F.10
These instructions determine the loads. The directive "LOAD" is an alias of the "CHAR" directive.
$ "CHARGE" ; "LOAD" $ < "CONSTANTE" . . . > < ndcha $[ "FACTORISEE" . . . ; "PROGRAMMEE" . . . ]$ > < "ADDF" . . . > < "SPEC" . . . > < "FCTE" . . . > < "FIMP" . . . > < "FDYN" . . . > < "AIRB" . . . >
The various subdirectives, detailed in the following pages, are summarized
hereafter:
1/ Constant loads : "CONSTANTE" $ "GRAVITE" gx gy < gz > $ $ "ROTATION" omega /LECTURE/ $ 2/ Factorized loads : "FACTORISEE" <ndfact> (  ( "DEPLA" . . . )   ( "FORCE" . . . )   ( "PRESS" . . . )  "TABLE" . . . ) 3/ Programmed loads : "PROGRAMMEE" ndprog $ "FORCE" . . . $ $ "PRESSION" . . . $ "ROUTINE" . . . < "ROUTINE" . . . > 4/ Generalized loads for advectiondiffusion calculations (JRC) "ADDF" $ "TIMP" . . . $ $ "FLUX" . . . $ $ "QGEN" . . . $ $ "CONV" . . . $ $ "RADI" . . . $ $ "PRES" . . . $ $ "VELO" . . . $ $ "BLOQ" . . . $ $ "VPLA" . . . $ $ "VLIN" . . . $ 5/ Seismiclike loads for use with spectral elements (JRC) "SPEC"  "POIN" . . .   "PLAN" . . .   "SISM" . . .  6/ New Constant loads: FCTE NODE /LECT/ $ FORC f ; MOME m $ VECT x y z 7/ Imposed timedependent loads: FIMP NODE /LECT/ $ FORC f ; MOME m $ VECT x y z NUFO nf 8/ Dynalpy loads: FDYN NODE /LECT/ PZER p0 COEF c VECT x y z ELEM e 9/ Air Blast (AIRB) loading: AIRB [ "X" x "Y" y <"Z" z> ; "NODE" /LEC1/ ] "MASS" m $[ "TINT" t ; "TAUT" ]$ <"OPOS"> <"ANGL"> <"CUBE"> <"COEF" cf> <"CONF" c> <"DECA" d> <"PMAX" pmax "TD" td "B" b> <"SHAD" /LECS/> /LECT/
1/ CONSTANTES
The constant loads act all along the calculation. It is the case
of body weight or of a fixed acceleration.
2/ FACTORISEES
The defined loads are multiplied by a coefficient which
varies in time and is interpolated from a table:
3/ PROGRAMMEES
The loads will be read and computed for some elementary
times which are fixed a priori by the user in a
subroutine given by him (FPROG or PPROG). EUROPLEXUS
will then perform a linear interpolation to determine
the loads at the precise instants of the calculation.
1/ Constant loads:
FCTE NODE /LECT/ $ FORC f ; MOME m $ VECT x y z
2/ Imposed timedependent loads:
FIMP NODE /LECT/ $ FORC f ; MOME m $ VECT x y z NUFO nf
3/ Dynalpy loads:
FDYN NODE /LECT/ PZER p0 COEF c VECT x y z ELEM e
4/ FCTE
The constant loads act all along the calculation. It is the case
of body weight or of a fixed load.
5/ FIMP
The defined loads are multiplied by a coefficient which
varies in time and is interpolated from a table:
6/ FDYN
These loads are only related to 1D elements of type TUBE or TUYA.
7/ AIRB
These loads result from an air blast wave. The parameters are
similar to those available in the IMPE AIRB
directive, see Page C.882, but here the load is applied
directly to a region of structural elements rather than by
using special CLxx elements. This facilitates the
treatment of element erosion and of mesh adapptivity.
These instructions are described in detail on the following pages.
F.25
This directive allows to read the initial conditions data from
an auxiliary file.
"CHARGE" ndcha < "FICHIER" 'nom.fic' >
In certain cases the data may be bulky. It is then recommended
to store them on an auxiliary file to shorten the main input
data file. The auxiliary file is activated by means of the
keyword "FICHIER" that precedes the file name (complete under Unix).
In the main data file then only the keywords "CHARGE"
"FICHIER" remain.
The auxiliary file (in free format) contains the whole set
of load data, except the keyword "CHARGE".
To return to the main input data, the auxiliary file must
be terminated by the keyword "RETOUR".
F.30
This directive allows
to introduce constant accelerations (most often gravity) during
the whole computation. It also gives the possibility to compute
a structure in a rotating frame (with a constant rotation
speed).
Definition of sinusoidal acceleration is available (PERIODE and PHASE). Is is also possible
that the acceleration is linear and then keeps a constant value (RAMPE).
"CONSTANTE" [ "GRAVITE" gx gy < gz > /LECTURE/ ; "ROTATION" omega /LECTURE/ ] <"PERIODE"> Tx Ty Tz <"PHASE"> Phix Phiy Phiz <"RAMPE"> tx ty tz
The component < g_{z}> of the acceleration only makes sense for a
threedimensional computation.
Forces due to gravity or the acceleration of a moving frame are
applied to the nodes of the structure defined in the directive
/LECTURE/
.
In the case of a calculation in a rotating frame, it is assumed
thet the rotation axis is Oz. The forces applied to the nodes are:
F_{x} = M ω^{2} x 
F_{y} = M ω^{2} y 
F_{z} = 0 
This force applies to the nodes specified by the following
/LECTURE/
directive.
If all nodes are concerned, it is sufficient to put
the word TOUS
in place of the directive /LECTURE/
.
In the case of pipelines, it is important to couple this directive
with "INIT" "DEBIT" (page E.120) so as to avoid the transient
due to sudden application of gravity.
For the tubes and the pipelines, the rotation constant charge does not
make sense. Note that, although there is just one d.o.f. for the
elements of type TUBE
, the gravity vector may have
an arbitrary orientation.
For a sinusoidal acceleration, the amplitud is defined by the component of the acceleration
and is multiply by a sinus function. The user has to define the period of the function and
the phase. If a component is not exited, the period and the phase for this component have
to be zero.
The ramp acceleration is defined by a linear part that starts from zero at the initial time
and then grow linearly to pass by the point tx=gx (for example). Then after tx, the acceleration is kept
constant at a gx level.
If a component is not exited, the time for this component has
to be zero.
F.40
This directive allows
to input loads varying in time, of the following type:
Q(t) = A * C(t), with:
 A as a base value (displacement, force or pressure);
 C(t) as a coefficient whose values, depending on time, are
supplied by a table.
"FACT" ndfact ( ( "DEPLA" . . . ) ( "FORCE" . . . ) ( "PRESS" . . . ) ( "ACCE" . . . ) "TABLE" . . . )
The instruction "FACT" cannot be used more than once.
On the contrary, the sequence terminating with the "TABLE"
directive may be repeated as many times as necessary.
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.50
This option enables displacements depending on time
to be prescribed.
"DEPLA" /LECDDL/ d0 /LECTURE/
The displacements of the nodes defined by the procedure LECTURE
and along the directions determined by LECDDL, are of the following type:
C(t) is provided by the first array met after that option
(see "TABL").
That option can be used as many times as necessary .
If the imposed displacement is a blockage (d0 = 0), it is better
to use the
option "BLOQUE" of the instruction "LIAISON" (page D.30).
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.60
This option enables nodal forces, varying in time, to be imposed.
"FORCE" /LECDDL/ f0 /LECTURE/
The forces applied to the nodes defined by the procedure LECTURE
and according to the directions determined by LECDDL, have an
intensity of:
C(t) is provided by the first array (TABLE) met after that option
(see "TABL", page F.150).
That option may be used as often as necessary.
For an textbfaxisymmetric computation, the force must be divided
by 2π:
real force F0 =  2*pi
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.80
This option introduces a pressure which is exerted on a segment
set (2dimensional case) or on a surface composed of shell elements
(2dimensional or 3dimensional case), or on the faces of solid
elements (3dimensional case).
"PRESSION"  ( "SEGMENT" . . . )   ( "COQUE" . . . )   ( "FACE" . . . )   ( "NODE" . . . )   ( "ELDI" . . . ) 
The word "PRES" is the first keyword of the option.
There is no need to repeat "PRES" to redefine a new
line or surface corresponding to the same table (the one which
immediately follows the word "PRES").
On the contrary, it is compulsory to define again the word
"PRES" if it is necessary to create lines or surfaces
relative to another table.
F.90
This directive is mainly used to apply a pressure to 2D continuum
elements (in 3D cases, use PRES FACE).
It allows to enter a pressure which is exerted
on a certain number of adjacent segments or lines, in the case
of 2dimensional computation. The pressure may vary in time
(factorized loads) or be hydrostatic.
"SEGMENT" [ p0 ; "HYDRO" rho g z0 ] /LECTURE/
The user has the choice between a pressure p_{0} which varies in
time and a hydrostatic pressure. It is not allowed to define both at
the same time without reusing the word SEGM.
For a defined basic value p_{0}, the pressure intensity is:
p(t) = p_{0} C(t) 
C(t) is provided by the first array (TABL) met after the option
PRES (see also TABL).
If a hydrostatic pressure is defined (keyword HYDR), the pressure
is only applied to the segments of the line at levels z, such that:
g (z − z_{0}) ≥ 0 
From the previous expression it appears that, since the hydrostatic
pressure should be exerted on segmentes at z<z_{0}, then the
value of g specified should normally be negative.
Moreover, the intensity of the pressure is:
p = ρ g (z − z_{0}) 
The values ρ, g, z_{0} may be negative.
Each new option SEGM defines a different line.
If the line of segments is defined by giving the name of
a GIBI object, make sure that the line is oriented,
i.e. that the nodes are listed from one extremity
to the other in the correct order (not randomly, as it may sometimes
occur in some mesh generators).
If there is more than one line, and the lines are disjoint from
one another (i.e. the final node of one line is not the
initial node of the next one), then the PRES directive must be
repeated (one directive for each line). Otherwise,
a “spurious” segment joining the final node of a line to the initial
node of the next one in the list would also be considered as
subjected to pressure. This is particularly dangerous if
more than one GIBI object is listed in the same LECT.
In case of doubt, it is always safer to use a separate PRES
directive for each line.
The order in which the points of the line are read by
means of the procedure LECT, defines the orientation of the
contour of that line. The normal vector (n^{→})
results from a rotation of
π/2 of the contour itself.
Positive values will create forces in the orientation of the
normal (n^{→}) thus obtained.
The keyword TABL is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
TABL 2 t1 v t2 v, where v
is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.110
This directive is mainly used to apply a pressure to 2D or 3D shell
elements. For two or threedimensinal computations, this option enables
a pressure to be entered, which is exerted on a surface composed of
shell elements. The pressure may vary in time (factorized loads)
or be hydrostatic.
"COQUE" [ p0 ; "HYDRO" rho g z0 ; "HYDRO" rho gx gy gz x0 y0 z0 ] /LECTURE/
The user has the choice between a pressure p0 which varies
in time and a hydrostatic pressure. It is impossible to define both
at the same time, without reusing the word "COQUE".
If a basic value p0 has been defined,the pressure intensity is:
C(t) is provided by the first array met after the option
"PRESS" (see TABLE).
If a hydrostatic pressure is defined (keyword HYDR), the
pressure is applied to the points on the surface of
coordinates X,Y,Z such that :
The pressure intensity will be for these points:
In a twodimensional case, the definition of the hydrostatic
pressure is the same as for the subdirective "SEGMENT".
For a threedimensional computation, see the definition of
hydrostatic pressure with the subdirective "FACE".
Each new option "COQUE" defines a new pressure surface.
The normal vector on the surface is oriented according to the
numeration of the shell nodes. Positive pressures will create forces
in the orientation of that normal.
The orientation of the normal is given by the following rule
(Maxwell’s corkscrew rule).
An observer placed at the centre of the shell element which is
crossed by the normal from the bottom to the top, must be able to
notice that the shell element is numbered in increasing order, by
rotating in a trigonometric sense (anticlockwise).
If the mesh developped by means of "COCO" is used, the elements
are not necessarily oriented in the same way (this has to be
explicitly requested).
If the mesh is entered by the user, all elements
have to be numerated so that their orientation is coherent. A shell
surface composed of elements which are oriented in a different way,
may produce errors and confusion concerning the direction of the
pressures from the data point of view as well as from the results.
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
This directive is mainly used to apply apressure to 3D continuum
elements. For a threedimensional computation, this option enables
a pressure to be entered, which is exerted on a surface composed
of the sides of solid elements.
The pressure may vary in time (factorized loads) or be hydrostatic.
"FACE" iface [ p0 ; "HYDRO" rho gx gy gz x0 y0 z0 ] /LECTURE/
The user has the choice between a pressure P0 which varies in time
and a hydrostatic pressure. It is impossible to define both at the same
time without reusing the word "FACE".
For a defined basic value P0, the intensity of the pressure is:
C(t) is provided by the first array met after the option
"PRESS" (see TABLE).
If a hydrostatic pressure is defined (keyword HYDR), it is applied
to the points of the pressure surface of coordinates X,Y,Z such that:
For these points, the intensity is:
The free surface of the liquid is composed of the plane which
passes through the point M0 of coordinates (x0, y0, z0) and
perpendicular to the vector (G) whose components are : (gx,gy,gz).
If the vector (G) is drawn with the point M0 as origin, the
pressure will be applied to the points M of the pressure surface
which are located in the halfspace containing (G).
The pressure intensity at point M is:
Here h represents the distance between M and the free surface; g
represents the gravity.
The vector (G) with its 3 components enables the surface
of a liquid (horizontal) to be entered, when the vertical axis of
the mesh is distinct from the physical vertical line. In this case, the
surface is an inclined plane in the coordinate system of the mesh.
Each new definition of the option "PRES" "SEGMENT" generates
a new pressure surface.
The normal to the face of an element is the outward normal
of that element. A positive pressure creates a force in the
orientation of that normal.
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.140
This directive is mainly used to apply a pressure to continuum
elements (2D or 3D). This option enables
a pressure to be entered, which is exerted on a surface composed
of the nodes belonging to the edge of structure.
The pressure may vary in time (factorized loads) or be hydrostatic.
"NODE" [ p0 ; "HYDRO" rho gx gy gz x0 y0 z0 ] /LECTURE/
The user has the choice between a pressure P0 which varies in time
and a hydrostatic pressure. It is impossible to define both at the same
time without reusing the word "NODE".
For a defined basic value P0, the intensity of the pressure is:
C(t) is provided by the first array met after the option
"PRESS" (see TABLE).
This directive is decribed in 10.3.3 (page F.130).
The normal to the face of an element is the outward normal
of that element. A positive pressure creates a force in the
orientation of that normal.
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.142
This directive is used to apply pressure on the outer surface of a
cylinder made of discrete elements (ELDI).
The pressure may vary in time (factorized loads).
"ELDI" [ p0 ; "PAX1" x1 y1 z1 "PAX2" x2 y2 z2 "RAD " r <"TOLE" tol> ] /LECTURE/
A procedure selects the elements that are tangent to the outer surface of the cylindre. For each selected element, the pressure application area is calculated with the element’s radius r. In fact, we consider this area is the area of the circle of radius r (A=r^{2}).
For a defined peak value P0, the intensity of the pressure is:
So, for each selected element, the applied force modulus is:
This force is applied in the direction of the normal vector V to the cylinder at the considered element. C(t) is provided by the first array met after the option "PRESS" (see TABLE).
In practice, the sum of selected elements’ areas is always significantly lower than cylinder’s surface area. An adjustment is done to correct this point by multiplying the calculed force by the ratio of the cylinder’s outer surface area and the sum of the selected elements cross section areas.
The normal to the cylinder outer surface at the considered element is the outward normal. A positive pressure creates a force in the direction of that normal.
The instruction "TABL" is mandatory. For the case of charges that are constant in time, just give a twoentry table with the same value in both entries, i.e. of the form "TABL 2 t1 v t2 v", where v is the (constant) value, t1 is less or equal to the initial time of the computation and t2 is greater or equal to the final time of the computation.
F.145
This option enables additional acceleraration depending on time
to be prescribed.
"ACCE" /LECDDL/ g0 /LECTURE/
The external forces applied on the nodes defined by the procedure LECTURE
and along the directions determined by LECDDL, are of the following type:
M is the nodal mass. C(t) is provided by the first array met after that option
(see "TABL").
That option can be used to enter gravity like forces depending on time (for example,
deceleration forces inside a tank during a crash).
The instruction "TABL" is mandatory. For the case of charges
constant in time, just give a twoentry table with the same
value in both entries, i.e. of the form
"TABL 2 t1 v t2 v", where v is the (constant) value,
t1 is less or equal to the initial time of the computation
and t2 is greater or equal to the final time of the
computation.
F.150
The tables provide the different values of the coefficients C(t)
which appears in the options of the instruction
"CHARGE FACTORISEE" (factorised load).
The C(t) functions are continuous, linear by parts and therefore
defined by points. They can linearly interpolate more complex
functions.
"TABLE" npts*( tk ck )
Each array refers to the options "DEPL", "FORC", "PRES" which
are defined in the data set before the table and follow the
preceeding table, if it exists. The first table refers to all options
defined after the keyword "FACT". It is not allowed to have two
consecutive tables in the data set.
If the time t1 = 0 is not specified in the table, the point of
origin (0, 0) is assumed to belong to the curve.
The last time used in the array must be greater than the final
time of the computation.
F.180
This option enables the user to enter forces or pressures applied
to certain nodes or certain elements of the structure, for
time instants defined by the user himself.
In this case, the values are defined at each time by linear
interpolation.
"PROG" ndprog $ "FORCE" . . . $ $ "PRESSION" . . . $ "ROUTINE" . . . < "ROUTINE" . . . >
The word "PROG" is the first keyword of the option. It may be used
only once in the EUROPLEXUS data set.
There are 2 subdirectives "PRES" and "FORC" which respectively
enable pressures or forces to be input.
For each of them, the user has to initially provide a list,
which contains according to the circumstances:
 The numbers of the nodes defining the pressure line or the
numbers of the elements to which pressures are applied.
 The numbers of the degrees of freedom and the numbers of the
nodes to which forces are applied.
The list is entered by the means of the pocedures LECTURE and
LECDDL.
There are three ways to enter the values of the forces and
pressures at the different time increments.
1/ The user directly inserts, into the data set, the cards which
each correspond to one time increment. Each card successively
contains :
 The value of the time increment concerned.
 The values of the pressures and forces determined according
to the preceeding list.
2/ The user has at his disposal or creates a data file with an
imposed standard writing format. The file must successively store
several sets of values, each corresponding to one time increment.
Each set sequentially defines :
 The value of the time increment concerned
 The values of the pressures and forces determimed in the
same way as the cards.
3/ Regarless of the program, the user provides a subroutine
which computes the values of the forces or pressures for each
time increment before the program runs. These values are stored
in array F or P according to the list.
The data can be read on a file the format of which is not standard,
or the values can be directly entered by the means of an analytic
formula chosen by the user.
The keywords "ROUTINE" introduce respectively the data associated
with each of the subroutines FPROG and PPROG, written
by the user.
ATTENTION: the data relative to FPROG are read first.
If there are only forces (or only pressures), a single
keyword "ROUTINE" is sufficient to introduce the
corresponding data.
F.210
For each time increment, this option enables nodal forces
to be applied to certain nodes of the structure and
according to certain directions (degrees of freedom).
$ "FORCE" "DDL" /LECDDL/ /LECTURE/ ... $ $ "MXTF" ntmax  "CART" ( "INST" ti f1 ... fn )  $ $  "BAND" nb  $ $  "ROUTINE"  $
The directive "FORCE" may be used at most once.
For an axisymmetric calculation, the forces must be divided
by 2π, since the calculation refers to ONE radians.
The elements of the list defined by LECDDL and LECTURE are stored
according to their nodes and each node according to its degree of
freedom, in the order of their definitions in the procedures
LECTURE and LECDDL.
For example :
will define the list n(1,7) n(2,7) n(3,7) n(1,8) n(2,8) n(3,8)
n(1,10) n(2,10) n(3,10) where n(i,j) represents the i th degree of
freedom of the node j . The 7 th element of this list is the first
degree of freedom of the 10 th node.
The parameter ntmax represents the maximum number of time increments
for which the loads are defined. At the most ntmax cards or ntmax data
sets can be read on the file. If a subroutine is entered,
it is used ntmax times.
The user must choose between 3 input modes for the data :
CARD ( "CART" )FILE ( "BAND" )
SUBROUTINE ( "ROUTINE" )
Only one can be used.
The parameter nband repesents the number of the file from which
the data is read. The file has been first defined at the level
of the control cards.
The different sets of values are written on that file. Each
set contains:
 the value of the time increment to which the data of the set
is associated;
 the values of the forces F(j,t), as for the cards.
The number of the values F(j,t) must corresponds to the number of
the elements defined in the LECDDLLECTURE list, that is to say
s values ( s : number of nodes ; x : number of degrees of freedom).
The j th value F(j,t) represents the value of the force applied to
the node at time t, according to the direction defined by the
j th element of the list.
The values are written on the file unformatted.
If the user reaches the end of the file before he has read all
nt value sets, EUROPLEXUS considers that there are no more values to be
read. In this case, the loading is finished and the program goes to
the next option or instruction.
If there are more than nt data sets, the loading is considered
as finished after the reading of the nt th set.
In both cases, the last time increment must be greater than the
final time of computation defined in the instruction "CALCUL".
The reading of the nband number leads EUROPLEXUS to read the file
automatically.
The keyword "ROUT" must be the last data of the card. It
automatically calls the user’s subroutine. At the most, the latter
will be used nt times (but if he wants, the user can stop the
subroutine before the nt th . After each call, the subroutine
provides the EUROPLEXUS program with an array (F or P) which contains
as many values as elements defined in the LECDDLLECTURE list.
The j th value of the table is the value of the node to which a
force is applied according to the direction determined by the j th
element of the list. If he wants, the user can provide, after the
word "ROUTINE", the data which are written on new cards. This data
is read sequentially and in the order required by the subroutine.
For more explanations, see the chapter "PROGRAMMED LOADSSUBROUTINE".
F.240
This suboption enables loads (forces or pressures) to be read
on cards.
"CARTES" ( "INSTANT" ti f1 ... fs ) "TERMINE"
At the maximum, the word "INSTANT" is written nt times.
Each card must include, after the value of the time increment
ti, as many fj values as elements defined in the LECDDLLECTURE
list, that is to say s values. The j th fj value is the value of
the force which is applied, at time ti, to the node and according
to the direction defined by the j th element of the list.
All the numerical values are read in free format.
The word "TERM" indicates that there is no more data to be read.
The program considers the loading as finished and takes the next
option or instruction.
The last time increment to be read must be greater than
to the final time of computation defined in the instruction
"CALCUL".
The word "CARTE" leads EUROPLEXUS to read the cards automatically.
F.260
This option enables the following to be entered for each
time instant:
 a pressure which is exerted on a set of adjacent segments or
"pressure line", for twodimensional computations.
 a pressure which is exerted on shell elements defining
a surface, for two and threedimensional computations.
 a pressure which is exerted on the faces of solid elements
defining a "pressure surface".
$ "PRESS"  "SEGM" /LECTURE/  ... $ $  "COQU" /LECTURE/  $ $  "FACE" iface /LECTURE/  $ $ "MXTP" ntmax  "CART" ( "INST" ti f1 ... fn )  $ $  "BAND" nb  $ $  "ROUTINE"  $
The input syntax of the data is the same as for the
"PROGRAMMED FORCES".
The words "CART" "BAND" "ROUTINE" and the parameters ntmax
and nb have the same signification as for the "PROGRAMMED FORCES".
As for the latter, the jth value defined after the time increment,
on the cards or in the data sets written on the file, gives the
value of the pressure which is exerted, at that time increment,
on the jth element of the list provided by the procedure LECTURE.
The j th element of the array provided by the subroutine has
the same meaning (see the chapter "PROGRAMMED FORCES").
For a twodimensional computation, the options "SEGM" and "COQU"
can be used one after the other.
For example :
"PRES" "SEGM" "LECT" 1 2 3 4 "TERM" "COQU" "LECT" 9 13 18 "TERM"
The list given by the two procedures LECTURE is respectively
composed by the 3 segments 12 23 34, and by the 3 shells
9 13 18. The 6th element of the list represents the shell number 18.
For threedimensional computation, the options "COQU" and "FACE"
can be used one after the other.
For example :
"PRES" "COQU" "LECT" 9 10 25 "TERM" "FACE" 3 "LECT" 16 2 12 "TERM"
The list given by the two procedures LECTURE is respectively
composed of the shell elements 9 10 25, and the solid elements
16 2 12. The 4th element of the list repesents the solid element
number 16.
If there are two procedures LECTURE, the list which must take
into account the values of the cards, data sets or tables may be
obtained by putting the 2 lists defined by the procedures end to
end, in the order of their definitions ( the second list follows
the first).
If he wants, the user can define several times the words
"SEGM" "COQU" or "COQU" "FACE" with the corresponding lists, and
in any order. The principle used to obtain the final list on which
the loads are defined is the same one used if there are only
two LECTURE procedures.
Examples:
1/ 2D "PRES" "SEGM" /LECTURE/ "COQU" /LECTURE/ "SEGM" /LECTURE/ 2/ 3D "PRES" "FACE" 1 /LECTURE/ "COQU" /LECTURE/ "FACE" 4 /LECTURE/
For the conventions relative to the pressure signs, see the
chapter on FACTORIZED LOADS and the corresponding options.
F.290
This is a FORTRAN subroutine provided by the user and
compiled independently from the program.
There is one subroutine for the forces (FPROG) and one
for the pressures (PPROG).
For each time increment, these subroutines create an array
(F for forces and P for pressures), containing the values of the
forces and the pressures according to the list supplied by the
LECDDL  LECTURE procedures of the options "PROG" "FORC"
or "PROG" "PRES".
1. Programmed forces :
SUBROUTINE FPROG(KAR,IMP,IPT,T,N,NUF,FEP,TAB) IMPLICIT DOUBLE PRECISION(AH,OZ) DIMENSION FEP(*),TAB(*),NUF(2,*) . . . FORTRAN data set to compute the forces . . . RETURN END
2. Programmed pressures :
SUBROUTINE PPROG(KAR,IMP,IPT,T,N,IPOS,NUP,PRP,PRF,TAB) IMPLICIT DOUBLE PRECISION(AH,OZ) DIMENSION IPOS(N),NUP(*),PRP(*),PRF(N),TAB(*) . . . FORTRAN data set to compute the pressures . . . RETURN END
The user’s subroutine is called automatically nt times (nt is
the maximum number of elementary times). It has been defined in the
options "PROG" "FORC" and "PROG" "PRES".
However the user can stop the calling sequences before having
achieved nt calls, by giving a negative value to NB at the exit
of the subroutine (the call relative to the negative definition
of NB is not taken into account).
If the user wants to define loads for n elementary times, with
n inferior to nt, the value of NB must be negative at the
(n+1)th call. In any case, the last elementary time which has been
computed must be superior to the final time of computation defined in
the instruction "CALCUL".
F.300
Here is the sample routine FPROG contained in the program:
C FPROG SOUPLEX LPRE 91/06/07 19:19:31 SUBROUTINE FPROG(KAR,IMP,IPT,T,N,NUF,FEP,TAB) C C OBJET : LIRE LES FORCES AUX NOEUDS POUR UN INSTANT CONSIDERE C  C C ===> EN RETOUR : CHARGER T ET REMPLIR FEP CORRECTEMENT C C KAR : NUMERO DU FICHIER DE LECTURE ET INDICATEUR D'ARRET C IMP : NUMERO DU FICHIER DE SORTIE (IMPRIMANTE) C IPT : NUMERO DE L'INSTANT CONSIDERE C T : VALEUR DU TEMPS CONSIDERE C N : NOMBRE DE NOEUDS OU UNE FORCE EST APPLIQUEE C NUF(1,K) : NUMERO DU KIEME NOEUD DE LA LISTE C NUF(2,K) : DDL CONCERNE C FEP(K) : FORCE CORRESPONDANTE C TAB : TABLEAU DE TRAVAIL (DIM AJUSTABLE AVEC "TRAV" ) C C ===> IMPORTANT : NE PAS MODIFIER IPT, N, NUF. C C SI KAR EST MIS < 0 , ON ARRETE LA LECTURE AVANT D'AVOIR EPUISE C TOUS LES INSTANTS PREVUS C C IMPLICIT DOUBLE PRECISION (AH,OZ) C CHARACTER*(10) MOT C PARAMETER (NFORC=20) C DIMENSION NUF(2,*),FEP(*),TAB(NFORC,2) DIMENSION X(3) C C IF(KAR.LE.0) RETURN C READ (KAR,*) MOT IF(MOT.EQ.'TERMINE') GOTO 91 IF(MOT.NE.'INSTANT') GOTO 90 C C LECTURE D'UN BLOC (A T DONNE : NP COUPLES R,F ) READ (KAR,*) T,NP IF(NP.GT.NFORC) GOTO 88 READ (KAR,*) (TAB(K,1),TAB(K,2),K=1,NP) C WRITE (IMP,*) ' ===> INSTANT : ',T CALL DPRINT(IMP,NP,TAB(1,1),'RAYON') CALL DPRINT(IMP,NP,TAB(1,2),'VALEUR') C C COORDONNEES DU CENTRE : XC=0 YC=0 C C CALCUL DES FORCES PAR INTERPOLATION LINEAIRE DO 50 K=1,N NUPO=NUF(1,K) CALL QUIDNE(0,NUPO,LON,X) IF(LON.NE.3) GOTO 89 DX=X(1)XC DY=X(2)YC R=SQRT(DX*DX+DY*DY) CALL DITPL1(NP,TAB(1,1),TAB(1,2),R,F,DFSDR,NX,IER) IF(IER.NE.0) GOTO 87 FEP(K)=F 50 CONTINUE RETURN C C ERREURS ET SORTIE 87 CALL ERRMSS('FPROG','INTERPOLATION INCORRECTE') STOP 88 CALL ERRMSS('FPROG','IL Y A TROP DE VALEURS') STOP 89 CALL ERRMSS('FPROG','IL N Y A PAS 3 COORDONNEES') STOP 90 CALL ERRMSS('FPROG','SYNTAXE INCORRECTE') STOP 91 KAR=KAR RETURN C END
F.305
Here is the sample routine PPROG contained in the program:
C PPROG SOUPLEX LPRE 91/06/07 19:19:12 SUBROUTINE PPROG(KAR,IMP,IPT,T,N,IPOS,NUP,PRP,PRF,TAB) C C OBJET : LIRE LES PRESSIONS AUX NOEUDS POUR UN INSTANT CONSIDERE C  C C ===> EN RETOUR : CHARGER T ET REMPLIR PRP CORRECTEMENT C C KAR : NUMERO DU FICHIER DE LECTURE ET INDICATEUR D'ARRET C IMP : NUMERO DU FICHIER DE SORTIE (IMPRIMANTE) C IPT : NUMERO DE L'INSTANT CONSIDERE C T : VALEUR DU TEMPS CONSIDERE C N : NOMBRE DE FACES SOUS PRESSION C IPOS : POINTEUR SUR NUP ET PRP : C KDEB = IPOS(I) : ADRESSE DU DEBUT DE LA FACE I C KFIN = IPOS(I+1)1 : ADRESSE DE LA FIN DE LA FACE I C NBNF = IPOS(I+1)IPOS(I) : NBR DE NOEUDS DE LA FACE I C NUP(KDEB:KFIN) : NUMEROS DES NOEUDS DE LA FACE I C PRP(KDEB:KFIN) : PRESSION AUX NOEUDS DE LA FACE I C PRF : TABLEAU DE TRAVAIL (DIM N) : PAR EXEMPLE : C PRESSIONS APPLIQUEES SUR LES N FACES AU TEMPS T C TAB : TABLEAU DE TRAVAIL (DIM AJUSTABLE AVEC "TRAV" ) C C ===> IMPORTANT : NE PAS MODIFIER IPT, N, IPOS, NUP. C C SI KAR EST MIS < 0 , ON ARRETE LA LECTURE AVANT D'AVOIR EPUISE C TOUS LES INSTANTS PREVUS C C SI NUP(K) EST > 10000 : IL S'AGIT D'UN NOEUD APPARTENANT A UN C ELEMENT DE COQUE (SINON EL. MASSIF), LE NUMERO EST ALORS C NUCO=MOD(NUP(K),10000) C C IMPLICIT DOUBLE PRECISION (AH,OZ) C CHARACTER*(10) MOT C PARAMETER (NPRES=20) C DIMENSION IPOS(N),NUP(*),PRP(*),PRF(N),TAB(NPRES,2) DIMENSION X(3) C C IF(KAR.LE.0) RETURN C READ (KAR,*) MOT IF(MOT.EQ.'TERMINE') GOTO 91 IF(MOT.NE.'INSTANT') GOTO 90 C C LECTURE D'UN BLOC (A T DONNE : NP COUPLES R,P ) READ (KAR,*) T,NP IF(NP.GT.NPRES) GOTO 88 READ (KAR,*) (TAB(K,1),TAB(K,2),K=1,NP) C WRITE (IMP,*) ' ===> INSTANT : ',T CALL DPRINT(IMP,NP,TAB(1,1),'RAYON') CALL DPRINT(IMP,NP,TAB(1,2),'VALEUR') C C COORDONNEES DU CENTRE : XC=0 YC=0 C C CALCUL DES PRESSIONS PAR INTERPOLATION LINEAIRE DO 50 IFA=1,N KDEB=IPOS(IFA) KFIN=IPOS(IFA+1)1 NBNF=IPOS(IFA+1)KDEB PRF(IFA)=0 DO 40 K=KDEB,KFIN NUCO=MOD(NUP(K),10000) CALL QUIDNE(0,NUCO,LON,X) IF(LON.NE.3) GOTO 89 DX=X(1)XC DY=X(2)YC R=SQRT(DX*DX+DY*DY) CALL DITPL1(NP,TAB(1,1),TAB(1,2),R,P,DPSDR,NX,IER) IF(IER.NE.0) GOTO 87 PRP(K)=P PRF(IFA)=PRF(IFA)+P 40 CONTINUE PRF(IFA)=PRF(IFA)/NBNF 50 CONTINUE RETURN C C ERREURS ET SORTIE 87 CALL ERRMSS('PPROG','INTERPOLATION INCORRECTE') STOP 88 CALL ERRMSS('PPROG','IL Y A TROP DE VALEURS') STOP 89 CALL ERRMSS('PPROG','IL N Y A PAS 3 COORDONNEES') STOP 90 CALL ERRMSS('PPROG','SYNTAXE INCORRECTE') STOP 91 KAR=KAR RETURN C END
F.310
The user wants to enter FORCES into the directions x and y
(degrees of freedom 1 and 2). These forces are applied to the nodes
1, 3, 5, 7, 9, 11.
Their values are the same for all the nodes,for both directions;
these values are defined by analytical formulas:
F = 2.5 * Sin( pi * t ) For t .LE. 20 milliseconds
F = 2.9 * Sin( 2 * pi * t ) For t .GT. 20 milliseconds
The programming concerns 51 elementary times, a value is
calculated for each millisecond from 0 to 50.
At each elementary time, the user must provide 2*6=12 values
stored in array F (2 degrees of freedom and 6 nodes).
SUBROUTINE FPROG(KAR,IMP,IPT,T,N,NUF,F,TAB) C IMPLICIT DOUBLE PRECISION(AH,OZ) C DIMENSION F(*),TAB(*) DATA PI/3.1416/ C T=1E3*(IPT1) IF(IPT.GT.21) GOTO 20 DO 10 I=1,N 10 F(I) = 2.5 * DSIN( PI * T ) RETURN 20 IF(IPT.GT.51) GOTO 40 DO 30 I=1,N 30 F(I) = 2.9 * DSIN( 2*PI * T ) RETURN 40 KAR=KAR RETURN END
"CHARGE" 1 "PROG" 2 "FORCE" "DDL" 12 "LECT" 1 PAS 2 11 "TERM" "MXTF" 60 "ROUTINE"
The user can directly define these coefficients inside the
subroutine. There are no data cards of the user behind the
word "ROUTINE".
The value of ntmax must be superior or equal to 51, since the
subroutine has performed a test in order to stop the loading
at this value.
F.315
The user has at his disposal a file containing data sets
(elementary times and loads). It is supposed that there
are a hundred values of pressure per elementary time and each
data set is written under the form :
(F10.5,100F15.7).
The user wants to enter only one elementary time out of ten
(numbers 10, 20, 30, ...) from the initial file. For each elementary
time, the user selects the pressures occupying the ranks 1, 3, 7, 9,
11, 12 and 15 among the initial data sets. Therefore, 7 values must
be taken into account. The file has to be read completely and contains
no more than 100 value sets.
The file has been defined by number 9 at the level of the
control cards.
SUBROUTINE PPROG(KAR,IMP,IPT,T,N,IPOS,NUP,P,PRF,TAB) C IMPLICIT DOUBLE PRECISION(AH,OZ) C DIMENSION P(*),TAB(*),IPOS(*),NUP(*),PRF(*) DIMENSION NV(7) DATA NV/1,3,7,9,11,12,15/ C IF(IPT.GT.1) GOTO 10 C THE PRESSURES ARE EQUAL TO ZERO AT T=0 T=0 DO 5 I=1,N 5 P(I)=0 C READING OF THE NUMBER OF THE FILE AND THE LENGTH OF THE SETS READ(KAR,*) NB,NMAX RETURN 10 DO 20 I=1,10 READ(KAR,1000,END=50) T,(TAB(I),I=1,NMAX) 1000 FORMAT(F10.5,100F15.7) 20 CONTINUE C AT THE END OF THE LOOP ON RECORDS HAVE BEEN SKIPPED DO 30 I=1,7 30 P(I)=TAB(NV(I)) RETURN 50 KAR=KAR RETURN END
"CHARGE" 1 "PROG" 2 "PRESS" "COQUE" "LECT" 1 2 3 5 "TERM" "FACE" 3 "LECT" 7 9 11 "TERM" "MXTP" 101 "ROUTINE" 9 100
The subroutine gives an example of use of the work array TAB.
The data are read at the first call and the value of the pressures
at t = 0 is fixed on zero. The user selects 7 values (N = 7).
At the following calls, 9 records on the file are skipped in
order to get positionned on the sets 10, 20, 30, ... 100, at the
end of the reading loop. Then, the right values supplied by the work
array TAB must be stored in another array (P).
At the end of the file, the value of NB is 9 to inform the EUROPLEXUS
program that the loading is finished.
F.320
This option enables the user to enter generalized loads for
advectiondiffusion calculations (see also keyword "ADDF"
in Section A). These ’loads’ include:
 imposed timedependent temperatures  imposed timedependent heat fluxes  imposed timedependent heat generation  imposed timedependent heat convection  imposed timedependent heat radiation  imposed timedependent external pressure  imposed timedependent velocity  imposed zero velocity  imposed velocity parallel to a plane  imposed velocity parallel to a line
"ADDF" $ "TIMP" . . . $ $ "FLUX" . . . $ $ "QGEN" . . . $ $ "CONV" . . . $ $ "RADI" . . . $ $ "PRES" . . . $ $ "VELO" . . . $ $ "BLOQ" . . . $ $ "VPLA" . . . $ $ "VLIN" . . . $
The single suboptions are described below.
The word "ADDF" is the first keyword of the option . It should be used
only once in the EUROPLEXUS data set.
F.321
To prescribe timedependent nodal temperatures in an
advectiondiffusion calculation.
"TIMP" nti*( "NOEU" /LECTURE/ "TPOI" ntp*(T,t))
Remember to dimension sufficiently for the number of groups (nti)
and of time points (ntp), see Section A.
F.322
To prescribe a timedependent normal heat flux on element faces in an
advectiondiffusion calculation.
"FLUX" ntf*( "NELE" nel /LECTURE/ "TPOI" ntp*(flux,t))
Remember to dimension sufficiently for the number of groups (ntf)
and of time points (ntp), see Section A.
F.323
To prescribe a timedependent volumetric heat generation in an
advectiondiffusion calculation.
"QGEN" ntq*( "FIRS" n1 "LAST" n2 "TPOI" ntp*(Q,t))
Remember to dimension sufficiently for the number of groups (ntq)
and of time points (ntp), see Section A.
F.324
To prescribe a convective heat transfer condition in an
advectiondiffusion calculation.
"CONV" ntb*( "NELE" nel /LECTURE/ "TPOI" ntp*(H,T,t))
Remember to dimension sufficiently for the number of groups (ntb)
and of time points (ntp), see Section A.
F.325
To prescribe a radiation heat transfer condition in an
advectiondiffusion calculation.
"RADI" nrad*( "NELE" nel /LECTURE/ "TPOI" ntp*(Hr,T,t))
Remember to dimension sufficiently for the number of groups (nrad)
and of time points (ntp), see Section A.
F.326
To prescribe a timedependent external pressure in an
advectiondiffusion calculation.
"PRES" npres*( "NELE" nel /LECTURE/ "TPOI" ntp*(p,t))
Remember to dimension sufficiently for the number of groups (npres)
and of time points (ntp), see Section A.
F.327
To prescribe timedependent nodal fluid velocities in an
advectiondiffusion calculation.
"VTIM" nvel*( "NOEU" /LECTURE/ "TPOI" ntp*(v,t) $[ "PERP" ; "PARA" "ANG1" a1 "ANG2" a2 ]$ )
Remember to dimension sufficiently for the number of groups (nvel)
and of time points (ntp), see Section A.
F.328
To prescribe null nodal fluid velocities or velocities
parallel to a plane or to a line in an
advectiondiffusion calculation.
"VELO" $[ "BLOQ" /LECTURE/ ; "VPLA" /LECTURE/ ; "VLIN" "NOEU" /LECTURE/ $[ "PERP" ; "PARA" "ANG1" a1 "ANG2" a2 ]$ ]$
Subdirectives "BLOQ", "VPLA" and "VLIN", if present,
should appear in this order.
To impose seismiclike loads in a domain discretized by
spectral elements, for the simulation of earthquakes and
wavepropagation problems.
There are two main classes of loadings:
 punctual sources, introduced by the keyword "POIN";  plane wave sources, introduced by the keyword "PLAN";  seismic moment sources, introduced by the keyword "SISM".
F.360
This directive specifies punctual sources of loadings for
spectral elements. The load is computed as the product
of a time function and a function of space:
f(x,y,z,t) = h(t) * g(x,y,z)
"POIN" <"NODP" /LECT/> [ "BET" ; "COS" ] [ "DELT" ; "SPRE" ; "PRES" ; "SHEA" ] "SOUR" "AMP" amp "T0" t0 "BETA" beta "ALFA" alfa <"X" x0 "Y" y0 <"Z" z0>> <"NX" nx "NY" ny <"NZ" nz> >
h(t) = amp * (1  2*beta*(t  t0)^2) * exp(beta * ((t  t0)^2)
h(t) = amp * cos(Pi*beta*(t  t0)) * exp(0.5*beta^2 * ((t  t0)^2)
g(x,y,z) = exp(  alfa^2 * R^2 )
f_x = h(t) * 2 * alfa^2 * (x  x0) * exp(  alfa^2 * R^2 ) f_y = h(t) * 2 * alfa^2 * (y  y0) * exp(  alfa^2 * R^2 ) f_z = h(t) * 2 * alfa^2 * (z  z0) * exp(  alfa^2 * R^2 )
f_x =  h(t) * 2 * alfa^2 * (y  y0) * exp(  alfa^2 * R^2 ) f_y = h(t) * 2 * alfa^2 * (x  x0) * exp(  alfa^2 * R^2 )
h(t) = amp * (1  2*abs(beta)*(t  t0)^2)
h(t) = amp * cos(Pi*abs(beta)*(t  t0))
These loads are all volumetric (specific) forces, except in the case of
DELT. This is in order to avoid mesh dependency of the total energy
introduced in the system.
Therefore, amp represents the total force (per unit volume)
acting on all affected
nodes at time t0, and this quantity varies in time according
to h(t).
In the special case of DELT, the user is responsible of
calibrating the (nonvolumetric) force with respect to the nodal
mass of the application point.
F.370
This directive specifies loading sources in the
form of distributed loadings for
spectral elements. The load is applied to all
nodal points (typically) along a plane (or a line in 2D) and
varies in time according to the same time function in
all loaded points (except in the case "DLEN", see below).
"PLAN" [ "BET" ; "COS" ] "SOUR" "AMP" amp "T0" t0 "BETA" beta <"DLEN" dlen> "NX" nx "NY" ny <"NZ" nz> "NOEU" /LECTURE/
h(t) = amp * (1  2*beta*(t  t0)^2) * exp(beta * ((t  t0)^2)
h(t) = amp * cos(Pi*beta*(t  t0)) * exp(0.5*beta^2 * ((t  t0)^2)
F = 2*rho*c*(dh/dt)*vol*fac
fac = 2 / (dlen * W)
These loads are volumetric (specific) forces.
This is in order to avoid mesh dependency of the total energy
introduced in the system.
Therefore, amp represents the total force (per unit volume)
acting on all affected
nodes at time t0, and this quantity varies in time according
to h(t).
F.380
This directive specifies loading sources in the form of
seismic moment loadings for spectral elements. The load is applied
to a ’fault’ defined by a series of nodes, introduced by the
keyword NOEU. The program verifies the alignment of the
given nodes along a line in 2D and on a plne in 3D.
As a special case, a single fault node
can be specified (pointwise loading).
A slipping vector must be defined by
keywords SX, SY, SZ.
The user can also specify the normal to the fault by the keywords
NX, NY, NZ.
If the normal is missing, the program assumes it coincident
with the slipping vector.
The load applied to each nodal point varies in time according to
the distance from the ipocenter, defined by its coordinates
X, Y, Z.
The time delay in each point depends upon the above mentioned distance
and on the speed of transversal wave propagation. This speed is
automatically evaluated by the code, or can alternatively be imposed
by the keyword VRUP.
"SISM" [ "BET" ; "COS" ] "SOUR" "AMP" amp "T0" t0 "BETA" beta "SX" sx "SY" sy <"SZ" sz> <"NX" nx "NY" ny <"NZ" nz>> "X" x "Y" y <"Z" z> <"VRUP" vrup> "NOEU" /LECTURE/
h(t) = amp * (1  2*beta*(t  t0)^2) * exp(beta * ((t  t0)^2)
h(t) = amp * cos(Pi*beta*(t  t0)) * exp(0.5*beta^2 * ((t  t0)^2)
The present model has been borrowed from the ELSE code of CRS4
and is meshdependent in that the applied loadings
depend on mesh size. A slightly modified, meshindepenedent
implementation is also available in EUROPLEXUS, and is activated by
choosing a negative value for VRUP.
F2.20
This directive allows to introduce constant forces or moments
during the whole computation.
The loads may be applied
either to the nodes of a deformable body, or to
the centroid of a rigid body.
FCTE $[ NODE ; RIGI ]$ /LECT/ $[ FORC f ; MOME m ]$ VECT x y z
Three vector components must be specified, even in 2D calculations.
The vector is used to determine the direction of the applied force
or moment. It does not need to be unitary, since it is automatically
normalized immediately after reading.
The applied forces or moments must be expressed in the global reference
frame X, Y, Z (for rigid bodies, the rotational values are then converted
internally to the local reference frame, as appropriate).
The meaning of the vector components (VECT x y z) is as follows:
F2.30
This directive allows to introduce timedependent forces or moments
during the transient computation. The loads may be applied
either to the nodes of a deformable body, or to
the centroid of a rigid body.
The timedependency of the load is
specified by a function (see directive FONC on page E.15 and
following ones).
FIMP $[ NODE ; RIGI ]$ /LECT/ $[ FORC f ; MOME m ]$ VECT x y z NUFO nf
Three vector components must be specified, even in 2D calculations.
The vector is used to determine the direction of the applied force
or moment. It does not need to be unitary, since it is automatically
normalized immediately after reading.
The applied forces or moments must be expressed in the global reference
frame X, Y, Z (for rigid bodies, the rotational values are then converted
internally to the local reference frame, as appropriate).
The meaning of the vector components (VECT x y z) is as follows:
The defined load A is multiplied by a coefficient C(t) which
varies in time and is interpolated from the specified table:
F2.40
This directive allows to introduce timedependent dynalpy loads
in 1D elements of type TUBE or TUYA.
FDYN NODE /LECT/ PZER p0 COEF c VECT x y z ELEM e
Three vector components must be specified, even in 2D calculations.
The vector is used to determine the direction of the applied load.
It does not need to be unitary, since it is automatically
normalized immediately after reading.
These loads are only related to 1D elements of type TUBE or TUYA
and are defined as:
where p is the current pressure in the specified element.
F2.50
This directive allows to apply air blast loading
directly to a set of strucural elements (continuum, shells)
without using specialized CLxx elements with an associated IMPE AIRB
material. This simplifies the treatment of element erosion and mesh adaptivity.
AIRB [ "X" x "Y" y <"Z" z> ; "NODE" /LEC1/ ] "MASS" m $[ "TINT" t ; "TAUT" ]$ <"OPOS"> <"ANGL"> <"CUBE"> <"COEF" cf> <"CONF" c> <"DECA" d> <"PMAX" pmax "TD" td "B" b> <"SHAD" /LECS/> /LECT/
p(t)=p_{0}+p_{max}(1− 
 ) 

This model requires that the user adopts the standard Unit system, i.e. metres, Kilograms, seconds.
The equations of Kingery are only usable up to a scaled distance of Z=40. Above this distance, diagrams of Baker are used (linearised in the double logarithmic scale).
For more information on the physical models, consult the following references: