Python scripts reading Results

Purpose of the scripts

The scripts illustrate the reading of Nastran Results with FeResPost Python extension.

Script 1 : Python importation of Results from Nastran OP2 file

from FeResPost import *
import sys

os=sys.stdout

# Creates and initializes the DataBase :

db=NastranDb()
db.Name="tmpDB"
db.readBdf("../../MODEL/MAINS/orbit_unit_xyz.bdf")
db.readGroupsFromPatranSession("../../MODEL/PATRAN/groups.ses")

...

# Reading Results :

db.readOp2("../../MODEL/EXEC_OP2/orbit_unit_xyz.op2","Results")

...

# Maximum Von Mises stress :

targetGrp=db.getGroupCopy("pan_PZ_Al_2024")
stress=db.getResultCopy("ORBIT_ONE_MS2_Z","Statics","Stress Tensor","ElemCorners",targetGrp,[])
scalar=stress.deriveTensorToOneScal("VonMises")

...

Explanations

The different steps of the Nastran reading of Results in script above are:

The access to FeResPost compiled library.
The creation of a NastranDb FEM database into which the finite element model is read, and Groups are read from a Patran session file.
The reading of results from a Nastran OP2 result files. The results that are read are stored into the NastranDb FEM database.
Then results can be extracted from the NastranDb FEM database and can be manipulated (extraction on Groups, derivation of other results, extraction of minimum or maximum values, printing in a text file...).

The full script can be found in the Python example (TESTSAT/PYTHON/EX05/printStressMax.py).

Script 2 : Python importation of Results from Nastran XDB file

...

# Reading or generating Results :

lcNames=[]
lcNames.append("SINUS_X")

scNames=[]
scNames.append("Output 70 (f = 119.0000)")
scNames.append("Output 30 (f = 79.0000)")
scNames.append("Output 1 (f = 50.0000)")

resNames=[]
resNames.append("Accelerations, Translational (RI)")
resNames.append("MPC Forces, Forces (RI)")
resNames.append("MPC Forces, Moments (RI)")

xdbFileName="../../MODEL/EXEC_XDB/sol111_ri_xyz.xdb"
db.readXdb(xdbFileName,lcNames,scNames,resNames)

...

# Extracted Results :

resRI=db.getResultCopy(lcName,scName,"Accelerations, Translational (RI)","Nodes",tmpGroup,[])
Util.printRes(sys.stdout,"Accelerations resRI",resRI)

...

Explanations

The different steps of the Nastran reading of Results in script above are:

The access to FeResPost compiled library.
The creation of a NastranDb FEM database into which the finite element model is read, and Groups are read from a Patran session file.
The reading of results from a Nastran XDB result files. The results that are read are stored into the NastranDb FEM database. In the example, the Results correspond to a dynamic load case. Notice that one has limit the number of subcases (frequency outputs) in order to avoid problems related to memory exhaustion.
Then results can be extracted from the NastranDb FEM database and can be manipulated (extraction on Groups, derivation of other results, extraction of minimum or maximum values, printing in a text file...).

The full script can be found in the Python example (TESTSAT/PYTHON/EX17/manipComplex.py).

Script 3 : Python importation of Results from Nastran XDB file (by attachment)

...

# Reading Results :

xdbFileName="../../MODEL/EXEC_XDB/sol111_ri_xyz.xdb"
db.attachXdb(xdbFileName)

# Extracting Results :

lcName="SINUS_X"

scNames=[]
scNames.append("Output 13 (f = 62.0000)")
scNames.append("Output 14 (f = 63.0000)")
scNames.append("Output 15 (f = 64.0000)")
scNames.append("Output 16 (f = 65.0000)")
scNames.append("Output 17 (f = 66.0000)")
scNames.append("Output 18 (f = 67.0000)")

resNames=[]
resNames.append("Accelerations, Rotational (RI)")
resNames.append("Accelerations, Translational (RI)")
resNames.append("Displacements, Rotational (RI)")
resNames.append("Displacements, Translational (RI)")

grp=db.getGroupCopy("pan_MZ")

h=db.getAttachmentResults(xdbFileName,lcName,scNames,resNames,"Nodes",grp)
for id,res in h.iteritems():
    lcName=id[0]
    scName=id[1]
    resName=id[2]
    size=res.Size
    sys.stdout.write("%s - %s - %s : %d\n"%(lcName,scName,resName,size))

...

