continuous beam hinge support

[vesna]

To build a continuous beam in OpenSees, for nodes under support restrain vertical displacement and release the rotation and at all but one node release horizontal displacement (e.g., fix 5 0 1 0; # at node 5 restrain vertical displacement).

[vesna]

If you want to calculate the stiffness matrix of a continuous beam, first you need to identify the degrees of freedom. The stiffness matrix koefficient Kij is a force at displacement/rotation DOF i due to unit displacement/rotation at DOF j, with all other displacement/rotation DOFs equal to zero. For a continous beam, the only degrees of freedom are rotations above supports. For you to create the stiffness matrix using OpenSees you will have to do the following:

assume the beam has three spans of length 10 and end supports are fixed:

wipe
model BasicBuilder -ndm 2 -ndf 3;
set L 10.0

node 1 0. 0.
node 2 [expr 1*$L] 0.
node 3 [expr 2*$L] 0.
node 4 [expr 3*$L] 0.

#there are two degrees of freedom; rotation at node 2 and at node 3
#to calculate stiffness coefficients due to unit rotation at node 2

fix 1 1 1 1
fix 2 0 1 0
fix 3 0 1 1
fix 4 0 1 1

set TransfTag 1
geomTransf Linear $TransfTag;
set ABeam 1.0
set Iz 1.0
set E 29000

# define elements
element elasticBeamColumn 1 1 2 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 2 2 3 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 3 3 4 $ABeam $E $Iz $TransfTag;

#define load pattern (unit rotation at node 1)
timeSeries Linear 1
pattern Plain 1 1 {
sp 2 3 1.0
}

#define analysis objects
integrator LoadControl 0.2
algorithm Linear
numberer RCM
constraints Transformation
system ProfileSPD
analysis Static

analyze 5

set a [eleResponse 1 forces]
set b [eleResponse 2 forces]
puts " k11 [lindex $a 5]"
puts " k21 [lindex $b 5]"

set rot [nodeDisp 2 3]

puts "rot $rot"

for stiffness coefficient k22 you will need to slightly modify the code given above.

[vesna]

I am not sure I understand what you are trying to model. Are you talking about series of simple supported beams? To make moment release at the beam end equalDOF command is the right one to use.

If you want to model conventional continuous beam with pinned supports here is an example:

wipe
model BasicBuilder -ndm 2 -ndf 3;
set L 10.0

node 1 0. 0.
node 2 [expr 1*$L] 0.
node 3 [expr 2*$L] 0.
node 4 [expr 3*$L] 0.


fix 1 1 1 0
fix 2 1 1 0
fix 3 1 1 0
fix 4 1 1 0

set TransfTag 1
geomTransf Linear $TransfTag;
set ABeam 1.0
set Iz 1.0
set E 29000

# define elements
element elasticBeamColumn 1 1 2 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 2 2 3 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 3 3 4 $ABeam $E $Iz $TransfTag;

For this example, moments at the ends of the continuous beam will be zero and under intermediate supports nonzero.

[cromax]

thanks vesna

for continuous beam your example is clear.

I am sorry but my account has been erased and I can thanky you only now.

Excuse me, can you post a example where it is realised ( a 3d problem with 6 degree of freedom for node) a contiunuous beam supported by column fixed at the base and with head hinge. How can I simulate frame (column head) end release for rotation only?

I do not understand how use zerolenght or equalDOF. In my example different values (always hight) of the stiffness of zerolenght to fix translation degree (dir 1 2 3) of freedom and (alway small) for rotational stiffness (4 5 6) have different results during transient analysis. why?


Thanks


cromax

[cromax]

Dear all


sorry for the insistence.


I really need an example on the rotation end release in opensees for frame eelement in 3D problems (6 bdegrre of freedom for nodes).

can somebody post or send me (cromax@email.it) an example in opensees?

thanks very much

cromax

[vesna]

Here is a 2D example of a frame with braces where braces have hinges at both ends. If you understand the 2D the example, you will easily extrapolate it to 3D.

wipe
model basic -ndm 2 -ndf 3


# Set parameters for overall model geometry
set width 360
set height 144

# nodes
node 1 0.0 0.0
node 2 $width 0.0
node 3 0.0 $height
node 4 $width $height

node 11 0.0 0.0
node 22 $width 0.0
node 33 0.0 $height
node 44 $width $height

# constraints
fix 1 1 1 1
fix 2 1 1 1
fix 11 1 1 0
fix 22 1 1 0

equalDOF 3 33 1 2
equalDOF 4 44 1 2

#geometric transformation
geomTransf Linear 2

# elements

###columns
element elasticBeamColumn 1 1 3 360 4030 8640 2
element elasticBeamColumn 2 2 4 360 4030 8640 2

### beam
element elasticBeamColumn 3 3 4 360 4030 8640 2

### braces
element elasticBeamColumn 4 11 44 360 4030 8640 2
element elasticBeamColumn 5 22 33 360 4030 8640 2

# loads
pattern Plain 1 "Linear" {
load 3 100.0 0.0 0.0
load 4 100.0 0.0 0.0
}

#analysis
system BandGeneral
constraints Transformation
numberer RCM
test NormDispIncr 1.0e-12 10 3
algorithm Newton
integrator LoadControl 0.1
analysis Static

#analyze
analyze 10

#output
print node 3 33
print ele 1 2 3 4 5

[cromax]

Thank you very much vesna

Now I can study yur example and try to extend the solution for 3D problem.

I will post here my results.

Thank you very much

[cromax]

Dear Vesna

I have tried to modify for 3D problem your example but It does not work.Why?

error Warnin BandGenLinLapackSolver soolve () -Lapack routine returned 1
..
...
StaticAnalysis_analize()-the algoritm failed at iteration...
loadf factor 1
analyze failed ,returned :-3 error flag


I post It.

wipe
model basic -ndm 3 -ndf 6


# Set parameters for overall model geometry
set width 360
set height 144

# nodes
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

# node 11 0.0 0.0 0.0
# node 22 $width 0.0 0.0
node 33 0.0 $height 0.0
node 44 $width $height 0.0

# constraints
fix 1 1 1 1 1 1 1
fix 2 1 1 1 1 1 1
# fix 11 1 1 1 0 0 0
# fix 22 1 1 1 0 0 0

equalDOF 3 33 1 2 3
equalDOF 4 44 1 2 3

#geometric transformation
geomTransf Linear 1 0 0 -1
geomTransf Linear 2 0 1 0

# elements

###columns
#element elasticBeamColumn $eleTag $iNode $jNode $A $E $G $J $Iy $Iz $transfTag
element elasticBeamColumn 1 1 3 360 4030 1000 8640 8640 8640 1
element elasticBeamColumn 2 2 4 360 4030 1000 8640 8640 8640 1

### beam
element elasticBeamColumn 3 3 4 360 4030 1000 8640 8640 8640 2

### braces
# element elasticBeamColumn 4 11 44 360 4030 8640 2
# element elasticBeamColumn 5 22 33 360 4030 8640 2

# loads
pattern Plain 1 "Linear" {
load 3 100.0 0.0 0.0 0.0 0.0 0.0
load 4 100.0 0.0 0.0 0.0 0.0 0.0
}

#analysis
system BandGeneral
constraints Transformation
numberer RCM
test NormDispIncr 1.0e-12 10 3
algorithm Newton
integrator LoadControl 0.1
analysis Static

#analyze
analyze 10

#output
print node 3 33
print ele 1 2 3 4 5




Can you help me

[cromax]

can somebody help me?

[vesna]

You did not restrain torsional rotation with equalDOF and you did not define nodes of your beam well.

Here is the corrected file that works:

wipe
model basic -ndm 3 -ndf 6


# Set parameters for overall model geometry
set width 360
set height 144

# nodes
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

# node 11 0.0 0.0 0.0
# node 22 $width 0.0 0.0
node 33 0.0 $height 0.0
node 44 $width $height 0.0

# constraints
fix 1 1 1 1 1 1 1
fix 2 1 1 1 1 1 1
# fix 11 1 1 1 0 0 0
# fix 22 1 1 1 0 0 0

equalDOF 3 33 1 2 3 4
equalDOF 4 44 1 2 3 4

#geometric transformation
geomTransf Linear 1 0 0 -1
geomTransf Linear 2 0 1 0

# elements

###columns
#element elasticBeamColumn $eleTag $iNode $jNode $A $E $G $J $Iy $Iz $transfTag
element elasticBeamColumn 1 1 3 360 4030 1000 8640 8640 8640 1
element elasticBeamColumn 2 2 4 360 4030 1000 8640 8640 8640 1

### beam
element elasticBeamColumn 3 33 44 360 4030 1000 8640 8640 8640 2

### braces
# element elasticBeamColumn 4 11 44 360 4030 8640 2
# element elasticBeamColumn 5 22 33 360 4030 8640 2

# loads
pattern Plain 1 "Linear" {
load 3 100.0 0.0 0.0 0.0 0.0 0.0
load 4 100.0 0.0 0.0 0.0 0.0 0.0
}

#analysis
system BandGeneral
constraints Transformation
numberer RCM
test NormDispIncr 1.0e-12 10 3
algorithm Newton
integrator LoadControl 0.1
analysis Static

#analyze
analyze 10

#output
print node 3 33
print ele 1 2 3 4 5

[cromax]

Thank you very very much Vesna.

