A collection of OpenSees procedures is shipped with NextFEM Designer, in the file named “procedureXXX.tcl” in the installation folder.
See the manual for pre and postprocessing
See the manual for Response Spectrum analysis library
Response Spectrum analysis for OpenSees
To perform a Response Spectrum analysis based on modal results, use the following command:
dynModal $numModes $spectrum $patternID $comb $csi $dir1 $dir2 $dir3
where $numModes is the number of modes the user wants to combine, $spectrum is the name of the file containing the spectrum points, $patternID is the ID to be given to the load patterns created internally to perform the required linear static analyses, $comb let the user choose whether the SRSS or CQC method should be used, $csi is the damping ratio which is used to calculate the correlation coefficients needed when performing CQC.
The last three parameters ($dir1, $dir2, $dir3), which may assume a value of 0 or 1, are needed to specify the directions associated with the spectrum.
64 bit – updated 18th Aug 2020 – OpenSees 3.2.1
You must be logged in to freely download the program.
NOTE: the Response Spectrum library can encounter memory problems with the official OpenSees executable. If this is the case, compiling by your own the OpenSees framework with VS2017 can help – the official source is here
UmfPack2 solver for OpenSees
Beta version. External solver for OpenSees (any version) which improves the integrated UmfPack. Memory and speed improvements up to 70%; no need to set the LValueFact anymore. Tested with OpenSees 2.4.6. Usage inside Tcl scripts:
system umfpack2
You must be logged in to freely download the program.
NextFEM Designer  Use with OpenSees
User’s (short) guide
NextFEM Designer can act as a pre and post processor for OpenSees.
You can import any of your .tcl models with the command File / Import …. (not Import OpenSees results, this will be used to recorders’ output!) or by dragging the file into the viewport.
This tutorial will use the following portal frame as driving example:
# SET UP 
# units: kN, m, sec
wipe; # clear opensees model
# import procedure008.tcl supplied with NextFEM Designer
source procedure008.tcl
# required by procedures  they can run also for parallel analysis
set pid 0
file mkdir data; # create data directory
model basic ndm 3 ndf 6; # 2 dimensions, 3 dof per node
set modelName "frame_ex"; # model name, best if equal to .tcl filename
# define GEOMETRY 
set LCol 3.0; # column length
set LBeam 6.0; # beam length
set Weight 1000.; # superstructure weight
# mechanical properties
set fyk [expr 235*pow(10,3)]
set ftk [expr 360*pow(10,3)]
set Es [expr 210000*pow(10,3)]
set gammaM0 [expr 1.05]
set fyd [expr $fyk/$gammaM0]
# calculated parameters
set PCol $Weight; # nodal deadload weight per column
set g 9.81; # g acceleration
set Mass [expr $PCol/$g]; # nodal mass
# calculated geometry parameters
set A [expr 53.83*pow(10,4)]; # crosssectional area
set Iy [expr 3692.0*pow(10,8)]; # Column moment of inertia
set Iz [expr 1336.0*pow(10,8)]
set d [expr 190.0*pow(10,3)]
set bf [expr 200.0*pow(10,3)]
set tw [expr 6.5*pow(10,3)]
set tf [expr 10.0*pow(10,3)]
# nodal coordinates:
node 1 0 0 0; # node coords. X, Y, Z
node 2 0 $LCol 0
node 3 $LBeam 0 0
node 4 $LBeam $LCol 0
# Single point constraints  Boundary Conditions
fix 1 1 1 1 1 1 1; # node DX DY RZ
fix 3 1 1 1 1 1 1;
fix 2 0 0 1 1 1 0
fix 4 0 0 1 1 1 0
# nodal masses:
mass 2 $Mass $Mass 0. 0 0 0; # node#, Mx My Mz, Mass=Weight/g, neglect rotational inertia at nodes
mass 4 $Mass $Mass 0. 0 0 0
# Define ELEMENTS & SECTIONS 
set HE200A 1; # assign a tag number to the column section
set HE200ATemp 2
# MATERIAL parameters 
set steelMatID 1; # material ID tag
# 
set fyk [expr 275*pow(10,3)]
set ftk [expr 430*pow(10,3)]
set Es [expr 210000*pow(10,3)]
set nus [expr 0.3]
set Gs [expr $Es/2/(1+$nus)]
set Gammas [expr 78.5/pow(10,0)]
set gammaM0 [expr 1.05]
set fyd [expr $fyk/$gammaM0]
set Bs 0.01; # strainhardening ratio
set R0 18; # control the transition from elastic to plastic branches
set cR1 0.925; # control the transition from elastic to plastic branches
set cR2 0.15; # control the transition from elastic to plastic branches
uniaxialMaterial Steel02 $steelMatID $fyd $Es $Bs $R0 $cR1 $cR2; # MenegottoPinto model
# FIBER SECTION properties 
set nfdw 5; # number of fibers along web depth
set nftw 2; # number of fibers along web thickness
set nfbf 5; # number of fibers along flange width
set nftf 2; # number of fibers along flange thickness
set dw [expr $d  2 * $tf]
set y1 [expr $d/2]
set y2 [expr $dw/2]
set y3 [expr $dw/2]
set y4 [expr $d/2]
set z1 [expr $bf/2]
set z2 [expr $tw/2]
set z3 [expr $tw/2]
set z4 [expr $bf/2]
#
section fiberSec $HE200ATemp {
# nfIJ nfJK yI zI yJ zJ yK zK yL zL
patch quadr $steelMatID $nfbf $nftf $y1 $z4 $y1 $z1 $y2 $z1 $y2 $z4
patch quadr $steelMatID $nftw $nfdw $y2 $z3 $y2 $z2 $y3 $z2 $y3 $z3
patch quadr $steelMatID $nfbf $nftf $y3 $z4 $y3 $z1 $y4 $z1 $y4 $z4
}
set string1 P
set string2 Mz
set string3 Vy
section Aggregator $HE200A $steelMatID $string1 $steelMatID $string2 $steelMatID $string3 section $HE200ATemp
# define geometric transformation: performs a linear geometric transformation of beam stiffness and resisting force from the basic system to the globalcoordinate system
set ColTransfTag 1; # associate a tag to column transformation
geomTransf Linear $ColTransfTag 0 0 1 ;
set BeamTransfTag 2; # associate a tag to column transformation
geomTransf Linear $BeamTransfTag 0 0 1 ;
# element connectivity:
set numIntgrPts 5; # number of integration points for forcebased element
element nonlinearBeamColumn 1 1 2 $numIntgrPts $HE200A $ColTransfTag; # selfexplanatory when using variables
element nonlinearBeamColumn 2 3 4 $numIntgrPts $HE200A $ColTransfTag
element nonlinearBeamColumn 3 2 4 $numIntgrPts $HE200A $BeamTransfTag
# define GRAVITY LOAD 
pattern Plain 1 Linear {
eleLoad ele 3 type beamUniform 20 0; # distributed superstructureweight on beam
}
# define damping proportional to masses and to 1st mode
MDamping 0.05 1
# parameters for the subsequent analyses
set Tol 1.0e3; # convergence tolerance for test
set Tmax 15.0
set dt 0.005
set filePath "record10.30.dat"; # string with the 2 columns plain text seismic record
set ampl 1
set dir 1
# nonlinear static analysis for applying vertical loads
NonLinearStatic $Tol 0.1 10 $modelName
# modal analysis
Modal 3 1 $modelName 1
# dynamic analysis
DynamicAn $Tmax $dt $filePath 1 $dir $Tol $ampl $modelName
The procedure file procedure008.tcl has to be placed in the same folder of your .tcl model and can be imported with the command
source procedure008.tcl
and it contains a series of scripts for setting the analysis quickly, without specifying and studying in deep the parameters to set.
IMPORTANT: the given procedures work for any kind of model. Despite that, NextFEM Designer can read recorders generated by 3D models only (6 dofs per node).
All procedures are given with no warranty and no support; feel free to modify and use them by citing nextfem.it website.
All procedures require modelName, that is a string parameters specifying the name assigned to the model, which is at your will. To properly use NextFEM Designer as a postprocessor, set a modelName equal to the name of the .tcl file.
The most common commands in the procedure file are:
LinearStatic “modelName”
to run a static linear analysis with a simgle load increment.NonLinearStatic $tol $step $nsteps “modelName”
to perform a nonlinear static analysis using load control.# tol : sets the convergence tolerance
# step : the step size
# nsteps : total number of steps
Modal $n $wr “modelName” $args
performs an eigen analysis.# n : the number of modes to be found
# wr : a flag that, if set to 1, allows to write eigenvalues and periods to file. Any other value does nothing.
# args : OPTIONAL argument. Put 1 if you want this procedure to create recorders. This is may be useful to import the deformed shapes in NextFEM Designer.
#Put any other value if the eigen analysis is functional to other types of analysis e.g. adaptive pushover and do not want it to overwrite results over and over.
Pushover $patternStart $type $mode $nodes $masses $cnode $cdof $tol $step $nsteps $modelName $checkProc
performs a pushover analysis.# patternStart :The first free tag. This proc uses patternStart and patternStart+1 IDs to create load patterns.
# type :used to define the type of distribution: 1  mode shaped load pattern, 2  mass proportional load pattern.
# mode :mode required for type 1 load distribution. Ignored for type 2 load distribution.
# nodes: list of nodes where lateral loads are applied.
# masses: list of masses. One per node. Should be in the same order of $nodes argument.
# cnode: control node. It is the node where the displacement is imposed.
# cdof : control dof. The direction of the imposed displacement.
# tol : convergence tolerance.
# step : step size.
# nsteps: number of steps.
SetDamping $flag $csi $args
Sets model damping ratios.# flag :defines damping type.
# 0: mass proportional damping. First mode is set as control mode.
# 1: mass proportional damping. $args contains the control mode.
# 2: Rayleigh damping. $args contains two control modes
#any other values causes an error.
# csi: damping ratio
# args: variable length argument. Contains the modes used to build the damping matrix.
MDamping $csi $modeI
Builds mass proportional damping matrix.#csi :damping ratio
#modeI : control mode
DynamicAn $Tmax $dt $filePath $patternStart $dir $TolDynamic $ampl $modelName
Performs a timehistory dynamic analysis.# Tmax : analysis length.
# dt : reference step
# filePath: file containing timeacceleration pairs.
# patternStart: The first free tag. This proc uses patternStart and patternStart+1 IDs to create load patterns.
# dir: motion direction
# TolDynamic: convergence tolerance.
# ampl : accelerogram scale factor.
To import results in NextFEM Designer, select File / Import OpenSees results. The following mask will be shown:
Tick the checkboxes showed above to import the eigen results (with deformed shapes) and results from the dynamic analysis.
You will be able also to see beam diagrams, if available in the recorders.
Download the example from here: frame_ex

NextFEM rSpectrum for OpenSees
Version C
© NextFEM 20152020 
INDEX
Description
The Response Spectrum library for OpenSees 3.2.1 is available on www.nextfem.it/it/openseestools/
Such library accepts as input a response spectrum (defined in period T vs. acceleration Sa) and calculates the response in terms of displacements, reactions on restrained nodes and element forces. The acceleration must consistent with the model units.
The library is versionspecific – supported OpenSees versions are 2.5.0, 3.0.3 and 3.2.1.
General usage
To use the commands described below, you must preemptively load the DLL with the command:
loadPackage rSpectrum ; # load the dll with the new commands
Response Spectrum Analysis (RSA) performs the following steps:
Reading the input spectra,
Performing an Eigen analysis,
Computation of participation factors,
Creation of load patterns starting from modal forces and spectral information,
Performing a linear elastic analysis and response retrieval,
Modal combination (CQC or SRSS).
Steps 3 to 5 need to be repeated for each mode and excitation direction the user wants to consider. Thus, this type of analysis may become expensive when performed for large models as the responses for each mode and direction should be stored and then combined.
Commands in Response Spectrum Library
WARNING: all the subsequent command example are available in the rSpectrum.dll. To use them from the OpenSees prompt, you have to load a model and to load the DLL with the command:
loadPackage rSpectrum; # load the dll with the new commands
IMPORTANT: place the DLL in the same folder of the model.
IMPORTANT: Such last command can be issued only when the model command has been given (e.g. model BasicBuilder ndm 3 ndf 6).
pFactors
The Tcl command purposely created for this purpose is pFactors whose syntax is the following:
pFactors <file filename> m $numMode <v> <s> <o>
where $numModes is the number of modes the user wants to consider, v sets the verbose mode and the optional flag –file saves the results to a file named filename.
pFactors calculates:
1) Participation factors
2) Participating masses
3) Participating mass ratios
file flag is optional. it redirect the function output to a file. s flag must not be set.";
m flag is mandatory and must be followed by an integer flag.
It defines for how many modes the command has to calculate the results.
v flag is optional. It enables the verbose mode to check the progress.
s flag is optional. If set, matrix results won't be displayed to screen or written to file.
o flag is optional. It disables the output to a variable.
Without this flag you can write something like:
set results [pFactors m $numModes]
pFactors also stores M*phi to allow the retrieval with getMphi command (useful for RSA);
The output given by this command is a list structured as follows:
{1} {2} {3} where each number represent one the three groups of values
described above. Each list is made up of $numModes lists:
{0} ...{i} ...{$numModes1}
Each one of these lists contains ndf values, where ndf is the number of dofs
per node:
0th value 1st value ...jth value ...(ndf1)th value
The output file “factors.dat” contains:
1) Participation factors
2) Participating masses (in units consistent with the model)
3) Participating mass ratios
printG
printG is an alias of pFactors, and can be useful to print again the previously computed values.
printG <d> m $numMode <v> <s> <o>
printK
It prints the dense stiffness matrix of the model.
printK <file filename.dat>
printM
It prints the dense mass matrix of the model.
printM <file filename.dat>
printC
It prints the dense damping matrix of the model.
printEleK
It prints stiffness contribution of each element in the model.
Modal dynamic analysis  dynModal
To perform a Response Spectrum analysis based on modal results, use the following command:
dynModal $numModes $spectrum $patternID $comb $csi $dir1 $dir2 $dir3
where $numModes is the number of modes the user wants to combine, $spectrum is the name of the file containing the spectrum points, $patternID is the ID to be given to the load patterns created internally to perform the required linear static analyses, $comb let the user choose whether the SRSS (Eq. 1) or CQC (Eq. 2) method should be used, $csi is the damping ratio which is used to calculate the correlation coefficients needed when performing CQC.
The last three parameters ($dir1, $dir2, $dir3), which may assume a value of 0 or 1, are needed to specify the directions associated with the spectrum.
(1)
(2)
The command dynModal gives as output:
1) nodal displacement envelope
2) nodal reaction envelope
3) element forces envelope
dynWrapper
It could be easier to access the dynWrapper function from procedure009.tcl supplied with NextFEM Designer. The command syntax is the following:
DynWrapper $numModes $patternID $comb $csi $directions $spectra
where
$numModes is the number of modes the user wants to combine,
$patternID is the ID to be given to the load patterns created internally when dynModal is called,
$comb let the user choose whether the SRSS or CQC method should be used,
$csi is the damping ratio which is used to calculate the correlation coefficients needed when performing CQC.
The $directions parameter is a list containing the directions grouped by spectrum, while $spectra is a list containing the filenames where the spectra are saved. The correlation between these two parameters is given by the order used to fill the lists.
Examples: for the same spectrum in X and Y directions:
DynWrapper 12 100 2 0.05 {{X Y}} {"slvOS.txt"} $modelName
For 2 difference spectrum in X and Y directions:
DynWrapper 12 100 2 0.05 {{X} {Y}} {"specX.txt" "specY.txt"} $modelName
For the same spectrum in X and Y directions and a different spectrum in Z:
DynWrapper 12 100 2 0.05 {{X Y} {Z}} {"specXY.txt" "specZ.txt"} $modelName
The command produces 4 output files:
RSdisp.out contains the displacement of each node, separated by spaces. The nodes are ordered like in any other recorder;
RSreact.out contains the reaction of each node, separated by spaces. The nodes are ordered like in any other recorder;
RSforces.out contains the element forces of each element in the model, separated by spaces. The nodes are ordered like in any other recorder but in global coordinates for each element;
RSpartFact.out contains the output of pFactors command. For the output order, see the pFactors command description.
The results for each file are appended by default to each file above (1 row per analysis). To have a new file each time the analysis runs, change lines 1987 and subsequent ones in procedure008.tcl as:
set fo [open "RSreact.out" w]
License
NextFEM, 20152020
By using this library, the user accomplishes to the following terms and conditions.
By using the software provided by NextFEM, you agree to be bound by these terms and conditions. The contents of the NextFEM site and all software provided, including the following terms and conditions, are subjected to changes and regular updates.
NextFEM is not responsible for the results obtained with this software of with any of its parts.
NextFEM is not liable to any part for direct, indirect, special, collateral, incidental or consequential damages, including lost profits, arising with the use of this software.
NextFEM provides this software "as is" and has no obligations to provide maintenance, support, updates, enhancements or modifications.
The disassembly of this library is prohibited.