Section 5 Model Verification.

Section 5 Model Verification

Modeling PAGE Overview 5 Singularities and Mechanisms 6
MSC.NASTRAN Automatic Checking Procedure AUTOSPC How AUTOSPC Works Problems with Autospc Autospc with CQUAD4s Autospc Problems Autospc Output Autospc Autospc Workshop

Modeling (cont.) PAGE Diagnosing Errors 34 Model Debugging 35
Debugging Workshop Model Debugging Debugging Workshop Further Model Debugging Analysis Health Checks Essential QA Checks Applied Load Summation Reaction Load Summation Actual Applied Load Check

Modeling (cont.) PAGE Essential QA Checks – Workshop 71
Good Modeling Practice MultiPoint Constraints, Rigid Elements Multipoint Constraints Multipoint Constraints Workshop R-type Elements RIGID Elements RIGID Elements Workshop RIGID Elements RIGID Elements Workshop

Modeling (cont.) PAGE Useful Model Summary Information 102 ELSUM 103
MAX/MIN DISPLACEMENT AND SPCFORCE OUTPUT Element Geometry Checks GEOMCHECK Element Geometry Checks Structural Symmetry

Overview Typical errors; Singularities and Mechanisms
MSC.NASTRAN’s automatic checking procedure Diagnosing errors Health checks the user should be making RIGID elements and MPC’s Element Geometry Checks Symmetry

Typical errors; Singularities and Mechanisms

Singularities and Mechanisms
A singularity is caused by a degree of freedom without any structural stiffness present, or with a low stiffness The Stiffness Matrix cannot be inverted if it is Singular Some examples of singularities are: Forgetting to eliminate Rigid Body Motions Connecting Dissimilar Element Types Cross connecting wrong Degrees of Freedom

Singularities and Mechanisms (cont.)
Rigid Body Motions Sufficient Nodal Displacement should be specified so that the 6 “rigid body” modes of movement are fixed. Rigid Body Motion Adequate Constraints

Singularities and Mechanisms (cont.)
Rigid Body Motions Forgetting to ‘Equivalence’ in MSC.PATRAN or other preprocessors is a very common error. Results in unconnected meshes.

MSC.NASTRAN’s automatic checking procedure

AUTOSPC If obvious singularities exist, MSC/NASTRAN attempts to automatically deal with them. The Bulk Data entry PARAM,AUTOSPC,YES instructs the program to automatically apply SPCs to these singularities. PARAM, AUTOSPC, YES is the default in most of the structured solutions.

How Autospc works GRID 99 Stiffness Terms Hexa Element T1 T2 T3 R1 R2

How Autospc works (cont.)
GRID 99 Stiffness Terms Successful Elimination of Zero Stiffness terms T1 T2 T3 R1 R2 R3 Hexa Element GRID 99

Problems with Autospc Solid Bar
No Elimination of Solid Element Zero Stiffness terms T1 T2 T3 R1 R2 R3 T1 T2 T3 R1 R2 R3 Bar Element GRID 99 Hexa Element

Problems with Autospc (cont.)
Combined Stiffness Terms No Elimination of Solid Element Zero Stiffness terms T1 T2 T3 R1 R2 R3 Bar Element GRID 99 Hexa Element

3 Mechanisms ! Bar Element GRID 99 Hexa Element

Solutions Manual SPC MPC’s (later) Rigid Links (later) Bar Element GRID 99 Hexa Element

Autospc with CQUAD4’s GRID 106 Stiffness R3 = 0.0 T3 T1,R1 T2,R2 T1 T2

Autospc Problems GRID 106 Stiffness T3 Possible Mechanisms !
2 CQUAD4’s Possible Mechanisms ! T1 T2 T3 R1 R2 R3 ? T1 T2 T3 R1 R2 R3 ? T3

Autospc Problems (cont.)
Solutions PARAM,K6ROT, kvalue Not Recommended – for Non Linear usage PARAM,SNORM, angle Recommended All vectors within ‘angle’ are averaged 2 * angle

Autospc Output Output includes a grid point singularity table. This table should be inspected carefully for potential singularities. Default stiffness ratio = 1.0E-8 G R I D P O I N T S I N G U L A R I T Y T A B L E POINT TYPE FAILED STIFFNESS OLD USET NEW USET ID DIRECTION RATIO EXCLUSIVE UNION EXCLUSIVE UNION G E B F SB SB G E B F SB SB G E B F SB SB G E B F SB SB

Autospc Output (cont.) What does the USET term mean?
Consider all grid point and scalar point degrees of freedom in a finite element model as the members of a single displacement set. This global set is called the g-set; the displacement set is known as ug. [Kgg] must be nonsingular in order to solve this equation. To achieve a nonsingular stiffness matrix, the user can specify the independent subsets of {ug} to be partitioned out during matrix reduction. For example: um Degrees of freedom eliminated by multipoint constraints us Degrees of freedom eliminated by single-point constraints Elimination of the M and S sets results in the F (free) set, which is typically solved to obtain the unknown displacements, For a thorough discussion of constraint and partitioned displacement sets, see Appendix B of the MSC.Nastran Quick Reference Guide and MSC.NASTRAN Linear Static Analysis Users’ Guide.

Autospc Controlling AUTOSPC Write out ‘failed’ DOF’s to .pch File
All ‘failed’ DOF are written to Grid Point Singularity Table Can get very large – obscure real problems Write out ‘failed’ DOF’s to .pch File Param,spcgen,1 param,checkout,yes Re-use generated SPC1 data selectively

Autospc Workshop Run the MSC.NASTRAN input files
section5_1.bdf set of solid elements section5_2.bdf set of plate elements Evaluate the Grid Point Singularity Tables Section5_3.bdf solid/plate combination Section5_4.bdf plate/bar combination Evaluate the Tables and check the Fatal Messages

Autospc Workshop (cont.)
section5_1.bdf

section5_1.bdf G R I D P O I N T S I N G U L A R I T Y T A B L E POINT TYPE FAILED STIFFNESS OLD USET NEW USET ID DIRECTION RATIO EXCLUSIVE UNION EXCLUSIVE UNION G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * GRID 1

section5_2.bdf

section5_2.bdf G R I D P O I N T S I N G U L A R I T Y T A B L E POINT TYPE FAILED STIFFNESS OLD USET NEW USET ID DIRECTION RATIO EXCLUSIVE UNION EXCLUSIVE UNION G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * R3 = 0.0

section5_3.bdf CQUAD4’s HEXA’s

section5_3.bdf G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * GRID 13 What happens along here !! G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S *

section5_3.bdf THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL. SUBCASE 1 GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL R E E+02 ^^^ USER FATAL MESSAGE 9050 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS.

section5_4.bdf G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * G E BF F SB S * What happens here !! No Grid Point Singularity terms for GRID 13

section5_4.bdf THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL. SUBCASE 1 GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL R E E+05 ^^^ USER FATAL MESSAGE 9050 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS.

Diagnosing errors

Model Debugging The previous workshop examples Section5_3.bdf
Resulted in FATAL errors due to the presence of mechanisms. This section shows how to identify the type of error.

Model Debugging (cont.)
from file section5_3.f06 This is the most common FATAL ERROR Check the FATAL MESSAGE ID Check the Description THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL. SUBCASE 1 GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX R E E+02 ^^^ USER FATAL MESSAGE 9050 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS.

from file section5_3.f06 A Singularity or Mechanism is indicated It is seen at GRID 13, DOF R2 Is anything special about this point? THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL. SUBCASE 1 GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL R E E+02 ^^^ USER FATAL MESSAGE 9050 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS.

from file section5_4.f06 A Singularity or Mechanism is indicated It is seen at GRID 13, DOF R3 Is anything special about this point? THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL. SUBCASE 1 GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL R E E+05 ^^^ USER FATAL MESSAGE 9050 (SEKRRS) ^^^ RUN TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL. ^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO CONTINUE THE RUN WITH MECHANISMS.

Debugging Workshop Using SPC or SPC1 entries,
Correct the MSC.NASTRAN input files Section5_3.bdf (hint: GRIDS form the joint) Section5_4.bdf Evaluate the results and the implication of the changes

Debugging Workshop (cont.)
Corrections to Section5_3.bdf Evaluate the results and the implication of the changes Constrained DOF 4,5,6 Looks OK, but be careful!!

Corrections to Section5_3.bdf Evaluate the results and the implication of the changes The displacement of the solid section implies small edge rotations of connecting shells– we have constrained them out

Corrections to Section5_4.bdf Evaluate the results and the implication of the changes No complications seen Constrained DOF 6

Model Debugging So far we have seen two examples of FATAL errors caused by excessive pivot ratios during an analysis Fatal Message 9050 In practice there are many checks that MSC.NASTRAN will perform to flag errors prior to analysis in syntax checking and general data checking, as well as during the analysis The form of the FATAL message will be similar. The key ingredients are the ID and the description Further details on the meaning of the FATAL message can be found in the Reference Guide, or more conveniently, the On Line Encyclopedia

Debugging Workshop Run Section5_5.bdf
Evaluate the messages and correct the analysis

Section5_5.f06 What is characteristic about the elements in the group that are subject to warning? What does the WARNING message imply? *** USER WARNING MESSAGE 5487 (EBCHKD) ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS. ORIENTATION VECTOR DEFINED FOR THE ELEMENT ID = IS NEARLY PARALLEL, IT MAY GIVE POOR RESULTS.

Section5_5.f06 Again, look at the group causing the FATAL error Look up the message ID in the On Line Encyclopedia *** USER FATAL MESSAGE 2026 (EMG) ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX. ELEMENT GEOMETRY YIELDS UNREASONABLE MATRIX.

On Line Encyclopedia – result of search for ‘2026’ 2026 *** USER FATAL MESSAGE 2026, ELEMENT **** GEOMETRY OR MATERIAL PROPERTY YIELDS UNREASONABLE MATRIX. Referenced element geometry and/or properties yield a numerical result which causes an element stiffness or mass matrix to be undefined. Possible causes include, but are not limited to, (1) the length of a rod or bar is zero because the end points have the same coordinates, (2) the sides of a triangle or quadrilateral are collinear which leads to a zero cross product in defining an element coordinate system, (3) the bar orientation vector is parallel to the bar axis, or (4) a shear panel has zero thicknesss or modulus. Check GRID Bulk Data entries defining element end points for bad data.

Debugging Workshop Section5_5.bdf Correct the bar data and rerun
$ bar elements follow CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR CBAR

Further Model Debugging
To enable deeper understanding of the files that can be used for debugging the concept of DMAP needs to be introduced DMAP – Direct Matrix Abstraction Procedure The High Level Language that MSC.NASTRAN is written in Completely visible to Users Modifiable by Users DMAP modules perform the mathematical operations required to perform the requested solution sequence.

Further Model Debugging (cont.)
Schematic of DMAP – Direct Matrix Abstraction Procedure Solution Sequence DMAP Modules Source Code Interpret Input Syntax Check Partition SPC’s Partition MPC’s

.f04 File Description The ".f04" file contains a "road-map" of the MSC/NASTRAN modules used in the solution of your problem. Each time a DMAP module is executed, a line is created in the .f04 file contain in the module name and information on the current state of the run.

The cause of the error was clear in the portal frame example. If the messages do not provide enough explanation, the user should also check the .f04 file to determine at what point during data processing the analysis terminated. In Practice, understanding the DMAP Module flow may be difficult, but it will provide valuable information to MSC Support. 10:33: : PHASE1DR 104 (S)DBSETOFF BEGN 10:33: : PHASE1DR 106 (S)PHASE1A BEGN 10:33: : PHASE1A TA BEGN 10:33: : PHASE1A MSGHAN BEGN * 10:33: : PHASE1A (S)SEMG BEGN 10:33: : SEMG ELTPRT BEGN 10:33: : SEMG EMG BEGN 10:33: : SEMG (S)ERRPH BEGN 10:33: : ERRPH (S)PRTSUM BEGN 10:33: : PRTSUM PROJVER BEGN 10:33: : PRTSUM DBDICT BEGN 10:33: : PRTSUM PRTPARM BEGN 10:33: : ERRPH EXIT BEGN 10:33: : XSEMDR END SubDMAPs DMAP MODULES Analysis stops here

Analysis Health Checks

Analysis Health Checks
In the previous section we discussed the CURE: Debugging In this section we discuss PREVENTION Essential QA checks Good Modeling Practice

Essential QA checks Pre Analysis Element Distortion Consistent Units
Use your pre-processor to visually check distortion Use WARNING messages in .f06 to confirm Consistent Units Check with Force = Mass * Acceleration

Essential QA checks (cont.)
Element Distortions Aspect ratio Aspect ratio should be less than about 4:1 (much less in regions where stress levels change rapidly). In cases of nearly-uniaxial stress fields, larger aspect ratios are acceptable. a a b b

Element Distortions Skew Check Quadrilateral elements should be kept as square as possible

Element Distortions Taper Check

Warp Up to ~ 5% is normally acceptable. No real limit, but the element does not include warpage.

Post Analysis Epsilon Value Applied Load Summation Reaction Summation Strain Energy Values Peak Deflections

Post Analysis - Epsilon Value Standard Solution Expression Assumes no Rounding Errors In Practice there is a Residual (This on its own has dimensions) Make it an Energy Term Compare it to the System Energy

If 10-6 ,or greater ,it could be a sign of ill-conditioning. For your type of Structure, Idealization and Analysis Establish typical values for Epsilon Establish an agreed threshold *** USER INFORMATION MESSAGE 5293 (SSG3A) FOR DATA BLOCK KLL LOAD SEQ. NO EPSILON EXTERNAL WORK EPSILONS LARGER THAN ARE FLAGGED WITH ASTERISKS E E+04

Post Analysis - Applied Load Summation Use OLOAD request in Case Control Particularly Important For: Inertia Loading Complex Pressure Loading Complex Distributed Loading

Applied Load Summation
0 RESULTANTS ABOUT ORIGIN OF SUPERELEMENT BASIC COORDINATE SYSTEM IN SUPERELEMENT BASIC SYSTEM COORDINATES. OLOAD RESULTANT SUBCASE/ LOAD DAREA ID TYPE T T T R R R3 FX E E E+05 FY E E E+06 FZ E E E MX E MY E MZ E+00 TOTALS E E E E E E+05 FX E E E+00 FY E E E-10 TOTALS E E E E E E-10 FX E E E+00 FY E E E+05 TOTALS E E E E E E+05

Post Analysis - Reaction Summation Check that sense opposes and balances OLOAD summary

Reaction Load Summation
RESULTANTS ABOUT ORIGIN OF SUPERELEMENT BASIC COORDINATE SYSTEM IN SUPERELEMENT BASIC SYSTEM COORDINATES. SPCFORCE RESULTANT SUBCASE/ LOAD DAREA ID TYPE T T T R R R3 FX E E E+00 FY E E E+05 FZ E E E MX E MY E MZ E+00 TOTALS E E E E E E+05 FX E E E+00 FY E E E-09 TOTALS E E E E E E-09 FX E E E+00 FY E E E+05 TOTALS E E E E E E+05

Actual Applied Load Check
Request printout of applied loads at actual load application points OLOAD = n May produce large output for certain type loadings e.g., gravity load on a large model

Actual Applied Load Check (cont.)

Post Analysis - Strain Energy Values *** USER INFORMATION MESSAGE 5293 (SSG3A) FOR DATA BLOCK KLL LOAD SEQ. NO EPSILON EXTERNAL WORK EPSILONS LARGER THAN ARE FLAGGED WITH ASTERISKS E E+04 Work = ½ Total Force * Total Deflection = ( approx) ½ OLOAD * Peak Deflection ( if peak deflection is near mean line of loading action)

Post Analysis - Peak Deflections Set PARAM,PRTMAXIM,YES to output this The GRID ID is not included, and can be different for each DOF MAXIMUM DISPLACEMENTS T T T R R R3 E E E E E E+00 Value !!! Work = ( approx) ½ OLOAD * Peak Deflection ( 2e3 * 36.5 *.5 = 36.5e3 )

Essential QA checks - Workshop
Run section5_6.bdf Go through the Essential QA checks: Epsilon Value Applied Load Summation Reaction Summation Strain Energy Values Peak Deflections

Good Modeling Practice

Good Modeling Practice
Essentials Mesh Density – fit for purpose Mesh Quality – fit for purpose Loading Boundary Conditions Displacement Boundary Conditions

Good Modeling Practice (cont.)
Mesh Density – fit for purpose

Mesh Quality – fit for purpose

Loading Boundary Conditions Simple Point Loading? Poor stress distribution locally Good stress distribution locally

Loading Boundary Conditions More sophisticated loading?

Displacement Constraint Considerations Wrongly defining Output Coordinate Systems at SPC’s, MPC’s, RIGID Elements etc. can wreck a model Over constraining a model can give rise to Poisson contraction stresses that distort the true stress field. A single nodal constraint (or force) produces a singularity in the stress field - stress results at this point are likely to be erroneous.

Displacement Constraint Considerations A special technique called inertia relief is available to perform quasi-static analysis on unconstrained (free) structures under uniform (i.e., zero or constant) acceleration. Aero Loads Inertia Loads

MultiPoint Constraints, Rigid Elements

Multipoint Constraints
A multipoint constraint (MPC) is a user-imposed linear equation that relates displacement degrees of freedom. MPCs are useful to Define the relative motion between two or more grid points as a degree of freedom Join dissimilar elements; for example, to join elements with rotational degrees of freedom to elements which have only translational degrees of freedom (e.g., to join shell elements to solid elements) Distribute loads to several points in a structure Model rigid connections between grid points

Multipoint Constraints (cont.)
Assume GRID 145 and 146 are forced to move together in x and y ( a bracket may connect them) -1.0*Ux *Ux146 = 0.0 146 -1.0*Uy *Uy146 = 0.0 145 General Form is S ai*Ui= 0.0 where a = constraint coefficient u = displacement degree of freedom

Multipoint Constraints (cont.)
Case Control SUBCASE 1 SUBTITLE=edge MPC = 1 SPC = 2 LOAD = 2 ……. Bulk Data $ SID GRID DOF A1 GRID DOF A2 MPC MPC The first component (C) defined in the equation is considered to be the dependent coordinate and is placed in the Um set. This component cannot belong to any other subset of ug.

Multipoint Constraints Workshop
Rework section5_4.bdf Use an MPC to remove the singularity, rather than an SPC 0.25 0.25

R-TYPE ELEMENTS MSC.Nastran contains several commonly used MPC relationships defined in the form of various R-type elements. To avoid possible errors, it is strongly recommended that the user who is unfamiliar with writing MPC equations use rigid elements whenever possible. Unlike MPCs, R-type elements are not selected in the Case Control. They are defined only in the Bulk Data on the following entries:

RIGID ELEMENTS RBAR - Rigid bar with six degrees of freedom at each end RBE2 - A rigid body connected to an arbitrary number of grid points RBE3 - Defines a constraint relation in which the motion at a “reference” grid point is the weighted average of the motions at other grid points

RIGID ELEMENTS (cont.) RSPLINE Defines a constraint relation whose coefficients are derived from the deflections and slopes of a flexible tubular beam connected to the referenced grid points RSSCON Used to connect plate elements to solid elements See Section 2.10 of the MSC/NASTRAN Application Manual for 10 examples that use rigid elements and two examples that use MPCs.

RIGID ELEMENTS (cont.) RBAR Example
The explicit MPC in section5_4.bdf could be replaced by an RBAR Internally MPC equations are created

RIGID ELEMENTS (cont.) RBAR EXAMPLE
An RBAR is preferred over creating a ‘stiff beam’ as it has no relative stiffness side effects $ RBAR Creation $ $ ID GRID1 GRID2 DOF1 DOF2 RBAR

RIGID ELEMENTS (cont.) RBE2 Example
The explicit MPC in section5_4.bdf could be replaced by an RBE2 Internally MPC equations are created Acts like a rigid ‘spider’

The DOF at the centre of the ‘spider’ is the Independent DOF The others are Dependent DOF’s and must not be cross coupled

RIGID ELEMENTS (cont.) RBE2 Example RBE2 method SPC method
RBE2 constrains the ‘backing structure’

RIGID ELEMENTS (cont.) RBE2 Examples
Connect in a component approximation Engine Block Antennae Dish Connect different mesh regions Detailed fitting in a shaft

The explicit MPC in section5_4.bdf could be replaced by an RBE3 Mathematically very complex – a single dependent moves as a average of multi independents Acts like a soft ‘spider’

The DOF at the centre of the ‘spider’ is the Dependent DOF The others are Independent DOF’s and can be cross coupled

RIGID ELEMENTS (cont.) RBE3 Examples
Connect in a component approximation Antennae Dish – flexible backing structure Connect different mesh regions Fuselage beam to shell – flexible ovalisation of fuselage Connect Payload Smears payload to required attachments

RIGID ELEMENTS Workshop
Use file section5_3.bdf Modify to try out: RBAR RBE2 RBE3 Compare the displacement distributions

RIGID ELEMENTS RSSCON Example Solid to Shell Connection Writes MPC’s

RIGID ELEMENTS (cont.) RSSCON Example – Element Method

RIGID ELEMENTS (cont.) RSSCON Example – GRID Method 109 102 47 108 46
101 RSSCON,110,GRID,46,101,102,47,108,109

RIGID ELEMENTS Workshop
Use file section5_4.bdf Modify to try out: RSSCON – GRID RSSCON - ELEMENT Compare the displacement distributions

Useful Model Summary Information

ELSUM The ELSUM Case Control command provides a summary description of the requested elements Output includes Element ID Material ID Length or thickness Area Volume Structural Mass Non-Structural Mass Total Mass Total Weight

ELSUM Format: ELSUM = I Limitations:
Where I – a set number or ‘ALL’ Limitations: Mass data is produced only for CBAR, CBEAM, CBEND, CHEXA, CONROD, CPENTA, CQUAD4, CQUAD8, CQUADR, CROD, CSHEAR, CTETRA, CTRIAR, CTRIA3, CTRIAX6, and CTUBE elements

MAX/MIN DISPLACEMENT AND SPCFORCE OUTPUT
In SOL 101, there is an option to obtain MAX/MIN output summaries by SUBCASE for displacements and SPC forces If requested, this output is in addition to the standard output

$ file maxmin.dat sol 101 cend title = cantilever beam model subtitle = OLOAD OUTPUT spc = 1 disp=all maxmin(vmag=2,disp,spcf)=all subcase 1 label = pload1 load = 1 subcase 2 label = load in x, y, and z load = 2 begin bulk pload1,1,1,fy,fr,0.,1.,1.,1. =,=,*(1),== =(6) force,2,9,,1.,1.,1.,1. PARAM GRDPNT 0 PARAM POST -1 $ cord2r,1,,0.,0.,0.,0.,1.,0. ,1.,0.,1. GRID GRID GRID GRID GRID GRID GRID GRID GRID $ CBEAM CBEAM CBEAM CBEAM CBEAM CBEAM CBEAM CBEAM SPC PBEAML BAR MAT ENDDATA GRID point 9 uses CORD2R 1 for output

*** T1 *** D I S P L A C E M E N T M A X / M I N V A L U E S U M M A R Y RESULTS FOR SUBCASE MAXMIN OPTIONS: SET=ALL, CID=BASIC, VMAG=2, VMAG=2, COMP=T1 POINT ID. TYPE CID ***TMAG*** T T R R R3 1 G BASIC E E E E E E+00 2 G BASIC E E E E E E+00 8 G BASIC E E E E E E+00 9 G BASIC E E E E E E+00 9 G E E E E E E+00 1 CANTILEVER BEAM MODEL FEBRUARY 13, MSC.NASTRAN 1/17/01 PAGE 12 OLOAD OUTPUT *** R1 *** D I S P L A C E M E N T M A X / M I N V A L U E S U M M A R Y RESULTS FOR SUBCASE MAXMIN OPTIONS: SET=ALL, CID=BASIC, VMAG=2, VMAG=2, COMP=R1 POINT ID. TYPE CID T T T ***RMAG*** R R3 Maximum Translations Displacements in System 1 for GRID 9 Maximum Rotations Vector Magnitude for GRID 9

Element Geometry Checks

Pre-processors are notorious for generating elements with bad geometry (aspect ratio, taper, warp, skew, etc) In the past, there was a separate message for each element which did not satisfy the recommendations for MSC.Nastran (this often resulted in pages upon pages of messages which most users ignored) There is now an option which provides user-control of these messages (so if you want to ignore them, you can disable their printout – NOT RECOMMENDED) This is done by the GEOMCHECK executive control statement

Structural Symmetry Reflective symmetry can often be employed in the modeling process to reduce the cost of the analysis.

Structural Symmetry (cont.)
The following example demonstrates the use of symmetric modeling techniques to analyze the frame. Full Model

Symmetric Model SUBCASE 1 2500 lb P P 2 2 2 3 SPC DOF 1,5,6 at Grid Point 3 for symmetry 1 Y X

Anti-Symmetric Model SUBCASE 2 Displaced Shape 2500 lb 2 3 SPC DOF 2,3,4 at Grid Point 3 for antisymmetry 1 Y X

D SYM,EX TIME 5 SOL 101 CEND $ TITLE =EXAMPLE OF USING SYMMETRY/ANTISYMMETRY CONSTRAINTS DISP = ALL $ SUBCASE 1 LABEL = SYMMETRY CONSTRAINTS SPC = LOAD = 1 $ SUBCASE 2 LABEL = ANTISYMMETRY CONSTRAINTS SPC = LOAD = 1 $ SUBCOM 3 LABEL = LEFT SIDE OF MODEL SUBSEQ 1.0, 1.0 $ SUBCOM 4 LABEL = RIGHT SIDE OF MODEL SUBSEQ 1.0, $ BEGIN BULK $ GRID GRID GRID $ CBAR CBAR PBAR $

MAT E $ FORCE $ SPC SPC $ ENDDATA

SUBCASE SUBCASE = SUBCOM 3

SUBCOM 4 results in the displaced shape of the right side of the model. B C - = SUBCASE 1 - SUBCASE 2 = SUBCOM 4

The output for SUBCOM3 and SUBCOM 4 represent the full model.

Blank Page

Section 5 Model Verification.

Similar presentations

Presentation on theme: "Section 5 Model Verification."— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

Section 5 Model Verification.

Similar presentations

Presentation on theme: "Section 5 Model Verification."— Presentation transcript:

Similar presentations

About project

Feedback