Model Description Language (MDL)
The Model Description Language (MDL) is a data driven language for describing the geometrical, the physical, and the mathematical properties of a problem, and the numeric parameters for the solver(s). To enable parametric models, MDL has features such as variable assignment, substitution, and some flow control statements.
MDL Language Elements
MDL features variable assignment, substitution, and flow control. These features enable the writing of parametric input files. This functionality proves useful in a wide range of contexts, but it cannot replace real programming languages (such as Python).
MDL format
MDL language elements are placed in text files. These files may be created with text editors or by means of scripts.
MDL is interpreted as a stream of items which are separated by space characters and newline characters. It does not matter how many space or newline characters are present. Example:
One
two
three 4
is equivalent to
One two three 4
Items pertaining to the parametric input either begin with a reserved word or are enclosed in parentheses. Such items are processed and may expand to new data items. This is illustrated by means of the following example:
(a=4) One to three (a)
The item “(a=4)” assigns the integer value 4 to the variable “a”, and the item “(a)” expands the current contents of variable “a”. Thus, the expanded MDL is
One to three 4
Comments, i.e. explanatory text, begin with the # character and stretch until the end of the line.
Numeric data
Integer (or int) numbers contain the characters 09, possibly prefixed by the unary operators + or . Examples:
100 1 +1234
Floatingpoint (or float) numbers have either a decimal point (.), an exponent (letter e or E, possibly followed by + or , and followed by 13 digits), or both. They may be prefixed by the unary operators + or . Examples:
0. 1. 123.1 .1 1e20 1.234E+2 +0.0002
Character string and text string data
Unquoted character strings begin with an alphabetic character, followed by an arbitrary number of alphanumeric characters and/or the dot (.) and underscore (_) characters. Such unquoted character strings are used for both attribute names and attribute values. Examples:
ischeme GAUSS3X3
eltype B2.S.RS
analysis dynamic_nonlinear
Text strings (or str data) may contain any printable characters and must be delimited by single quotes (’) or double quotes (“). Example:
"A text string with 8 words and one number"
Special characters must be preceded by the backslash () character. Example:
"A text string with \"quotes\" and a newline character\n"
List data
Lists are sequences of primitive data, usually integer or floatingpoint numbers, character strings, or text strings. Lists are enclosed by square brackets. Example:
[ 1 2 3 4 ]
For longer lists, ranges can be specified inside the list. Example:
[ 1 10/20 45 46 50 ]
generates a list of integers in the form of
[ 1 10 11 12 13 14 15 16 17 18 19 20 45 46 50 ]
A step size can optionally be specified. The following
[ 1 10/20/2 45 46 50 ]
generates a list of integers in the form of
[ 1 10 12 14 16 18 20 45 46 50 ]
Include files
Portions of MDL can be placed in separate files which can be inserted by
means of the include
statement:
include FILENAME
FILENAME
must be a valid file name without any escape
sequences. If it contains spaces, dot characters (.), slash characters
(/), or other special characters, it must be enclosed by single or
double quotes. File names are relative w.r.t. the directory of the MDL
file containing the include
statement. Examples:
include "../../materials.mdl"
include "case_def.mdl"
Variable assignment
Variables are assigned by means of the assignment operator = and the expression must be enclosed by parentheses. Example:
(i=3)
will assign the integer value 3 to the variable i.
Variable names begin with an alphabetical character (az, AZ), followed by zero or more alphanumeric and/or underscore (_) characters.
The value that will be assigned to the variable is evaluated from the expression that follows the assignment operator. From the expression’s type, the type of the variable is inferred.
The operator ?=
assigns only if the variable has not already been
assigned. In conjunction with the define
commandline option, it
can be used to specify default values that can be overridden on the
command line. Example:
(eltype?="Q9.S.MITC")
This is identical to the following:
if (not isdefined(eltype)) {
(eltype="Q9.S.MITC")
}
Data types
For variable assignment, evaluation of expressions, and substitution of expressions, the following primitive data types are supported:
Data type 
Description 

bool 
Represents boolean values. Only the constant values 
int 
Represents 32bit signed integer numbers. 
float 
Represents 64bit IEEE754 floatingpoint numbers. 
str 
Represents text strings. 
Data type conversion
Expressions can be converted from one data type to another by means of
the functions bool()
, int()
, float()
, str()
. Example:
(a=int(4.2**3))
assigns the int value 74 to the variable “a”.
Substitution
Any expression, variable, or constant of one of the aforementioned data types, when enclosed by parentheses, constitutes a substitution statement. Example:
(eltype="Q4.S.MITC") (t1=2.5) (t2=1.5)
eltype (eltype) mid 1 thickness (t1+t2) eccent (t2/2)
is equivalent to
eltype "Q4.S.MITC" mid 1 thickness 4. eccent .75
Expressions
Number of Operands 
Operator 
Description 

binary 
and, or 
Logical “and”, “OR 
unary 
not 
Logical “not” 
All logical operators return bool values.
The “not” operator has a higher precedence than the “and” and “or” operators.
The following relational operators yield bool values:
==, !=, <, <=, >, >=
The operands may be of any type. Operands of type bool and int are converted to type float. Values of type str are always “greater” than bool and numerical values. Relational operators have higher precedence than logical operators.
The following arithmetic operators (for expressions of type int and float) are available. They are listed with increasing precedence (all of them with higher precedence than relational operators), with the addition and subtraction operators having the lowest precedence, and the power operator the highest.
Number of Operands 
Operator 
Description 

binary 
+,  
Addition and subtraction. 
binary 
*, / , mod 
Multiplication, division, and modulus. 
unary 
+,  
Defines the sign of the numeric operand. 
binary 
** 
Power. 
All these operators can be applied to operands of type int and type float. For binary operators, when both operands are of type int, the result is also of type int. When both operands are of type float, the result is also of type float. When one operand is of type int and the other of type float, the int operand is first converted to a float, and the result is of type float.
For str expressions, the binary operator + means concatenation:
("A " + "string " + "with " + "several " + "words.")
Subexpressions may be enclosed in parentheses to override the operator precedence rules. Example:
(e=73.1e3) (p=0.33) (g=e/(2*(1+p)) (g)
Builtin functions and constants
Function name 
Description 

abs(x) 
Returns the absolute value of x. The type of x (integer or floatingpoint number) is preserved. 
isdefined(x) 
Returns 
max(x, y, …) 
Returns the argument with the maximum value. The arguments may have different types. A string is always “greater” than a number. 
min(x, y, …) 
Returns the argument with the minimum value. The arguments may have different types. A string is always “greater” than a number. 
Function name 
Description 

math.acos(x) 
Returns the arc cosine (measured in radians) of x. 
math.asin(x) 
Returns the arc sine (measured in radians) of x. 
math.asin(x) 
Returns the arc tangent (measured in radians) of x. 
math.cos(x) 
Returns the cosine of x (measured in radians). 
math.degrees(x) 
Converts angle x from radians to degrees. 
math.exp(x) 
Returns math.e**x 
math.log(x) 
Returns the natural logarithm of x. 
math.log10(x) 
Returns the base 10 logarithm of x. 
math.radians(x) 
Converts angle x from degrees to radians. 
math.sin(x) 
Returns the sine of x (measured in radians). 
math.sqrt(x) 
Returns the square root of x. 
math.tan(x) 
Returns the tangent of x (measured in radians). 
Constant name 
Description 

math.e 
The Euler number (2.718281828459045) 
math.pi 
The number Pi (3.141592653589793) 
Conditional processing
The if
statement allows for conditional processing. Example:
if (a < 0) {
"a is smaller than zero"
} elif (a == 0) {
"a is zero"
} else {
"a is greater than zero"
}
There can be zero or more elif
parts. The else
part is optional.
The conditionally processed parts are enclosed in curly brackets ({ and
}).
Conditional loops
The while
statement can be used to process the same part several
times, as long as the condition evaluates to true. Example:
(i=1) while (i <= 10) {(i**2) (i=i+1)}
evaluates to
1 4 9 16 25 36 49 64 81 100
The break and continue statements
The break
statement exits the directly enclosing loop. The
continue
statement stops the processing of the current iteration of
the loop and continues with the next iteration of the loop. Example:
(i=1) while (1) {(i**2) if (i==10) {break} (i=i+1)}
MDL Commands
MDL commands are text blocks describing specific data, such as node
coordinates, material properties, etc. Each block starts with a
keyword and is terminated by end
.
Upper case text in the input descriptions of blocks and all other specifications of this chapter signifies replaceable or variable.
The tables below summarize all MDL blocks of the mesh definition, the boundary conditions definition, the material properties definition, and analysis control.
Command 
Description Summary 

Specify branches in a multibranch (multimesh) model. 

Defines branch local to global coordinate systems. 

Defines element edge sets. 

Defines single elements. 

Defines element and node patches. 

Defines single elements of current branch (mesh). 

Defines element sets. 

Defines element face sets. 

Couples adjacent incompatible surface meshes. 

Connects nodes of meshes. 

Defines single nodes of current branch (mesh). 

Defines node sets. 

Defines local DOF coordinate systems. 
Command 
Description Summary 

Defines ambient temperatures. 

Defines initial DOF conditions. 

Defines initial timederived DOF conditions. 

Defines essential boundary conditions (constraints). 

Defines linear constraint equations. 

Defines natural boundary conditions. 

Defines node temperatures. 
Command 
Description Summary 

Defines element materials. 

Defines beam element properties. 
Command 
Description Summary 

Analysis directives 

Specifies analysis case parameters. 

Specifies analysis stage parameters. 
Command 
Description Summary 

Specifies Problem title. 

Specifies local DOF coordinate system transformations. 
adir
adir
specifies the analysis cases to be processed and directives
that apply to all analysis cases. adir
may only be defined once in
a MDL file.
MDL Specification
adir
directives...
end
Directives (required)
case IDENT  cases [IDENT1 IDENT2 ...]
Specifies the analysis case(s) to be processed (required). The identifier
IDENT
refers to a specific analysis case, see the case command.
Directives (optional)
add_ssc_elements
Automatically add shelltosolid coupling (SSC) elements on interfaces between shell and solid elements. Note that the shell intersection detection algorithm is inhibited if the
iponly
option is specified in calling the B2000++ input processor.
drills V
The drill stiffness factor
V
is used by the MITC shell elements to stabilize the 6^{th} degreeoffreedom (RZ). The default value is 1e8.
shell_intersection_angle V
MITC shell elements only: The node type with 5 or 6 degreesoffreedom is determined in function of topological and geometric properties of the Finite Element mesh, as well the essential boundary conditions. The shell intersection angle
V
specifies the minimum angle in degrees (default is 30.0) at which elements meet. Thus, nodes of elements joining at an angle greater than v will have 6 degreesoffreedom.Note that the shell intersection detection algorithm is inhibited if the iponly option is specified in calling the B2000++ input processor.
symmetry_plane PX PY PZ NX NY NZ
Specifies a symmetry plane by specifying a point p=(PY,PY,PZ) of the plane and the normal of the symmetry plane n=(NY,NY,NZ). Up to 6 symmetry planes can be defined. Note that defining symmetry planes does not entail that the symmetry planes will be used by B2000++. Specific solvers, such as the heat analysis radiation solver, will check for symmetry planes.
atemperatures
atemperatures
specifies ambient temperature values at nodes for
defining convective conditions in heat analysis in conjunction with
the heat convection ‘overlay’ elements` defining the set number (a
positive integer). To specify temperatures at nodes inducing thermal
strains in stress analysis, please refer to the command. An
atemperatures
set is identified by IDENT
, a nonnegative integer
which must be unique for the atemperatures
conditions of the
current model. IDENT
is the number which is referenced by the
atemperatures
parameter of the case command. Sets with an
IDENT
of 0 will be active for all analysis cases.
MDL Specification
atemperatures ID
parameters
node specifications...
end
Parameters
value V
Specifies the current ambient temperature value
V
assigned to subsequently specified nodes.
Node specifications
allnodes
Assign the ambient temperature values to all defined nodes of the current branch.
branch BR
For models that consist of several branches. Specifies the external branch number
br
. To be used in conjunction with the allnodes and nodes directives.
epatch ID PX  EX  FX  B
Selects nodes from an epatch. Individual patch vertex nodes are specified with the strings
P1
toP8
. Patch edge nodes are specified with the stringsE1
toE12
. Patch face nodes are specified with the stringsF1
toF6
. Patch body nodes of the whole patch body are specified with the stringB
.
node N  nodes [N1 N2 ...]
Specifies a node or a list of nodes (of the current branch) to which the ambient temperature value will be assigned.
atemperatures
generates the dataset(s) ATEMP.br.0.0.<IDENT>
.
branch
The branch
command sets the current branch of the mesh
specifications. All meh specifications will pertain
to the branch until a new branch
command is issued. If not
specified, the default branch is 1: All MDL specifications
thereafter will refer to branch 1.
MDL Specification
branch IDENT
mesh specification...
end
Additional
A “branch” (or mesh) is a finite element mesh consisting of nodes and
elements and identified uniquely by the mode and element IDENT
(positive integers). Each branch is identified by its unique positive
integer number. The default branch is 1: All model specifications will
refer to branch 1.
Most finite element models (including those that were converted from other finite element codes) consist of a single branch or mesh, and in this case it is not necessary to specify the branch command. Defining multiple branches may be useful e.g in multidisciplinary or multidomain analysis, when combining different finite element meshes.
In the presence of multibranch (multimesh) models, the nodes (and degreesoffreedom) between branches (meshes) must be connected with the join or the link commands.
branch_orientation
branch_orientation
specifies the orientation of all node
coordinates of the current branch/mesh (or the default branch 1) with
respect to the global Cartesian coordinate system. If no
branch_orientation
is specified, the node coordinates are
expressed in the global coordinate system.
MDL Specification
branch_orientation
[base u1 u2 u3 v1 v2 v3]
[rotate axis xyz angle a]
[translate tx ty tz ]
end
Parameters
base u1 u2 u3 v1 v2 v3
Calculate the base from the vectors \(u\) and \(v\) as follows: \(u\) defines the branch base \(e_1\), \(u \times v\) defines the branch base \(e_3\), and \(e_3 \times u\) defines the branch base \(e_2\).
rotate axis xyz angle a
Rotate the current branch base about the x, y, or z axis by
a
degrees, and according to the righthand rule. Successive rotations can be specified.
rotate axis u1 u2 u3 angle a
Rotate the current branch base about the axis defined by the vector
u
bya
degrees, and according to the righthand rule. Successive rotations can be specified.
translate tx ty tz
Translate the current branch by
tx
in the xdirection,ty
in the ydirection, andtz
in the zdirection. All values are float values. The default translation is 0.0 in all three directions.
Example
The current branch is translated by x=50, y=20 and rotated by 30 degrees about the zaxis:
branch_orientation
translate 50.0 20.0 0.0
rotate axis z angle 30.0
end
The same transformation is defined by
branch_orientation
translate 50.0 20.0 0.0
base 0.866 0.5 0.0 0.5 0.866 0.0
end
case
case
specifies all ingredients needed for the analysis case
identified by IDENT
(positive int), in particular the boundary
conditions, the initial conditions, and the solution strategy
parameters.
To activate the analysis case in the solver, a case must be specified
with they the case
parameters of the adir command.
MDL Specification
case IDENT
parameters
end
Parameters
The attributes enumerated in this section pertain to most types of analyses and concern the specification of initial conditions sets, boundary condition sets, and constraint sets. Solverspecific attributes are explained in the Solvers.
analysis T
Optional type of analysis for the present analysis case. If several cases are specified in an MDL input file the analysis type must be the same of all cases. The string
T
is one of
linear
Linear static (or stationary) analysis, see Linear Static Solver. This is the default analysis type (new from version 4.5.3. Previous versions MUST specify the analysis type!).
nonlinear
Nonlinear static or stationary) analysis, see Static Nonlinear Solver (B2000++ Pro).
linearised_prebuckling
Bifurcation buckling analysis (solid mechanics), see Linearized PreBuckling Solver.
free_vibration
Free vibration analysis (solid mechanics), see Undamped Free Vibration Solver.
dynamic_nonlinear
Nonlinear dynamic (transient or nonstationary) analysis, see Dynamic Nonlinear Solver (B2000++ Pro).
frequency_dependent_free_vibration
Frequencydependent free vibration analysis. See FrequencyDependent Undamped FreeVibration Solver (B2000++ Pro).
atemperatures IDENT [sfactor Ssfunction "EXPRESSION"]
Include the ambient temperatures set
IDENT
in the analysis (heat analysis).sfactor
andsfunction
are explained below.
component NAME type "ARGUMENT" [sfactor Ssfunction "EXPRESSION"]
Specifies a component to be included in the current analysis case. Components are extensions to B2000++. They implement specific natural boundary conditions, essential boundary conditions, initial conditions, or sets of constraints. The component and
type
parameters are used to identify the component, while theargument
parameter is given to the component at the start of the analysis (stage).sfactor
andsfunction
are explained below.
dof_init IDENT
dof_init
includes the initial DOF conditions identified byIDENT
. Note that only one singledof_init
identifier can be specified for the current case.
dofdot_init IDENT
`dofd_init
includes the time derivatives of the initial DOF conditions identified byIDENT
. Note that only one singledofdot_init
identifier can be specified for the current case.
ebc IDENT [sfactor Ssfunction "EXPRESSION"]
Includes the essential boundary conditions identified by
IDENT
. Note that essential boundary conditions are not cumulative, i.e. if several essential boundary condition sets are specified, all values of common degreesoffreedom must be equal.sfactor
andsfunction
are explained below.
field_transfer IDENT
Includes the field_transfer set identified by
IDENT
. Thefield_transfer
set with anIDENT
of 0 is automatically added to all analysis cases.Alternatively, several or all
field_transfer
sets may be specified:field_transfer 123 field_transfer allThe accuracy of the calculated solution cannot always be ensured when
field_transfer
conditions are active. Therefore, a contraint method other thatn the default reduction methods must be specified, Linear and Nonlinear Constraint Control.
join IDENT
Includes the join set identified by
IDENT
in the current analysis case. Note that ajoin
set with an identifier of 0 is automatically added to all analysis cases.
gradients VALUE
Controls the computation of the gradients (strains, stresses, heat transfer, etc.) for the current case. Specifying a positive integer value (e.g. 1) for
VALUE
meansyes
. A value of 0 meansno
. Default is0
.
gradients_only yesno
Specifies whether only gradients (and reaction forces) should be computed, while the solution vector is defined solely by the the initial conditions and the boundary conditions. Default is
no
.
linc IDENT
Includes the :ref:
linear constraints <mdl.linc>` set identified by ``IDENT
in the current analysis case. Note that alinc
set with an identifier of 0 is automatically added to all analysis cases.
nbc IDENT [sfactor Ssfunction "EXPRESSION"]
Includes the natural boundary conditions set identified by
IDENT
in the current analysis case. Natural boundary conditions are cumulative, i.e. if several natural boundary condition sets are specified the resulting natural boundary condition forIDENT
is the sum of all natural boundary condition sets multiplied by their respective scaling.sfactor
andsfunction
are explained below.
rcfo_restrict WHAT
Specifies to which nodes the calculation of reaction forces shall be restricted in postprocessing. This parameter is ignored by the B2000++ solvers. If not specified, the relevant Simples functions or baspl++ will loop over all nodes of the model to calculate the reaction forces.
WHAT
is one of:
epatch IDENT P1P8E1E12F1F6B
epatch IDENT PX  EX  FX  B
Selects nodes from an epatch. Individual patch vertex nodes are specified with the strings
P1
toP8
. Patch edge nodes are specified with the stringsE1
toE12
. Patch face nodes are specified with the stringsF1
toF6
. Patch body nodes of the whole patch body are specified with the stringB
.
nodeset NAME
Specifies the name of the node set to be included.
sparse_linear_solver dmumpsdmumps_dpdlldmfdmf_oocdmf_ooc_nommapdpastixicgigmres
Override the automatically selected sparse solver type by prescribing a specific sparse linear solver type (string). See Sparse Linear Equation Solvers.
stage IDENT [sfactor Ssfunction "EXPRESSION"]
Includes an analysis stage identified by
IDENT
. One or more stages can be defined for the current case. If more than one stage is specified, the solver will solve for one stage after the other in the order stages have been listed. If one or morestage
parameters are specified for a given analysis case, no other may be specified for that particular case.
subcase parameters ... end
Defines a subcase of the current case. The subcase will inherit all case options, specifically the essential boundary conditons. In the present version only
nbc
case parameters also apply to subcase.
temperatures IDENT [sfactor Ssfunction "EXPRESSION"]
Includes the temperatures set identified by
IDENT
to be included for thermal stress analysis.sfactor
andsfunction
are explained below.
title 'TEXT'
Optional title describing the case.
sfactor and sfunction
In linear analysis, the optional parameter sfactor
specifies a
scale factor S
by which the set is multiplied, the default value
being 1.0.
In nonlinear direct analysis and in incremental analysis, the set is
scaled by the load factor (static analysis) or by the time (dynamic
analysis). The optional parameter sfactor
specifies an additional
scale factor S
by which the set is multiplied, the default value
being 1.0. Alternatively, the optional parameter sfunction
specifies a function which is being evaluated at each load or time
increment and by which the set is multiplied.
PerStage Commands in Multistage analysis
During nonlinear analysis, it is often necessary to split the loading path into a series of stages. In this example, case 3 is executed, which consists of two stages (defined by stages 1 and 2). To ensure convergence of the nonlinear solver in the presence of buckling (loadcontrolled by default), artificial damping is performed to stabilize the problem.
stage 1
ebc 1
nbc 1
end
stage 2
ebc 2
step_size_init 0.05
step_size_max 0.05
end
case 3
analysis nonlinear
residue_function_type artificial_damping
stage 1
stage 2
end
adir
case 3
end
The B2000++ solver initializes many of its internal procedures and
data structures on a percase basis, not on a perstage basis. The
commands for the various methods are interpreted only during this
initialization phase. Specification of commands like
residue_function_type
in a case defining stages will be ignored.
Instead, they must be placed in the definition of another case (case
3 in the above example). Consequently, residue_function_type
will
be active for both stages.
On the other hand, commands controlling the step size and the
tolerances for the residual, solution, etc., can be defined in a case
containing stage
specifications.
Components
A component can implement a weaklycoupled fullynonlinear aeroelastic toolchain. In this case, the values taken by the component are the current (nodal) displacements (calculated by B2000++), and the values returned by the component are the (nodal) forces. To this end, at each Newton iteration (or each nth Newton iteration), the component invokes the spatial coupling tool, the CFD mesh deformation tool, the CFD solver, and again the spatial coupling tool.
dof_init, dofdot_init
dof_init
and dofdot_init
define initial boundary conditions,
i.e DOF fields (such as displacements or temperatures) or initial time
derivatives of DOF fields (such as velocities). The dynamic
(transient) or nonstationary solver will include initial DOF fields
at time=0. If no initial conditions are specified the solver will
assume all initial boundary conditions to be 0. A dof_init
or
dofdot_init
set is identified by IDENT
(nonnegative
int). IDENT
is the number which is referenced by the dof_init
and dofdot_init
options of case. Sets with an identifier of
0 will be active for all analysis cases.
MDL Specification
dof_init IDENT  dofdot_init IDENT
value V
DOFLIST...
NODESPECIFICATION...
...
end
Values and DegreesofFreedom
value V
Specifies the value
V
(float) to be assigned to subsequently specified nodes. The value is assigned to a subsequently defined DOF’s!
dof I1
or dof [I1 I2 ...]
Specifies the DOF(s) identifier(s) for which the value
v
will be assigned. DOF identifiers can be integers (DOF numbers are 1,2,3,…) or strings:
During stress analysis,
UX
,UY
, andUZ
represent the displacement in the x, y, and zdirection, respectively.During stress analysis,
RX
,RY
, andRZ
represent the rotation (in radians) about the x, y, and zaxes, respectively.During heat analysis,
T
means the temperature.The degreesoffreedom that are present at a given node depend on the elements to which this node is connected. Specifying a value for a degreeoffreedom that does not exist will have no effect.
Node Specification
allnodes
Assign the initial conditions to all defined nodes of the current branch.
branch BR
Specifies the external branch number
BR
. Default is 1.
epatch IDENT P1P8E1E12F1F6B
Includes nodes generated with an existing epatch identified by
IDENT
. Individual patch vertex nodes are specified withP1
toP8
. Patch edge nodes are specified withE1
toE12
.Patch face nodes are specified withF1
toF6
. The patch body nodes are specified withB
.
nodes N
or nodes [N1 N2 ...]
Explicitly specifies a nodes identifiers (of the current branch) to which the initial conditions will be assigned.
nodeset NAME
Specifies the name of the node set which the initial conditions will be assigned.
Examples
Create a uniform dofdot
(velocity field) in the global
zdirection. Note that all other DOFS are implicitly set to 0.
dofdot_init 123
value 5 dof UZ allnodes
end
The field must be activated with the dofdot_init
parameters of
case:
case 1
...
dofdot_init 123
...
end
ebc
The ebc
command specifies essential boundary conditions, such as
singlepoint constraints, and assigns them to variables, such as
displacements in case of solid mechanics, temperatures in case of heat
transfer analysis, etc. An``ebc`` set is identified by the identifier
IDENT
(nonnegative int). IDENT
is the number which is
referenced by the ebc
parameter of the case definition. Sets
with an identifier of 0 will be active for all analysis cases.
Essential boundary conditions can be specified for nodes or, in case where elements have internal degreesoffreedom, for elements.
MDL Specification
ebc IDENT [system S] [title T]
parameters
nodespecifications
end
Parameters
system BRANCH  LOCAL
Specifies the reference frame in which the conditions are formulated. The default reference frame is
LOCAL
.BRANCH
means that the constraints are formulated with respect to the branchglobal reference frame, irrespective of nodelocal reference frames at any node.LOCAL
means that the constraints are applied to the nodelocal reference frame(s) where defined, and to the branchglobal reference frame otherwise.
title "TEXT"
Specifies an optional title for the
ebc
set.
dof I
or dof [I1 I2 ...]
Specifies the DOF(s) identifier(s) for which the value
V
will be assigned. DOF identifiers can be integers (DOF numbers are 1,2,3,…) or strings:
During stress analysis,
UX
,UY
, andUZ
represent the displacement in the x, y, and zdirection, respectively.During stress analysis,
RX
,RY
, andRZ
represent the rotation (in radians) about the x, y, and zaxes, respectively.During heat analysis,
T
means the temperature.The degreesoffreedom that are present at a given node depend on the elements to which this node is connected. Specifying a value for a degreeoffreedom that does not exist will have no effect.
value V
Specifies the value
V
(float) to be assigned to subsequently specified nodes. The value is assigned to a subsequently defined DOF’s!
Node Specification
allnodes
or allelements
Assign the initial conditions to all defined nodes of the current branch.
branch BR
Specifies the external branch number
BR
. Default is 1.
epatch IDENT P1P8E1E12F1F6B
Includes nodes generated with an existing epatch identified by
IDENT
(node specification only). Individual patch vertex nodes are specified withP1
toP8
. Patch edge nodes are specified withE1
toE12
.Patch face nodes are specified withF1
toF6
. The patch body nodes are specified withB
.
nodes N
or nodes [N1 N2 ...]
Specifies node identifiers (of the current branch) to which the initial conditions will be assigned.
nodeset NAME
or elementset NAME
Includes nodes or elements from a nodeset or from an elementset.
Examples
Specify the ebc
set 123: For the mesh node 1, set all 6 DOF’s
to 0. For the mesh nodes 9,10,11,12, set the zrotation to 0, and for
mesh node 9, the ydisplacement 2 to 0.12.
ebc 123
value 0. dof [UX UY UZ RX RY RZ] nodes 1
value 0. dof RZ nodes 9
value 0.12 dof UY nodes [9 10 11 12]
end
The ebc
set must then be activated by referencing it in one of the
cases to be computed. Example:
case 20
...
ebc 123
...
end
Elementinternal DegreesofFreedom
Some element formulations involve internal degreesoffreedom. With
the ebc
command it is possible to prescribe values to these DOFs,
e.g for debugging purposes. With elements, the individual
degreesoffreedom are identified by numbers, starting from
1.
For example the shell element Q4.S.MITC.E4
is an
enhancedassumedstrain element with 4 internal degreesoffreedom.
Locking them for all elements is done as follows:
value 0 dof [1/4] allelements
Additional information
To activate essential boundary condition sets, add the required essential boundary condition set identifiers to the case definition.
Nodelocal coordinate systems can be defined with the transformations command. The B2000++ coordinate systems are described in the programming manual.
Natural boundary conditions can be defined with the nbc command.
Please read the additional notes in the description of the join command for information on branch connectivity.
edgeset
edgeset
defines an element edge set list containing pairs
(IDENT
, EX
) of a specific branch. IDENT
is the external
element identifier and EX
the edge identifier (E1
, E2
,
…). The list is identified by the NAME
of the set (a string not
exceeding 40 characters). Note hat edge sets are not defined for
special elements, such as RBE.
MDL Specification
edgeset NAME sortedunsorted
branch BR
EX
edgeset NAME1
epatch IDENT
n1 n2 ...
end
Parameters
sorted  unsorted
sorted
creates an ordered set with all duplicates removed.unsorted
adds nodes as they are specified. Default isunsorted
.sorted
orunsorted
must be specified directly afterNAME
and before any other parameter.
branch BR
Specifies the branch number to which subsequently defined element identifiers will be assigned. The default branch is 1.
BR
remains active until a new branch is specified orend
is encountered.
EX
Specifies the edge number x (1.:12). All subsequently listedelements will inherit this edge number. The default element edge identifier is
E1
. Chapter gelements describes the element edge definitions for relevant elements.edgeset IDENT
Copies all edge identifiers found in an existing edge set
IDENT
to the current face set.
epatch IDENT E1 ... E12
Copies all edge identifiers of the edge
Ex
of the existing epatch with identifierIDENT
.
N1 N2 ...
Specifies a list of external element identifiers. The current edge number will be assigned to these element identifiers until a new edge number is specified (if any).
Examples
Specify the edge set edge1
containing the edge identifiers of the
edge of a plate patch consisting of 2 by 2 Q4 elements for (default)
branch 1.
edgeset "edge1"
e1 1 2
e3 3 4
end
epatch
MDL Specification
epatch IDENT
parameters
end
Description
epatch
generates simple onedimensional, twodimensional, and
threedimensional regular meshes. For onedimensional patches,
straight or arc lines can be modeled. For twodimensional patches,
foursided surfaces described by analytical functions can be modeled,
creating Q shelltype elements. For three dimensional patches, cubes
described by analytical functions can be modeled, creating HE
solidtype elements. In addition to nodes end elements, epatch
also generates lists containing vertex, edge, face, and body node
indices and element indices, thus facilitating the generation of
boundary conditions. Note, however, that the epatch
command is by
no means a substitute to any modeling and meshing software.
Any number of element patches can be generated within the same branch definition, provided that the patch boundary nodes match, i.e. nodes are not merged automatically if several element patches are generated in one and the same branch. Thus, it is often easier to generate one element patch per branch and connect the branches with the automatic option of the join command.
Element patches generate elements as follows (see also the figure below for the definition of i, j, and k): For all elements in the kdirection, for all elements in the jdirection, generate elements in the idirection, incrementing the element number by one.
Note that the default initial element number and the default initial
node number are both set to the highest internal element or node number
plus 1, defined so far for the current branch. Internal element and node
numbers start with 1. If patches and element and node definitions with
the elements
and nodes
commands are defined within the same
branch please consider making use the element start index
start_element_id
or the node start index start_node_id
options
to avoid conflicts with external element or node numbers defined by the
elements
or nodes
commands and the epatch
element and node
generation, which generates internal node numbers.
A patch is meshed independently of any other patches, and when defining multiple patches, the coinciding nodes of adjacent patches will not be connected. Coinciding nodes can be connected by means of the join (using the automatic option).
Parameters
eltype T
Specifies the element type
T
of the patch. For 1D patches elements of type B, C, L and R are allowed. For 2D patches elements of type T and Q are allowed. For 3D patches, element types HE and  to some extent  TE are allowed. The element type may only be specified once for one and the same patch.
geometry GTYPE
Specifies the geometry type of the patch to be generated. The following geometry types
GTYPE
and their parameters can be defined:
ARCH
Creates a line mesh of beam/rod/cable/line elements along a circular arch that is defined in the branch xy plane and with the origin of the circular segment at (0,0,0). Required meshing parameters are the number of elements
ne1
(int), the radiusR
(float), the start angleangle1
(float), and the end angleangle2` `(float). The optional parameter ``open
(YES````NO
) applies only in case where the segment makes a full circle. By default, the coinciding nodes are merged. Settingopen
toYES
retains the duplicate nodes.
cylinder
Specifies a cylindrical shell segment. The generated segment is defined in the branch xy plane, with the origin of the circular segment at (0,0,0), a radius
r
, and with the anglesphi1
(start angle) andphi2
(end angle) rotating around the zaxis. The axial direction is in the branch zdirection. Required meshing parameters are the number of elementsne1
in the circumferential idirection and the number of elementsne2
in the axial jdirection. Thethickness
parameter is element type dependent.
cube
Creates an isoparametric solid mesh of a cube defined by the 8 corner nodes
p1
top8
. Required meshing parameters are the number of elementsne1
in the idirection, the number of elementsne2
in the jdirection, and the number of elementsne3
in the kdirection. All other parameters are element type dependent.
line
Creates a straight line mesh of beam/rod/cable/line elements extending from point
p1
to pointp2
, with an optional area or thicknesst
. Required meshing parameters are the number of elementsne1
in the idirection. All other parameters are element type dependent.
plate
Generates an isoparametric rectangular plate mesh defined by the four corner nodes
p1
top4
. The plate has a optional uniform thicknesst
. Required meshing parameters are the number of elementsne1
in the plate idirection and the number of elementsne2
in the plate jdirection. All other parameters are element type dependent. Thethickness
parameter is element type dependent.
ring
Specifies a 2D shell element mesh of a ring. The ring is defined in the branch xy plane, with the origin of the circular segment at (0,0,0) and with the following keywords:
phi1
(start angle) andphi2
(end angle) rotating around the zaxis define the angles. The ring segment has an inner radiusradius1
and an outer radiusradius2
. Required meshing parameters are the number of elementsne1
in the circumferential (i) direction and the number of elementsne2
in the radial (j) direction. Thethickness
parameter is element type dependent. Theopen
parameter applies only in case where the segment makes a full circle. By default, the coinciding nodes are merged. Settingopen
toyes
retains the duplicate nodes.
tube
Specifies a solid mesh of a tube. The tube section is defined in the branch xy plane, with the origin of the circular segment at (0,0,0) and with the following keywords: The angles
phi1
(start angle) andphi2
(end angle) rotating around the zaxis defined the angles. The tube has an inner radiusradius1
and an outer radiusradius2
. The length of the tube is defined by thelength
. Required meshing parameters are and the number of elementsne1
in the circumferential (i) direction, the number of elementsne2
in the radial (j) direction, and the number of elementsne3
in the global z (k) direction. Theopen
parameter applies only in case where the segment makes a full circle. By default, the coinciding nodes are merged. Settingopen
toyes
retains the duplicate nodes.
local NONE  EDGES  ALL
Specifies if the generated nodes will be assigned a nodelocal DOF reference coordinate system (see transformations and nodes). The nodelocal coordinate system is generated according to the geometry type.
edges
generates local reference coordinate systems for all nodes placed on patch edges.ALL
generates local reference coordinate systems for all nodes.
ne1 N
Specifies the number of elements in regular patch in the logical idirection, see figure above (required for all patches).
ne2 N
Specifies the number of elements in regular patch in the logical jdirection, see figure above (required for 2D and 3D patches).
ne3 N
Specifies the number of elements in regular patch in the logical kdirection, see figure above (required for 3D patches).
orientation UX UY UZ VX VY VZ
Defines a local base by which all epatch nodes are rotated (refer to the section on orientation below for more details).
start_element_id IDENT
Element identifier of first element generated. All subsequent elements are generated by incrementing the element identifier by 1, first in the idirection, then in the jdirection, and, finally, in the kdirection. The default value is 1.
start_node_id IDENT
Node identifier of first node generated. All subsequent nodes are generated by incrementing the node identifier by 1, first in the idirection, then in the jdirection, and, finally, in the kdirection. The default value is 1.
translation TX TY TZ
Translates the patch in the branch global x, y and zdirection.
All other keywords are elementdependent.
The orientation
directive allows to change the orientation of any
patch. This may be useful in the case of cylindrical patches which
have a default orientation (the cylindrical axis is aligned with the
branchglobal zdirection).
orientation
[base u1 u2 u3 v1 v2 v3]
[rotate axis xyz angle a]
[rotate axis u1 u2 u3 angle a]
[translate x y z]
end
The following directives can be used to modify the orientation:
base u1 u2 u3 v1 v2 v3
Calculate the base from the vectors u and v as follows: u defines the patch base e_{1}, u x v defines the patch base e_{3}, and e_{3} x u defines the patch base e_{2}.
rotate axis XYZ angle A
Rotate the current patch base about the X, Y, or Z axis by A degrees, and according to the righthand rule. Successive rotations can be specified.
rotate axis U1 U2 U3 angle A
Rotate the current patch base about the axis defined by the vector u_{1} u_{2} u_{3}, by a degrees, and according to the righthand rule. Successive rotations can be specified.
translate TY TY TZ
Translate the current patch by TX in the xdirection, TY in the ydirection, and TZ in the zdirection. TX, TY, and TZ are float values. The default translation is 0.0 in all three directions.
All element attributes are element type dependent and can be consulted in the elements sections of the user manual.
Examples
Generate a cylindrical panel mesh with a 90 degree opening, starting at phi=0. The panel has a radius of 1., a thickness of 0.002, and a length of 1. All nodes shall have a local cylindrical coordinate system (r, phi, z). The panel is meshed with Q9 shell elements.
epatch 1
geometry cylinder
radius 1.0 thickness 0.002 phi1 0.0 phi2 90.0 length 1.0
local all
ne1 10 ne2 5
eltype Q9.S.MITC
mid 1
end
Generate a cylindrical panel mesh identical to the one in the
preceding example, i.e with a 90 degree opening, starting at
phi=0. The panel has a radius of 1., a thickness of 0.002, and a
length of 1. All nodes shall have a local cylindrical coordinate
system (r, phi, z). The panel is meshed with Q9 shell elements. The
cylinder shall be rotated by +90 degrees around the yaxis: This is
achieved by defining local base vectors with the orientation
parameter.
epatch 1
geometry cylinder
radius 1.0 thickness 0.002 phi1 0.0 phi2 90.0 length 1.0
orientation
base 1 0 0 0 0 1
end
local all
ne1 10 ne2 5
eltype Q9.S.MITC
mid 1
end
Generate a cylindrical panel mesh with a 90 degree opening, starting at phi=0. The panel has a radius of 1., a thickness of 0.002, and a length of 1. All nodes shall have a local cylindrical coordinate system (r, phi, z). The panel is meshed with 10 by 5 Q8 shell elements.
epatch 1
geometry cylinder
eltype Q8.S.MITC
radius 10. thickness 2.0 phi1 45.0 phi2 135.0 length 20.
local all
ne1 10 ne2 5
mid 1
end
Additional Information
Nodes generated by epatch
commands are stored as NODESET
datasets
in the form NODESET.br.0.0.name`, where the name is generated as
follows:
Type of set 
Name 
Additional information 

Body node set 


Edge sets of nodes 


Face sets of nodes 


Epatch vertices 


Type of set 
Name 
Additional information 

Body element set 


Type of set 
Name 
Additional information 

Edge sets of nodes 


Type of set 
Name 
Additional information 

Face sets of nodes 


elements
elements
defines mesh elements on a one by one element basis. To
generate elements (and nodes) for various simple geometries, make use
of the epatch command.
An element is defined by the element type, the parameters describing
the element properties and the external element identifier IDENT
and the element node connectivity list.
MDL Specification
elements
eltype ET
parameters
IDENT N1 N2 N3 ...
...
end
Parameters
Except for the element type and the node connectivity definition below, the required and optional element parameters depend on the element type and are explained in the specific element sections.
eltype ET
Specifies the element type (required if element property parameters are defined). All elements defined thereafter will be of type
ET
until a newET
is specified.eltype
always invalidates all required attributes and resets all optional attributes to their default values.It is possible to initially specify a dummy element type when defining the element connectivities and to change it later. This can be useful when the mesh and the elementsets are created by an external program, or when the mesh definition shall be independent of the operator. In this case, the correct element type and the element attributes need to be set at a later stage (see below). The following dummy element types are available:
P
for point elements.
L2
andL3
for linear and quadratic line elements, respectively.
T3
andT6
for linear and quadratic triangular elements, respectively.
Q4
,Q8
, andQ9
for quadrilateral elements.
TE4
andTE10
for linear and quadratic tetrahedral elements, respectively.
PR6
andPR15
for linear and quadratic prismatic elements, respectively.
HE8
,HE20
, andHE27
for hexahedral elements.
IDENTD N1 N2 N3 ...
Specify a single element with external element identifier
IDENT
and external element node identifiersN1 N2 N3...
defining the element node connectivity. See the specific elements sections for a definition of the element node connectivity.
IDENT [ni  nodeset NAME ...]
Defines an element with external identifier
IDENT
and a variable number of node identifiers specified explicitly or by referencing.nodeset
includes all nodes of a nodeset in the current list.
Examples
Define two four node quadrilateral shell element with the external numbers 10001 and 10002, having a constant shell thickness of 1.3 (for the element parameter see Shell Elements):
elements
eltype Q4.S.MITC
mid 2
thickness 1.3
10001 1 2 4 5
10002 2 3 5 6
10001 1 2 11 12
end
For elements with a potentially large number of nodes, such as RBE elements, the use of one or several nodesets (not node lists!) may be convenient:
eltype RBE
1001 [100001 nodeset left]
1002 [100002 nodeset right]
1003 [100002 nodeset front nodeset back]
end
Specify 4 elements: Two four node quadrilateral shell elements with a constant thickness of 1.3, and two elements of the same element type with a constant thickness of 1.5:
elements
eltype Q4.S.MITC
mid 1
thickness 1.3
10001 1 2 11 12
10002 2 3 12 13
thickness 1.5
10003 3 4 13 14
10004 4 5 14 15
end
Like the previous example, but this time, the element type and element attributes are specified after the element connectivities:
# Specify element shape and connectivities only
elements
eltype Q4
10001 1 2 11 12
10002 2 3 12 13
10003 3 4 13 14
10004 4 5 14 15
end
# Define element sets
elementset thin
10001 10002
end
elementset thick
10003 10004
end
# Now add element parameters
elements
eltype Q4.S.MITC mid 1 thickness 1.3 elementset thin
eltype Q4.S.MITC mid 1 thickness 1.5 elementset thick
end
elementset
elementset
defines a list containing external element identifiers
N1
, N2
, … The list is identified by the NAME
of the set
(a string not exceeding 40 characters). Element identifiers are positive
int values. Element sets can be specified for all element types.
MDL Specification
elementset NAME sortedunsorted
branch BR
elementset NAME1
epatch IDENT
N1 N2 ...
end
Parameters
sorted  unsorted
sorted
creates an ordered set with all duplicates removed.unsorted
adds nodes as they are specified. Default isunsorted
.sorted
orunsorted
must be specified directly afterNAME
and before any other parameter.branch BR
Specifies the branch number to which subsequently defined element identifiers will be assigned. The default branch is 1.
BR
remains active until a new branch is specified orend
is encountered.elementset NAME
Copies all element identifiers found in an existing element set
NAME1
to the current set.epatch IDENT
Copies all elements identifiers defined for the existing epatch with identifier
IDENT
to the current set.
faceset
faceset
defines a list assigning face number to elements, creating
pairs (elementid
, faceid
) of a specific branch. elementid
is the external element identifier and FX
the face identifier (see
below). The list is identified by the NAME
of the set (a string
not exceeding 40 characters). Note hat face sets are not defined for
wire (beam, rods) elements nor for special elements, such as RBE
elements.
MDL Specification
faceset NAME sortedunsorted
branch BR
Fx
faceset NAME
epatch IDENT
N1 N2 ...
...
end
Parameters
sorted  unsorted
sorted
creates an ordered set with all duplicates removed.unsorted
adds nodes as they are specified. Default isunsorted
.sorted
orunsorted
must be specified directly afterNAME
and before any other parameter.branch BR
Specifies the branch number to which subsequently defined element identifiers will be assigned. The default branch is 1.
BR
remains active until a new branch is specified orend
is encountered.Fx
Specifies the face number x (1..7). All subsequently listed elements will inherit this face number. The default element face number is 1. Chapter gelements describes the element face definitions for relevant elements.
faceset NAME
Copies all face identifiers found in an existing face set
NAME
to the current face set.epatch IDENT F1  F2  F3  F4  F5  F6
Copies all face identifiers of the face
Fx
of the existing epatch with identifierIDENT
.N1 N2 ...
Specifies a list of external element identifiers. The current face number will be assigned to these element identifiers until a new face number is specified (if any).
Examples
Specify the face set surface1
containing the face identifiers of the
element faces (face F1) of a plate patch consisting of 2 by 2 Q4
elements 1, 2, 3, and 4 of (default) branch 1:
faceset "surface1"
F1 1 2 3 4
end
field_transfer
MDL Specification
field_transfer IDENT
parameters
end
field_transfer
specifies coupling conditions between two adjacent
but in general incompatible surface meshes. In stress analysis, it
represents a kinematic coupling condition. A typical application is
globallocal analysis with shelltosolid, shelltoshell, or
solidtosolid coupling. Another application is skinstiffened
structures with independent meshes for skin, stringers, frames,
etc. In heat analysis, it couples the temperature fields of the two
adjacent surfaces.
The coupling is a weightedresidual method based on the \(L:{2}\) norm of the difference of the interpolated fields at the surfaces.
A field_transfer
condition must be activated in the case
command. If the identifier IDENT
is 0, the coupling condition will
be automatically added to all analysis cases. It is required to
specify a constraint method other than the default reduction
method for which the accuracy of the calculated solution cannot be
guaranteed when field_transfer
conditions are active. The
constraint method is defined in the case block, see
section Linear and Nonlinear Constraint Control.
The surfaces to be coupled are defined by interface i
where i is
either 1 or 2. An arbitrary number of surface sets faceset
may be added to each interface.
When the analysis is started, a commonrefined mesh consisting of
surface triangles is created from the intersection of the two coupling
interfaces, according to the element face shapes. In the case of flat
geometries, this commonrefined mesh coincides exactly with both surface
meshes. In the case of curved geometries, the commonrefined mesh
approximates both surface meshes. The approximation error can be reduced
by setting num_subdivision
to a positive value. In this case, the
surface mesh of the respective interface will be ntimes recursively
subdivided.
The calculation of the interpolated field at the interfaces is conducted using the shape functions of the involved elements. Integration over the triangles of the commonrefined mesh is carried out according to the element interpolation order(s). This way, the coupling is accurate for loworder as well as for highorder elements.
The transfer
directive specifies the type of field to be transferred
and on which interface i
the residuum shall be minimized.
Parameters
interface I faceset IDENT
Adds a faceset to the interface
I
.
interface I epatch IDENT FX
Adds an epatch face
FX
to the interfaceI
, where x=1..7.
interface I num_subdivisions N
Subdivides the interface by
N
subdvisions.
transfer displacement minimise_on interface I
transfer temperature minimise_on interface I
Field to be transferred.
join
join
command specifies equality between the DOF’s of nodes joined
together. join
is identified by IDENT
(positive or zero value
int). IDENT
is the identifier referenced by the join
option of
case. join
sets with an identifier of 0 will be activated for all
analysis cases.
The join
command is required if more than one branch (mesh) is
defined and the branches (meshes) are to be connected or if nodes of
the same branch (mesh) are to be connected explicitly. Note that the
same effect can be obtained by specifying linear constraints, see
linc, although on a DOF by DOF base.
join
must be follow all nodes and elements specifications of an MDL file.
MDL Specification
join IDENT
parameters
coupling conditions...
end
Parameters
delta V
Specifies the threshold value
V
in the global x, y and zdirections for comparing nodes (relevant for theautomatic
parameter only). This option must be issued beforeautomatic
in order to take effect. If not specified, the threshold value will be computed as a function of the bounding box.
automatic
Establishes the node connectivity automatically by comparing node positions. The nodes are transformed to the globalglobal coordinate system. If the nodes are close enough (see
delta
parameter) they will be linked. Note that thenode
anddof
coupling commands may not be specified if automatic is selected. No other parameter can be specified after the ``automatic`` option.
Coupling Conditions Specification
node BR1 N1 BR2 N2
Generates links nodewise. Node
N1
of branchBR1
is linked to nodeN2
of branchBR2
. Theautomatic
command may not be specified ifnode
is selected. Branch and node numbers are external.
dof BR1 N1 DOF1 BR2 N2 DOF2
Generates links between degreesoffreedom. The degreeoffreedom
DOF1
of nodeN1
of branch`` BR1`` is connected to the degreeoffreedomDOF2
of nodeN2
of branchBR2
. Branch and node numbers are external. degreeoffreedom numbers are positive integers.
Examples
The most common use of join
is:
join 0
automatic
end
Explicit joining of nodes: Connect node 3 t node 33, both in branch (mesh) 1.
join 0
node 1 3 1 33
end
Additional Notes
Master nodes are automatically determined as follows: The node belonging to the lower branch number in the link list becomes the master node.
For automatically computed link lists, the node lists are compared branchwise and in ascending order (internal branch numbering). The first encountered node that matches another node in the list becomes the master node. The matching criteria are defined by a cube of size (delta, delta, delta) constructed around the node.
linc
MDL Specification
linc IDENT [tol_drop V]
equation1
equation2
...
end
Description
The linc
command specifies one or more linear constraint equations.
Linear constraint equations and their terms can be specified in any
order. There are no a priori restrictions on the nodes and
degreesoffreedom that may be specified in linear constraints, since
B2000++ does not distinguish between master and slave nodes.
A linc
set is identified by IDENT
(positive or zero value
int). IDENT
is the number which is referenced by the linc
option of the case command.
Note
Sets with an IDENT
of 0 will be active for all analysis cases.
The constraint equations are of the form
where the coefficients \(c_{i}\) pertain to the dof’s of the global equation system.
In case nodes are to be explicitly connected it is preferable to make use of the join command, because it connects all DOF’s and it also ensures that node types are processed properly.
Parameters
tol_drop V
Sets the value for the drop tolerance. Default is 1e4. Any term of subsequently specified equations with an absolute weight below the drop tolerance will be ignored.
Equations Specification
equation NC C_0 B1 N1 DOF1 C1 ... Bn Nn DOFn Cn
Specifies a complete constraint equation with n terms as listed above. Each term is described by the external branch number
Bi
, the external node numberNi
, the degreeoffreedomDOFi
relating to nodeNi
, and the constantCi
.
Additional Information
Depending on how linear constraints are enforced (see
Linear and Nonlinear Constraint Control), the system of linear equations may
need to be modified to ensure a well conditioned global stiffness
matrix. Automatically generated linear constraint equations may
contain very small weights, which my result in a poorly conditioned
global stiffness matrix. When using the default reduction method for
linear constraints, it is recommended to set tol_drop
to a
sufficiently large value.
If weights below 1e4 are specified but the drop tolerance is smaller, the B2000++ input processor b2ip++ will print a warning.
To check whether the calculated solution is accurate, an error analysis on the matrix factorization and backsubstitution process can be conducted by specifying the B2000++ commandline option
b2000++ l 'debug of linear_algebra' DBNAME
when executing B2000++.
Example
Establish a rigid link between displacements in the xdirection (dof 1) by coupling node 23 of branch 1 to node 45 of branch 4:
linc 0
equation 2 0.0 1 23 1 1.0 4 45 1 1.0
end
material
material
specifies the physical properties of an element material.
Element materials are identified by a positive integer IDENT
,
which is then referenced by the elements (see
elements). Element material definition is branchindependent,
i.e. the element material identifiers IDENT
are global. The
material
command creates the data set MATERIAL.id
. The
detailed material specification is described in the materials section.
MDL Specification
material IDENT
type T
parameters
end
nbc
The nbc
command specifies natural boundary conditions (NBC)
applied to the DOF’s of specific nodes. Natural boundary conditions
will be part of the righthand side of the problem to be solved.
An nbc
set is identified by the identifier IDENT
(nonnegative
int). IDENT
is the number which is referenced by the nbc
option
of the case definition. Sets with an identifier of 0 will be
active for all analysis cases.
An nbc
is of a certain type (i.e. concentrated forces, line loads,
surface fractions, heat) and is specified either in the branchglobal
reference frame, the nodelocal reference frame, the element edge or
face reference frame, or the deformed element edge or face reference
frame.
A natural boundary condition set is activated with the nbc
option
of the case command.
See also Loads in Nonlinear Analysis
MDL Specification
nbc IDENT [type T] [system S] [title "text"]
parameters...
node specification...
...
end
General Parameters
type concentrated_loads  line_loads  surface_tractions  pressure  body_loads  accelerations  body_heat
Specifies the type of the natural boundary conditions defined in the current set. Default is
concentrated_loads
.
system branch  local  local_deformed
Specifies the reference frame in which the conditions are formulated. The default reference frame depends on the selected
type
.
title "text"
Specifies an optional title for the
nbc
set.
nbc Concentrated Loads
The type concentrated_loads
(the default) means that concentrated
loads (i.e. forces in stress analysis and heat in heat transfer
analysis) are assigned to degreesoffreedom at individual nodes or
multiple nodes.
See also Loads in Nonlinear Analysis
MDL Specification
nbc IDENT [type concentrated_loads] [system S] [title T]
value V
dof list
node specification...
value V
dof list
node specification...
...
end
Parameters
The degreesoffreedom that are present at a given node depend on the elements to which this node is connected. Specifying a value for a degreeoffreedom that does not exist will have no effect.
value V
Specify the magnitude of a single value (float) i.e concentrated load or heat). This value is then assigned to one or several degreesoffreedom by means of the directive
dof
. The couple (value, degreesoffreedom) is then assigned to individual nodes or collections of nodes. You can only specify a single valueV
.
dof I1
dof [I1 I2 ...]
The directive
dof
is followed by a list which identifies the degreesoffreedom:
In stress analysis,
FX
,FY
, andFZ
represent a force in the x, y, and zdirection, respectively.In stress analysis,
MX
,MY
, andMZ
represent a moment about the x, y, and zaxes, respectively.In heat analysis,
Q
means the rate of heat flow (power).
Node Specification
allnodes
Assign the concentrated loads to all defined nodes of the current branch.
branch BR
Specifies the external branch number
BR
(positive int). Default is 1.
epatch IDENT p1p8  e1e12  f1f6  b
Applies to conditions to node lists of an existing epatch identified by
IDENT
. Individual patch vertex nodes are specified withp1
top8
. The collection of nodes that are located at a patch edge are specified withe1
toe12
. The collection of nodes that are located at a patch face are specified withf1
tof6
. The collection of nodes of the whole patch body are specified withb
.
nodes N
ornodes [N1, N2 ...]
Apply the condition(s) to a node or a list of nodes.
nodeset NAME
Specifies the name of the node set to which the concentrated loads will be assigned.
Examples
Set the force in the ydirection to 25.0 for mesh node 5. For mesh nodes 9,10,11,12, set the moment in the ydirection to 60.0. Since the default reference frame is nodelocal, the directions will be the nodelocal directions if there are local coordinate system defined for these nodes. Otherwise, the directions will be aligned with the branch reference frame.
nbc 1
value 25.0 dof FY nodes 5
value 60.0 dof MY nodes [9 10 11 12]
end
Apply a concentrated force in zdirection to the center node (p5
)
of a square plate meshed with the epatch
command. Note: The center node
is defined only if the number of elements in the patch directions
(ne1
and ne2
) are even!
epatch 1
geometry plate
p1 0. 0. 0.
p2 1. 0. 0.
p3 1. 1. 0.
p4 0. 1. 0.
thickness 0.01
eltype Q9.S.MITC
mid 1
ne1 10
ne2 10
end
nbc 1
value 5. dof FZ epatch 1 p5
end
nbc Line Loads
MDL Specification
nbc IDENT type line_loads [system S] [title T]
line_loads L1 L2 L3
edge specification...
line_loads L1 L2 L3
edge specification...
...
end
Specifying type line_loads
means that the set consists of line
loads (force per unit length in stress analysis), which will be
integrated along the element edges during the analysis by the element
implementations. The element thickness is not taken into account.
Line loads are meaningful for shell elements (edges 14), 2D elements
(edges 14), and cable/rod and beam elements (edge 1). Irrespective of
the element type, line loads are specified with 3 components L1 L2
L3
(no square brackets!).
The default reference frame is local
. For cable/rod elements and
beam elements, this means the element axis. Only the value of L1
is used while L2 L3
will be ignored. For shell elements and 2D
elements, the edgelocal reference frames will be used. They are
identical to the facelocal reference frames of a corresponding solid
element:
L1
coincides with the edge direction.L2
coincides with the element surface normal. For cable/rod elements, beam elements, and 2D elements,L2
will be ignored.L3
coincides with the outwardpointing face/edge normal. For cable/rod and beam elements,L3
will be ignored.
The reference frame local_deformed
is intended for geometrically
nonlinear stress analysis and otherwise identical to local
. The
reference frame branch
means that L1 L2 L3
is in the
branchglobal x, y, and zdirection, respectively.
See also Loads in Nonlinear Analysis
Warning
The default reference frame is local
. If you want to generate
loads in the (branch) global system, you must specify
system branch
before generating loads.
Parameters
edgeset "NAME"
Specifies the name of the edge set to which the line loads will be assigned.
epatch IDENT e1e12
Specifies an epatch edge to which the line loads will be assigned.
Examples
A line load in ydirection is applied to the outer edge of a clamped cantilever beam.
epatch 1
geometry plate
p1 0. 0. 0.
p2 100. 0. 0.
p3 100. 10. 0.
p4 0. 10. 0.
thickness 0.01
eltype Q9.S.2D.TL
mid 1
ne1 10
ne2 1
end
ebc 1
value 0. dof [UX UY] epatch 1 e4
end
nbc 1 type line_loads
line_loads 0 .1 0
epatch 1 e2
end
nbc Surface Traction and Pressure Loads
MDL Specification
nbc IDENT type surface_tractions [system S] [title T]
surface_tractions T1 T2 T3  pressure P
face specification...
surface_tractions T1 T2 T3  pressure P
face specification...
...
end
Surface tractions are forces of heat per unit area. The will be integrated along the element faces during the analysis by the element implementations. In case of 2D elements and shell elements, the element thickness is taken into account.
Surface traction loads are meaningful for 3D elements (faces 16), shell
elements (faces 14 for the sides, face 5 for the lower surface, face 6
for the upper surface, and face 7 for the midsurface), and 2D elements
(faces 14 for the sides). Surface traction load are specified with 3
components T1 T2 T3
.
Specifying pressure P `` is equivalent to ``surface_tractions 0 0
P
.
The default reference frame is local
, which means that the
facelocal reference frames of the initial configuration will be used
(see also Generic Elements):
T1
coincides with the edge direction in case of 2D and shell elements.T2
coincides with the element surface normal in case of 2D and shell elements.T3
coincides with the outwardpointing face normal.
The reference frame local_deformed
is intended for geometrically
nonlinear stress analysis and otherwise identical to local
. The
reference frame branch
means that T1 T2 T3
is in the
branchglobal x, y, and zdirection, respectively.
See also Loads in Nonlinear Analysis
Parameters
faceset "NAME"
Specifies the name of the face set to which the loads will be assigned.
epatch IDENT f1f7
Specifies an epatch face to which the loads will be assigned.
Examples
A uniform pressure is applied to the midsurface of a square plate
which is simplysupported. The plate is generated with epatch
command. The nbc
2 is equivalent to the nbc
set 1.
epatch 1
geometry plate
p1 0. 0. 0.
p2 1. 0. 0.
p3 1. 1. 0.
p4 0. 1. 0.
thickness 0.01
eltype Q9.S.MITC
mid 1
ne1 4
ne2 4
end
nbc 1 type surface_tractions
surface_tractions 0. 0. 1.
epatch 1 f7
end
nbc 2 type pressure
pressure 1.
epatch 1 f7
end
nbc Body Loads
MDL Specification
nbc IDENT type body_loads [system S] [title T]
body_loads FX FY FZ
element specification...
body_loads FX FY FZ
element specification...
...
end
Generates body loads by integrating a forceperunitvolume field over the element volume.
Note
Do not make use of body loads in case you want to generate loads due to the own mass of a structure under a gravity (acceleration) field  refer to inertia loads.
Body loads can be applied to all 1D 2D and 3D elements, but they
should not be used with pointmass elements (the type
accelerations
should be used instead).
Body loads are specified with 3 components F1 F2 F3
, defined in
the branchglobal reference frame (local reference frames are not
permitted).
The default reference frame is branch
, which means that F1 F2
F3
are specified in the branchglobal x, y, and zdirection,
respectively. If the reference frame local
is specified, the
elementlocal reference frame will be used (see also Generic
Elements). The reference frame local_deformed
is
intended for geometrically nonlinear stress analysis and otherwise
identical to local
.
See also Loads in Nonlinear Analysis
Element Specification
allelements
Assign the body loads to all defined elements of the current branch.
branch BR
Specifies the external branch number
BR
. Default is 1. directive.
elementset "NAME"
Specifies the name of the element set to which the body loads will be assigned.
epatch IDENT b
Specifies the name of the epatch to which the body loads will be assigned.
Examples
A body load in y direction is applied to a clamped cantilever beam.
epatch 1
geometry plate
p1 0 0 0
p2 100 0 0
p3 100 1 0
p4 0 10 0
thickness 0.01
eltype Q9.S.2D.TL
mid 1
ne1 10
ne2 1
end
nbc 1 type body_loads
body_loads 0 1 0
epatch 1 b
end
nbc Inertia Loads
MDL Specification
nbc IDENT type accelerations [system S] [title T]
accelerations A1 A2 A3
element specification...
accelerations A1 A2 A3
element specification...
...
end
Generates inertia loads or gravity loads (d’Alembert forces) by applying a given acceleration vector with components \(a = a_x, a_y, a_z)\) to the mass in the branch global system.
Note
There is currently no global definition for inertia loads, i.e all
elements with inertial loads have to be listed explicitly. To apply
inertia loads to all elements please make use of the
allelements
option (see below).
Inertia loads are applied to solidelements, shell and ther 2D elements, rod/cable elements, beam elements, and pointmass elements. During the analysis, the accelerations will be multiplied with the material density and non structural mass (if any) and integrated by the element implementations over the volumes of the specified elements. For pointmass elements, the translational inertia loads are generated by multiplying the accelerations by the element mass.
The default reference frame is branch
, which means that the
accelerations are specified in the branchglobal x, y, and
zdirection, respectively. If the reference frame local
is
specified, the elementlocal reference frame will be used. The
reference frame local_deformed
is intended for geometrically
nonlinear stress analysis and otherwise identical to local
.
Note
Inertia loads will not take effect if the material density is no specified! The default material density is 0.
See also Loads in Nonlinear Analysis
Element specification
allelements
Apply the acceleration vector to all defined elements of the current branch.
branch BR
Specifies the external branch number
BR
. Default is 1. directive.
elementset "NAME"
Specifies the name of the element set to which the accelerations apply.
epatch IDENT b
Specifies the name of the epatch to which the accelerations apply.
Examples
An acceleration load in the z direction is applied to a thin clamped cantilever plate consisting of two regions with different materials.
epatch 1
geometry plate
p1 0. 0. 0.
p2 50. 0. 0.
p3 50. 10. 0.
p4 0. 10. 0.
thickness 1.
eltype Q9.S.MITC
mid 1
ne1 5
ne2 1
end
epatch 2
geometry plate
p1 50. 0. 0.
p2 100. 0. 0.
p3 100. 10. 0.
p4 50. 10. 0.
thickness 1.
eltype Q9.S.MITC
mid 2
ne1 5
ne2 1
end
material 1
# aluminium
type isotropic
e 70e3
nu 0.3
density 2.77e9
end
material 2
# steel
type isotropic
e 200e3
nu 0.3
density 8e9
end
ebc 1
value 0. dof [UX UY UZ RX RY RZ] epatch 1 e4
end
nbc 1 type accelerations
accelerations 0 0 9.806e3
allelements
end
nbc Body Heat Loads
Body heat loads (power per volume) are heat sources or heat sinks. Body heat loads are meaningful for all heat conduction elements.
To specify heat convection or heat radiation boundary conditions
(vonNeumann boundary conditions), the nbc
command cannot be
used. Instead, specific heat convection and heat radiation ‘overlay’
elements are provided for that purpose.
MDL Specification
nbc IDENT type body_heat [title T]
body_heat H
element specification...
...
end
Element Specification
allelements
Assign the body loads to all defined elements of the current branch.
branch BR
Specifies the external branch number
BR
. Default is 1. directive.
elementset "NAME"
Specifies the name of the element set to which the heat will be assigned.
epatch IDENT b
Specifies the name of the epatch to which the heat will be assigned.
Example
A body heat load is applied to a square plate. A fixed temperature is
imposed at boundary of the plate (ebc
command).
epatch 1
geometry plate
p1 0. 0. 0.
p2 1. 0. 0.
p3 1. 1. 0.
p4 0. 1. 0.
thickness 0.01
eltype Q9.HEAT.CONDUCTION.2D
ne1 4 ne2 4
mid 1
end
material 1
type heat
k 0.7
end
ebc 1
value 20. dof 1
epatch 1 e1
epatch 1 e2
epatch 1 e3
epatch 1 e4
end
nbc 1 type body_heat
body_heat 10.e5 allelements
end
nodes
The nodes
command specifies individual mesh nodes. Node
coordinates are specified in the branch coordinate system if defined,
otherwise, they are defined in the global coordinate system. The
nodes
command may be specified more than once.
Note that nodes and elements with specific simple predefined geometric shapes can be generated instead using the epatch command.
Natural boundary conditions nbc and essential boundary
conditions ebc, when applied to the DOF’s and the local
coordinate systems, refer to the coordinate system defined here.
Consequently, if boundary conditions are to be defined in local
coordinates, specify dofref
for all nodes with local coordinate
systems.
MDL Specification
nodes
parameters
nodespecification
...
end
Parameters
dofref IDENT
Assigns the nodelocal DOF reference coordinate system identified by
IDENT
(a positive int).IDENT
references the transformation defined by the corresponding transformations command. By settingIDENT
to 0, any nodelocal DOF referenceframe is inactivated for all subsequently defined nodes, which is also the default. Nodelocal coordinate systems affect only the degreesoffreedom. Note thatdof_ref
,dref
, andtransformation
are aliases to dofref`.
Node Specification
IDENT Y Z
Specifies a single node by specifying the external node identifier
IDENT
(a positive int) and the three float coordinate componentsX
,Y
, andZ
. Note that B2000++ requires \(\mathbb{R}^3\) space.
Assigning and Changing Node Parameters
Node parameters can be specified after the definition of the nodes, and node parameters may be changed anytime. To this end, the nodes whose parameters shall be set or changed need to be defined in node sets, see example below.
Examples
Define the nodes 1001, 2002, 1003, and 1004. Node 1002 has a local DOF reference frame identified by the transformation 23:
nodes
1001 10. 0. 0.
dof_ref 23
1002 20. 0. 0.
dof_ref 0
1003 30. 0. 0.
1004 40. 0. 0.
end
Define all nodes of a model and assign new parameters (here: a local DOF reference system) to a set of nodes.
nodes
1 0 0 0
2 10 0 0
3 20 5 0
4 30 20 0
end
...
nodeset abc
1 2 3 4
end
# Assign new dof ref to nodes 1,2,3,4:
nodes
dof_ref 2 nodeset abc
end
nodeset
nodeset
defines a list containing external node identifiers
N1
, N2
, … The list is identified by the NAME
of the set
(a string not exceeding 40 characters). Node identifiers are positive
int values. Node sets can be specified for all element types.
MDL Specification
nodeset NAME sortedunsorted
branch  nodeset  epatch
N1 N2 ...
end
Parameters
sorted  unsorted
sorted
creates an ordered set with all duplicates removed.unsorted
adds nodes as they are specified. Default isunsorted
.sorted
orunsorted
must be specified directly afterNAME
and before any other parameter.branch BR
Specifies the branch number
BR
to which subsequently defined node identifiers will be assigned. The default branch is 1.nodeset IDENT
Copies all node identifiers found in the existing defined node set
IDENT
to the current node set.epatch IDENT Ex  Fx  b
Copies all node identifiers found in the existing node list for the existing epatch with identifier
IDENT
. Nodes located on the epatch edges are specified withEx
(x in the range 1..12). Nodes located on the epatch faces are specified withF6
( x in the range 1..7). Nodes located on the epatch body (all nodes of the epatch) are specified withb
.
Examples
Define the node set left_edge_1
:
nodeset "left_edge_1"
1 2 3 4 11 6 7 8 9 10
end
The resulting list
1 2 3 4 11 6 7 8 9 10
Define the sorted node set left_edge_1
:
nodeset "left_edge_1"
1 2 3 4 11 6 7 8 9 10
end
The resulting list
1 2 3 4 6 7 8 9 10 11
Define the node set left_edge_and_right_edge
containing the set
‘left_edge_1’ and additional nodes for (default) branch 1:
nodeset "left_edge_and_right_edge"
set "left_edge_1"
20 30 40 50
end
The resulting list
1 2 3 4 11 6 7 8 9 10 20 30 40 50
property
The property
command defines element properties identified by the
identifier IDENT
, a positive integer. In the current version only
Bx.S.RS
beam elements understand``property``!
MDL Specification
property IDENT
type T
parameters...
end
A property is specified with the property type T
and the
parameters pertaining to the selected property.
Type 
Description 








beam_constants
beam_constants
describes a beam section by all relevant constants.
They can be either defined by the cross section constants or by the
stiffness value, which allow for a more general definition, i.e for
nonhomogeneous materials. The specific stiffness components are
selected by the B2000++ solvers as follows: B2000++ first checks if a
component’s stiffness is specified. If found, it is selected. If not,
the constants forming the specific component are selected.
Parameter 
Description 


Second area moments J_{yy}, J_{zz}, and J_{yz} (floats). 

Bending stiffness coefficients E*J_{yy}, E*J_{zz},
E*J_{yz} (floats). If 

Section y and zcoordinates of the neutral axis point (floats). This is the point where, when aligned with the beam axis, an applied axial force does not result in a bending deformation. For cross sections that are made of a homogeneous material, the neutral axis point is identical to the centroid. The y and z coordinates are given with respect to the beam axis. Default is 0.0 for all values. 

Mass per unit length of beam (float). If 

Section y and zcoordinates of mass center with respect to the beam axis (floats). Default is 0.0 for all values. 

Mass inertia moments I_{yy}, I_{zz}, and I_{yz} (floats). 

Element material identifier (positive int). Required. 

Nonstructural mass per unit beam length (float). Default is 0.0. 

Section y and zcoordinates of nonstructural mass center with respect to the neutral axis point (floats). Default is 0.0 for all values. 

Shear force correction factors K_{yy}, K_{zz}, and K_{yz} (floats). 

Shear stiffness A*G*K_{yy}, A*G*K_{zz}, and A*G*K_{yz} (floats). If 

Defines stress evaluation points at section coordinates y and z. No checks are made, i.e the section stress evaluation procedure will simply compute the stresses at section positions (y,z). 

Torsional constant J_{t} (float). 

Torsional stiffness J_{t}*G (float). If


Axial beam stiffness E*A (F type float). If

beam_section
The beam_section
type generates beam element section properties
for some predefined simple beam section shapes, together with the
shape
parameter. shape
defines the beam section shape,
followed by the relevant dimension parameters (keywords Dx
) the
actual dimensions.
The beam section properties are calculated with respect to the local coordinate system placed at the centroid of the section. The local coordinates \(y_{local}\) and \(z_{local}\) coincide with the beam local \(y_{local}\) and \(z_{local}\) coordinates. The shear center offset is defined with respect to the local coordinate system.
Parameter 
Description 



Rectangular cross section: 


Rectangular thinwalled box: 


Thinwalled C shape cross section: 


I shape cross section: 


Thinwalled L shape cross section: 


Unspecified cross section shape restricted to rod elements
(elements without bending). 


Upsidedown T cross section: 


Circular tube cross section: 

Red dot: Centroid. Blue dot: Location of shear center. Green dots: Stress point locations (if any). 
beam_section_matrix
beam_section_matrix
Describes the beam section by the Timoshenko
beam constitutive 6x6 matrix, as obtained by using external
crosssectional analysis tools. Refer to the beam section
submodel definition property for
direct integration with the B2000++ crosssection solver.
Parameter 
Description 


A list of 36 floats, specifying the symmetric beam constitutive
(6x6) matrix in rowmajor order, calculated at the


Section y and zcoordinates of the neutral axis with respect to the beam axis (floats). Default is 0.0 for all values. 

The mass of the beam cross section per length unit (float). Default is 0. 

Section y and zcoordinates of mass center with respect to the beam axis (floats). Default is 0.0 for all values. 

Mass inertia moments I_{yy}, I_{zz}, and I_{yz} (floats). 
beam_section_submodel
Describes the beam section by a dedicated, separate B2000++ FE submodel. The B2000++ processor will then extract from the submodel database the Timoshenko beam constitutive matrix and the other required constants.
Parameter 
Description 


Name of the B2000++ MDL file containing the crosssection model,
or name of the database containing the FE crosssection model
mesh and the results. If 

Load case identifier 
Examples
Specify a bar section property with identifier 123. The bar has the radius of 2.3.
property 123
shape bar
D1 12.3
end
Example with two properties 1 and 2 specifying crosssection submodels
for a framestringer fuselage. The corresponding database frame.b2m
and the MDL file stringer.mdl
must exist. In the case of the latter,
the B2000++ crosssection solver will be executed at the beginning of
the analysis.
property 1 type beam_section_submodel
name frame
case 1
end
property 2 type beam_section_submodel
name stringer.mdl
case 1
end
Type 
DIM1 
DIM2 
DIM3 
DIM4 
DIM5 
DIM6 

BAR 
D1 (w) 
D2 (h) 

BOX 
D1 (w) 
D2 (h) 
D3 (tflanges) 
D4 (twebs) 

C (CHAN) 
D1 (w) 
D2 (h) 
D3 (tweb) 
D4 (tflanges) 

I 
D1 (h) 
D1 (wlower) 
D3 (wuppper) 
D4 (tweb) 
D5 (tlower) 
D6 (tupper) 
L 
D1 (w) 
D2 (h) 
D3 (tflange) 
D4 (tweb) 

ROD 
D1 (radius) 

Circular TUBE 
D1 (radius1) 
D2 (radius2) 
stage
The stage
command specifies the analysis stage identified by
IDENT
(positive int). An analysis stage contains ingredients such as
initial conditions (if the stage is the first stage during
nonstationary analysis), boundary conditions, and solution strategy
parameters. The analysis type is fixed for all stages, i.e it is not
possible to select the analysis type on a perstage basis.
The stage
is activated by referencing it in the case command.
MDL Specification
stage IDENT
parameters
end
Parameters
The parameters listed below pertain to most types of analyses and
concern the specification of initial conditions, boundary conditions,
and constraints. Solverspecific attributes are explained in Solvers. The parameters of stage
are
a subset of the case parameters without stages.
atemperatures IDENT [sfactor S  sfunction "EXPRESSION"]
Specifies the ambient temperatures set
IDENT
to be included for certain types of analysis, like heat analysis.During linear analysis, the optional parameter
sfactor
specifies a scale factorS
by which the set is multiplied, the default value being 1.0.During nonlinear direct analysis and in incremental analysis, the set is scaled by the load factor (static analysis) or by the time (dynamic analysis). The optional parameter
sfactor
specifies an additional scale factor by which the set is multiplied, the default value being 1.0. Alternatively, the optional parametersfunction
specifies a function which is being evaluated at each load or time increment and by which the set is multiplied.component NAME type "ARGUMENT" [sfactor S  sfunction "EXPRESSION"]
Specifies a component to be used in the current analysis stage. Components are extensions to B2000++. They implement specific natural boundary conditions, essential boundary conditions, initial conditions, or sets of constraints.
The
NAME
andTYPE
parameters are used to identify the component (the component is registered under this name). TheARGUMENT
parameter is given to the component at the start of the analysis (stage).In linear analysis, the optional parameter
sfactor
specifies a scale factor by which the values returned by the component are multiplied, the default value being 1.0.In nonlinear direct analysis and in incremental analysis, the values returned by the component are scaled by the load factor (static analysis) or by the time (dynamic analysis). The optional parameter
sfactor
specifies an additional scale factors
by which the values returned by the component are multiplied, the default value being 1.0. Alternatively, the optional parametersfunction
specifies a function which is being evaluated at each load or time increment and by which the values returned by the component are multiplied.dof_init IDENT  dofdot_init IDENT
Specifies the initial conditions set
IDENT
or the timederivative of the initial conditions set for the current analysis stage. The stage must be the first stage.ebc IDENT [sfactor S sfunction "EXPRESSION"]
Adds the essential boundary conditions set
IDENT
to the current analysis stage. Note that essential boundary conditions are not cumulative, i.e. if several essential boundary condition sets are specified, all values of common degreesoffreedom must be equal.In linear analysis, the optional parameter
sfactor
specifies a scale factor by which the set is multiplied, the default value being 1.0.In nonlinear direct analysis and in incremental analysis, the set is scaled by the load factor (static analysis) or by the time (dynamic analysis). The optional parameter
sfactor
specifies an additional scale factor by which the set is multiplied, the default value being 1.0. Alternatively, the optional parametersfunction
specifies a function which is being evaluated at each load or time increment and by which the set is multiplied.field_transfer IDENT
Adds the field transfer set
IDENT
to the current analysis stage. Note that a field transfer set with anIDENT
of 0 is automatically added to all analysis cases and stages.Alternatively, several or all field transfer sets may be specified:
field_transfer 123 field_transfer all
It is required to specify a constraint method other than the default
reduction
method for which the accuracy of the calculated solution cannot be always ensured whenfield_transfer
conditions are active. See Linear and Nonlinear Constraint Control.join IDENT
Adds the join set IDENT` (int) to the current analysis stage. Note that an
IDENT
of 0 is automatically added to all analysis cases and stages.linc IDENT
Adds the linear constraints set
IDENT
(int) to the current analysis stage. Note that anIDENT
of 0 is automatically added to all analysis cases and stages.nbc IDENT [sfactor S  sfunction "EXPRESSION"]
Adds the natural boundary conditions set
IDENT
to the current analysis stage. Natural boundary conditions are cumulative, i.e. if several natural boundary condition sets are specified the resulting natural boundary condition forIDENT
is the sum of all natural boundary condition sets multiplied by their respective scaling.During linear analysis, the optional parameter
sfactor
specifies a scale factor by which the set is multiplied, the default value being 1.0.During nonlinear direct analysis and incremental analysis, the set is scaled by the load factor (static analysis) or by the time (dynamic analysis). The optional parameter
sfactor
specifies an additional scale factor by which the set is multiplied, the default value being 1.0. Alternatively, the optional parametersfunction
specifies a function which is being evaluated at each load or time increment and by which the set is multiplied.temperatures IDENT [sfactor Ssfunction "EXPRESSION"]
Specifies the temperatures set
IDENT
to be included for certain types of analysis, like thermal stress analysis.During linear analysis, the optional parameter
sfactor
specifies a scale factor by which the set is multiplied, the default value being 1.0.During nonlinear direct analysis and in incremental analysis, the set is scaled by the load factor (static analysis) or by the time (dynamic analysis). The optional parameter
sfactor
specifies an additional scale factor by which the set is multiplied, the default value being 1.0. Alternatively, the optional parametersfunction
specifies a function which is being evaluated at each load or time increment and by which the set is multiplied.title 'TEXT"'
Optional title describing the analysis stage.
title
The optional command title
specifies a problem title, the title
text being enclosed in single or double quotes. For practical
purposes the length of the title string should be limited to 64
characters or less, although titles up to 1024 characters in size can
be specified.
title "..."
Specifies the problem title.
temperatures
temperatures
specifies node temperature values, such as
temperatures inducing thermal loads in stress analysis. To specify
ambient temperature values at nodes for defining convective conditions
in heat analysis, please refer to the atemperatures command.
A temperatures
set is identified by I
, a nonnegative integer
which must be unique for the temperatures
conditions of the
current model. IDENT
is the number which is referenced by the
temperatures
parameters of the case command. Sets with an
identifier of 0 will be active for all analysis cases.
MDL Command
temperatures IDENT
parameters
node specifications...
end
Parameters
value V1 [V2, ...]
Specifies the temperature values
V
assigned to subsequently specified nodes. Depending on the element type, more than one temperature value is required:
For the MITC shell element, 2 values per node are required. The first value designates the temperature at the bottom surface while the second value designates the temperature at the top surface. Linear interpolation of the temperature between the bottom and top surfaces is performed.
For rod/cable, beam, 2D, and 3D stress elements, a single value per node is required. If a second value is specified, it will be ignored.
Node Specification
allnodes
Assign the ambient temperature values to all defined nodes of the current branch.
branch BR*
For models that consist of several branches. Specifies the external branch number br. To be used in conjunction with the allnodes and nodes directives.
epatch IDENT p1p8  e1e12 f1f6  b
Selects nodes from an epatch. Individual patch vertex nodes are specified with the strings
p1
top8
. Patch edge nodes are specified with the stringse1
toe12
. Patch face nodes are specified with the stringsf1
tof6
. Patch body nodes of the whole patch body are specified with the stringb
.node N  nodes [N1 N2 ...]
Specifies a node or a list of nodes (of the current branch) to which the ambient temperature value will be assigned.
nodeset NAME
Specifies the name of the node set to which the temperature values will be assigned.
Import Temperatures from External Databases
Temperature sets defined in external databases can be imported
specified by means of the dataset
directive.
import dataset NAME from DBNAME
Reads nodal temperatures from the datasets matching
NAME
stored in the databaseDBNAME
, and sets them for the nodes, overwriting any previously defined data.The
import dataset
directive allows to use results from a thermal analysis, stored in another database, for a subsequent stress analysis. The dataset name pattern isTEMP.*.cycle.0.case
where*
means that all branches will be selected,cycle
is the load increment (0 for a linear heat analysis), andcase
is the load case identifier.
Additional Information
temperatures
generates the dataset(s) TEMP.branch.0.0.id
,
where branch
designates the branch number and id
the set
identifier.
transformations
transformations
specifies local DOF coordinate systems (rotations)
with respect to the (branch) global coordinate reference system.
transformations
only specifies the transformation, it does not
transform any coordinates or DOF’s, the effective transformations
being executed for the respective coordinates or DOF’s by the relevant
b2000++ processor. The dofref
parameter of the nodes
command specifies the DOF reference system transformation identifier
to be applied to specific nodes.
transformations
can be specified more than once.
transformations
parameters
end
Parameters
Transformation specification:
IDENT TYPE P1X P1Y P1Z P2X P2Y P2Z [P3X P3Y P3Z]
Specifies a transformation by its identifier
IDENT
(positive int), the type of transformationTYPE
, and the points P1, P2, and P3 defining the transformation.If the transformation type is set to
CARTESIAN
(change of orthogonal base), p_{1}, p_{2}, and p_{3} are required and a change of orthogonal base will be applied.If the transformation type is set to
CYLINDRICAL
a cylindrical transformation will be applied, P1 defining the cylinder zaxis, P2 the cylinder radial direction, and P3 the the cylinder angular direction.If the transformation type is set to
SPHERICAL
a spherical transformation will be applied, with P1, P2, P3 being required.If the transformation type is set to
BASE
, P1 and P2 are required, P1 defining the base vector e1* and P2 the base vector e2d*. The base vector e3 is calculated with P1 x P2. The base vectors need not be normalized to 1.
Examples
Specify a cylindrical coordinate system with identifier 123, with the cylinder axis identical to the global zaxis, i.e. by P1=(0,0,0) and P2=(0,0,1) , such that P2P1=(0,0,1).
transformations
123 cylindrical 0. 0. 0. 0. 0. 1. 0. 0. 0.
end
Additional Information
The Cartesian coordinate system transformation is defined as follows: The origin is equal to the point \(P_1\). The local zaxis is defined by \(z = P_2  P_1\), the local yaxis by \(y=(P_2  P_1) \times P_3\), and the local xaxis by \(x=y \times (P_2  P_1)\).
The cylindrical coordinate system transformation is defined as follows: The origin is equal to the point \(P_1\). The cylinder zaxis is defined by \(z = P_2  P_1\). The tangential (\(\phi\)) direction of a point \(P\) is then defined by \(t = (P  P_1) \times z\) and the cylinder’s radius direction \(r = z \times P_3\). Point \(P_3\), together with \(P_1\) and \(P_2\), spans a plane in which \(\phi=0\), rotating in the positive direction around the local zaxis \(z = P_2  P_1\). Note: \(_3\) is ignored,i.e. the local \((r,\phi,z)\) system is uniquely defined by the node coordinate \(P\) and points \(P_1\) and \(P_2\).
The spherical coordinate system transformation is defined as follows:
The origin is equal to the point \(P_1\). The sphere zaxis is
defined by \(z = P_2  P_1\). The tangential (\(\phi\))
direction of a node \(P\) is then defined by \(t = (P  P_1)
\times z\) and the sphere’s \(\theta\) direction \(r = z
\times P_3\). The declination \(\theta\) rotates in a positive
direction starting from z. Note: p_{3} is ignored for
transformation
, i.e. the local \((\phi,\theta\),z) system is
uniquely defined by points \(P_1\) and \(P_2\).
Additional Information: Node transformations
Given the transformation definitions and the coordinates, the B2000++
input processor computes the effective DOF transformation matrices for
all nodes involved. The transformation matrices are stored in datasets
NLCS
and referred to by the second column of the datasets
NODA
. The transformation is defined as \(u_{nl} = T \cdot
u_{bg}\), where \(u_{nl}\) is a vector referring to the nodelocal
system and \(u_{bg}\) to the branch global system. The
transformation \(T\) contains the 3 normalized base vectors
\(e_i\) rowwise. \(e_i\) defines \(i^{th}\) base vector
of the nodelocal system with respect to the branchglobal system: