Problems with eleLoad

[jazzieman]

I'm currently working on a 3D RC frame model on openseespy. I'm having several problems which I've managed to resolve some of them. Now, while trying correct and error I became aware that when I use the command eleLoad to apply a load to a beam or column (with type 'beamUniform' for example) I get zeros on the nodes/elements responses. For the sake of verifying if the error is within my code, I used the example code 5 in of the structural examples (14.1.5. Reinforced Concrete Frame Gravity Analysis, https://openseespydoc.readthedocs.io/en ... avity.html) and changed the loads applied the nodes for a 'beamUniform' on it works. Now, if I change the 2D model to a 3D one, I get zero reactions or forces at nodes/elements.

Code: Select all

print("==========================")

from openseespy.opensees import *
import openseespy.postprocessing.Get_Rendering as opsplt
wipe()
print("Starting RCFrameGravity example")

# Create ModelBuilder (with two-dimensions and 3 DOF/node)
model('basic', '-ndm', 3, '-ndf', 6)

# Create nodes
# ------------

# Set parameters for overall model geometry
width = 360.0
height = 144.0

# Create nodes
#    tag, X, Y
node(1, 0.0, 0.0, 0.0)
node(2, width, 0.0, 0.0)
node(3, 0.0, height, 0.0)
node(4, width, height, 0.0)

# Fix supports at base of columns
#   tag, DX, DY, RZ
fix(1, 1, 1, 1, 1, 1, 1)
fix(2, 1, 1, 1, 1, 1, 1)

# Define materials for nonlinear columns
# ------------------------------------------
# CONCRETE                   tag  f'c    ec0    f'cu   ecu
# Core concrete (confined)
uniaxialMaterial('Concrete01', 1, -6.0, -0.004, -5.0, -0.014)

# Cover concrete (unconfined)
uniaxialMaterial('Concrete01', 2, -5.0, -0.002, 0.0, -0.006)

# STEEL
# Reinforcing steel
fy = 60.0;  # Yield stress
E = 30000.0;  # Young's modulus
#                         tag  fy E0    b
uniaxialMaterial('Steel01', 3, fy, E, 0.01)

# Define cross-section for nonlinear columns
# ------------------------------------------

#  some parameters
colWidth = 15
colDepth = 24

cover = 1.5
As = 0.60  # area of no. 7 bars

# some variables derived from the parameters
y1 = colDepth / 2.0
z1 = colWidth / 2.0

section('Fiber', 1, '-GJ', 1e100)

# Create the concrete core fibers
patch('rect', 1, 10, 1, cover - y1, cover - z1, y1 - cover, z1 - cover)

# Create the concrete cover fibers (top, bottom, left, right)
patch('rect', 2, 10, 1, -y1, z1 - cover, y1, z1)
patch('rect', 2, 10, 1, -y1, -z1, y1, cover - z1)
patch('rect', 2, 2, 1, -y1, cover - z1, cover - y1, z1 - cover)
patch('rect', 2, 2, 1, y1 - cover, cover - z1, y1, z1 - cover)

# Create the reinforcing fibers (left, middle, right)
layer('straight', 3, 3, As, y1 - cover, z1 - cover, y1 - cover, cover - z1)
layer('straight', 3, 2, As, 0.0, z1 - cover, 0.0, cover - z1)
layer('straight', 3, 3, As, cover - y1, z1 - cover, cover - y1, cover - z1)

# Define column elements
# ----------------------

# Geometry of column elements
#                tag

geomTransf('PDelta', 1, *[0,0,1])

# Number of integration points along length of element
np = 5

# Lobatto integratoin
beamIntegration('Lobatto', 1, 1, np)

# Create the coulumns using Beam-column elements
#               e            tag ndI ndJ transfTag integrationTag
eleType = 'forceBeamColumn'
element(eleType, 1, 1, 3, 1, 1)
element(eleType, 2, 2, 4, 1, 1)

