The Fields Function enables the creation and maintenance of a library of complex data sets in a simple and straightforward manner. Fields are used to define loads and boundary conditions as a function of one, two, or three variables; material properties as functions of temperature, strain, strain rate, time and frequency. Data Fields are used in the material properties, loads and boundary conditions, and element properties applications. Fields can be either scalar or vector in nature. Complex scalar fields are also permitted if you are using the MSC Nastran Analysis Preference.

An important purpose of the Fields functionality is to provide a means of interpolating, or applying the results of one finite element analysis onto the same or different geometry or FEM model. Real scalar, complex scalar, and real vector results can be interpolated. This powerful capability is useful for multidisciplinary analyses, for example, a thermal analyst creates a model from a resident geometry model and does an analysis. A structural analyst then creates a separate model using the same geometry, reads in the thermal analysis results, and automatically interpolates them onto the structural model.

Field: A field is a set of data defined by relationships between one or more independent variables. The fields available in Patran support up to three dimensions and are divided into three types: spatial, material property, and non-spatial fields. Fields can be created either from tabular input, mathematical relationships expressed in PCL or as scalar or vector results on a collection of finite elements. These are described in detail below:

General Field: All three of the above field types may be created using the “General Field” method in addition to the Tabular or PCL methods. A General Field is defined by creating a function expression in PCL to describe the data variation. The terms of the function expression may consist of independent variables, constants and PCL functions related by mathematical operators. The PCL function terms can include user written PCL functions which utilize custom forms for data input. The General Fields implementation for this release is limited; it supports only scalar fields and will primarily be useful for the incorporation of custom PCL functions and forms. It will be expanded upon in future releases.

Continuous FEM Field: A special type of Spatial Field which is created from a finite element mesh and associated results values. By utilizing the connectivity of the mesh, a Continuous FEM Field can be evaluated (via interpolation) at any point within its space. A Continuous FEM Field is created from the graphical display of values on a mesh contained in a group. The field remains valid as long as the mesh and group are defined. Interpolation occurs automatically whenever the Continuous FEM Field is applied.

Discrete FEM Field: A Spatial Field consisting of values defined at elements or nodes. A Discrete FEM Field is created by the importation of Loads or Boundary Conditions via a Patran Neutral file, or with the Fields User Interface. As there is no mesh associated with this field, it is only defined at discrete points. No interpolation is available. The Discrete FEM Field was formerly known as the LBC Field.

The fields function is used to create and maintain a library of data fields; they are not applied here. Fields that have been created in this area of Patran are then selected and applied in other functional areas such as: material properties, loads and boundary conditions, and element properties.

Spatial fields are commonly used to control application of pressures and temperatures in the Loads/BCs application, although they can also be applied to displacements and other generalized loads. Spatial fields can be scalar or vector in nature and can be applied in either real or parametric space. Input is either tabular, via PCL function, external PCL routine or through the General Field. Multiple spatial fields can be simultaneously applied.

Material property fields are applied to individual properties (modulus, CTE, etc.) in the Materials Application. These fields can be one-, two-, or three-dimensional in nature with the independent variables being temperature, strain, strain rate, time and frequency (singly or in combination).

Non-Spatial Fields are principally used to specify time and frequency varying data. Time and frequency dependent loads and boundary conditions, and frequency-dependent material properties are all defined via Non-Spatial Fields. Non-Spatial functions of temperature, displacement, velocity, and user-defined variables can also be created. In addition, complex scalar functions of frequency can be created when the MSC Nastran Analysis Preference is selected.

The default size of all tabular fields is 30 entries in each dimension, although it can be increased to up to 1000 in the Options forms. Also, alternative methods of extrapolation can be selected if field table ranges are exceeded.

Flexibility: The structure of fields is flexible and generalized. While each type of field has intrinsic characteristics and uses (time or frequency dependence, material property or spatial dependence), the format of each is unspecified. Fields may be entered with tabular input, a PCL function, a General Field function or a FEM field; data may be vector or real scalar or complex scalar and up to three dimensions. All fields spreadsheet input forms, allow import and export of comma separated value (CSV) files. This provides compatibility with popular spreadsheet programs such as Microsoft Excel.

Ease of Use: Complicated data fields may be modeled using intuitive forms which lead the user through the entire field generation process. Descriptive names are allowed for every field. The fields function provides a convenient location for all data fields where they may be created, shown and modified before application to the model.

Archival Record: All fields created remain in the database unless deleted. This represents a history of all fields used in previous analyses. Also, it permits old fields to be retained, modified, and reapplied.

Field Creation from Analysis Results: Spatial Fields can be created from an imported finite element mesh and associated results or loads. This so called Continuous FEM Field will automatically interpolate result values for any points within its defined space. This capability is useful for mapping one set of analysis results onto another finite element model.