|
|
|
|
The first example is a simple truss structure. The purpose of this example is to show that model generation in OpenSees can resemble typical finite element analysis programs with the definition of nodes, materials, elements, loads and constraints. The example also demonstrates how an analysis object is 'built' from component objects.
This example is of a linear-elastic three bar truss, as shown in the figure, subject to static loads.
Files Required
Model
The model consists of four nodes, three truss elements, a single load pattern with a nodal load acting at node 4, and constraints at the three support nodes. Since the truss elements have the same elastic material, a single Elastic material object is created.
Analysis
The model is linear, so we use a solution Algorithm of type Linear. Even though the solution is linear, we have to select a procedure for applying the load, which is called an Integrator. For this problem, a LoadControl integrator advances the solution. The equations are formed using a banded system, so the System is BandSPD (banded, symmetric positive definite). This is a good choice for most moderate size models. The equations have to be numbered, so typically an RCM numberer object is used (for Reverse Cuthill-McKee). The constraints are most easily represented with a Plain constraint handler.
Once all the components of an analysis are defined, the Analysis object itself is created. For this problem a Static Analysis object is used.
Output Specification
When the analysis is complete the state of node 4 and all three elements will be printed to the screen. Nothing is recorded for later use.
OpenSees Script
The Tcl script for the example is shown below. A comment is indicated by a \# symbol. In the comments below, the syntax for important commands are given.
# OpenSees Example 1.1
# OpenSees Primer
#
# Units: kips, in, sec
# ------------------------------
# Start of model generation
# ------------------------------
# Create ModelBuilder (with two-dimensions and 2 DOF/node)
model BasicBuilder -ndm 2 -ndf 2
# Create nodes & add to Domain - command: node nodeId xCrd yCrd
node 1 0.0 0.0
node 2 144.0 0.0
node 3 168.0 0.0
node 4 72.0 96.0
# Set the boundary conditions - command: fix nodeID xResrnt? yRestrnt?
fix 1 1 1
fix 2 1 1
fix 3 1 1
# Define materials for truss elements
# -----------------------------------
# Create Elastic material prototype - command: uniaxialMaterial Elastic matID E
uniaxialMaterial Elastic 1 3000
# Define elements
# ---------------
# Create truss elements - command: element truss trussID node1 node2 A matID
element truss 1 1 4 10.0 1
element truss 2 2 4 5.0 1
element truss 3 3 4 5.0 1
# Define loads
# ------------
# Create a Plain load pattern with a linear TimeSeries
pattern Plain 1 "Linear" {
# Create the nodal load - command: load nodeID xForce yForce
load 4 100 -50
}
# ------------------------------
# End of model generation
# ------------------------------
# ------------------------------
# Start of analysis generation
# ------------------------------
# Create the system of equation, a SPD using a band storage scheme
system BandSPD
# Create the DOF numberer, the reverse Cuthill-McKee algorithm
numberer RCM
# Create the constraint handler, a Plain handler is used as homo constraints
constraints Plain
# Create the integration scheme, the LoadControl scheme using steps of 1.0
integrator LoadControl 1.0
# Create the solution algorithm, a Linear algorithm is created
algorithm Linear
# create the analysis object
analysis Static
# ------------------------------
# End of analysis generation
# ------------------------------
# ------------------------------
# Start of recorder generation
# ------------------------------
# create a Recorder object for the nodal displacements at node 4
recorder Node -file example.out -load -node 4 -dof 1 2 disp
# --------------------------------
# End of recorder generation
# ---------------------------------
# ------------------------------
# Finally perform the analysis
# ------------------------------
# Perform the analysis
analyze 1
# Print the current state at node 4 and at all elements
print node 4
print ele
Results
Node: 4
Coordinates : 72 96
commitDisps: 0.530093 -0.177894
unbalanced Load: 100 -50
Element: 1 type: Truss iNode: 1 jNode: 4 Area: 10 Total Mass: 0
strain: 0.00146451 axial load: 43.9352
unbalanced load: -26.3611 -35.1482 26.3611 35.1482
Material: Elastic tag: 1
E: 3000 eta: 0
Element: 2 type: Truss iNode: 2 jNode: 4 Area: 5 Total Mass: 0
strain: -0.00383642 axial load: -57.5463
unbalanced load: -34.5278 46.0371 34.5278 -46.0371
Material: Elastic tag: 1
E: 3000 eta: 0
Element: 3 type: Truss iNode: 3 jNode: 4 Area: 5 Total Mass: 0
strain: -0.00368743 axial load: -55.3114
unbalanced load: -39.1111 39.1111 39.1111 -39.1111
Material: Elastic tag: 1
E: 3000 eta: 0
For the node, displacements and loads are given. For the truss elements, the axial strain and force are provided along with the resisting forces in the global coordinate system.
The file example.out, specified in the recorder command, provides the nodal displacements for the x and y directions of node 4. The file consists of a single line of code:
Results
1.0 0.530093 -0.177894
The 1.0 corresponds to the load factor (pseudo time) in the model at which point the recorder was invoked. The 0.530093 and -0.177894 correspond to the response at node 4 for the 1 and 2 degree-of-freedom. Note that if more analysis steps had been performed, the file would contain a line for every analysis step that completed successfully.
|
|
|