Skip to content

Boundary

*Boundary, [amplitude=<amplitude name>, <type>]
<node set name>, <dof>, <...>

This command is used to prescribe boundary conditions on nodes or node sets. It is possible to define more than one *Boundary command per step. However, the defined boundary conditions are only active in the step for which they are defined. The *Boundary command has the following keywords:

  • amplitude=<amplitude name>

    The optional amplitude parameter allows for the specification of an amplitude by which the boundary values are scaled (mainly used for non-linear static and dynamic calculations). This only makes sense for non-zero boundary values. Thus, in that case, the values entered on the sub-lines of the *Boundary command are interpreted as reference values to be multiplied with the (time dependent) amplitude value to obtain the actual value.

    Example: *Boundary, amplitude = loading-ramp

  • <type>

    The second optional keyword <type> can be used to prescribe more "advanced" boundary conditions.

    Type Description Section
    none prescribe degree of freedom (dof) Section 1
    type=velocity first time derivative of the prescribed dof Section 2
    type=acceleration second time derivative of the prescribed dof Section 3
    type=increment increment (i.e. the change) of a dof Section 4
    type=hydrostatic hydrostatic (linear increase with depth) distribution Section 5
    type=moving-hydrostatic hydrostatic distribution with a "moving" zero-level Section 6

  • <node set name> = name of the node set to which the boundary condition is applied

  • <degree of freedom> = the degree of freedom to be constrained. The following degrees of freedom can be modified:

    Degrees of freedom Description
    u1 Displacement in x1-direction
    u2 Displacement in x2-direction
    u3 Displacement in x3-direction
    r1 Rotation in x1-direction (only beam elements)
    r2 Rotation in x2-direction (only beam elements)
    r3 Rotation in x3-direction (only beam elements)
    pw Pore-water pressure
    pa Pore-air pressure
    w1 Water displacement in x1-direction
    w2 Water displacement in x2-direction
    w3 Water displacement in x3-direction

  • Good to know

    • Boundary conditions can only be applied to degrees of freedom that are actually defined for the chosen element type. For example, in single-phase solid elements of type u-solid, you can prescribe a boundary condition for the horizontal displacement u1, but attempting to prescribe a boundary condition for pw would raise an error, since pw is not an active degree of freedom for these elements.

    • Boundary conditions defined using this command can vary in time but are active at all nodes of the assigned node set.

    The theory behind the implementations

1. Default

For the default case (no type prescribed), the command takes the flowing form: 

*Boundary
<node set name>, <dof>, <value>

They can be repeated as often as needed.

  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <value> = set this parameter equal to the value to be prescribed to the boundary condition. Notice that this value is interpreted as a reference value, which is multiplied with the amplitude value (in case an amplitude is assigned to the boundary condition).

2. Velocity

For type=velocity the first derivative of the selected dof w.r.t. time is prescribed. The command takes the flowing form: 

*Boundary
<node set name>, <dof>, <value>

They can be repeated as often as needed.

  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <value> = set this parameter equal to the value to be prescribed to the boundary condition. Notice that this value is interpreted as a reference value, which is multiplied with the amplitude value (in case an amplitude is assigned to the boundary condition).

3. Acceleration

For type=acceleration the second derivative of the selected dof w.r.t. time is prescribed. The command takes the flowing form: 

*Boundary
<node set name>, <dof>, <value>

They can be repeated as often as needed.

  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <value> = set this parameter equal to the value to be prescribed to the boundary condition. Notice that this value is interpreted as a reference value, which is multiplied with the amplitude value (in case an amplitude is assigned to the boundary condition).

4. Increment

For type=increment, the increment (i.e. the change) of the selected dof relative to its original value at the start of the step. The command takes the flowing form: 

*Boundary
<node set name>, <dof>, <value>

They can be repeated as often as needed.

  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <value> = set this parameter equal to the value to be prescribed to the boundary condition. Notice that this value is interpreted as a reference value, which is multiplied with the amplitude value (in case an amplitude is assigned to the boundary condition).

5. Hydrostatic

If type=hydrostatic is used to define the boundary condition, the command differs from the ones above and takes the form: 

*Boundary
<node set name>, <dof>, <slope>, <zero level>
  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <slope> = slope of hydrostatic distribution, e.g. unit weight of water in case of a hydrostatic distribution pore water pressure.
  • <zero level> = coordinate (y-coordinate in 2-D and z-coordinate in 3-D) where the distribution is zero, e.g. location of the water table in case of a hydrostatic distribution of pore water pressure

An example for the hydrostatic boundary condition is depicted in Figure1 for two different geometrical settings (scenario 1 and scenario 2).

Figure 1: Example for boundary conditions of type `hydrostatic`

Although the term 'hydrostatic' implies that this boundary condition is intended for the pore water pressure degree of freedom (DOF), it can also be applied to other degrees of freedom. For instance, it can be used to describe the horizontal movement of a hinged sheet pile wall.

6. Moving Hydrostatic

If type=moving-hydrostatic is used to define a more general form of the type=hydrostatic boundary condition, the command takes the form: 

*Boundary
<node set name>, <dof>, <dir>, <slope>, <zero-level 0>, <t0>, <zero-level 1>, <t1>
  • <node set name> = name of the node set to which the boundary condition is applied
  • <dof> = the degree of freedom to be constrained.
  • <dir> = Direction of action in global coordinates (x=1, y=2, z=3)
  • <slope> = slope of hydrostatic distribution, e.g. unit weight of water in case of a hydrostatic distribution pore water pressure.
  • <zero-level 0> = coordinate of the initial zero-level for the hydrostatic distribution at time t0
  • <t0> = initial time t0
  • <zero-level 1> = coordinate of the final zero-level for the hydrostatic distribution at time t1
Figure 2: Example for boundary conditions of type `moving-hydrostatic`

For times smaller than t0 the zero-level for the hydrostatic distribution is <zero-level 0> and for times larger than t1 the zero-level corresponds to <zero-level 1>