Using mech_dpf to output stress components in cylindrical coordinate systems

I want to output stress components for specific nodes, at specific time steps, of an analysis for further post processing.
I can do this in cartesian coordinate system but need the results in polar coordinate system.

I am currently working in 21R2, and would like to do this in mechanical scripting as I am not able to interact with mechanical from external python yet and the python results is still beta in 21R2.

Eventually I will export stresses to a file but for simplicity I am only printing now.

My questions are:
1) How can this be done without coding transformation calculations?
It seems feasible as shown here but I have not been able to implement this solution.
2) Can this be done by referencing and using existing polar coordinate system in the model?
3) Can I optimize requesting this data in the utilization of dpf for larger result files?

A simplified version of my current code is below:

import mech_dpf
import Ans.DataProcessing as dpf


# user inputs
model_num = 0
node_num_list = [74]
time_steps = [1,2,3,4,5,6,7,8,9,10]

# get the analysis, result file, set the data source, and set the model
analysis = Model.Analyses[model_num]
rstFile=analysis.WorkingDir+"file.rst"
data_source = dpf.DataSources(rstFile)
model = dpf.Model(data_source)

# set the location scoping
nodal_scoping = dpf.Scoping(Location = dpf.locations.nodal)
nodal_scoping.Ids = node_num_list

# set the time scoping
time_scoping = dpf.Scoping(Location = dpf.locations.time_freq_sets)
time_scoping_list= []
for i in time_steps:
    # Note: the result time frequencies start at 0
    ts = model.TimeFreqSupport.GetTimeFreqCummulativeIndex(i-1,-1)+1
    time_scoping_list.append(ts)
time_scoping.Ids = time_scoping_list

# set requested values and the scoping
opx = dpf.operators.result.stress_X()
opy = dpf.operators.result.stress_Y()
opz = dpf.operators.result.stress_Z()
opxy = dpf.operators.result.stress_XY()
opyz = dpf.operators.result.stress_YZ()
opxz = dpf.operators.result.stress_XZ()
operator_list = [opx, opy, opz, opxy, opyz, opxz]
for op in operator_list:
    op.inputs.data_sources.Connect(data_source)
    op.inputs.mesh_scoping.Connect(nodal_scoping)
    op.inputs.time_scoping.Connect(time_scoping)

# get the outputs
output_list = []
for op in operator_list:
    output = op.outputs.fields_container.GetData()
    output_list.append(output)

# print the history
for i in time_steps:
    output_str = str(i) + ": " 
    for output in output_list:
        output_val = output[i-1].Data[0]
        output_str += str(round(output_val,2)) + ", "
    print(output_str)

Find more posts tagged with

AnsysACT

Mechanical

PyDPF

scripting

Accepted answers

All comments

Mike.Thompson

@Shad ,
I believe the post you referenced has the correct operator you need: dpf.operators.geo.rotate_in_cylindrical_cs_fc

The issue is likely you are getting all the stress components individually from their own operators. To do a coordinate system conversion you need to have all the stress tensor data in a single field with multiple stress components. The way to do this is to use the stress operator:
dpf.operators.result.stress()

This will get you the entire stress tensor as these fields will have 6 components in them each. Do the geo.rotate... operator on this data.

Set the time scoping to multiple (or all) time points and you should have a fields container, which should be operated on as a single entity (rotating all the fields in one operation). This will be the way to scale this to large data sets in mesh domain and time points.