Overview of postprocessing capabilities in Ansys

Javier Vique

In civil engineering, APDL has been traditionally used for both building up the models and postprocessing. Nowadays, many engineers are building their models in Mechanical, but they still use APDL snippet commands for getting some output data into txt files that are used afterwards in in-house tools. Which are the alternatives to this workflow?

Javier Vique

The model of a 3D frame modeled by beam elements shown below is used as demo for giving an overview of the different options for postprocessing with Ansys. The final target of the user would be making an output of SMISC1 (axial force on i node) and SMISC2 (y bending on i node) on specific named selections (NS1 & NS2) for the last substep of the only available step. This output will be used in an in-house tool made in Excel.

APDL snippet commands:
*VWRITE commands are used for getting the output. Here the script:

/POST1

set,last

*get,elem_min,elem,,num,mind           !Min element in model
*get,elem_max,elem,,num,maxd           !Max element in model

etable,etaxial,smisc,1
etable,etbendingY,smisc,2

*dim,aaxial,array,elem_max          
*vget,aaxial(1,1),elem,elem_min,etab,etaxial

*dim,abendingY,array,elem_max          
*vget,abendingY(1,1),elem,elem_min,etab,etbendingY


*do,i,1,%ARG1%
CMSEL,S,NS_%i%
*GET,ELEMCOUNT,ELEM,0,COUNT            !Elements in named selection
*DIM,EARRAY,ARRA,ELEMCOUNT,1           !Elements array
*VGET,EARRAY(1,1),ELEM,,ELIST          !Elements list
*dim,emask,array,elem_max              !Mask to select elements in named selection
*vget,emask(1),elem,,esel

ALLSEL

*cfopen,'Beams_NS_%i%','txt'
*vlen,1
*vwrite,'Beam','Axial','BendingY'
 (A11,X,A15,X,A15)


*vmask,emask(1)
*dim,results_ns%i%,array,ELEMCOUNT,2    
*vfun,results_ns%i%(1,1),comp,aaxial(1,1)
*vmask,emask(1)
*vfun,results_ns%i%(1,2),comp,abendingY(1,1)  

*vwrite,EARRAY(1,1),results_ns%i%(1,1),results_ns%i%(1,2)
 (F11.0,X,F15.3,X,F15.3)
*cfclos
*enddo

Mechanical scripting:
Two user-defined results (UDR) are created and they are evaluated for both named selections, making use of ExportToTextFile method. Here the script:

import os

folderpath = r'here_my_path'

Solution = ExtAPI.DataModel.Project.Model.Analyses[0].Solution
NamedSelections = ExtAPI.DataModel.GetObjectsByType(DataModelObjectCategory.NamedSelection)

AxialSol = Solution.AddUserDefinedResult()
AxialSol.Expression = 'SMISC1'
BendingYSol = Solution.AddUserDefinedResult()
BendingYSol.Expression = 'SMISC2'

for NS in NamedSelections:
    axial_name = NS.Name + '_axial.txt'
    bendy_name = NS.Name + '_bendingY.txt'
    filename1 = os.path.join(folderpath,axial_name)
    filename2 = os.path.join(folderpath,bendy_name)
    AxialSol.ClearGeneratedData()
    AxialSol.Location = NS
    AxialSol.EvaluateAllResults()
    AxialSol.ExportToTextFile(filename1)
    BendingYSol.ClearGeneratedData()
    BendingYSol.Location = NS
    BendingYSol.EvaluateAllResults()
    BendingYSol.ExportToTextFile(filename2)

An alternative, which would be more efficient, is using Result Reader and BEAM_AXIAL_F & BEAM_BENDING_M. Additionally, this would allow to make the export directly to Excel, but please be aware that the output is slightly different, since this output gives 2 values per element (node i and node j), so it is giving SMISC1-14 and SMISC2-15, not just SMISC1 & SMISC2. For details about result reader, please have a look at our user manual:
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v232/en/act_cust_mech/Postprocess_externalResultRetrieval.html?q=result reader

Data Postprocessing Framework:
DPF allows us to make this export, bringing the data into Excel. Here the script:

## Here an Excel is open following solution available in Dev Forum:
# https://discuss.ansys.com/discussion/308/write-information-to-excel-example-on-mesh-quality
import clr
clr.AddReferenceByName('Microsoft.Office.Interop.Excel')
from Microsoft.Office.Interop import Excel
excel = Excel.ApplicationClass()
excel.Visible = True # makes the Excel application visible to the user
excel.ScreenUpdating = True     # Enables screen refreshing
# opening a workbook
filename = r"here_your_path\Book1.xlsx" #Specify existing Excel document
workbook = excel.Workbooks.Open(filename)
# adding a worksheet
ws = workbook.Worksheets.Add() # Add a new worksheet and change its name
ws.Name = "MyNewSheet"

ws.Cells(1,1).Value = "Named Selection"
ws.Cells(1,2).Value = "Element"
ws.Cells(1,3).Value = "Axial"
ws.Cells(1,4).Value = "BendingY"
i = 2

## Here mech-dpf is used to get SMISC1 & SMISC2
import os
import mech_dpf
import Ans.DataProcessing as dpf

folderpath = r'D:\01.Support\Salesforce\00033923\DPF_results'

analysis=Model.Analyses[0]
dataSource = dpf.DataSources(analysis.ResultFileName)

model=dpf.Model(dataSource)

named_selections = ['NS_1','NS_2']

op_smisc = dpf.operators.result.mapdl.smisc()
op_smisc.inputs.data_sources.Connect(dataSource)
op_smisc.inputs.item_index.Connect(1)
smisc1 = op_smisc.outputs.fields_container.GetData()

op_smisc.inputs.item_index.Connect(2)
smisc2 = op_smisc.outputs.fields_container.GetData()

for j in named_selections:
    ns = model.GetNamedSelection(j)
    for elemid in ns.Ids:
        ws.Cells(i,1).Value = j
        ws.Cells(i,2).Value = elemid
        ws.Cells(i,3).Value = smisc1[0].GetEntityDataById(elemid)[0]
        ws.Cells(i,4).Value = smisc2[0].GetEntityDataById(elemid)[0]
        i = i + 1

print('Script has finished, review your Excel file')

For big models, there might be some alternatives to GetEntityDataById(elemid) to get results faster.

Below the verification for element 100: