Next: Uniform Pressure
Up: FG-to-NASTRAN
Previous: Analysis Control
NASTRAN load data is included as part of the model history data which is
in turn divided into steps (see chapter 6). The association of a FEMGEN load with an
NASTRAN step is achieved via the FEMGEN loadcase number argument
in the 'PROPERTY LOAD' command. All loads with loadcase number 1 will be associated
with the first NASTRAN step and so on.
All FEMGEN load commands have the following form:
PROPERTY LOAD load_type [load_name] [loadcase_no] part_name/ALL args
Argument | Meaning |
load_type | Load type (e.g. PRESSURE). |
load_name | Optional load name identifier (for reference purposes). |
loadcase_no | Optional FEMGEN loadcase No. |
part_name/ALL | Geometric part to which load is applied. |
args | Varying arguments depending on load_type |
Table 7.1:
FEMGEN load command arguments.
Notes:
- 1.
- The part name may be either a single part in the model geometry or a set of
such parts. In either case the interface expands the geometry-based load definition
into a series of nodal, element face, or whole element loads. The user does not
need to consider node/element numbers or element face identifiers;
the interface derives these automatically.
- 2.
- The use of ALL for the
part name is only valid in circumstances where all parts of the model have a valid
geometry for the load in question. For example a pressure load applied to ALL of a
model which contains FEMGEN bodies would be invalid. A temperature load applied to
the same model would be valid.
- 3.
- The command arguments vary with the load type and are described in the following
sections. For all loads types, the actual load values (be it per unit depth, area, or circumference)
must be entered correctly by the user. The interface, for example, does not attempt to multiply load
values by element thicknesses or areas.
Notes on advanced loading:
- Load Masks, Local Coordinate Systems, Space Curves, defined with the FEMGEN 'CONSTRUCT'
command, can be attached to loads using the FEMGEN command 'PROPERTY ATTACH'. The interface
program supports some of these new features for most loads. Please note that Time Curves are
not supported by this interface program . More detailed information on advanced loading
may be found in the FEMGV User Manual.
The following load types are supported:
Generic Load Type | FEMGEN Load Type | Application |
Uniform Pressure | PRESSURE | Element faces. |
Concentrated Force | FORCE | Nodes. |
Prescribed Displacement | DISPLACE | Nodes. |
Gravity | GRAVITY | Whole elements. |
Temperature | TEMPERAT | Nodes. |
Hydrostatic Pressure | HYDROSTA | Element faces. |
Centrifugal Force | CENTRIFU | Whole elements. |
Table 7.2:
NASTRAN Load Types Supported
Next: Uniform Pressure
Up: FG-to-NASTRAN
Previous: Analysis Control
Femsys Limited
8/18/1999