For surfaces to be fully connected they must share a common line
  • For lines to be fully connected they must share a common point

Connectivity checks can therefore be done at the geometry level as well as at the mesh level.

Checking Connectivity

1. Checking Higher Order Features with Datatips

Higher order features of a selected item can be checked quickly by hovering the cursor over the selected item in the graphics window and a datatip will appear. To check that two adjacent surfaces are connected at a shared line, the line can be selected and the datatip can be checked as listing the two surfaces as being defined by the line.

2. Selected Items and Cyclable Items

Selected Items and Cyclable Items windows can be used to interrogate regions of geometry and mesh.  To check the items that are in the current selection, a window can be displayed showing the Selected Items. This can be accessed via:

View menu > Browse Selection... (or Selection Panels and then Selection in V16 onwards)

A window will appear on the screen which will list all the selected items.

This tool can be useful to check mesh connectivity by, for example, box selecting an area that should contain one node/point and to check that there is not more than one. This window can be ‘docked’ in the Modeller window frame if it is to be made permanently visible.

3. Viewing the Mesh as an Outline Plot

Turning off the Geometry layer and other layers and then viewing the Mesh layer as an Outline only set in the Mesh layer Properties can help to identify disconnected surface or volume mesh.

The mesh outline plot will show lines at the mesh boundaries, splits, creases, joins and other significant changes of angle, as well as the locations of bar or beam elements.

4. Check the Deformed Mesh

A simple analysis of the model can be run as an initial check, for example a linear static analysis for self weight and then the Deformed Mesh can be inspected with a specified factor of deformation. 

View menu > Drawing Layer > Deformed Mesh

If parts of the model are totally disconnected and unsupported, they will be displayed evidently having been displaced from the model under free body motion.

For partially connected parts of the model, the Deformed Mesh viewed for a specified magnitude will reveal splits in the mesh or unexpected deformations due to connectivity problems.

5. Geometry Layer – Colour by Connectivity

In the Properties of the Geometry layer there is a setting to Colour by "Line/Surface Connectivity".  Please see the following references for further information:

Help menu > Help Topics > Contents > Modeller Reference Manual>Chapter 2 - Using Modeller>Using Layers

Help menu > Help Topics > Contents > Modeller Reference Manual>Chapter 4 - Model Geometry>Visualising Geometry

6. Mesh Layer – Colour by Connectivity

Similarly, the mesh can be coloured to check connectivity. This is set via the Properties of the Mesh layer using the Colour by option set to "Connectivity". This will show how many elements are connected to each node (by colour coding the nodes) and how many elements are connected to each element edge (by colour coding the element edges with the same key).

7. Using a Labels Layer

The Labels layer can be useful for identifying any duplicated or overlapping geometry. For example where two points occupy the same location rather than one.

8. Checking the Distance between Points

Coincident points within a small region of the model may be identified by selecting a small number of points and then by going to:

Geometry menu > Point > Distance Between Points

This will give the distances between each possible pair of points for the selection, which may help in finding the two closest points for a small number of selected points.

9. Feature Properties – Checking a Geometry Feature’s Hierarchy

The Properties of a geometry feature, such as a line for example, can be accessed by selecting a single feature and then right-click and choose Properties from the context menu. The Hierarchy tab can be viewed to establish a line’s lower order points and higher order surfaces.

10. Using Advanced Selection

Advanced Selection enables the current selection to be filtered for a particular feature number, element name, stress model or geometric or material attribute. 

Edit menu > Advanced Selection

The Advanced Selection dialog may also be activated from the graphics window context menu (by right-clicking in blank space). For checking connectivity of two coincident points, for example, one point could be selected and Advanced Selection used to select higher order features to see what each point is connected to.

11. Using Visibility

Features may be made visible by:

  • Selecting All Visible from the context menu activated from the graphics window (right-click in blank space > All Visible)
  • Making a group visible from the Groups tab of the Tree View (right-click on a group > Visible or Set as Only Visible)
  • Making features assigned with a selected attribute visible from an attribute's context menu in the Attributes tab of the Tree View (right-click on a attribute > Visible or Set as Only Visible)
  • Using the Advanced Visibility dialog activated from the graphics window context menu (right-click in blank space > Advanced Visibility)

The Advanced Visibility dialog allows fine control on the visible items by controlling the visibility of higher order and lower order features. This allows all lines attached to a point to be made visible or all surfaces connected to a line to be made invisible.  

Correcting Connectivity Problems

Having used the methods given in the previous section to check connectivity, this section now moves on to look at ways of resolving the connectivity problems found.

1. Merging Coincident Features

Coincident features will merge automatically by default or can be made to merge by selecting them and going to:

Geometry menu > Point/Line/Surface > Make Mergable first, and then Merge

The default Merge Action is “Exact”, where features are merged only if all assignments are identical.  Please see the following reference for further information:

Help menu > Help Topics > Contents > Modeller Reference Manual > Chapter 4 - Model Geometry > Merging and Unmerging Features

To ensure that the assignments intended for the geometry are correct and remain after merging, it is recommended to allow merging with the merge action set to “Exact” and to assign attributes to all intended geometry.  Geometry can also be constructed and merged as necessary prior to the assignment of attributes avoiding anything not merging due to differing assignments.

2. CAD Export Settings

The required precision of geometry defined for an FEA analysis is much finer than that generally required for CAD modelling.  Consequently CAD packages tend to have a much coarser default modelling tolerance than an FEA package.  In the CAD package used, the modelling tolerance should be set prior to creating and exporting geometry.  The tolerance set should be as tight as is reasonable, but ideally comparable to the default merge tolerance in Modeller of 1.0E-6.

3. Ensuring Elements Sharing Nodes have Compatible Nodal Freedoms

Please see the page Rules for connecting elements on our user area for further details.  Also see the following reference which summarises the nodal freedoms of each element (as well as other properties):

Help menu > Help Topics > Contents > Element Reference Manual > Element Summary Tables

4. Splitting Geometry

Where there are overlapping lines, the simple solution is often to split a line at a point.  To do this, the line and a point part way along it are selected and then the following menu item is used to split the line into two at that point:

Geometry menu > Line > By Splitting > At a Point…

Similarly, a surface can be split at a line.  To do this, a surface and a line (which completely spans across the surface) are selected and then the following menu item is used to split the surface into two at that line:

Geometry menu > Surface > By Splitting > By Line…

Also see the following reference for further useful geometry operations that can be used to split lines, surfaces or volumes:

Help menu > Help Topics > Contents > Modeller Reference Manual > Chapter 4 – Model Geometry > Points/Lines/Surfaces/Volumes

5. Redefining Geometry

Depending on the complexity of the model and the extent of connectivity issues found, the analyst may judge it to be more practical and take less time to redefine geometry in Modeller to resolve connectivity issues, rather than to try and fix them.  With regard to redefining geometry or creating it from scratch, the following recommendations are given:

  • Complete the import, manipulation and any editing of geometry before making any assignments (including mesh) if possible
  • Try to create all surfaces such that they are defined by 3 or 4 lines only
  • Plan the geometry required in terms of the features to be modelled, the assignments to be made, results to be extracted and the areas where the mesh may need to be controlled/refined
  • Use the Move, Copy and Sweep commands

Please see the example referenced below which demonstrates this recommended approach to building up geometry.

Help menu > Help Topics > Contents > Application Examples Manual (Bridge, Civil & Structural) > Buckling Analysis of a Plate Girder

The use of scripting in LUSAS is very helpful for automating repetitive tasks and a number of example scripts are provided to download from our User Area. For example, one of the scripts provided on this page will automate the redefining of multiple surfaces from a large selection of lines “Create Multiple Surfaces from a Large Selection of Lines”.  Also the scripts “Check and Detect Short Lines” and “Select Nearby Features” can be helpful when dealing with connectivity issues.


innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.