(800) 566-9190 Contact Us Follow SimuTech Group on LinkedIn Follow SimuTech Group on Facebook SimuTech Group’s Twitter account SimuTech Group’s YouTube Channel

SimuTrain® is ANSYS training on demand!

  • Basic & Advanced Level Training Modules
  • ANSYS & SimuTech Training Videos
  • Lectures, Tutorials & Workshops
  • 1 hour Web-based ANSYS Sessions to Practice Hands-on Workshops

Learn more about SimuTrain or get started today by purchasing your subscription.


Follow SimuTech Group on LinkedIn Follow SimuTech Group on Facebook Follow SimuTech on Twitter SimuTech Group’s YouTube Channel

Creation of a Path between Nodes in ANSYS® Mechanical (Workbench) v14.5

ANSYS Node Path 1

Figure 1: ANSYS Mechanical (Workbench) Model with a Path for Stress Linearization



ANSYS Mechanical (Workbench) has a Construction Geometry object to let a user insert a Path or a Surface. A means of creating a Path between nodes of a meshed model is reviewed in this article.

Create a Path for Results Review in ANSYS Mechanical (Workbench)

A user can place a Path along an Edge in WB Mechanical, or between two points. The Two Points approach can use vertices, or model face locations. To start with creation of a Path, a model needs a Construction Geometry branch:

ANSYS Node Path 2

Figure 2: Addition of a Construction Geometry Branch at the Model Level


One or more Paths or Surfaces can be inserted into the Construction Geometry branch:

ANSYS Node Path 3

Figure 3: Insertion of a Path


The user must enter Details for a new Path to complete its definition. The path should be named appropriately.

Before proceeding, if the use of two nodes to define a Path is wanted, it helps to make the mesh visible:

ANSYS Node Path 4

Figure 4: Show Mesh to Aid in Selecting Path Points


After clicking on the Path entry in Construction Geometry, a Path Type based on “Two Points” can be selected. That requires definition of the Start and the End points for the path:

ANSYS Node Path 5

Figure 5: The Two Points Method of Path Definition


“Two Points” typically selects two vertices. A toolbar icon can be used to select locations on faces in the model:

ANSYS Node Path 6

Figure 6: Hit Point Coordinate for the Two Points Method for Path Definition 


Each of the two points can be defined in turn. First the Location of the Start is chosen:

ANSYS Node Path 7

Figure 7: Click on the "Click to Change" Line for Location


The “Click to Change” box changes to provide an Apply button:

 ANSYS Node Path 8

Figure 8: Click to see the Apply Button


Then, go to the graphics window to click on a location for the first point on the path. Rotate and zoom the model so that the element faces where the first node is to be chosen are visible, as illustrated below.

Click very close to the first node to be chosen, zooming as required:

ANSYS Node Path 9

Figure 9: Clicking Close to the First Node


After clicking on the location on the surface, right-click the mouse, and select “Snap to mesh nodes”...

ANSYS Node Path 10

Figure 10: Snap to Mesh Nodes


Then, click the Apply button for the Start point:

ANSYS Node Path 11

Figure 11: Apply to Define Start Point at Node

Now repeat for the node at the other end of the path. Rotate the model as needed. Click on the Location box for the End point so that Apply appears:

ANSYS Node Path 12

Figure 12: Defining the End Point for the Path


Now click close to the location of interest for the End point, right-click and choose “Snap to Mesh Nodes”, and go back to the Location box and click the Apply button. The path should appear as desired, travelling between two nodes on exterior faces of the model:

ANSYS Node Path 13

Figure 13: The Resulting Path between Nodes


Once the path exists, results of interest can be mapped onto the path for postprocessing purposes, including linearized results that may be of interest when satisfying design codes.

Linearized Stress

A linearized stress can be inserted below the Solution branch for an environment of interest.

ANSYS Node Path 14

Figure 14: Insert a Linearized Stress Results Object


The Path of interest can be chosen by name from a drop-down list in the Details for the linearized result:

ANSYS Node Path 15

Figure 15: Choose the Path of Interest by Name from the Drop-Down List


With a path for data mapping chosen, right-click at the Solution branch, and choose “Evaluate All Results” to see the linearized stress plot and data.

The results of the path linearization can be observed, and optionally promoted to parameters, as needed:

ANSYS Node Path 16

Figure 16: Path Linearized Stress Result


Many paths can be created, and for any given path, many linearized results can be defined and observed.


There are tools in ANSYS Workbench Mechanical that permit Paths for stress linearization to be created between node pairs, not just between pairs of vertices, or along edges in a model. Turning on a mesh view with “Show Mesh”, and using “Snap to Mesh Nodes” makes it possible to position the desired path Start and End point so that the path terminates at existing nodes in the model.

Objects for reviewing linearized results on paths can be inserted for postprocessing at the Solution branch in the Workbench Mechanical Outline. Various solution results can be mapped onto each of the paths created in a model. The stress linearization output should help in the satisfaction of various design codes of interest to a user.

Looking for more ANSYS Tips & Tricks?

Check out 300+ more videos and articles on our SimuTrain® Portal.

Get SimuTrain Now!