Explanations

The different steps of the Nastran reading of Results in script above are:

The access to FeResPost compiled library.
The creation of a NastranDb FEM database into which the finite element model is read, and Groups are read from a Patran session file.
In this example, the XDB file is attached to the NastranDb FEM database, but not really read. Actually, some information is read from the file (list of load cases, of sub-cases, or result names...). The information that is being read is stored in the the NastranDb FEM database and will later be used to extract Results from the XDB file.
Then Results can be extracted from the XDB file and manipulated. In this case, the manipulation consists only in printing the Results in a text file.
Note that each call to ``db.getAttachmentResults'' leads to reading part of the XDB file that is attached to the NastranDb FEM database. This means that the XDB file must remain attached to the database and is therefore open in reading until the file is detached from the XDB.
Attaching XDB files instead of reading directly Results into the FEM database allows to reduce the allocation of memory needed to store the results into the FEM database. On the other hand the number of disk accesses increases and this can be time consuming.
When reading dynamic load response Results, we have observed that the performance of reading deteriorates when XDB files are large. This is related to the organization of XDB files generated by Nastran that leads to the reading of a significant number of pages for each frequency output. Then, the switching to HDF files is recommended as the file orgnaization seems more adapted. (See below.)

The full script can be found in the Python example (TESTSAT/PYTHON/EX17/printXdbLcScResSizes.py).

Script 4 : Python importation of Results from Nastran HDF file (by attachment)

from FeResPost import *
import sys

os=sys.stdout

Post.loadHdf5Library("C:/NewProgs/HDF5/HDF5-1.8.20-win64/bin/hdf5.dll")

# Creates and initializes the DataBase :

dirName="D:/SHARED/FERESPOST/TESTSAT/MODEL/EXEC_HDF5"
baseName="unit_xyz"

lcIndex=0
scIndex=0

bdfName=("%s/%s.bdf"%(dirName,baseName))
hdfName=("%s/%s.h5"%(dirName,baseName))
xdbName=("%s/%s.xdb"%(dirName,baseName))

db=NastranDb()
db.readBdf(bdfName)

...

# Reading Results :

db.attachHdf(hdfName)

lcNames=db.getHdfAttachmentLcNames(hdfName)
lcName=lcNames[lcIndex]
scNames=db.getHdfAttachmentScNames(hdfName,lcName)
scName=scNames[scIndex]
resNames=db.getHdfAttachmentResNames(hdfName,lcName)
hdfResNames=list(resNames)

db.readHdfAttachmentResults(hdfName,lcName,scName,resNames)

for lcName in db.iter_resultKeyCaseId():
    os.write("LOADCASE: \"%s\"\n"%(lcName))

for scName in db.iter_resultKeySubCaseId():
    os.write("SUBCASE: \"%s\"\n"%(scName))
for lcName,scName in db.iter_resultKeyLcScId():
    os.write("LOADCASE and SUBCASE: \"%s\" - \"%s\"\n"%(lcName,scName))
for resName in db.iter_resultKeyResId():
    os.write("RESULT: \"%s\"\n"%(resName))

for tpName in hdfResNames:
    tmpRes=db.getResultCopy(lcName,scName,tpName)
    if (tmpRes):
        os.write("%-20s%-25s%-60s%-10d\n"%(lcName,scName,tpName,tmpRes.Size))
        os.write("%10d%10d%14g%14g : %s\n"%(tmpRes.getIntId(0),tmpRes.getIntId(1),tmpRes.getRealId(0),tmpRes.getRealId(1),tmpRes.Name))
        Util.printRes(os,tmpRes.Name,tmpRes)
    else:
        print(lcName,scName,tpName)


...

Explanations

The different steps of the Nastran reading of Results in script above are:

The access to FeResPost compiled library.
The creation of a NastranDb FEM database into which the finite element model is read, and Groups are read from a Patran session file.
The loading of HDF5 shared library must be done before any use of other HDF methods of NastranDb class.
An HDF file produced by Nastran is attached to the NastranDb FEM database.
Different HDF methods of the NastranDb class are used to obtained information on the Results stored in the HDF files (name of load cases, sub cases, results...).
An HDF file must always be attached to a NastranDb FEM database in order to have access to its content. No equivalent to the "readXdb" method exists for HDF files. On the other hand, if an HDF file is attached, its content can be read into the database with ``readHdfAttachmentResults'' method. This is generally the most efficient approach to deal with Results stored in HDF files. (Note however that the Results can also be extracted from HDF attachments without importing them first into the FEM database.)
Results are manipulated (printed).

The full script can be found in the Python example (TESTSAT/PYTHON/EX23/testHDF.py).

References

More information on this example, and the manual explaining the functions used in this example are given in FeResPost Reference Manual.

FeResPost Home Page