OpenSees Commands for u–p–U Elements {#Tcl commands for upU elements}

There are two different node elements:

  • 8 node brick u-p-U element Brick8N_u_p_U and

  • 20 node brick u-p-U element Brick20N_u_p_U

Due to the coexistence of the solid and fluid, there are 7 degrees of freedom at each node. The changes in the model building, analysis procedure commands are explained as below.

The model Command {#The model Command}

The model command defines the ModelBuilder object to be constructed.

model BasicBuilder -ndm ndm? <-ndf ndf?>

The string -ndm that followed by an integer defines the dimension of the problem,i.e. one, two or three dimensional problem. The string -ndf that followed by an integer defines the number of degree-of-freedom at a node. The angle bracket around the -ndf ndf? mean these arguments are optional. By default, the number of degree-of-freedom at a node depends on the dimension of the problem. For ndm=1, ndf=1;for ndm=2,ndf=3;for ndm=3, ndf=6.

For upU element,each node has 3 solid displacements, one pore pressure, and 3 fluid displacements, so the degree-of-freedom of each node is 7. The ModelBuilder command for upU element is:

model BasicBuilder -ndm 3 -ndf 7

The fix Command {#The fix Command}

The fix command is used to construct the single-point boundary conditions.

fix nodeTag? (ndf values?)

where the nodeTag is the node needs to be constrained. The ndf values can be 1 or 0. If the value of i-th ndf is specified as 1, then the degree-of-freedom at the DOF is constrained. Otherwise 0 means that it is left free..

The fix command for upU element is:

fix nodeTag (7 values (1 or 0))

for example

fix 1 1 1 1 1 1 1 1

fix all the degree-of-freedom of Node 1.

fix 5 1 1 0 0 1 1 0

fix the solid and fluid displacement for Node 5 in x and y directions, while the z direction of solid ,fluid and pore pressure are left free.

The element Command {#The element Command}

The element command is used to construct an Element object.

element eleType <specific element type args>

The second argument is the element type. The element names for the upU are given as Brick8N_u_p_U (for 8-node-brick-upU element) and Brick20N_u_p_U(for 20 node brick u-p-U element). The arguments in the angle bracket specify the properties of each type of element.

For upU element, the element command is:(for example 20-node-upU element):

element Brick20N_u_p_U eleTag? 1st_node? 2nd_node?...20th_node materialID?
x_body_force? y_body_force? z_body_force? porosity? alpha? solid_density?
fluid_density? x_permeability? y_permeability? z_permeability?
solid_bulk_modulus? fluid_bulk_modulus? pressure?

One upU element command might look like:

element Brick20N_u_p_U 1 5 6 7 8 1 2 3 4 13 14 15 16 9 10 11 12 17 18 19
20 1 0.0 0.0 -9.81 0.4 1.0 2.0 1.0 1.0e-5 1.0e-5 1.0e-5 1.0e5 1.0e5 0

The element is 20-node-brick-upU element Brick20N_u_p_U. The element tag is 1.The node numbers of the element is 5 6 7 8 1 2 3 4 13 14 15 16 9 10 11 12 17 18 19 20. The material tag is 1. The body forces in x and y directions are zeros, while in z direction is -9.81. The porosity of the element is 0.4, and alpha is 1.0. The solid density is 2.0, and fluid density is 1.0. The permeability in x, y and z directions are all 1.0e-5. The bulk moduli of solid and fluid are both 1.0e5, and the pressure is zero.

The pattern Command {#The pattern Command}

The pattern command is used to construct the LoadPattern object. There are Load and Constraint objects for the pattern.

pattern patternType patternTag? <arguments for pattern type>

Currently, there are three valid types of pattern: Plain, UniformExcitation and MultipleSupport. The Plain pattern has the form:

pattern Plain patternTag? {TimeSeriesType and Args}{
load ...
sp ...
}

The arguments Plain is used to construct an ordinary LoadPattern object with a unique patterTag. The fourth argument is a list to construct the TimeSeries object associated with the LoadPattern object. The arguments load and sp are used to create a nodal load and single-point constraint.

In upU example, the Plain pattern of Linear type:

pattern Plain 2 Linear{
load 5  0 0 $p 0 0 0 0
load 6  0 0 $p 0 0 0 0
load 7  0 0 $p 0 0 0 0
load 8  0 0 $p 0 0 0 0
load 13 0 0 $np 0 0 0 0
load 14 0 0 $np 0 0 0 0
load 15 0 0 $np 0 0 0 0
load 16 0 0 $np 0 0 0 0
}

create a load pattern with vertical load $p(depends on the value p and np, if use command set p 5, then $p=5 and set np 10, then $np=10) acting on nodes 5 6 7 8 ,and $np acting on node 13 14 15 16.

After careful inspecting the derivations and resulting equations, following recommendations are made for application of loads on coupled systems:

  • For drained (vertical) distributed load \(f\): all of the load \(f\) must be loaded to the solid matrix, no load goes to the fluid part and the fluid DOF must remain free. That is, the loading may be considered as only effective load without any pore pressure load.

  • For undrained (vertical) distributed load \(f\): \((1-n) f\) is to be loaded to the solid matrix, \(n f\) is to be loaded load to the fluid part and the fluid DOF must be constrained.

Back to top