Скачать презентацию

Идет загрузка презентации. Пожалуйста, подождите

Презентация была опубликована 2 года назад пользователемДарья Тихомирова

1 S5-1NAS105, Section 5, May 2005 SECTION 5 MODEL CHECKOUT

2 S5-2NAS105, Section 5, May 2005

3 S5-3NAS105, Section 5, May 2005 TABLE OF CONTENTS SectionPage COMMON TYPES OF ERRORS………………………………………………………………..5-5 COMMON MODELING ERRORS……………………………………………………………….5-7 DIAGNOSIS OF A NEW MODEL – PARAMs …………………………………………………5-8 DIAGNOSIS OF A NEW MODEL – DIAGs ……………………………………………………5-9 F04 OUTPUT………………………………………………………………………………………5-10 DIAG 8 F04 OUTPUT – MATRIX TRAILERS………………………………………………….5-11 SPECIAL OUTPUTS…………………………………………………………………………… GRID POINT STRESS AND STRESS DISCONTINUITIES………………………………….5-13 SURFACE DATA………………………………………………………………………………….5-14 MINIMUM RECOMMENDED MODEL CHECKS………………………………………………5-15 STIFFNESS MATRIX CHECKS…………………………………………………………………5-22 OUTPUT FROM ground_check_1a…………………………………………………………… DESCRIPTION OF ground_check_1a OUTPUT………………………………………………5-27 ground_check_1b-MODEL WITH A BAD ELEMENT………………………………………….5-30 OUTPUT FROM ground_check_1b…………………………………………………………… RESULTS OF ground_check_1b………………………………………………………………..5-33

4 S5-4NAS105, Section 5, May 2005 TABLE OF CONTENTS (CONT) SectionPage ground_check_1c – MODEL WITH A BAD MPC………………………………………………5-34 ground_check_1c – IMPROPER MPC………………………………………………………….5-35 OUTPUT FROM ground_check_1c…………………………………………………………… DISCUSSION OF ground_check_1c RESULTS………………………………………………5-38 ground_check_2a – MODEL ERROR………………………………………………………… HOW TO AVOID SERIOUS MODELING MISTAKES……………………………………… CHECK FOR BAD MODES………………………………………………………………………5-41 SOME ADDITIONAL DEBUGS FOR DYNAMICS…………………………………………….5-42 SAMPLE OF SHRINK PLOTS………………………………………………………………… SOME RECOMMENDATIONS………………………………………………………………….5-44

5 S5-5NAS105, Section 5, May 2005 COMMON TYPES OF ERRORS n Mistakes in engineering judgment n Approximations to physical behavior u Engineering theory u Finite element theory u Finite element implementation u Modeling l Bolted connection l Welded connection l Corners l Transitions n Modeling errors u Connections l Beam to plate l Beam to solid l Plate to solid u Beam orientation u Beam releases u Loading (how well do you know the loading yourself?)

6 S5-6NAS105, Section 5, May 2005 COMMON TYPES OF ERRORS (CONT) n Finite element error n Round-off error (can be disastrous when it occurs) u Computers use binary arithmetic (If you enter.1, internally it may be ) n Program bugs (nobodys perfect) u A list of known errors is maintained and distributed Eternal Vigilance is the Price of a Good Analysis

7 S5-7NAS105, Section 5, May 2005 COMMON MODELING ERRORS n Plates not lining up = zipper n Any connections depending on in-plane rotational stiffness of plates, or any rotational stiffness on solids n Instabilities – for example, releasing both ends of a beam in torsion n Offsets of elements in wrong coordinate system (should be in the output coordinate systems of the grid points for Bars and Beams) n Member properties wrong (beam orientation) – also plates – membrane only – left out bending n Beam end releases – are they local or global n Element force output is normally in element coordinate system

8 S5-8NAS105, Section 5, May 2005 DIAGNOSIS OF A NEW MODEL - PARAMs PARAMOperation AUTOSPC, EPPRT, MAXRATIOCheck relative magnitudes of matrix terms FIXEDBSolve superelements individually Statics = fixed-boundary solution Dynamics = calculated component modes IRESLoad Error GRDPNTCheck mass, CG, M. Moment of Inertia USETPRTPrint set tables SESEFStrain energy fractions (superelements – SOL 103) TINYMinimum percentage value of element strain energy forprintout (Values not printed are not available for post-processing)

9 S5-9NAS105, Section 5, May 2005 DIAGNOSIS OF A NEW MODEL - DIAGs DIAGOperation 8Print matrix trailers 14Print DMAP listing 15Print table trailers 56List Qualifier changes as the solution progresses – also, list all DMAP statements executed on the.f04 file (normally only modules are listed) n MSC.NASTRAN DATA BLOCK NAME CONVENTION FOR MATRICES whereY = type: A, D, 4I,J = col, row sets K = stiffnessM = mass B = viscous dampingG = transformation D = rigid body transformationU = displacement P = loadQ = force of constraint

10 S5-10NAS105, Section 5, May 2005 n Prints matrix trailers as the matrices are created DAY TIME ELAPSED I/O SEC DEL_I/O CPU SEC DEL_CPU SUB_DMAP/DMAP_MODULE MESSAGES 16:56:390: SEPREP217GP1BEGN 16:56:400: SEPREP217GP1END subDMAP Elapsed Time for Job (used for time limit) Wall Clock – Elapsed Seconds F04 OUTPUT: Time Log and DMAP Trace Format Time of Day File Operations DMAP Sequence ID Module Name

11 S5-11NAS105, Section 5, May 2005 DIAG 8 F04 OUTPUT – Matrix Trailers n Sample printout using DIAG8 n Definitions F(orm)1=square, 2=rectangle, 3=diagonal, 6=symmetric, etc. T(ype)1=single precision real, 2=double precision real, 3=single precision complex, 4=double precision complex NzwdsLargest Number of nonzero words among all columns Den Density, (number of nonzero terms) (Rows x Columns)) BlockTNumber of GINO blocks (1 block = buffsize -1 words) DAY TIMEELAPSEDI/O MBDEL_MBCPU SECDEL_CPUSUB_DMAP/DMAP_MODULE MESSAGES 14:16:23 0: SEMG 28 EMG BEGN *8** Module DMAP Matrix Cols Rows F T NzWds Density BlockT StrL NbrStr EndAvg BndMax NulCol EMG 28 KELM D *8** 14:16:24 0: SEMG 111 EMG BEGN *8** Module DMAP Matrix Cols Rows F T NzWds Density BlockT StrL NbrStr EndAvg BndMax NulCol EMG 111 KJJM D *8**

12 S5-12NAS105, Section 5, May 2005 SPECIAL OUTPUTS Strain energy densityESE – use to determine where to make changes most efficiently. Grid point forcesGPFORCE – use to trace loads thru the structure and verify load paths. Stress sortingPARAMS: S1, NUMOUT, BIGER, SRTOPT Grid point stressesGPSTRESS Stress DiscontinuitiesGPSDCON, ELSDCON

13 S5-13NAS105, Section 5, May 2005 GRID POINT STRESS AND STRESS DISCONTINUITIES (ALL CASE CONTROL) n Use GPSTRESS, ELSDCON, or GPSDCON to select surfaces and volumes. n Use OUTPUT (POST) or SETS DEFINITION with u SURFACE data to define surfaces u VOLUME data to define volumes SURFACE Entry Definition

14 S5-14NAS105, Section 5, May 2005 SURFACE DATA n Recommendations for discontinuous structures u Use tolerance and branch tests to handle discontinuous stresses u Use local coordinate systems for orientation u Use GEOMETRIC method when element sizes differ u Try dividing into smaller surfaces u Use several options in one run and compare them n Remember that the elements are isoparametric, that is, ideal elements are mapped onto the real elements in the model. If the grid point stresses differ when different options are used (or if the discontinuities are too large), it may indicate any of the following conditions: u Mesh too coarse u Elements badly shaped u Modeling errors

15 S5-15NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS Pre-Analysis n Understand the structure and the elements u Make small models – understand the problem u Use pilot models in areas of uncertainty u If you are not familiar with using the element type or SOLution you expect to use, make simple models and compare the answers to theoretical results (with a simple model, you should be able to obtain excellent correlation with theoretical results). n Model checks before the analysis u Geometry l Pre-processor (or Undeformed plots) n Look at connections between different element types u Based on knowledge of elements u Based on loads u Look at corners (QUAD plates) n Shrink plots

16 S5-16NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) n Elements u Beam and bar l Check that I1 and I2 have proper orientation and values l Check all end releases (in member coordinates) l Verify all offsets (in output coordinate system of GRIDs) l Material – need E, (or G), and u Plates and Shells l Check aspect ratios, taper, and warpage l Check orientation – Z, surfaces consistent l Check attachments – especially any depending on in-plane rotational stiffness, any corners, and shells l Verify any offsets (in element coordinate system) l Material – need E, (or G), and l Property entry – be sure to get the correct properties. (One of the most commonly made errors is not specifying MID2 for bending plates

17 S5-17NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) n Solids u Check aspect ratios u Check taper u Check attachments. If any attachments depend on rotational stiffness, special modeling effort is required u Material – need E, (or G), and n Mass properties u Check on MATi entries u Check NSM on property entries l Bars, beams = mass/unit length l Plates = mass/unit area u Submit with PARAM, GRDPNT, xxxx where xxxx = ID of GRID point to calculate mass properties about l Always check center of gravity and total weight (mass) versus known values

18 S5-18NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) n Loadings: u Verify they are correct (OLOAD RESULTANT) n Constraints: u Verify that they are defined (often they are forgotten) u Verify they are correct (location and orientation – in output coordinate system of the GRID points) u Verify that they are applied (SPC CASE CONTROL command) n Static Checks – ALWAYS RUN STATICS FIRST!!! u Apply 1–g in X, Y, and Z directions independently l Check load paths (GPFORCE) l Check reactions (SPC FORCE) n Does total = applied load? n Are the reactions at the correct locations and do they have the correct orientation? l In Dynamics, approximate frequency: where d = center of gravity displacement in direction of applied g-load g = acceleration due to gravity

19 S5-19NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) n Equilibrium check – verify model is not over- constrained u Run free-free. Remove known constraints and check for unconstrained motion under applied loads or imposed displacements. or u Use the Case Control Command GROUNDCHECK, to check for over-constrained systems. u Thermal equilibrium check – if thermal loads are to be considered. u Check on MATi entries u Check for unconstrained thermal expansion – on a copy of your model l Apply a determinate set of constraints l Use the same for all materials l Apply a uniform T to the structure. It should expand freely, that is, with no reactions, element forces, or stresses

20 S5-20NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) After the Analysis n Statics u Check EPSILON and MAXRATIO l Epsilon > may indicate trouble l MAXRATIO > 10 6 may indicate trouble u Check reactions. Do they equal the applied loads ( applied loads are printed as OLOAD RESULTANT in superelement solutions)? u Check load paths – use grid point force balance to trace loads l Check stress contours for consistency n Sharp corners indicate bad modeling n Use different options (i.e., topological and geometric) and compare results n Check stress discontinuities n Compare values to hand calc or small model results

21 S5-21NAS105, Section 5, May 2005 MINIMUM RECOMMENDED MODEL CHECKS (CONT) n Dynamics – normal modes u Check frequencies. Are they in the expected range? (Did you forget WTMASS???) l If free-free, are there six rigid-body (f=0.0) modes? l Are there any mechanisms (f=0.0)? n More than six rigid-body modes in free-free? n Any rigid-body modes in constrained modes? u Check mode shapes, and Identify modes l Plots and/or animation l Effective weight and kinetic energy (Case Control Commands MEFFMASS and EKE) help to identify significant modes

