Which variables are in the output database?

In the first step of the elastomeric foam example, a set of options is included to control the data output during each step of the analysis. Abaqus/Standard writes this output to the Field Output or History Output portion of the output database, depending on the output type.

Field Output

The Field Output portion of the output database contains variables that should be output relatively infrequently during the analysis; in this case, after every 10 increments and after the last increment of a step. Typically, you select output for your entire model or a large region of your model, and Abaqus writes every component at the selected frequency. Only the selected variables are written to the output database.

The following input file fragment shows the options that control the field output variables in the elastomeric block example:

OUTPUT, FIELD, FREQUENCY=10
CONTACT OUTPUT, SLAVE=ASURF, MASTER=BSURF,
VARIABLE=PRESELECT
NODE OUTPUT
U,
ELEMENT OUTPUT, ELSET=FOAM
S,E

Abaqus/Standard writes the following variables to the Field Output portion of the output database after every 10 increments and at the end of each step:

  • the stress components of every integration point in the foam block;

  • the logarithmic strain components of every integration point in the foam block (by default, the logarithmic strain is written to the output database when the user requests strain for a geometrically nonlinear analysis);

  • the displacement of every node in the model; and

  • the default contact output variables (clearance, pressure, shear stress, and tangential motion) resulting from the contact between the punch and the foam block.

History Output

The History Output portion of the output database contains variables that may be output relatively frequently during the analysis, as often as every increment. To avoid generating large amounts of data, you typically select output from a small area of your model, such as a single element or a small region. In addition, you must select the individual components of the variables that are written to the output database. History output is typically used for generating X–Y data plots.

The following input file fragment shows the options that control the history output variables in the elastomeric block example:

OUTPUT, HISTORY, FREQUENCY=1
NODE OUTPUT, NSET=N9999
U2, V2, A2
ELEMENT OUTPUT, ELSET=CORNER
MISES, E22, S22

Abaqus/Standard writes the following variables from the punch's rigid body reference node (contained in node set N9999) to the history portion of the output database after every increment:

  • the vertical displacement,

  • the vertical velocity, and

  • the vertical acceleration.

In addition, after every increment Abaqus/Standard writes the following variables from the element at the corner of the block to the history portion of the output database:

  • von Mises stress,

  • the logarithmic strain in the 2-direction on the 2-plane, and

  • the stress in the 2-direction on the 2-plane.

The stress and strain variables are written for all the integration points in the element.