Reply To: Creep analysis – Linear and Quadratic mesh

[peteroznewman]

You should do a Mesh Convergence Study to determine the "true" value of stress in the model with the quadratic mesh. Add a Mesh Sizing control on the blend radius and make the element size a Parameter.  Make a Stress Result at the End Time and make the Maximum Equivalent Stress a Parameter.

Open the Parametric Set box from Workbench. Now you can type smaller and smaller element sizes in row after row. Ideally, make the element size a constant ratio such as 1.5 between rows. If the first row has a size of 1.5 mm, then the sequence of sizes is

• 1.5
• 1.0
• 0.6667
• 0.4444
• 0.2963

Click the Update All Design Points and Ansys will automatically run through all these analyses and place the peak stress in the column with the lightning bolts in it, assuming the solution is not prevented by limits of the Student license or the resources of the computer.

Plot those 5 points and extrapolate to a zero element size.  That is the "true" stress for this model.