ofrece las siguientes mejoras y novedades más importantes:
Dynamic Software Interfaces
Ratio Output for Composites
constraint mode method of enforced motion, which was referred to as the
relative method in NX Nastran 4.1, uses a formulation in which the response
output is calculated with both the normal mode shapes, and the constraint
mode shapes. A change in the default has occurred in NX Nastran 5. The
absolute displacement formulation is used as the default SPC/SPCD method.
new mode acceleration formulation with improved performance has been added
in this release to supplement the current algorithm. The improved
performance makes mode acceleration a more attractive option when increased
accuracy is desired.
until the release of NX Nastran version 4.0, only auto spectrum PSD
functions of response could be output for random results. It was required to
use DMAP alters to obtain cross spectrum results. In NX Nastran 4.1, the
option to output cross-power spectral density functions became available.
Now with NX Nastran 5.0, it is possible to also request cross-correlation
Dynamic Design Analysis Method (DDAM) is a list of procedures to determine
modal shock response. To complete DDAM analysis procedures in previous
releases of NX Nastran, the use of dmap alter files were required. Now in NX
Nastran 5,these DDAM procedures have been streamlined and automated, thus
eliminating the alter requirement.
element strain (ESE), kinetic (EKE), and damping (EDE) case control commands
have been improved to allow the output of element energy information in
SORT2 complex format. This format is suitable for plotting complex function
data from frequency domain dynamic solutions. In previous releases, you
could only output the real magnitude of element energy, thus no phase
information was written. In addition, only SORT1 format could be output,
which is not convenient for function plotting.
dynamics can now be used in a modal frequency response solution, SOL 111, to
calculate the dynamic response of a rotating system. This new response
calculation adds to the existing rotor dynamics capability, direct complex
mode solution, SOL 110, whose output is used to create Campbell diagrams.
the modal method is used for dynamic response calculations, understanding
which modes contribute to the response helps understand the dynamic behavior
of the simulated system, and can provide insight as to how to improve the
dynamic performance. In this release a new capability has been introduced to
compute the modal contributions in modal frequency response.
structural damping matrix can now be included with a model in NX Nastran 5
using the new K42GG case control command. This ability adds to the other
direct matrix capabilities of stiffness, mass, and damping matrices using
DMIG bulk entries.
new sparse data recovery option is available for the modal frequency
response analysis (SOL 111), modal transient response analysis (SOL 112),
and optimization (SOL 200) as the new default. For SOL 111 and 112, this
feature reduces the cost of matrix-multiplications inside DDRMM modules when
large amount of data are requested to recover in the modal analysis.
Similarly, SOL 200 utilize the partitioning of eigenvector matrix in order
to reduce the cost of matrix-matrix multiplies.
parallel processing method Distributed Memory Parallel (DMP) has been
enhanced in NX Nastran 5 with the following additions:
normal mode calculation portion of an optimization solution (SOL 200)
can now use DMP.
new linear statics (SOL 101) DMP option, Load Domain Static Analysis
(LDSTAT), now exists to decrease the solution times when large numbers
of load cases exist.
NX Nastran release includes support for a new sparse Cholesky decomposition.
All users of Cholesky decomposition (including the Givens and Householder
eigensolver methods) will utilize sparse decomposition by default, which can
be considerably faster than the non-sparse Cholesky decomposition method
used in earlier NX Nastran versions.
Nastran Version 5.0 introduces the new REDMULT performance option for use
when solving vibration problems with the Lanczos method. This option reduces
the cost of matrix-vector multiplies inside the READ module when the mass
matrix involved is relatively dense, which can occur when a large number of
MFLUID is present in the model.
Dynamic Software Interfaces
release includes interoperability between NX Nastran and the FunctionBay RFI
(RecurDyn Flex Input) file product. You can now create a RecurDyn Flex Input
file (RFI) directly from NX Nastran. The RFI contains the reduced order
matrices from the results of a NX Nastran non-restart SOL 103 analysis. The
RFI can be imported into RecurDyn and used to represent a flexible component
in a multi-body dynamics analysis. This direct RFI export capability
streamlines the process of creating flexible components from FE models,
making it possible to obtain more accurate results from multi-body
Nastran 5 enhances the ADAMS MNF file creation process with a new results
recovery capability. The results from an ADAMS multi-body dynamics analysis,
along with an optional component modal definitions file (OUTPUT2 format),
are used in a consecutive NX Nastran SOL 103 results recovery solution.
set-up of a flex body modal solution in NX Nastran for export to ADAMS MNF
or Recurdyn RFI files requires special considerations for the modal
solution. This is because flex bodies will be attached to other components
in the multi-body dynamic (MBD) simulation and local flexibility effects at
the connection locations are thus important. A modal solution method called
Component Mode Reduction of Residual Structure (CMR of RS) is recommended
for flex body solutions because it includes both global and local effects.
The details of this method are presented in the multi-body dynamic chapter.
Nastran 5 introduces a new optimizer option, UGS-ADS, which is based on
public domain ADS code.
CTDISP option has been created on the NXSTRAT bulk entry to prevent contact
conditions from updating.
new option on the NXSTRAT bulk entry, CTDAMP, has been created to stabilize
the portions of the model experiencing rigid body motion, thus helping the
solution to continue and converge.
new option when INIPENE=3 is available which will include both penetration
and now gaps. This option is particularly beneficial when contact conditions
are defined on the faces of concentric cylinders.
NX Nastran 4.1, a new contact segment option became available for SOL 601
which improved contact results. This improvement matches the order of the
contact segments with the order of the elements. The restrictions which
existed in NX Nastran 4.1 when CSTYPE=1 have been eliminated in NX Nastran
contact algorithm has been improved in NX Nastran 5 to be more robust for
contact with friction.
option to “glue” element faces together during a 601 solution is
available in NX Nastran 5. The glue option connects predefined surfaces
together and prevents relative motion in all directions. Predefined regions
of element free faces are used to detect where the glue elements are
option to define element birth and death times for a specific set of
elements is available in NX Nastran 5.
Nastran 5 offers an automated method to simplify the multisolution process
of bolt preloads with SOL 601.
new shell thickness result output option is available when using advanced
nonlinear to solve large strain problems.
new 3D-iterative solution option is now available in NX Nastran 5 for SOL
601 to efficiently solve large models containing mainly higher order 3-D
solid elements (e.g., 10-node CTETRA, 20-node CHEXA, etc.).
new contact solution parameters, INTORD and REFINE, are now available in NX
Nastran 5 on the BCTPARM bulk entry to improve the accuracy of the contact
in NX Nastran 5, a contact definition can be included in a normal mode
solution (SOL 103), and in an optional modal dynamic response calculation
(SOLs 111 and 112).
NX Nastran 5, the use of superelements is now permitted in solution
sequences which support contact (SOLs 101, 103, 111 and 112). The only
requirement is that the contact definition must occur in the residual
in NX Nastran 5, the linear contact solution can include the shell element
ZOFFS when evaluating the contact surfaces.
Ratio Output for Composites
ratio is now output together with the failure index when using the PCOMP
bulk entry. Strength ratio is a more direct indicator of failure than
failure index since it demonstrates the percentage of applied load to the
Expansion of Rigid Elements
option to include rigid elements in thermal expansion calculations is
available in NX Nastran 5. The new case control command, RIGID, should be
assigned to “LAGRAN” to use the new method. In addition, the coefficient
of thermal expansion (ALPHA) has been added as an additional entry on the
rigid elements: RBAR, RBE1, RBE2, RROD, RTRPPLT. This capability is
supported in solutions 101 through 112.
the RIGID case control command is set to the default of “LINEAR”, the
original linear elimination method is used. This method treats rigid
elements as an MPC equation without thermal loading effects. The new RIGID
case control command is duplicated below for convenience.
components of an assembly are bolted together, a specified torque translates
into an axial bolt preload. Bolts should be properly preloaded in this way
before service conditions are applied to the assembly. When analyzing preloaded
bolts, you may be interested in obtaining the stresses due to the preload
condition alone, or due to a combination of the bolt preload and service load.
You can manually determine the preloaded bolt condition by using equivalent
thermal loads, although using this method is approximate and typically requires
many solution iterations when multiple bolts exist.
Nastran 5 offers an automated method to simplify this multisolution process. A
bolt analysis can be selected by including the new case control command
BOLTLD=n, where "n" selects the new BOLTFOR bulk data entry containing
the bolt preload value. The bolts should be modeled as beam elements, and
included in the new BOLT bulk entry. One BOLT entry is required to define each
physical bolt. The service loads can also be included and are selected using the
LOAD case control command. Superelements are permitted with preloaded bolts but
the elements which define the bolts must be in the residual structure.
Nastran uses the following two solution process to automate the preloading of
beam elements which represent the bolts are reduced in stiffness by the
value of the parameter BOLTFACT which makes their stiffness insignificant.
bolt preloads are applied at the ends of the bolts in the axial direction.
linear statics solution runs to get the relative displacements, U2 and U1,
for each pair of grids.
bolt strains are calculated as:
Strain = – (U2-U1)/L – P/AE
where U1 and U2 are the deflections at the ends of the bolts, P is the
preload, and A is the area of the bolt.
the final solution step, the bolts are treated as they were modeled
(beam elements), then the calculated bolt strains are applied plus any
service loads (if defined).
Iterative Solver Support of Surface Glue
NX Nastran 4.1, a new option to “glue” element faces together during a
solution became available. Glue definitions, which are supported in all solution
sequences except for SOL 701, create stiff springs to connect the pre-defined
surfaces. Glue elements connect components together in such a way as to prevent
all relative motion. Glue definitions in a SOL 153 heat transfer analysis are
treated as near infinite conductivity connections.
surface-to-surface glue capability was supported by the global iterative solver
in NX Nastran 4.1, but not by the element iterative solver. Now in NX Nastran 5,
the surface-to-surface glue definitions can be included when using the element
iterative solver. To utilize the element based iterative solver, add the keyword
Nastran uses pre-defined source and target regions of element free faces to
detect glue conditions in the model. More specifically, the solver uses the
element faces from a source region to project normals, then checks if these
normals intersect with other element faces on a target region.
Mejoras en Glue-Contact de
NX NASTRAN V5.0
glue element is created if:
Nastran finds an intersection between element faces, and
distance between the two faces is equal to or less than a distance that you
number of glue elements created and their distribution determine the accuracy of
the glued interface
new glue solution parameters, INTORD and REFINE, are now available in NX Nastran
5 on the BGPARM bulk entry to improve the accuracy of the glue solution. The
updated BGPARM bulk entry is repeated below for convenience.
the number of locations where normals were projected (glue points) from the
source region was dependent on the element type. For example, the linear
triangle face would always project a single normal, while the parabolic quad
would project 4 normals.
in NX Nastran 5, the number of glue points used is dependent on the value
assigned to the new INTORD parameter, and on the element face type. By default,
INTORD=2 and the number of glue points increases as compared to the previous
release. When INTORD=1, the number of glue points is the same as the previous
release. The following table summarizes how the INTORD value adjusts the number
of glue points for a particular element face:
of Glue Points Used in Glue Element Evaluation
new REFINE parameter increases the number of glue points by refining the mesh on
the source region. Part of the refinement process is to project element edges
and grids from the associated target region back to the source region. The
resulting refinement on the source region is then more consistent with the
target side, which then gives a better distribution of glue elements. The
refined grids and elements are only used during the solution. The glue results
are transferred back to the original mesh for post processing results.
default, REFINE=1 and mesh refinement occurs. REFINE=0 turns off the refinement
Element Z-offset with Surface Glue
elements such as the CQUAD4 can be offset relative to the mean plane of their
connected grid points using the ZOFFS option. In NX Nastran 5, the surface glue
solution can include the shell element ZOFFS when evaluating the glue surfaces.
The value assigned to the new ZOFFSET option on the BGPARM bulk entry determines
if the glue solution recognizes the ZOFFS value. By default, ZOFFSET=0 and the
ZOFFS value is used when evaluating the glue surfaces. When ZOFFSET=1, the ZOFFS
value is not used when evaluating the glue surfaces.