Thanks

[sb1966]

Dear Vesna,
Thanks a lot for your examples. Based on them, I have analysed a three-span continuous beam with udl on each span. But I am unable to get moments at the intermediate supports. May i know where my mistake is? My script adopted from yours is as follows:
========================================
wipe
model BasicBuilder -ndm 2 -ndf 3;
set L 10.0

node 1 0. 0.
node 2 [expr 1*$L] 0.
node 3 [expr 2*$L] 0.
node 4 [expr 3*$L] 0.


fix 1 1 1 1
fix 2 1 1 0
fix 3 1 1 0
fix 4 1 1 1

set TransfTag 1
geomTransf Linear $TransfTag;
set ABeam 1.0
set Iz 1.0
set E 2900

# define elements
element elasticBeamColumn 1 1 2 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 2 2 3 $ABeam $E $Iz $TransfTag;
element elasticBeamColumn 3 3 4 $ABeam $E $Iz $TransfTag;
#Apply Load
set timeSeriesTag 1
timeSeries Linear 1
pattern Plain 1 1 {
#Applying UDL on Beams along X Direction
eleLoad -ele 1 -type -beamUniform 0 -6.05
eleLoad -ele 2 -type -beamUniform 0 -6.05
eleLoad -ele 3 -type -beamUniform 0 -6.05
}

print ele 1
#print node
recorder Element -file [format eleForceConti.out] -time -eleRange 1 3 forces
constraints Penalty 1e12 1e12
numberer RCM
system BandGeneral
test NormDispIncr 1.0e-6 10
algorithm Newton
integrator LoadControl .1
analysis Static
analyze 10

set a [eleResponse 1 forces]
set b [eleResponse 2 forces]
set c [eleResponse 3 forces]
puts "P1 [lindex $a 0]"
puts "V1 [lindex $a 1]"
puts "M1 [lindex $a 2]"
wipe
=======================================
Thanks and Regards

[sb1966]

Dear Vesna and All,
Sorry to bother you. I have wrongly used the eleLoad command for ndm=3 instead of ndm=2. After correcting, I am getting appropriate results.
Thanks a lot and regards

[Djeras]

Hello Vesna! In my model I also considered pinned beams apart from pinned braces. Editing the previous code you wrote for a 2D model, can the following modification take place on defining the beam element?
-----------------------------
> wipe
> model basic -ndm 2 -ndf 3
>
>
> # Set parameters for overall model geometry
> set width 360
> set height 144
>
> # nodes
> node 1 0.0 0.0
> node 2 $width 0.0
> node 3 0.0 $height
> node 4 $width $height
>
> node 11 0.0 0.0
> node 22 $width 0.0
> node 33 0.0 $height
> node 44 $width $height
>
> # constraints
> fix 1 1 1 1
> fix 2 1 1 1
> fix 11 1 1 0
> fix 22 1 1 0
>
> equalDOF 3 33 1 2
> equalDOF 4 44 1 2
>
> #geometric transformation
> geomTransf Linear 2
>
> # elements
>
> ###columns
> element elasticBeamColumn 1 1 3 360 4030 8640 2
> element elasticBeamColumn 2 2 4 360 4030 8640 2
>
> ### beam
> element elasticBeamColumn 3 33 44 360 4030 8640 2
>
> ### braces
> element elasticBeamColumn 4 11 44 360 4030 8640 2
> element elasticBeamColumn 5 22 33 360 4030 8640 2

----------------------------------

Moreover, imagine a 3D problem with the nodes 3 and 4 part of a rigid diaphragm. Can we still use this ?
> equalDOF 3 33 1 2
> equalDOF 4 44 1 2

[fmk]

you can make the beam pinned in the same way you made the braces pinned .. ad 2 additional nodes and use the equalDOF command