NODAL_LOADS
NODAL_LOADS load_time_function_number = ltime , etc...
< etc..., terminate with a
blank record >
Create the list of nodal loads.
The value specified is a force if the corresponding nodal boundary
condition restraint code is zero, or a displacement, velocity or acceleration
if the corresponding restraint code is non-zero (see Section 5.1). Two options are available. The nodal loads may be read in directly as a
list (optionally from another file), or may be generated.
Note Variable Name Type Default Description
Load_case_number integer [*] Load
case number (only required
in
Restart mode)
Generation_type list [*] Generation
case
list
Cartesian
Variable list [*] Nodal
variables selection:
all all
degrees of freedom
solid_displacement solid
displacement
solid_rotation solid
rotation
solid_displacement_and_rotation solid
displacement and rotation
fluid_velocity fluid
velocity
temperature temperature
pressure pressure
potential potential
electric_potential electric
potential
scalar_transport scalar
transport
level_set level
set
stream_fct stream
function
mesh_motion ale
mesh motion
solid_force solid
force
bending_moment bending
moment
fluid_traction fluid
traction
pressure_gradient pressure
gradient
heat_flux heat
flux
potential_flux potential
flux
electric_potential_flux electric
potential flux
scalar_flux scalar
transport flux
Type list [*] Load
type
constant
/ time_dependent
Space_time_dependence list [*] Space
time dependence
uniform /
nonuniform
(cont'd)
Note Variable Name Type Default Description
Load_time_function_number integer [0] Load
time function number
(only
applicable to uniform space time
dependence case)
File_name string [none] File name
(optional). Name must
be enclosed in quotation marks
• No Generation (List) Case
Nodal loads must follow in the form:
– Uniform space time dependence case:
< Node_number , load_X , load_Y , load_Z ,
etc...>
< etc..., terminate with a blank record >.
– Nonuniform space time dependence case:
< Node_number , load_time_function_number,
load_X , load_Y , load_Z , etc...>
< etc..., terminate with a blank record >.
• Generation Case (Only applicable to uniform space time dependence.)
Nodal loads generation data must follow.
< terminate with a blank record >.
EXAMPLE
NODAL_LOADS \
load_time_function_number
= ltime \
file_name
= "nodal_load_file" #
read nodal loads from file: nodal_load_file
7.1.1 Applied Nodal Forces and/or Kinematics Generation Data
Note Variable Default Description
(1) N [0] Node number 
1 and 
NUMNP
(2) NUMGP [0] Number of generation points 0
=
0, no generation
≠
0, generate data
(3) F(1,N,LC) [0.0] Degree of freedom 1 force or
kinematics
F(2,N,LC) [0.0] Degree of freedom 2 force or
kinematics
- - -
etc. - etc.
- - -
F(NDOF,N,LC) [0.0] Degree of freedom NDOF force or
kinematics
Notes/
(1) Applied nodal force or kinematics data must be included for
each node subjected to a nonzero applied force or nonzero prescribed
kinematics. Terminate with a blank record.
(2) If NUMGP is greater than zero, this record initiates an
isoparametric data generation sequence.
The scheme used is the same as the one for coordinate and initial
displacement/velocity generation (see Chapters 4 and 6, respectively). Records 2 to NUMGP of the sequence define the
applied forces/kinematics of the additional generation points (see Section
7.2). The final records of the sequence
defines the nodal increment information and is identical to the one used for
coordinate generation (see Section 4.3).
After the generation sequence is completed, additional nodal applied
forces/kinematics data records, or generation sequences, may follow.
The generation may be performed along a line, over a
surface, or over a volume. For additional information concerning these options
see Note (2) of Section 6.1.
(3) The elements of the array F(NDOF,NUMNP,NLC) are initialized to
zero. If the applied forces/kinematics
of node N are input and/or generated more than one time, the last value takes
priority.
7.1.2 Generation Applied Nodal Forces / Kinematics Data
The applied forces/kinematics of each generation point
are defined by a generation point applied force/kinematics record. The records must be read in order (J = 2,
3,...,NUMGP) following the nodal applied force/prescribed kinematics record
which initiated the generation sequence (J = 1). A nodal increments record (see Section 7.1.3)
follows the last generation point record (J = NUMGP) and completes the
sequence.
Note Variable Default Description
M [0] Node number
MGEN [0] Generation parameter
= 0, applied
forces/kinematics of the Jth generation points are input
on this record; M is ignored
= 1, applied
forces/kinematics of the Jth generation point are set
equal to applied forces/kinematics of node M which were previously defined;
applied forces/ kinematics on this record are ignored.
TEMP(1,J) [0.0] Degree of freedom 1 applied
force/kinematics
for generation point J
TEMP(2,J) [0.0] Degree of freedom 2 applied
force/kinematics
for generation point J
- - -
etc. - etc.
- - -
TEMP(NDOF,J) [0.0] Degree of freedom NDOF applied
force/kinematics
for generation point J
7.1.3 Nodal Increments Data
Note Variable Default Description
NINC(1) [0] Number of nodal increments for
direction 1
INC(1) [0] Node number increment for
direction 1
(1) NINC(2) [0] Number of nodal increments for
direction 2
INC(2) [0] Node number increment for
increment 2
(1) NINC(3) [0] Number of nodal increments for
direction 3
INC(3) [0] Node number increment for
direction 3
Notes/
(1) Each option is assigned an option code (IOPT) as follows:
IOPT Option
1 Generation along a line
2 Generation over a surface
3 Generation over a volume
IOPT is determined by the following logic:
IOPT = 3
IF(NINC(3)
= 0) IOPT = 2
IF(NINC(2)
= 0) IOPT = 1
|
Figure 7.1.3 Load Vector Generation
|
with j = load_time_function (i) , i = Load_case