FdScript

Since FEM-Design 17.01.001, we support a basic automation workflow through scripting. It is capable to load/save file, execute analysis calculation and create outputs as .csv list or .docx documentation. Using scripting you can batch-analyze models created and execute long calculations during the night.

Concept

The installation of FEM-Design creates the fdscript.xsd and example.fdscript in the templates folder. The latter can be used as a starting point of custom scripts since it has all the commands intended for users and useful comments on how to proceed.

In order to learn how the .fdscript file is formatted, we will do a step by step inspection of the main part of the file.

fdscript

<?xml version="1.0" encoding="UTF-8"?>
<fdscript xmlns:xsi="http://www.w3.org/2001/XMLSchema-instance" xsi:noNamespaceSchemaLocation="fdscript.xsd">
  <!-- SCRIPT HEADER  ==================================================================================  -->
  <fdscriptheader>
    <title>FEM-Design example script</title>
    <version>2100</version>
    <module>SFRAME</module>
    <!-- log file where warnings from calculation and other interesting entries may appear -->
    <logfile>e:\x.log</logfile>
  </fdscriptheader>


  <!-- command for menu file/open use the filename with extension -->
  <cmdopen command="; CXL CS2SHELL OPEN">
    <filename>e:\x.struxml</filename>
  </cmdopen>

 
  <!-- command for calculation on Analysis tab  -->
  <cmduser command="; CXL $MODULE RESMODE" />
  <cmdcalculation command="; CXL $MODULE CALC">
    <analysis
      calcCase = "1"
      calcCstage = "0"
      calcImpf = "0"
      calcComb = "1"
      calcGmax = "0"
      calcStab = "0"
      calcFreq = "0"
      calcSeis = "0"
      calcFootfall = "0"
      calcMovingLoad = "0"
      calcBedding = "0"
      calcThGroundAcc = "0"
      calcThExforce = "0"
      calcDesign = "0"
      
      elemfine = "1"
      diaphragm = "0"
      peaksmoothing = "1"
    >
      <stage ghost = "0" />
      <comb
        NLEmaxiter = "30"
        
        PLdefloadstep = "20"
        PLminloadstep = "2"
        PLmaxeqiter = "30"
        
        NLSMohr = "1"
        NLSinitloadstep = "10"
        NLSminloadstep = "10"
        NLSactiveelemratio = "5"
        NLSplasticelemratio = "5"
        
        CRloadstep = "20"
        CRmaxiter = "30"
        CRstifferror = "2"
      >
        <combitem
          ImpfRqd = "0"
          StabRqd = "0"
          
          NLE = "0"
          PL = "0"
          NLS = "0"
          Cr = "0"
          f2nd = "0"
          Im = "0"
          Waterlevel = "0"
        />
      <freq
        Numshapes = "2"
        MaxSturm = "0"
        X = "1"
        Y = "1"
        Z = "1"
        top = "0.0"
        AutoIter = "5"
        NormUnit = "0"
      />
      <footfall TopOfSubstructure = "-0.01" />
      <bedding 
        Ldcomb = "a" 
        Meshprep = "0" 
        Stiff_X = "0.5" 
        Stiff_Y = "0.5" 
      />
    </analysis>
  </cmdcalculation>


  <!-- command for calculation on RC design tab for load combinations, autodesign may be false if reinforcement present in input file -->
 <cmduser command="; CXL $MODULE RCDESIGN" />
 <cmdcalculation command="; CXL $MODULE CALC">
  <design>
   <cmax />
   <autodesign>true</autodesign>
    <check>true</check>
  </design>
 </cmdcalculation>
  

  <!-- command for calculation on steel design tab, set autodesign to true if needed  -->
 <cmduser command="; CXL $MODULE STEELDESIGN" />
 <cmdcalculation command="; CXL $MODULE CALC">
  <design>
   <cmax />
   <autodesign>false</autodesign>
    <check>true</check>
  </design>
 </cmdcalculation>


  <!-- command to generate csv file output as from list panel batch, use proper filenames and "1" if want the checkbox option   -->
  <cmdlistgen command="$ MODULECOM LISTGEN" bscfile="e:\x.bsc" outfile="e:\x.csv" regional="0" fillcells="0" headers="0" />
  <cmdlistgen command="$ MODULECOM LISTGEN" bscfile="e:\y.bsc" outfile="e:\y.csv" regional="0" fillcells="0" headers="0" />
  <!-- repeat for additional batches if i.e each has just one table  -->


  <!-- command to make documentation from doc template   -->
  <cmdchild>e:\x.dsc</cmdchild>


  <!-- command to export documantation to .docx   -->
  <cmdsavedocx command="$ DOC SAVEDOCX">
    <filename>e:\x.docx</filename>
  </cmdsavedocx>


  <!-- command to save the model, use extension with filename!  -->
  <cmdsave command="; CXL CS2SHELL SAVE">
    <filename>e:\x1.str</filename>
  </cmdsave>


  <!-- command to quit the program -->
  <cmdendsession/>


  <!-- END SESSION 	===================================================================================  -->
</fdscript>

tip

The example script can be edited using notepad but it is more convenient to use a code editor such as Visual Studio Code.

Procedure

Log file

Enter the location for the log file that will contain all the information about performed calculations, errors and warnings. Always use absolute path for files.

<fdscriptheader>
    <title>FEM-Design example script</title>
    <version>2100</version>
    <module>SFRAME</module>
    <logfile>e:\x.log</logfile>
</fdscriptheader>

Open model

Enter the location of the model that will be executed by the Run script function. The model can be saved both as .struxml or .str file type.

<cmdopen command="; CXL CS2SHELL OPEN">
    <filename>e:\x.struxml</filename>
</cmdopen>

Analysis

Select the type of analysis calculations that you wish to perform running the script. This is done by typing "1" or "0" next to the corresponding calculation type in the script example, where "1" means to perform that calculations. The listed calculation types exactly correspond to the order of calculations in the Calculation dialog in FEM-Design.

analysis

<cmduser command="; CXL $MODULE RESMODE" />
<cmdcalculation command="; CXL $MODULE CALC">
<analysis
    calcCase = "1"
    calcCstage = "0"
    calcImpf = "0"
    calcComb = "1"
    calcGmax = "0"
    calcStab = "0"
    calcFreq = "0"
    calcSeis = "0"
    calcFootfall = "0"
    calcMovingLoad = "0"
    calcBedding = "0"
    calcThGroundAcc = "0"
    calcThExforce = "0"
    calcDesign = "0"
    
    elemfine = "1"
    diaphragm = "0"
    peaksmoothing = "1">
</analysis>
</cmdcalculation>

The example script contains more options to set up calculation parameters, for example details of construction stages analysis, Eigenfrequencies or calculation options for load combinations calculations.

eigen-freq

<freq
    Numshapes = "2"
    MaxSturm = "0"
    X = "1"
    Y = "1"
    Z = "1"
    top = "0.0"
    AutoIter = "0"
    NormUnit = "0"/>

<footfall   TopOfSubstructure = "-0.01" />
</analysis>

Design

Select whether you want to perform Auto design or Check calculations, by typing "false" or "true" in the corresponding design module part of the script.

<cmduser command="; CXL $MODULE RCDESIGN" />
<cmdcalculation command="; CXL $MODULE CALC">
    <design>
        <cmax />
        <autodesign>true</autodesign>
    <check>true</check>
    </design>
</cmdcalculation>

<cmduser command="; CXL $MODULE STEELDESIGN" />
<cmdcalculation command="; CXL $MODULE CALC">
    <design>
        <cmax />
        <autodesign>false</autodesign>
    <check>true</check>
    </design>
</cmdcalculation>

Create design group

<cmddesgroup command="$ CODE_COM DESGROUP" 
      name="A" color="0" force="false" type="STBAR">
  <GUID>2e290437-e86a-4e36-af7d-acde6a6146c8</GUID>
  <GUID>2cba9c00-255d-4258-94fb-f164aafff214</GUID>
</cmddesgroup>

valid types are:
"FNISOLATED", "FNWALL", "FNSLAB", "RCSURFLONG", "RCSURFSHEAR", "RCPUNCH", "STBARSHELL", "STJOINT", "TMBAR", "TMPANEL", "TMPANELCLT", "MS", "COCOLUMN", "CODELTABEAM", "RCBAR", "RCHIDDENBAR", "STBAR", "STFIRE", "TMFIRE", "CLTFIRE" without force the group must not already exist. To delete a group use force="true" and empty guid list All entities must be conforming to the group type. remember that you must pass analytical entities!

Apply design changes

<cmduser command="; CXL FEM $CODE(DESCHANGESAPPLY)" />

Generate csv output file

It is possible to generate a csv file from List tables batch. First, select all the tables in List tables dialog in FEM-Design and save it as a batch file (.bsc).

bsc

Then replace the name and location of the batch file (.bsc) and output file (.csv) in the script example.

<cmdlistgen command="$ MODULECOM LISTGEN" bscfile="e:\x.bsc" outfile="e:\x.csv" regional="0" fillcells="0" headers="0" />

Set project description

<cmdprojdescr command="$ MODULECOM PROJDESCR"
  read="0" reset="0"
  szProject="t1"
  szDescription="t2"
  szDesigner="t3"
  szSignature="t4"
  szComment="t5">
    <item id="a" txt="a_txt"/>
    <item id="b" txt="b_txt"/>
</cmdprojdescr>

Global configurations

<cmdglobalcfg command="$ FEM $CODE(GLOBALCFG)"> 
  <soil_calculation
    fSoilAsSolid = "0"
  />
  <mesh_general
    fAdjustToLoads = "0"
  />
  <mesh_elements
    fElemCalcRegion = "1"
    rElemSizeDiv = "6.0"
    fCorrectToMinDivNum = "1"
    sDefaultDivision = "2"
    rDefaultAngle = "15.0"
    sDefaultEdgeDivision = "1"
  />
  <mesh_functions
    fRefineLocally = "1"
    sRefineMaxStepNum = "5"
    fMaxIterWarning = "0"
    fReduceSize = "1"
    sSmoothStepNum = "3"
    fCheckMeshGeom = "1"
    rCheckGeomMinAngle = "10.0"
    rCheckGeomMaxAngle = "170.0"
    rCheckGeomMaxSideRatio = "8.0"
    fCheckMeshOverlap = "1"
    fCheckMeshTopology = "1"
  />
  <mesh_prepare
      fAutoRegen = "1"
      fThPeak = "1"
      fThBeam = "0"
      fThColumn = "1"
      fThTruss = "0"
      fThFicBeam = "0"
      fThFreeEdge = "0"
      fThRegionBorder = "0"
      fThSuppPt = "1"
      fThSuppLn = "0"
      fThSuppSf = "0"
      fThEdgeConn = "0"
      fThConnPt = "0"
      fThConnLn = "0"
      fThConnSf = "0"
      fThLoadPt = "0"
      fThLoadLn = "0"
      fThLoadSf = "0"
      fThFixPt = "0"
      fThFixLn = "0"
      fAutoRebuild = "1"
      fAutoSmooth = "1"
      fAutoCheck = "0"
  />
  <peaksm_method
      sPeakFormFunc_M = "1"
      sPeakFormFunc_N = "1"
      sPeakFormFunc_V = "1"
  />
  <peaksm_auto
      fPeakBeam = "0"
      fPeakColumn = "1"
      fPeakTruss = "0"
      fPeakFicBeam = "0"
      fPeakPlate = "0"
      fPeakWall = "0"
      fPeakFicShell = "0"
      fPeakSuppPt = "1"
      fPeakSuppLn = "0"
      fPeakSuppSf = "0"
      fPeakConnPt = "0"
      fPeakConnLn = "0"
      fPeakConnSf = "0"
      rPeakFactor = "0.5"
  />
</cmdglobalcfg>

Interaction surface

<cmdinteractionsurface command="$ CODE_COM INTERACTIONSURFACE" guid="2e290437-e86a-4e36-af7d-acde6a6146c8" offset="0.0" fUlt="false" outfile="e:\res\a.txt"  />

Load groups to load combinations

<cmdldgroup2comb command="$ LOAD LDGROUP2COMB" 
    fU="true" fUa="true" fUs="true" fSq="true" fSf="true" fSc="true"
    fSeisSigned="true" fSeisTorsion="true" fSeisZdir="false"
    fSkipMinDL="true" fForceTemp="true" fShortName="true" >
  <GUID>2e290437-e86a-4e36-af7d-acde6a6146c8</GUID>
  <GUID>2cba9c00-255d-4258-94fb-f164aafff214</GUID>
</cmdldgroup2comb>

Export documentation to .docx file

It is possible to export documentation in .docx file. Simply replace the name and location of the .docx file in the sample script.

<cmdsavedocx command="$ DOC SAVEDOCX">
    <filename>e:\x.docx</filename>
</cmdsavedocx>

Save the model

The model with documentation and results file will be saved to selected location.

<cmdsave command="; CXL CS2SHELL SAVE">
    <filename>e:\x1.str</filename>
</cmdsave>

End session

<cmdendsession/>

Launching

To launch the script use the menu command Tools -> Run script

RunScript

or start the program with the command line:

fd3dstruct /s c:\mydir\example.fdcsript

For example,

C:\Program Files\StruSoft\FEM-Design 18\fd3dstruct.exe  /s C:\Users\xxx\Desktop\MyDir\ExampleScript.fdscript

Concept​

Procedure​

Log file​

Open model​

Analysis​

Design​

Create design group​

Apply design changes​

Generate csv output file​

Set project description​

Global configurations​

Interaction surface​

Load groups to load combinations​

Export documentation to .docx file​

Save the model​

End session​

Launching​