# Define beam elment
# -----------------------------

# Geometry of column elements
#                tag
geomTransf('Linear', 2, *[0,0,1])


#  a parameter for the axial load
P = 180.0;  # 10% of axial capacity of columns  

# Create the beam element                       
#                           tag, ndI, ndJ, A,     E,      G,     J,    Iy,   Iz,   transfTag
element('elasticBeamColumn', 3,   3,   4, 360.0, 4030.0, 1733, 1e100, 8640, 8640.0, 2)


# Define gravity loads
# --------------------


# Create a Plain load pattern with a Linear TimeSeries
timeSeries('Linear', 1)
pattern('Plain', 1, 1)

eleLoad('ele', 3, '-type', '-beamUniform', 2*P/width, 0.)
# Create nodal loads at nodes 3 & 4
#    nd  FX,  FY, MZ
# load(3, 0.0, -P, 0.0)
# load(4, 0.0, -P, 0.0)

# ------------------------------
# End of model generation
# ------------------------------


# ------------------------------
# Start of analysis generation
# ------------------------------

# Create the system of equation, a sparse solver with partial pivoting
system('BandGeneral')

# Create the constraint handler, the transformation method
constraints('Transformation')

# Create the DOF numberer, the reverse Cuthill-McKee algorithm
numberer('RCM')

# Create the convergence test, the norm of the residual with a tolerance of
# 1e-12 and a max number of iterations of 10
test('NormDispIncr', 1.0e-12, 10, 3)

# Create the solution algorithm, a Newton-Raphson algorithm
algorithm('Newton')

# Create the integration scheme, the LoadControl scheme using steps of 0.1
integrator('LoadControl', 0.1)

# Create the analysis object
analysis('Static')

# ------------------------------
# End of analysis generation
# ------------------------------


# ------------------------------
# Finally perform the analysis
# ------------------------------

# perform the gravity load analysis, requires 10 steps to reach the load level
analyze(10)

# Print out the state of nodes 3 and 4
# print node 3 4

# Print out the state of element 1
# print ele 1
reactions()
u3 = nodeDisp(3, 2)
u4 = nodeDisp(4, 2)

results = open('results.out', 'a+')

if abs(u3 + 0.0183736) < 1e-6 and abs(u4 + 0.0183736) < 1e-6:
    results.write('PASSED : RCFrameGravity.py\n')
    print("Passed!")
else:
    results.write('FAILED : RCFrameGravity.py\n')
    print("Failed!")

results.close()

print("==========================")

# Display the active model with node tags only
opsplt.plot_model('nodes','elements')

Now, for the code to run (for the 3D version) I had to eliminate the hyphen before 'ele' at the eleLoad command, otherwise I get a singular matrix error (viewtopic.php?f=12&t=67585&p=116955#p116955). Don't know what I'm doing wrong. Any help would be appreciated.

[mhscott]

Please try a simply-supported elastic beam with distributed load and see if you can get that to work.

[jazzieman]

Professor, thanks for the reply. I tried a simply supported beam (in 3D) and still getting zero response.

Code: Select all

from openseespy.opensees import *
import openseespy.postprocessing.Get_Rendering as opsplt
wipe()


# Create ModelBuilder (with 3 dimensions and 6 DOF/node)
model('basic', '-ndm', 3, '-ndf', 6)

# Set parameters for overall model geometry
width = 360.0


# Create nodes
#    tag, X, Y, Z
node(1, 0.0, 0.0, 0.0)
node(2, width, 0.0, 0.0)


# Boundary Conditions
fix(1, 1, 1, 1, 0, 0, 0)
fix(2, 0, 1, 0, 0, 0, 0)

# Define materials for nonlinear columns
# ------------------------------------------
# CONCRETE                   tag  f'c    ec0    f'cu   ecu
# Core concrete (confined)
uniaxialMaterial('Concrete01', 1, -6.0, -0.004, -5.0, -0.014)

# Cover concrete (unconfined)
uniaxialMaterial('Concrete01', 2, -5.0, -0.002, 0.0, -0.006)

# STEEL
# Reinforcing steel
fy = 60.0;  # Yield stress
E = 30000.0;  # Young's modulus
#                         tag  fy E0    b
uniaxialMaterial('Steel01', 3, fy, E, 0.01)

# Define cross-section
# ------------------------------------------

#  some parameters
colWidth = 15
colDepth = 24

cover = 1.5
As = 0.60  # area of no. 7 bars

# some variables derived from the parameters
y1 = colDepth / 2.0
z1 = colWidth / 2.0

section('Fiber', 1, '-GJ', 1e10)

# Create the concrete core fibers
patch('rect', 1, 10, 1, cover - y1, cover - z1, y1 - cover, z1 - cover)

# Create the concrete cover fibers (top, bottom, left, right)
patch('rect', 2, 10, 1, -y1, z1 - cover, y1, z1)
patch('rect', 2, 10, 1, -y1, -z1, y1, cover - z1)
patch('rect', 2, 2, 1, -y1, cover - z1, cover - y1, z1 - cover)
patch('rect', 2, 2, 1, y1 - cover, cover - z1, y1, z1 - cover)

# Create the reinforcing fibers (left, middle, right)
layer('straight', 3, 3, As, y1 - cover, z1 - cover, y1 - cover, cover - z1)
layer('straight', 3, 2, As, 0.0, z1 - cover, 0.0, cover - z1)
layer('straight', 3, 3, As, cover - y1, z1 - cover, cover - y1, cover - z1)

# Transformation:
geomTransf('Linear', 1, *[0,0,1])

# Distributed load:
W = 180.0/width;

# Create the beam element                       
#                           tag, ndI, ndJ, A,     E,      G,     J,    Iy,   Iz,   transfTag
element('elasticBeamColumn', 1,   1,   2, 360.0, 4030.0, 1733, 1e10, 8640, 8640.0, 1)


# Create a Plain load pattern with a Linear TimeSeries
timeSeries('Linear', 1)
pattern('Plain', 1, 1)

# Define gravity loads
# --------------------
eleLoad('ele', 1, '-type', '-beamUniform', W, 0.)


# ------------------------------
# End of model generation
# ------------------------------


# ------------------------------
# Start of analysis generation
# ------------------------------

# Create the system of equation, a sparse solver with partial pivoting
system('BandGeneral')

# Create the constraint handler, the transformation method
constraints('Transformation')

# Create the DOF numberer, the reverse Cuthill-McKee algorithm
numberer('RCM')

# Create the convergence test, the norm of the residual with a tolerance of
# 1e-12 and a max number of iterations of 10
test('NormDispIncr', 1.0e-12, 10, 3)

# Create the solution algorithm, a Newton-Raphson algorithm
algorithm('Newton')

# Create the integration scheme, the LoadControl scheme using steps of 0.1
integrator('LoadControl', 0.1)

# Create the analysis object
analysis('Static')

# ------------------------------
# End of analysis generation
# ------------------------------


# ------------------------------
# Finally perform the analysis
# ------------------------------

# perform the gravity load analysis, requires 10 steps to reach the load level
analyze(10)

# Obtain reactions:
reactions()


# Display the active model with node tags only
opsplt.plot_model('nodes','elements')

[mhscott]

Thanks for the elastic beam.

• You'll need to use -ele instead of ele
• Your boundary conditions are not sufficient. You have node 1 as 1 1 1 0 0 0 and node 2 as 0 1 0 0 0 0 - you need to fix torsion at one and and also out of plane translation at node 2 - so for node 1 use 1 1 1 1 0 0 and for node 2 use 0 1 1 0 0 0

[mhscott]

In the RC frame script, GJ is set to 1e100 for the section and the elastic beam!!! Reduce that to something reasonable. Also, use -ele.

[jazzieman]

Thanks professor, that worked!! I'm still having problems with my 3D RC frame model, but they are related to another topic. Again, thanks!!