## *INITIAL CONDITIONS

Keyword type: model definition

This option is used to define initial temperatures, initial velocities, initial stresses and initial plastic strains. There are two parameters: TYPE and USER. The parameter TYPE is required. It can take the following values:

• TYPE=DISPLACEMENT: initial displacements
• TYPE=FLUID VELOCITY: initial fluid velocities for 3D fluid calculations
• TYPE=MASS FLOW: initial mass flow for networks
• TYPE=PLASTIC STRAIN: initial inelastic strains
• TYPE=PRESSURE: initial static fluid pressures for 3D fluid calculations
• TYPE=SOLUTION: initial internal variables
• TYPE=STRESS: initial stresses
• TYPE=TEMPERATURE: initial temperatures for structural, network or 3D fluid calculations
• TYPE=TOTAL PRESSURE: initial total pressures for network calculations
• TYPE=TURBULENCE: turbulence parameters
• TYPE=VELOCITY: initial structural velocities (for dynamic calculations)

For shell elements TYPE=TEMPERATURE can be used to define an initial temperature gradient in addition to an initial temperature. The temperature applies to nodes in the reference surface, the gradient acts in normal direction. For beam elements two gradients can be defined: one in 1-direction and one in 2-direction. Default for the gradients is zero.

The plastic strain components defined with this option are subtracted from the strain components computed from the displacement field. If thermal strains are relevant they are additionally subtracted. The resulting strain is used to compute the stress and tangent stiffness matrix using the appropriate constitutive equations.

The parameter USER can only be used if TYPE=STRESS or TYPE=SOLUTION is specified. In that case, the user must define the initial stresses or internal variables by user routine sigini.f or sdvini.f, respectively.

Please note that vector and tensor quantities have to be provided in the GLOBAL (rectangular) coordinate system, no matter whether an *ORIENTATION card or *TRANSFORM card applies to the corresponding element or node, respectively.

First line:

• *INITIAL CONDITIONS
• Enter any needed parameters and their values.

Following line for TYPE=DISPLACEMENT:

• Node number or node set label.
• Degree of freedom in the GLOBAL coordinate system.
• Magnitude of the displacement.

Following line for TYPE=PLASTIC STRAIN:

• Element number.
• Integration point number.
• Value of first plastic strain component (xx) in the GLOBAL coordinate system x-y-z.
• Value of second plastic strain component (yy) in the GLOBAL coordinate system x-y-z.
• Value of third plastic strain component (zz) in the GLOBAL coordinate system x-y-z.
• Value of fourth plastic strain component (xy) in the GLOBAL coordinate system x-y-z.
• Value of fifth plastic strain component (xz) in the GLOBAL coordinate system x-y-z.
• Value of sixth plastic strain component (yz) in the GLOBAL coordinate system x-y-z.
Repeat this line if needed. The strain components should be given as Lagrange strain components for nonlinear calculations and linearized strain components for linear computations.

Following line for TYPE=PRESSURE, TYPE=TOTAL PRESSURE or TYPE=MASS FLOW:

• Node number or node set label.
• Static pressure, total pressure or mass flow value at the node.
Repeat this line if needed.

Following line for TYPE=SOLUTION if USER is not specified:

• Element number.
• Integration point number.
• Value of first internal variable.
• Value of second internal variable.
• Etc.
Repeat this line if needed. Each line should contain exactly 8 entries (including the element and integration point number in the first line), except for the last line, which can contain less. For instance, if the number of internal variables is 11, the first line contains 6 and the second 5. If you have 20 internal variables, the first line contains 6, the second 8 and the third 6. The number of internal variables must be specified by using the *DEPVAR card.

There is no line following the first one for TYPE=SOLUTION,USER.

Following line for TYPE=STRESS if USER is not specified:

• Element number.
• Integration point number.
• Value of first stress component (xx) in the GLOBAL coordinate system x-y-z.
• Value of second stress component (yy) in the GLOBAL coordinate system x-y-z.
• Value of third stress component (zz) in the GLOBAL coordinate system x-y-z.
• Value of fourth stress component (xy) in the GLOBAL coordinate system x-y-z.
• Value of fifth stress component (xz) in the GLOBAL coordinate system x-y-z.
• Value of sixth stress component (yz) in the GLOBAL coordinate system x-y-z.
• Etc.
Repeat this line if needed. The stress components should be given in the form of second Piola-Kirchhoff stresses.

There is no line following the first one for TYPE=STRESS,USER.

Following line for TYPE=TEMPERATURE:

• Node number or node set label.
• Initial temperature value at the node.
• Initial temperature gradient in normal direction (shells) or in 2-direction (beams).
• Initial temperature gradient in 1-direction (beams).
Repeat this line if needed.

Following line for TYPE=VELOCITY or TYPE=FLUID VELOCITY:

• Node number or node set label.
• Degree of freedom in the GLOBAL coordinate system.
• Magnitude of the velocity.

Following line for TYPE=TURBULENCE:

• Node number or node set label.
• First turbulence parameter.
• Second turbulence parameter, if any.
Use as many entries as turbulence parameters. Right now, only 2-parameter models are implemented.

Examples:

*INITIAL CONDITIONS,TYPE=TEMPERATURE
Nall,273.


assigns the initial temperature T=273. to all nodes in (node) file Nall.

*INITIAL CONDITIONS,TYPE=VELOCITY
18,2,3.15


assigns the initial velocity 3.15 to degree of freedom 2 of node 18.

Example files: beam20t, beamnlt, beamt3, resstress1, resstress2, resstress3, inistrain.