Read element type and keyopts with ACT Python from RST

ThomasDD

With Ansys ACT Python you have full access to the data of the RST, such as the stress tensor of an element:

elemId = 14588
analysis = Model.Analyses[0]
reader = analysis.GetResultsData()
reader.CurrentTimeFreq = 1
stress = reader.GetResult('S', MechanicalUnitSystem.StandardNMMton)
S = stress.GetElementValues(elemId)
print S

You can also query the type of the element:

meshData = analysis.MeshData
elem = meshData.ElementById(elemId)
elem_typ = elem.Type
print elem_typ

But what you get here is a string like "kHex8". Is it possible to get the real Ansys element type (like 185 for 8-node solids) and how do I get the set keyopts with ACT Python for a specific element? The calculation within my ACT extension must take the set element options into account...

Thanks for helping.

ThomasDD

I found the element number!!

result = reader.GetResult('PNUM', MechanicalUnitSystem.StandardNMMton)
result.SelectComponents(['ENAM'])
enam = result.GetElementValues(elemId)[0]
print enam # = 185

But I still need the key options ...

Pernelle Marone-Hitz

@ThomasDD perhaps using DPF would be easier and faster here. This post could help: https://discuss.ansys.com/discussion/4566/how-to-use-selection-logic-in-dpf-in-mechanical-example-select-solid186-elements-with-keyopt-2-1

ThomasDD

Sorry, DPF is no option, because with DPF you only have access to selected field variables. For example I can not found the elastic strain energy density with DPF...

ACT Python:

analysis = Model.Analyses[0]
reader = analysis.GetResultsData()
for name in reader.ResultNames:
    print name
# AENE
# BFE
# CDM
# DENE
# ECENT
# EDIR
# EFFNU_ZERO_EPTO
# EFFNU_ZERO_EPTT
# ENERGY
# ENFO
# EPEL
# EPELEQV_RST
# EPPL
# EPPLEQV_RST
# EPTH
# EPTHEQV_RST
# EPTO
# EPTOEQV_RST
# EPTT
# EPTTEQV_RST
# F
# LAYNUMBER
# LOC
# LOC_DEF
# MESH_
# NDIR
# PDMG
# PENERGY
# PFC
# PNUM
# PRIN_S
# S
# SEND
# SENG
# SPSD
# STEN
# U
# UALL
# VOLUME
# WEXT

DPF:

import mech_dpf
import Ans.DataProcessing as dpf
analysis = ExtAPI.DataModel.Project.Model.Analyses[0]
filepath = analysis.ResultFileName
dataSources = dpf.DataSources()
dataSources.SetResultFilePath(filepath)
print model.ResultInfo
# Available results: 
# U Displacement :nodal displacements 
# RF Force :nodal reaction forces 
# ENF Element nodal Forces :element nodal forces 
# S Stress :element nodal component stresses 
# ENG_VOL Volume :element volume 
# ENG_SE Energy-stiffness matrix :element energy associated with the stiffness matrix 
# ENG_AHO Hourglass Energy :artificial hourglass energy 
# ENG_TH thermal dissipation energy :thermal dissipation energy 
# ENG_KE Kinetic Energy :kinetic energy 
# ENG_CO co-energy :co-energy (magnetics) 
# ENG_INC incremental energy :incremental energy (magnetics) 
# EPEL Strain :element nodal component elastic strains 
# ETH Thermal Strains :element nodal component thermal strains 
# ETH_EQV Thermal Strains eqv :element nodal equivalent component thermal strains 
# ETH_SWL Swelling Strains :element nodal swelling strains 
# BFE Temperature :element structural nodal temperatures

Pernelle Marone-Hitz

DPF should be able to give you any result that has been stored in the .rst file. The elastic strain energy density should be available:

If you need to access the keyoptions without using DPF, I'm afraid the only solution would be to write some Python code to parse the input file (ds.dat which is basically a text file).

ThomasDD

Thanks. At the moment we can not switch the result reading routines in our ACT Exctension. What I need is the integration rule (reduced or full integration, keyopt 2) of 185 / 186 elements:

185:
0 -- Uniform reduced integration (default)
1 -- Full integration
186:
0 -- Full integration with method (default)
1 -- Uniform reduced integration with hourglass control
2 -- Enhanced strain formulation
3 -- Simplified enhanced strain formulation

Perhaps there is a way to query this via the ACT interface...

ThomasDD

I get some element informatio (type, mat, real, elementname) and I get some information about the element type. But none of this points to the integration scheme....

elemId = 123
results = analysis.GetResultsData()
eleminfo = results.GetResult('PNUM', MechanicalUnitSystem.StandardNMMton)
el_type, el_real, el_mat, el_sec, el_esys, el_elem, el_enam = eleminfo.GetElementValues(elemId)
print el_type, el_real, el_mat, el_sec, el_esys, el_elem, el_enam
print results.GetElemTypeProps(el_type)

ThomasDD

For both cases (reduced and full integration) I get 48 stress values per element, 6 components for each of the 8 integration points. The only indication I can see at the moment as to whether reduced integration is present is that the stress vector is the same for each integration point:

Pernelle Marone-Hitz

@ThomasDD Indeed the integration type will not be written anywhere else than in the ds.dat. Only solution would be to read it as a text file and extract info from here. Or, as you suggested, identify cases where the stress value is the same for all integration points.

ThomasDD

Thanks!