How to retrieve all stress components for a node selected graphically?

Tasos

My goal is to select a node in the geometry window in Mechanical and then retrieve the six stress components for that node with a script.

Tasos

You can use DPF to retrieve the stress components for a selected node. Here's an example workflow to do this:

Import and initialise the DPF modules:

import mech_dpf

import Ans.DataProcessing as dpf

mech_dpf.setExtAPI(ExtAPI)

Select the node of interest by graphically picking it in the geometry window before executing the script. The following line will retrieve the node ID for that node:

node_id =  ExtAPI.SelectionManager.CurrentSelection.Ids

Use the following script to specify the data source:

analysis = ExtAPI.DataModel.Project.Model.Analyses[0]

filepath = analysis.ResultFileName

dataSources = dpf.DataSources()

dataSources.SetResultFilePath(filepath)

model=dpf.Model(dataSources)

Specify the scoping particulars:

my_scoping          = dpf.Scoping()

my_scoping.Ids      = node_id

my_scoping.Location = 'Nodal'

Create a field container for stress and use the scoping specified above:

stress_fc = dpf.operators.result.stress()

stress_fc.inputs.data_sources.Connect(dataSources)

stress_fc.inputs.mesh_scoping.Connect(my_scoping)

stress_field = stress_fc.outputs.fields_container.GetData()[0]

stress_field.Data will return a list containing [SX, SY, SZ, SXY, SYZ, SXZ]