truss roof

The model can be downloaded. truss-roof.zip

Model

Node

A 2D truss model is developed. To define nodes, use the node command. As this is a 2D model, each node is defined by two coordinates, thus the command looks like this: node <tag> <x> <y>.

# file: node
node  1 15  0
node  2 15  7
node  3 20  7.5
node  4 25  0
node  5 30  0
node  6 35  0
node  7 35  4
node  8 30  6
node  9 25  7
node  10  10  0
node  11  5 0
node  12  5 4
node  13  10  6
node  14  0 0
node  15  20  0
node  16  40  0

Here we define 16 nodes. The truss roof has a span of 40 and an apex height of 7.5.

Element

To model truss elements, we use the T2D2 element. (Yes! The same designation as in ABAQUS!)

# file: element
element T2D2 1 1 2 1 0.2 ! element 1 connecting nodes 1 and 2 using material 1 with cross-sectional area 0.2
element T2D2 2 3 2 1 0.2
element T2D2 3 4 3 1 0.2
element T2D2 4 5 4 1 0.2
element T2D2 5 6 5 1 0.2
# ...

Here the first five elements are shown. The cross sectional area can be directly specified with T2D2. Alternatively, the truss section can be built up manually using basic shapes, see the T2D2S element for details.

You may have noticed that the material model used is not defined. Do not worry, for model definitions, the order is not important, see Structure for explanation.

Load and BC

Definitions of nodes and elements are stored in files node and element. We load it first using file command.

# file: truss-roof.supan
file node
file element

For material, we simply define an elastic Elastic1D material with a Young's modulus of $3E4$.

# file: truss-roof.supan
material Elastic1D 1 30E3

The left-most node 14 is fixed, while the right-most node 16 is roller supported. This means for node 14, both x and y displacements are fixed, while for node 16, only y displacement is fixed. One can use either fix (penalty method) or fix2 (multiplier method) to apply homogeneous boundary conditions. Both shall lead to the same result.

# file: truss-roof.supan
fix2 1 1 14 ! fix x-displacement (dof 1) of node 14
fix2 2 2 14 16 ! fix y-displacement (dof 2) of nodes 14 and 16

For load, we apply a vertical displacement load on top of the apex.

# file: truss-roof.supan
displacement 1 0 -1 2 3 ! a displacement load with tag 1 on node 3 dof 2 (vertical) with a magnitude of -1

The second parameter 0 is a placeholder for amplitude, a 0 means a default Ramp is used.

Analysis

A simple static step is required to analyse the model.

# file: truss-roof.supan
step static 1
set ini_step_size 1
set fixed_step_size true

analyze ! perform analysis

Probe Result

It is possible to probe the simple results of the analysis, for example, one can check the displacement and resistance of node 3 by using the peek command. To record various results, one may want to use recorder command.

peek node 3

The following printout shall be expected.

Node 3:
Coordinate:
   20.0000    7.5000
Displacement:
   0.2238  -1.0000
Resistance:
  -1.7053e-13  -7.4093e+01

Bye

Do not forget to quit.

exit

Results

The deformation is shown.

deformation of truss roof