Elastic Frame Example
This example is of an elastic frame structure, as shown in the figure, subject to static loads. Here is the file: ElasticFrame.tcl
NOTE:
- The lines in the dashed boxes are lines that appear in the input file.
- all lines that begin with # are comments, they are ignored by the program (interpreter) but are useful for documenting the code. When creating your own input scripts you are highly encouraged to use comments.
Parameters
Before we build the model we are going to set some parameters using tcl variables and expression evaluation. We are going to set variables for PI, the gravtational constant g, and variables for each of our floor masses.
set PI [expr 2.0 * asin(1.0)] set g 386.4 set m1 [expr 2370.0/(2.0*4*$g)]; # 2 frames in building, 4 nodes per floor set m2 [expr 2370.0/(2.0*4*$g)] set m3 [expr 1940.0/(2.0*4*$g)]
Model
The model consists of sixteen nodes, twenty one elastic beam-column elements, a single load pattern with distributed loads, and constraints totally fixing the nodes at the base of the building. There are no material objects associated with the elastic elements, but there are geometric transformations. For this example all the columns have a PDelta transformation, and all the beams a linear transformation.
# Units: kips, in, sec
# Remove existing model
wipe
# Create ModelBuilder (with two-dimensions and 2 DOF/node)
model BasicBuilder -ndm 2 -ndf 3
# Create nodes & add to Domain -
# command: node nodeId xCrd yCrd <-mass $massX $massY $massRz>
# NOTE: mass is optional
node 1 0.0 0.0
node 2 360.0 0.0
node 3 720.0 0.0
node 4 1080.0 0.0
node 5 0.0 162.0 -mass $m1 $m1 0.0
node 6 360.0 162.0 -mass $m1 $m1 0.0
node 7 720.0 162.0 -mass $m1 $m1 0.0
node 8 1080.0 162.0 -mass $m1 $m1 0.0
node 9 0.0 324.0 -mass $m2 $m2 0.0
node 10 360.0 324.0 -mass $m2 $m2 0.0
node 11 720.0 324.0 -mass $m2 $m2 0.0
node 12 1080.0 324.0 -mass $m2 $m2 0.0
node 13 0.0 486.0 -mass $m3 $m3 0.0
node 14 360.0 486.0 -mass $m3 $m3 0.0
node 15 720.0 486.0 -mass $m3 $m3 0.0
node 16 1080.0 486.0 -mass $m3 $m3 0.0
# Set the boundary conditions - command: fix nodeID xResrnt? yRestrnt? rZRestrnt?
fix 1 1 1 1
fix 2 1 1 1
fix 3 1 1 1
fix 4 1 1 1
# Define geometric transformations for beam-column elements
geomTransf Linear 1; # beams
geomTransf PDelta 2; # columns
# Define elements
# Create elastic beam-column elements -
# command: element elasticBeamColumn eleID node1 node2 A E Iz geomTransfTag
# Define the Columns
element elasticBeamColumn 1 1 5 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 2 5 9 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 3 9 13 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 4 2 6 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 5 6 10 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 6 10 14 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 7 3 7 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 8 7 11 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 9 11 15 91.4 29000.0 4330.0 2; # W14X311
element elasticBeamColumn 10 4 8 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 11 8 12 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 12 12 16 75.6 29000.0 3400.0 2; # W14X257
# Define the Beams
element elasticBeamColumn 13 5 6 34.7 29000.0 5900.0 1; # W33X118
element elasticBeamColumn 14 6 7 34.7 29000.0 5900.0 1; # W33X118
element elasticBeamColumn 15 7 8 34.7 29000.0 5900.0 1; # W33X118
element elasticBeamColumn 16 9 10 34.2 29000.0 4930.0 1; # W30X116
element elasticBeamColumn 17 10 11 34.2 29000.0 4930.0 1; # W30X116
element elasticBeamColumn 18 11 12 34.2 29000.0 4930.0 1; # W30X116
element elasticBeamColumn 19 13 14 20.1 29000.0 1830.0 1; # W24X68
element elasticBeamColumn 20 14 15 20.1 29000.0 1830.0 1; # W24X68
element elasticBeamColumn 21 15 16 20.1 29000.0 1830.0 1; # W24X68
Analysis - Gravity Load
We will now show the commands to perform a gravity load analysis. As the model is elastic we will use a Linear solution algorithm and use a single step of load control to get us to the desired load level.
# Create the system of equation
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
Output Specification
For this analysis, we will record the displacement at node 4, and all the element forces expressed both in the global coordinate system and the local system.
Perform The Analysis
After the objects for the model, analysis and output has been defined we now perform the analysis.
analyze 1
Print Information to Screen
In addition to using recorders, it is possible to specify output using the print and puts commands. When no file identifiers are provided, these commands will print results to the screen.
puts "node 4 displacement: [nodeDisp 4]" print node 4 print element
Results
When you run this script, you should see the following printed to the screen:
In addition, your directory should contain the following 3 files with the data shown: