(844) 825-5971
• Home
• Support
• Tips & Tricks
• FEA
• ANSYS Workbench Mechanical: Averaged vs. Unaveraged Contour Results

### ANSYS Tips & Tricks

Want to get the latest “tips & tricks”? Sign-up for our monthly newsletter.

# ANSYS Workbench Mechanical: Averaged vs. Unaveraged Contour Results

ANSYS Workbench Mechanical:  Averaged vs. Unaveraged Contour Results

Have you wondered what other tools may be useful in determining the quality of your results?  In addition to the convergence tools, you can also use contour results to help ensure quality results.  Normally, contour results in the Mechanical application are displayed as averaged results.  Each element calculates a unique, elemental nodal stress which is typically different than the other elements connected to that node.  Averaged contours will average elemental nodal results across element and geometric discontinuities but will never average results across bodies.  Some results can also display as unaveraged contours.

You can change the averaging on contour results by setting the Display Option field, shown in the figure below, to one of the following:

• Unaveraged: Displays unaveraged results.
• Averaged: Displays averaged results.
• Nodal Difference: Computes the maximum difference between the unaveraged computed result (for example, total heat flux, equivalent stress) for all elements that share a particular node.
• Nodal Fraction: Computes the ratio of the nodal difference and the nodal average.
• Elemental Difference: Computes the maximum difference between the unaveraged computed result (for example, total heat flux, equivalent stress) for all nodes in an element, including midside nodes.
• Elemental Fraction: Computes the ratio of the elemental difference and the elemental average.
• Elemental Mean: Computes the elemental average from the averaged component results.

The Nodal Difference, Nodal Fraction, Elemental Difference, and Elemental Fraction aid in determining mesh quality.  If there are large differences in results calculated by elements attached to shared nodes, then a refined mesh in that region may be necessary.

The Elemental Mean will create a checkerboard of results where each element will have one value.  The behavior is similar to the ETABLE feature within ANSYS Mechanical APDL.  Results can be exported to Microsoft Excel and subsequent calculations, such as summations, can be performed.