Accessing Results on Shell and Layer Elements

You can access results on shell and layer elements. A shell element is a specific case of a layer element. It is simply a layer element that has only one layer.

For a shell or layer element, the results can have different shapes, depending on the data location. Results can be nodal, element nodal, or elemental.

For a nodal location, values are localized at each node of the element. No additional specification on the shape or position is necessary.
For an element nodal location (such as stress), results are available on four positions: Top, Bottom, Middle, and Top/Bottom. You must specify the position for which to access result values. The default position is Top/Bottom.
For an elemental location (such as bending stress), the result for the different components is given by one value by element.

The result reader has a property LayeredSolidStressStyle that you use to specify the shape for the required result. The default value is Top/Bottom.

For a layer element, the result reader has the property Layer that you use to specify the layer number for the required result. The layer number is 0 by default, which is equivalent to selecting Entire Section in the Mechanical interface.

The following table shows how to specify the properties LayeredSolidStressStyle and ShellPosition, depending of the result required.

Result Type Exposed in Worksheet	Location	LayeredSolidStressStyle	ShellPosition
U, R, …	Nodal	(Not Applicable)	(Not Applicable)
S, EPEL, …	Element Nodal	Top/Bottom	Tom, Bottom, Middle, Top/Bottom
BENDING_STRESS, MEMBRANE_STRESS, …	Elemental	Bending, Membrane	(Not Applicable)

The following IronPython functions access a shell element result: stress S for the Y component.

# create a result reader
resultReader = result.Analysis.GetResultsData()

# get the layer number
resultReader.Layer = 0

#specify the shape of the result
resultReader.LayeredSolidStressStyle = StressStyle.TopAndBottom

# select the shell position 
resultReader.ShellPosition = ShellPosition.Top

# set the result reader to get the stress on the Y axis (SY) for the current step
resultReader.CurrentResultSet = stepInfo.Set
stress_result = resultReader.GetResult("S")
stress_result.SelectComponents(["Y"])

# get the elemental values SY on "Top" position on the shell 
for id in resultCollector.Ids: 
    valuesSY = stress_result.GetElementValues(id)
    resultCollector.SetValues(id,valuesSY)

For a shell or layer element with the position set to Top, Bottom, or Middle, the method SetValues must be used:

for id in collector.Ids:
    values = stress_result.GetElementValues(id)
    collector.SetValues(id,values)

For a shell or layer element with the position set to Top/Bottom, the method SetAllValues can be used:

values = stress_result.GetElementValues(collector.Ids,False)
lengths = reader.NumberValuesByElement(collector.Ids)
collector.SetAllValues(lengths,values)

While the code for the method SetAllValues is bit more complicated, this method does offer better performance when setting a large amount of data.

Note: The supplied extension ACTResults defines a toolbar with buttons for calculating custom results for a shell element, a layer element, and a contact. The extension ACTResults combines the next three extension examples into a single extension. The three-button toolbar for it is shown in the figures.