# Elastic Frame Example
__NOTOC__ This example is of an elastic frame structure, as shown in the figure, subject to static loads. Here is the file: ElasticFrame.tcl
NOTE:
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. We are using the tcl set and expr commands.
<pre> set PI [expr 2.0 * asin(1.0)] set g 386.4 set ft 12.0 set m1 [expr 1185.0/(4*$g)]; # 4 nodes per floor set m2 [expr 1185.0/(4*$g)] set m3 [expr 970.0/(4*$g)] set w1 [expr 1185.0/(90*$ft)] set w2 [expr 1185.0/(90*$ft)] set w3 [expr 970.0/(90*$ft)] </pre>
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.
<pre>
wipe
model BasicBuilder -ndm 2 -ndf 3
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 $m3 0.0
fix 1 1 1 1 fix 2 1 1 1 fix 3 1 1 1 fix 4 1 1 1
geomTransf Linear 1; # beams geomTransf PDelta 2; # columns
element elasticBeamColumn 1 1 5 75.6 29000.0 3400.0 2; # W14X257 element elasticBeamColumn 2 5 9 75.6 29000.0 3400.0 2; # W14X257 element elasticBeamColumn 3 9 13 75.6 29000.0 3400.0 2; # W14X257 element elasticBeamColumn 4 2 6 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 5 6 10 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 6 10 14 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 7 3 7 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 8 7 11 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 9 11 15 91.4 29000.0 4330.0 2; # W14X311 element elasticBeamColumn 10 4 8 75.6 29000.0 3400.0 2; # W14X257 element elasticBeamColumn 11 8 12 75.6 29000.0 3400.0 2; # W14X257 element elasticBeamColumn 12 12 16 75.6 29000.0 3400.0 2; # W14X257
element elasticBeamColumn 13 5 6 34.7 29000.0 5900.0 1; # W33X118 element elasticBeamColumn 14 6 7 34.7 29000.0 5900.0 1; # W33X118 element elasticBeamColumn 15 7 8 34.7 29000.0 5900.0 1; # W33X118 element elasticBeamColumn 16 9 10 34.2 29000.0 4930.0 1; # W30X116 element elasticBeamColumn 17 10 11 34.2 29000.0 4930.0 1; # W30X116 element elasticBeamColumn 18 11 12 34.2 29000.0 4930.0 1; # W30X116 element elasticBeamColumn 19 13 14 20.1 29000.0 1830.0 1; # W24X68 element elasticBeamColumn 20 14 15 20.1 29000.0 1830.0 1; # W24X68 element elasticBeamColumn 21 15 16 20.1 29000.0 1830.0 1; # W24X68
pattern Plain 1 1 { eleLoad -ele 13 14 15 -type -beamUniform -$w1 eleLoad -ele 16 17 18 -type -beamUniform -$w2 eleLoad -ele 19 20 21 -type -beamUniform -$w3 } </pre>
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.
<pre>
system BandSPD
numberer RCM
constraints Plain
integrator LoadControl 1.0
algorithm Linear
analysis Static </pre>
After the objects for the model, analysis and output has been defined we now perform the analysis.
<pre> analyze 1 </pre>
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. We use the nodeReaction command to return the reactions at the individual nodes and the tcl lindex command to obtain the values from these lists.
<pre>
reactions
set node1Rxn [nodeReaction 1]; # nodeReaction command returns nodal reactions for specified node in a list set node2Rxn [nodeReaction 2] set node3Rxn [nodeReaction 3] set node4Rxn [nodeReaction 4]
set inputedFy [expr -$Load1-$Load2-$Load3]; # loads added negative Fy direction to ele set computedFx [expr [lindex $node1Rxn 0]+[lindex $node2Rxn 0]+[lindex $node3Rxn 0]+[lindex $node4Rxn 0]] set computedFy [expr [lindex $node1Rxn 1]+[lindex $node2Rxn 1]+[lindex $node3Rxn 1]+[lindex $node4Rxn 1]]
puts "\nEqilibrium Check After Gravity:" puts "SumX: Inputed: 0.0 + Computed: $computedFx = [expr 0.0+$computedFx]" puts "SumY: Inputed: $inputedFy + Computed: $computedFy = [expr $inputedFy+$computedFy]" </pre>
Now we prepare to add our lateral loads to the model. First we need to set the gravity loads acting constant, i.e. we do not want them changing as we apply more loads to the model. Then we will create load pattern with nodal loads to add to the model.
<pre>
loadConst -time 0.0
timeSeries Linear 2 pattern Plain 2 2 { load 13 220.0 0.0 0.0 load 9 180.0 0.0 0.0 load 5 90.0 0.0 0.0 } </pre>
We will create an element recorder to record the forces at the bottom story columns.
<pre> recorder Element -file eleForces.out -ele 1 4 7 10 forces </pre>
After the objects for the model, analysis and output has been defined we now perform the analysis.
<pre> analyze 1 </pre>
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.
<pre> reactions
set node1Rxn [nodeReaction 1]; # nodeReaction command returns nodal reactions for specified node in a list set node2Rxn [nodeReaction 2] set node3Rxn [nodeReaction 3] set node4Rxn [nodeReaction 4]
set inputedFx [expr 220.0+180.0+90.0] set computedFx [expr [lindex $node1Rxn 0]+[lindex $node2Rxn 0]+[lindex $node3Rxn 0]+[lindex $node4Rxn 0]] set computedFy [expr [lindex $node1Rxn 1]+[lindex $node2Rxn 1]+[lindex $node3Rxn 1]+[lindex $node4Rxn 1]]
puts "\nEqilibrium Check After Lateral Loads:" puts "SumX: Inputed: $inputedFx + Computed: $computedFx = [expr $inputedFx+$computedFx]" puts "SumY: Inputed: $inputedFy + Computed: $computedFy = [expr $inputedFy+$computedFy]"
print ele 1 4 7 19 </pre>
After the lateral load analysis has completed we will look at the period of the structure. To do this we use the eigenvalue command to obtain the eigenvalues. These are returned in a tcl list. From the list we obtain the eigenvalue for the mode using the tcl lindex command and use the expr command to determine the period.
<pre> set eigenValues [eigen 5]
puts "\nEigenvalues:" set eigenValue [lindex $eigenValues 0] puts "T[expr 0+1] = [expr 2*$PI/sqrt($eigenValue)]" set eigenValue [lindex $eigenValues 1] puts "T[expr 1+1] = [expr 2*$PI/sqrt($eigenValue)]" set eigenValue [lindex $eigenValues 2] puts "T[expr 2+1] = [expr 2*$PI/sqrt($eigenValue)]" set eigenValue [lindex $eigenValues 3] puts "T[expr 3+1] = [expr 2*$PI/sqrt($eigenValue)]" set eigenValue [lindex $eigenValues 4] puts "T[expr 4+1] = [expr 2*$PI/sqrt($eigenValue)]"
recorder Node -file eigenvector.out -nodeRange 5 16 -dof 1 2 3 eigen 0
record </pre>
When you run this script, you should see the following printed to the screen: