SYSTEM, TAN 4002, autosupa.v707

M. A. Gockel, April 13, 1999
Revised February 22, 2000 to describe a modal method of inertia relief.


   LANCZOS METHOD, rnormal.v707, TAN 4383, M. A. Gockel, January 14, 2000


A DMAP alter package that uses a modal method of computing rigid body modes for
inertia relief analysis is now introduced, autosupa.v707. A new method for
automated support of models for static analysis with inertia relief effects
based on geometric methods of computing rigid body modes was introduced in
Version 70.7. All methods of inertia relief available in MSC/NASTRAN are
described and compared in this revision.


Inertia relief analysis is applicable for free bodies undergoing constant
loads. The response is measured after all transients have died out and the
structure is in a steady acceleration state. SOL 144 provides one type of
automated inertia relief analysis, and SOL 101 a less automated option. An
example of inertia relief analysis is an aircraft in a steady turn. Inertial
centrifugal force effects would appear to make the structure heavier. These
conditions are described in the aero world, for example, as a “2 g turn”. In
SOL 144 aerodynamic effects are considered when generating a stiffness-like
matrix representing air forces that react these g forces, and the analysis
adjusts the aircraft controls to trim the aircraft in this steady state. If
the same aerodynamic loads were applied by hand this same analysis could be
done in SOL 101 (static analysis) as well. SOL 101 does not have any automatic
balancing effect capability such as the aero stiffness, so it is the modeler's
responsibility to also model similar effects there with loads or stiffness
effects. Examples in SOL 101 are more difficult to imagine. Consider an
elevator falling at a constant rate of acceleration of about 0.5 g's. It has
restraining cables whose control system is tuned to provide a lifting force of
one-half the weight of the elevator during descent. The applied loads on the
structure are then gravity loads, acting in a downward direction, somewhat
compensated by inertia loads and cable loads, acting upwards. The modeler
prescribes the gravity loads and cable loads. The acceleration state and the
resulting inertia loads are computed automatically. The simplifying assumption
is made that this is a steady-state problem, valid when all transients are
negligible. This work was done in research for methods to improve SOL 144. It
is delivered initially in SOL 101 because that is a simpler implementation.

When the inertia relief option for static analysis is requested all
displacements are measured relative to a moving reference frame rather than to
ground (“inertial coordinates”), unlike conventional static analysis where the
structure must be grounded. The reference frame accelerates at a constant rate
towards infinite displacements, so the inertial displacement of the reference
system is not of interest, it is a variable eliminated from the equations. The
applied loads accelerate the reference frame. The acceleration state is used
to automatically generate inertial loads at DOFs with mass. The inertial loads

are calculated internally, in a manner that exactly balances their resultant
with the resultant of the applied loads. The equations can now be solved
because the structure is in a state of static equilibrium. In an older method
of inertia relief the user was required to define the reference frame by use of
the SUPORTi entry. In the newer methods the reference frame is generated
automatically, without the requirement of a SUPORTi entry.

In the newer methods the rigid body mode shapes of the structure are computed
from either grid point geometry or a real mode analysis. They are stored in
the shape function matrix, Dar. These shape functions are used to compute the
rigid body mass of the structure and the resultants of the applied loads on
this point mass. The accelerations of the point mass are then computed, then
transformed to all locations with mass. These accelerations generate inertial
loads that balance the applied loads.


All methods of inertia relief analysis are based on the a-set equation in
inertial coordinates

             Kaa   Rar        uabar          Paa                Pa
         [               ][           ]= [         ] + Pi = [        ]   (1)
             Rar’ 0rr         -qr            Yr                 Yr

The first set of loads is the applied loads, and the second set the inertial
loads required for the structure to be in equilibrium. The qr terms are the
unknown constraint forces associated with the constraint equations Rar. They
are applied on the reference set, the r-set. The Yr terms are generalized
enforced displacement variables. The various methods differ in how the
constraint equations Rar are derived, and how the equation is solved. The
inertia loads are calculated by first obtaining a matrix of rigid body shapes,
Dar. There are several means to obtain these shapes, described below. They
are used to compute the rigid body mass of the structure and the resultant of
the applied loads

         Mrr = Dar’*Maa*Dar

         Pr = Dar’*Pa

The rigid body acceleration ar and the resulting inertial loads Pia are

         ar = Mrr-1*Pr

         Pia = Maa*Dar*ar

It is more convenient to solve the equations in a non-inertial coordinate
system of a type called relative coordinates. The inertial coordinates uabar
are replaced with relative coordinates ua,

         uabar = T*ua

In some methods it is useful to partition the a-set into the reference set (r-
set) and the leftover set (L-set). Unlike other subscripts, an upper case L is
used to distinguish this symbol from 1 (one).

         ua = [ ]


The transformation matrix T has the components

                ILL DLr
        T = [             ]
                0rL Drr

This transformation relates the total (inertial) motion of the L-set to the
motion of the L-set relative variables uL plus the translation of the r-set
displacements ur multiplied by the rigid body modes, DLr*ur. We have made the
simplifying assumption that there are DOFs in a reference set known as the r-
set in the inertial basis, but they are not necessarily parallel to the
directions of the Yr variables, as evidenced by the equation

        ur = Drr*Yr

For some of the methods described below Drr is an identity matrix, and ur and
Yr are equivalent, but a full (but non-singular) Drr matrix is also allowed for
the general case.

The first equation    is transformed to the relative basis by partitioning the a-
set terms into the    L- and r-sets, and pre-multiplying by T’ and post-
multiplying by T.     A useful identity that simplifies the new equations results
from the fact that    motion of the rigid body modes does not result in reaction

        Kaa*Dar = 0

When all of the algebra is done and the simplifications are performed, the
resulting equation in relative coordinates is

         KLL 0Lr RrL’    uL     PL
        [0rL 0rr DRrr’][ ur] = [Dar’*Pa]                     (2)
         RrL DRrr 0rr   -qr     Yr

where DRrr= Dar’Rar. The right hand side contains both the applied and
inertial loads. This equation shows that moving the ur point while holding the
uL relative variables fixed causes no strain energy. This is plausible because
a motion of ur in relative coordinates causes the ulbar terms in the inertial
basis to move in rigid body motion only. Note that the second row can be
solved for qr, independent of stiffness terms or displacements,

        qr = -DRrr’-1*[Dar’*Pa]

This equation expresses the concept that Kaa has no internal constraints (it
represents a free body), so that the constraint forces can be computed merely
by summing the applied loads as transferred by the constraint equations, while
ignoring internal load paths in the structure.

2.   Rigid body shapes by Static Analysis or Geometry

In the oldest style of inertia relief, now known as the single support option,
static analysis rigid body shapes, the basic equation is solved with Yr = Irr,
Rrl = 0, Rrr=Irr, Drr = Irr and Pa=0 to find Dar. The resulting equations are

        KLL*DLr +KLr*Irr = 0

        KLL*DLr <= -KLr

        Dar = [         ]

A more economical but less general method to compute Dar is from the geometry
of its grid points, disregarding stiffness effects. This is done in the
VECPLOT module. It generates output than can be used to compute a set of
vectors Dg6 that represent 6 rigid body modes due to unit motion of a reference
grid point. This method does not deal correctly with scalar points that have
applied loads and/or masses and some other special effects. There are
additional equations, described in the DMAP for SOL 101 and perhaps elsewhere,
added to account for cases when there are less than 6 rigid body modes, but no
provision for more than 6 rigid body modes or disjoint components in the same
model. The static analysis method and the modal method described next do not
have these limitations because they find these shapes from the same matrices
used in the total analysis where all special effects are present. At present,
the static analysis method for computing rigid body mode effects is present
only in SOL 1, and not SOL 101. SOL 1 does not support superelements, p
elements, and other modern features. There are no plans to implement the
single point option in SOL 101, as the modal method described later is

4.   Rigid Body Modes by Dynamic Analysis

The most modern method, introduced in the alter package described in this note,
computes rigid body modes in the eigensolver module by the Lanczos method. It
also computes a few flexible modes to insure that all rigid body modes have
been found, then discards the flexible modes. It produces PHIgrbar, where rbar
is not necessarily the r-set defined by SUPORT entries, but the Nr calculated
modes whose natural frequency is below a test criteria. SUPORTi entries are
optional. If the user adds the proper number and type of SUPORTi entries this
r-set is used to refine the rigid body modes to make them repeatable from run
to run. In this case the rbar- and r-sets are identical If the user supplies
an inadequate set the SUPORT entries are ignored, and the rigid body modes are
used as is from the eigensolver. The method of refining the modes with the r-
set is described in Reference 1. This method has the advantage that it
correctly handles any allowable type of modeling option, including scalar
points, models with more or less than 6 rigid body modes, and all other special
conditions not handled well by the geometry-based rigid body modes. This
method allows completion of the solution even when an unacceptable r-set has
been chosen, in contexts where a good r-set is not needed for the remaining
operations. This method applies to all options in SOL 101, including
superelements and p elements. A test is made to determine that at least one
flexible mode is calculated, where the default number of modes calculated is
13. If more than two disjoint components are modeled, or if the first flexible
frequency is lower than the (present) default of 0.1 Hz., there are user
parameters described in the readme note that allow modeling any number of
disjoint components, and very soft structures whose lower modes may be be below
0.1 Hz.

It was found in testing that the rigid body mode shapes varied from run to run
due to very small changes in the model or in the method of solution. This is
proper and to be expected. There is no unique set of rigid body modes, merely

many sets that are linear combinations of one another. The inertial loads and
element loads and stresses were identical on all these cases, but the relative
displacements differed. This is because the rigid body mode shapes define the
reference frame, and choosing a different set of shapes is analogous to
changing the r-set for the single point option. Identical displacement
solutions from run to run are not a mathematical necessity. However, a
consistency of displacements between runs increases confidence when trying to
compare the results of two different analyses where the results should change
slightly, or not at all. A search was made for a method to produce repeatable
rigid body vectors from run to run.

All totally automatic methods for providing repeatable rigid body modes that
were evaluated failed one special case or another. Indeed, a case can be made
that, particularly for symmetric structures, some form of user input to define
a preferred direction is a requirement. For example, a uniform sphere modeled
in spherical coordinates has no obvious preferred direction. Ironically, the
best choice found to date for a user specification of set of directions is the
SUPORTi entry. Eliminating the requirement for this user input was the
motivating factor for this work. The DOFs on the SUPORTi entry must be capable
of restraining all rigid body modes. However, this is only a geometry
requirement, there is no stiffness requirement as there is for the older
methods. The SUPORTi entries may be applied to the proverbial end of a very
soft antenna, and good, repeatable results will be generated. The equations
for this operation are given in Reference 1. A Dar matrix identical in form to
that of Section 2 is produced from the rigid body modes, without the need to
decompose KLL to solve for DLr. DLr is defined in Section 2.

If a set is provided that does not meet the geometric criteria a behavior more
benign than a user fatal message results. A user warning message is printed to
the effect that the SUPORTi entries are inadequate, and they are ignored. The
somewhat arbitrary rigid body mode shapes provided by the eigensolver are used
as is. Two runs with very small changes in the model and an inadequate set of
SUPORTi entries will produce almost identical element stresses and inertial
loads, but their displacement solutions may differ appreciably because their
reference frames differ. In summary, while SUPORTi entries are not required,
their presence provides repeatable displacement solutions. They are not
required to meet stiffness criteria, and when mis-applied, do not cause a fatal
error exit except for cases of gross modeling errors. An example of this type
is a model with more than 3 disjoint components, using the default values of
the user parameters described in the readme note.

5.   Constraint Matrix Options

The single point option (SOL 1) sets Rrl = 0, Rrr= Irr.   This simplifies the
last row of the first equation to

        Irr*ur = Yr

There is at present no user interface for defining enforced displacements on r-
set DOFs, so Yr is identically 0. This simplifies to the equation

        ur = 0

When this option is chosen the displacements at the r-set DOFs are always
binary zeros, leading to the concept of all other displacements uL being
measured to a rigid reference frame that is attached to the r-set DOFs. The
“single point” name is somewhat misleading because it is necessary to spread

the r-set points to several grid points for cases where there is no stiff point
available that can react rotations. In this case two translation DOFs may be
used to react translation by their summed effect and rotation by their
difference coupled over the length between them. A more accurate, if awkward
name would be the statically determinate constraint option. There are exactly
the number of constrained DOFs necessary to react all rigid body modes, no
more, no less. They must also meet stiffness criteria to avoid numerical
truncation problems in the solution process.

When another adequate set of r-set DOFs is chosen the internal loads remain the
same, but the computed displacements differ. This is proper because the
displacements are being measured relative to a different set of reference
points. The “zero motion points” shift from the first r-set points to the
second r-set.

The distributed constraint option uses full matrices for the constraint
equations. Any number of constraint concepts could be used, such as having the
average displacements of all variables being zero. A more intuitive approach
is used, where weighted rigid body modes are used as the constraint equations.
It has the advantage that the interior constraint forces are proportional to
the mass of the grid point, which should have at least a weak correlation with
the stiffness of the point. This avoids adding large constraint forces on very
soft points, risking numerical instability. The last row of equation 1 is then

         Rar = Maa*Dar

         Rar’*uabar = Yr = 0

These equations infer that the motion of a reference frame attached to the c.g.
of the structure is zero. The motion of all points ua in general is non-zero,
but when structural deformation is plotted it will be seen that they tend to
displace about a line that goes through the c.g. If there happens to be a
point exactly at the c.g. whose axes are parallel to the mass principal axes of
the structure its motion will be computational zeros, but not binary zeros as
is possible for the prior option. (When used as an argument for the
superiority of the single point method, it is a spurious argument. The r-set
displacements of the single point method are binary zeros because they are
assumed to be zero and not computed, not because they are computed as binary
zeros.) Both options will provide identical OLOAD output (user-applied plus
internally computed inertial loads), and identical element forces and stresses.
The displacements will differ because they are measured relative to different
reference frames. In this sense, the displacements may be regarded as
intermediate output that may be useful when debugging the model, but if the r-
set is changed or a distributed support system is used the displacements can be
expected to change, while the other outputs are invariant with respect to these

When an omitted set is used or superelements are used, the displacements from
these two methods are identical, but differ for cases without omitted sets.
All methods produce identical internal loads. The reason for this shift in the
reference axis when omits are present is still under investigation. It may be
a proper shift, if an inelegant behavior. It may be due to causes that can be
corrected. Results of this investigation will be reported in updates to the
readme file.


The partitioned solution method solves each row of the initial equation
separately. Only the single point constraint methods use this option at
present. As a result DRrr = Irr, RLr = 0, and Yr = 0. The equation for Pa and
qr simplify to

        qr = -Dar’*Pa

         Pa = Paa + Pi = Paa - Maa*Dar*ar

  The first and third rows of equation 2, written out explicitly and ignoring
null terms, is

        KLL*uL = PaL + PiL

        ur = 0

All of the unknowns are now defined, and the system of equations can be solved
in parts. In theory, a distributed constraint system can also be solved with a
partitioned solution. There are practical reasons to seek another type of
solution. The fact that while Rlr is null for single point constraints it is
not null for distributed constraints leads to many more coupling terms, the
worst being an outer product that gets added to the stiffness matrix of the
form RLr*Krr*RLr’. This tends to be a full, unbanded matrix that can raise the
solution CPU time and memory requirements by an order of magnitude.

The Lagrange Multiplier Technique (LMT) solution method solves the equation 1
directly.   The only extra DMAP operations are the appending of the constraint
variables and their matrices to the a-set equations, and the partitioning of
the constraint forces from the solution vector. It does not require the
partitioning, explicit definition of relative coordinates, and solution by
parts of the prior method. The first part of the factor of the assembled
matrix is identical to that of the partitioned solution of KLL, a well-banded
matrix. The remaining rows are more coupled but are few in number. In general
there is never a large cost penalty for the LMT method, and often a cost


Automatic selection of the reference frame reduces user labor, and avoids the
class of modeling errors associated with a poor choice of r-set points. The
user interface for r-set specification is the SUPORT entry. It lists the DOFs
in the r-set, the reference set. Some skill is required to use this entry
correctly. When the r-set is chosen such that structure is not constrained in a
statically determinate manner, or if the stiffness attached to these points is
inadequate, the rigid body mode shapes may be poor. A poor static analysis
solution may also result from the poor constraints, independent of the loading
problems. Both effects may result in poor overall accuracy. Poor results can
occur with little warning when the SUPORT entry is misused.

The rigid body modes from an eigensolution eliminate the need for a SUPORT
entry. The reference frame is selected automatically, in a manner that poor
solutions are unlikely because of the choice of reference frame variables. It
is not possible to define a SUPORT entry incorrectly if you do not have to
supply one at all.

The constraints associated with the reference frame are distributed to all
points with mass. This means that structures with modeling errors, such as a

region of elements left out through oversight, will still give reasonable
results that can aid in diagnosing the modeling errors. A model in development
may contain many disjoint parts, inadvertently. Any part with three non-
collinear points with mass will be adequately constrained for solution.

The theory that states that all methods of inertia relief provide identical
loading data (OLOAD output) and element stresses and forces is confirmed in the
test problems described below. Their displacements will differ, but it can be
shown by hand calculation (with considerable labor) that they differ only by 6
constants times the length between grid points, due to use of differing
reference frames.

There is a subtle difference between the automatic constraint methods when
comparing modes calculated from geometry (Vecplot module shapes) with those
computed by eigensolution (Read module eigenvectors). The geometry method
assumes that there are six rigid body modes. When there are less, you are not
solving an inertia relief problem because there must be some constraints to
ground. It will be left as an exercise for the reader to provide physical
interpretations of what it means when some rigid body modes of the free
structure are grounded. The easiest interpretation is that you have made a
modeling mistake, although there may be some cases where it is done by intent
for legitimate reasons. In SOL 144, for example, where there are provisions to
model aerodynamic lift but not drag, for union jurisdiction reasons, it is
common to ground fore and aft motion to allow trimming the aircraft. Other
even more imaginative justifications for other applications are left to others.
With the modal method no assumptions are made on how many rigid body modes
exist. This number is regarded as an unknown to be determined by the
eigensolution. A planar model will have 3 rigid body modes, and two disjoint
components in the same model could have 12 in all. Each will be considered as
a unique shape function.

The single point option constraints can be visualized as supporting the
structure on knife-edges initially, in a statically determinate manner. This
implies that the constraints have both a geometric criterion to meet (all rigid
body modes must be constrained) and a stiffness criterion. The knife-edges
must be applied to stiff parts of the structure. Indeed, one method to
evaluate a point's stiffness for SUPORT entries is to ask yourself if you would
feel comfortable lifting the entire structure by a cable to this point in a
shop. Main wing frames or chassis spring mount points are good candidates. A
point on a soft engine cowl would tear out if the aircraft were hung by it, and
would likely lead to numerical difficulties if used for SUPORT entries.

A method to conceptualize a distributed constraint option of the geometric type
is by a flying waterbed. All components with mass are attached to constraints.
When there are two disjoint components they are coupled through the
constraints. When you shove down on one disjoint body you tend to raise the
other. (Couples who sleep on waterbeds can explain this effect to you.) The
extra shove is done in a manner that shifts the whole structure and does not
change internal loads, but it does change the reference frame. You should
never get “high maxratio” fatal exits because some connectivity was left out of
the model inadvertently, but the effects of unintended disjoint components may
be covered up by the automatic constraint system unless you look for evidence
of discontinuities in displacements and internal loads across component

For constraint system shapes from eigensolutions, by contrast, the modes for
one disjoint component can be uncoupled from those of the other, and in fact

they will be when SUPORTi entries are used. You can visualize several separate
water beds, one for each disjoint component. If you put an extra force on one
of the waterbeds it will not affect the motion of the other component. If your
intent was to model one continuous 3-dimensional free structure and you have
more or less than 6 rigid body modes, it is an unambiguous clue that something
is wrong.

Another subtlety becomes apparent when you try to compare the solution from one
method with that of the others. You will almost always see a difference in
displacements because different reference frames are being used, but on a good
model you can expect to see identical element forces with all methods. This
change in displacements is even true for the single point methods when you move
from one set of r-set DOFs to another. This was part of the motivation for
operating on the modal solutions for rigid body modes with the r-set. Rigid
body modes are not unique. A valid set can be transformed into another valid
set with a linear transformation. The r-set is used to force a repeatable
solution for the rigid body modes. This will result in repeatable deflections
for re-analysis in inertia relief analysis.


Selection        Rigid Body       Constraint                Solution Method
Method.          Mode Method      Option

0 or blank       None             None. SUPORT entries      Conventional static
                                  are equivalent to SPCs.   Analysis.

-1               Geometry         Single point, SUPORT      Partitioned solution.
                 (VECPLOT)        required.                 Superelements

-2               Geometry         Automatic, distributed.   LMT solution.
                 (VECPLOT)        SUPORT ignored.           Superelements not

-3               Eigensolution    Automatic, distributed    LMT solution.
                 (READ module)    SUPORT optional.          Superelements
                                  Provides repeatable       allowed.
                                  displacements when
                                  SUPORT present.

SOL 1 uses the SUPORT entry to compute rigid body modes by static analysis, and
uses a partitioned solution.

In theory, all options could be provided in all combinations. Present thinking
is that only the set described above will be maintained in the production
solution sequences later, as they adequately cover all known requirements, and
provide upward compatibility with past systems.

The single point constraint, partitioned solution, rigid body modes from
geometry option (inrel=-1) is the most economical general solution. It
requires input of a SUPORT entry that meets both geometric (rigid body control)
and numerical stability (stiff attach structure) criteria. It is awkward to
use when there are less than 6 rigid body modes. It is not useable if there
are more than 6 rigid body modes.

The distributed support option using geometric modes (inrel=-2) is best suited
for solid element models whose highly coupled mass matrices makes eigensolution
expensive. This option does not support superelements, and in fact was
developed for the ULTIMA product, which also does not support superelements.
It does not require the presence of a SUPORT entry. In version 70.7, a SUPORT
entry will cause a fatal error exit. This exit may be removed in a later
production version that would merely ignore the SUPORT entry.

The distributed support option using modes from eigensolution (inrel=-3) is
new, and has not yet had field experience. It has the potential to be a
primary model checkout tool. It may be added to aeroelastic static analysis
(SOL 144) at a later date. Many dynamic analysts put a new model through
static analysis before attempting to compute its modes or dynamic response
because static analysis is less costly and provides better diagnostics when
errors are encountered. Use of SOL 101 with inrel=-3 provides both a static
analysis and a check of the first few flexible modes, without the risk of
computing many flexible modes with a wounded model. If the first few natural
frequencies are not plausible it is unlikely that any other modes produced by
this model will be useful. On the very first run the SUPORT entries need not
be entered. It is easier to select good SUPORT DOFs for a model after you know
how many rigid body modes it has. On subsequent runs a SUPORT entry can be
tested. If it does not meet the geometric criteria it will be ignored, without
causing a fatal exit. This type of analysis can be used to iterate on SUPORT
entries until a valid set is found, at lower cost than for real mode analysis.
There is another alter (rnormal.v707) that uses the SUPORT entry in SOLs 103
and 110-112 in the same manner used here. That is, the optional SUPORT entry,
applied correctly, will make rigid body modes repeatable for the LAN method in
all dynamic analysis, in the same manner that it is for the other methods. See
Reference 1 for details.


All methods of inertia relief analysis provide the uninteresting solution of
zero displacements for GRAV loads. This is proper because the inertia relief
equations place an inertial load on each grid point that is equal and opposite
to its GRAV load. Although GRAV loads are an excellent loading for debugging
models that are constrained to ground, they produce uninteresting results for
inertia relief analysis unless combined with other types of loads. Some
sophisticates use GRAV loads on inertia relief models regardless, and find some
insight into suspected errors when there are non-zero solutions where there
shouldn’t be, but this is excessively esoteric to explain.

The automatic support options generate an indefinite stiffness matrix.
Although this matrix is stable for solution, the present “maxratio” diagnostics
are not computed correctly in the regions where the constraint equations are
evaluated. This leads up to six high ratio messages (typically, some with
values of 1.E15), and/or negative factor diagonal messages. This is actually
an error in the diagnostics, not in the solution. These diagnostics may be
ignored when using the alters for V70.6 and V70.7 described in the appendix.
This error in diagnostics is scheduled to be fixed in V71.

The automatic support methods do not allow use of DMIG, UACCEL inputs for
prescribing the acceleration state, rather than computing it from the
resultants of the applied loads. Requests for this feature will cause a fatal
error exit. The solutions by the automatic support method with this input
option are also the uninteresting zero displacement solution, for reasons
similar to the GRAV load discussion above. This option is therefore blocked.

It still functions with the manual method, where it gives more interesting

All VECPLOT methods ignore mass and loads on scalar points when computing rigid
body mass, load resultants, and inertia loads. External loads specified on
scalar points are applied, but the model will not be in a state of equilibrium.
On most models scalar point weights and loads are small, and the errors
associated with ignoring them should also be small. A model made up entirely
of scalar points will cause fatal errors early in the analysis. The
eigensolution shape functions are valid for all modeling options.

The automatic support method using VECPLOT shapes requires that the structure
have at least 6 rigid body modes, defined in a manner that the rigid body mass
matrix is non-singular. The manual method allows less than 6 rigid body modes,
as specified on SUPORTi entries. The eigensolution method allows any number of
rigid body modes, including none.

All methods of inertia relief do not process image superelements and
superelements positioned with SELOC entries correctly except for the
eigensolution method. Wrong answers will be provided, without warning.

The iterative solution method and the parallel solution methods are blocked for
the automatic support options. Their solvers are not yet ready for indefinite
stiffness matrices.


Sample problems autosup*.dat analyze a small beam structure with the single
point support method (param, inrel, -1; autosup1.dat), the automatic support
method with VECPLOT mode shapes (param, inrel, -2: -2.dat), and the automatic
support method with mode shapes from eigensolutions (param, inrel, -3; -3.dat).
The full input file for the newest method (inrel=-3) appears here, followed by
the changes necessary to convert the new method to the older methods. These
input files are also on the sssalter library available on the MSC web site. A
readme file named *.rdm that describes input and output features of the alter
is also present there. This example problem and other related test problems
are on MSC’s internal network on node Kodiak, in directory /app/etl/ir.
Clients with an interest in these problems can request them from their MSC
technical contact.

Verification Problems

$ file autosup3.dat inertia relief by rigid body modes
diag 8 $ useful for tracing matrix operations
SOL 101
Include 'autosupa.v707' $ required for inrel=-3
TITLE = inertia relief with r.b. modes constraints          autosup3
Subtitle = 6 rb modes from eigensoln., no s.e.s,
Label = elevator descending with constant 0.5 g acceleration
Echo = both
Oload = all
Elforce = all
Gpfo = all
Spcf = all
Load = 12
param, inrel, -3 $ request autosuport using eigenmodes
$ elevator cage, top rail
CBAR,   12,      12,     1,       2,     ,        1.0
$ I1 plane includes -2 direction
$ side rails
CBAR,   13       12      1        3,       ,       1.0
Cbar,   24,      12,     2,        4,      ,       1.0
$ floor
Cbar,   35,      12,     3,        5,      ,       1.0
Cbar,   54       12,     5,        4,      ,       1.0
PBAR,   12      21      1.0      2.0    1.0      1.25
$ tune so first mode about 0.1 hz.
MAT1,   21      1.0,     ,         .3      1.0
$       gid      cp      x         y       z
GRID,   1,        ,      -1.,      0.,     1.
GRID,   2,        ,      +1.,      0.,     1.
GRID,   3,        ,      -1.,      0.,     -1.
Grid,   4,       ,       +1.,      ,       -1.
Grid,   5,       ,       0.        0.      -1. $ on centerline
$ payload at center of floor
CONM2, 5         5,      ,         10.0
grav,   1,       ,       10.,      ,       ,       -1.

$ cable loads restraining gravity, about half of weight
force, 2         1,      ,        45.     0.,     0.,     1.
force, 2         2,      ,        45.     0.      0.      1.
Load,   12,      1.0     1.0      1       1.0     2 $ grav load
$ can not be in same set as other loads
$ optional inputs
param, grdpnt, 5 $ get weight summary. optional
suport, 5        123456 $ at floor center. Repeatable shape fcns.   optional
param, usetprt, 0 $ review user sets optional
[data beyond this point ignored by MSC/NASTRAN]

The elevator cage is a square, with a payload point at the center of the floor.
Cables are attached at each corner of the upper side rails. They are tuned to
input a constant force equal to one half of the gravitational load while it

This model uses arbitrary units of measure designed for easy hand calculation.

The following comparison problems should be run without the DMAP alter package.

To use inrel=-2, change param, inrel and remove the suport entry.
To use inrel=-1, change param, inrel but leave the suport entry as is.


To top