Skip to content
  • Register

    • Read element type and keyopts with ACT Python from RST

    Member Posts: 20
    10 Comments Name Dropper
    **
    in Structures

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

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

    You can also query the type of the element:

    1. meshData = analysis.MeshData
    2. elem = meshData.ElementById(elemId)
    3. elem_typ = elem.Type
    4. 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.

    Welcome!

    It looks like you're new here. Sign in or register to get started.
    Sign In
    Register

    Comments

    • Member Posts: 20
      10 Comments Name Dropper
      **

      I found the element number!!

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

      But I still need the key options ...

    • Member, Moderator, Employee Posts: 891
      100 Answers 500 Comments 250 Likes Second Anniversary
      ✭✭✭✭

      @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

    • Member Posts: 20
      10 Comments Name Dropper
      **

      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:

      1. analysis = Model.Analyses[0]
      2. reader = analysis.GetResultsData()
      3. for name in reader.ResultNames:
      4.     print name
      5. # AENE
      6. # BFE
      7. # CDM
      8. # DENE
      9. # ECENT
      10. # EDIR
      11. # EFFNU_ZERO_EPTO
      12. # EFFNU_ZERO_EPTT
      13. # ENERGY
      14. # ENFO
      15. # EPEL
      16. # EPELEQV_RST
      17. # EPPL
      18. # EPPLEQV_RST
      19. # EPTH
      20. # EPTHEQV_RST
      21. # EPTO
      22. # EPTOEQV_RST
      23. # EPTT
      24. # EPTTEQV_RST
      25. # F
      26. # LAYNUMBER
      27. # LOC
      28. # LOC_DEF
      29. # MESH_
      30. # NDIR
      31. # PDMG
      32. # PENERGY
      33. # PFC
      34. # PNUM
      35. # PRIN_S
      36. # S
      37. # SEND
      38. # SENG
      39. # SPSD
      40. # STEN
      41. # U
      42. # UALL
      43. # VOLUME
      44. # WEXT

      DPF:

      1. import mech_dpf
      2. import Ans.DataProcessing as dpf
      3. analysis = ExtAPI.DataModel.Project.Model.Analyses[0]
      4. filepath = analysis.ResultFileName
      5. dataSources = dpf.DataSources()
      6. dataSources.SetResultFilePath(filepath)
      7. print model.ResultInfo
      8. # Available results: 
      9. # U Displacement :nodal displacements 
      10. # RF Force :nodal reaction forces 
      11. # ENF Element nodal Forces :element nodal forces 
      12. # S Stress :element nodal component stresses 
      13. # ENG_VOL Volume :element volume 
      14. # ENG_SE Energy-stiffness matrix :element energy associated with the stiffness matrix 
      15. # ENG_AHO Hourglass Energy :artificial hourglass energy 
      16. # ENG_TH thermal dissipation energy :thermal dissipation energy 
      17. # ENG_KE Kinetic Energy :kinetic energy 
      18. # ENG_CO co-energy :co-energy (magnetics) 
      19. # ENG_INC incremental energy :incremental energy (magnetics) 
      20. # EPEL Strain :element nodal component elastic strains 
      21. # ETH Thermal Strains :element nodal component thermal strains 
      22. # ETH_EQV Thermal Strains eqv :element nodal equivalent component thermal strains 
      23. # ETH_SWL Swelling Strains :element nodal swelling strains 
      24. # BFE Temperature :element structural nodal temperatures
    • Member, Moderator, Employee Posts: 891
      100 Answers 500 Comments 250 Likes Second Anniversary
      ✭✭✭✭
      edited March 27

      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).

    • Member Posts: 20
      10 Comments Name Dropper
      **

      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...

    • Member Posts: 20
      10 Comments Name Dropper
      **

      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....

      1. elemId = 123
      2. results = analysis.GetResultsData()
      3. eleminfo = results.GetResult('PNUM', MechanicalUnitSystem.StandardNMMton)
      4. el_type, el_real, el_mat, el_sec, el_esys, el_elem, el_enam = eleminfo.GetElementValues(elemId)
      5. print el_type, el_real, el_mat, el_sec, el_esys, el_elem, el_enam
      6. print results.GetElemTypeProps(el_type)
    • Member Posts: 20
      10 Comments Name Dropper
      **

      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:

    • Member, Moderator, Employee Posts: 891
      100 Answers 500 Comments 250 Likes Second Anniversary
      ✭✭✭✭

      @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.

    • Member Posts: 20
      10 Comments Name Dropper
      **

      Thanks!

    Welcome!

    It looks like you're new here. Sign in or register to get started.
    Sign In
    Register

    Welcome!

    It looks like you're new here. Sign in or register to get started.
    Sign In
    Register

    Quick Links

    Categories