22 S5-22NAS105, Section 5, May 2005 STIFFNESS MATRIX CHECKS n The model (stiffness and mass matrices) should be checked to verify that the elements are not (obviously) bad and that the model is not over- constrained u Sample – CELASi between non coincident points or CELASi to ground n This check can be performed at various stages during the analysis – at each stage, a potential problem is checked u G-set – at this stage of the solution, the elements (including GENELs and K2GG) are checked for grounding u N-set – at this stage, the MPC equations are checked u A-set – (free-free only) check that the SPCs do not over-constrain the structure n Use the Case Control Control Command GROUNDCHECK

23 S5-23NAS105, Section 5, May 2005 STIFFNESS MATRIX CHECKS n Sample Model 1 – Cantilever Beam n Properties: I1 = 10 I2 = 10 J = 5 A = 1 E = 10,000,000. =.3 =.1 WTMASS =

24 S5-24NAS105, Section 5, May 2005 STIFFNESS (AND MASS) CHECKS (CONT) SOL 103 CEND TITLE = Cantilever Beam Modeled with 8 CBAR elements GROUNDCHECK=YES SUBCASE 1 SUBTITLE=Default LABEL = Perform Model Checks METHOD = 1 SPC = 1 VECTOR(SORT1,REAL)=ALL BEGIN BULK MAT PBAR, 1, 1, 1., 10., 10., 5. CBAR, 1, 1, 1, 2, 0., 1., 0. CBAR, 2, 1, 2, 3, 0., 1., 0. CBAR, 3, 1, 3, 4, 0., 1., 0. CBAR, 4, 1, 4, 5, 0., 1., 0. CBAR, 5, 1, 5, 6, 0., 1., 0. CBAR, 6, 1, 6, 7, 0., 1., 0. CBAR, 7, 1, 7, 8, 0., 1., 0. CBAR, 8, 1, 8, 9, 0., 1., 0. GRID GRID GRID GRID GRID GRID GRID GRID GRID PARAM GRDPNT 0 PARAM WTMASS PARAM AUTOSPC YES SPC EIGRL 1 5 ENDDATA Input File: ground_check_1a.dat

25 S5-25NAS105, Section 5, May 2005 OUTPUT FROM ground_check_1a CANTILEVER BEAM WITH 8 CBAR M O D E L S U M M A R Y NUMBER OF GRID POINTS = 9 NUMBER OF CBAR ELEMENTS = 8 O U T P U T F R O M G R I D P O I N T W E I G H T G E N E R A T O R REFERENCE POINT = 0 M O * E E E E E E+00 * * E E E E E E+00 * * E E E E E E+00 * * E E E E E E+00 * * E E E E E E+00 * * E E E E E E+01 * S * E E E+00 * * E E E+00 * * E E E+00 * DIRECTION MASS AXIS SYSTEM (S) MASS X-C.G. Y-C.G. Z-C.G. X E E E E+00 Y E E E E+00 Z E E E E+00 I(S) * E E E+00 * * E E E+00 * * E E E+00 * I(Q) * E+00 * * E+00 * Q * E E E+00 * * E E E+00 * * E E E+00 *

26 S5-26NAS105, Section 5, May 2005 OUTPUT FROM ground_check_1a (CONT) *** USER INFORMATION MESSAGE 7570 (GPWG1D) RESULTS OF RIGID BODY CHECKS OF MATRIX KGG (G-SET) FOLLOW: PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF E-01 DIRECTION STRAIN ENERGY PASS/FAIL E-09 PASS E-08 PASS E-08 PASS E-10 PASS E-06 PASS E-06 PASS SOME POSSIBLE REASONS MAY LEAD TO THE FAILURE: 1. CELASI ELEMENTS CONNECTING TO ONLY ONE GRID POINT; 2. CELASI ELEMENTS CONNECTING TO NON-COINCIDENT POINTS; 3. CELASI ELEMENTS CONNECTING TO NON-COLINEAR DOF; 4. IMPROPERLY DEFINED DMIG MATRICES; *** SYSTEM INFORMATION MESSAGE 6916 (DFMSYN) DECOMP ORDERING METHOD CHOSEN: BEND, ORDERING METHOD USED: BEND *** USER INFORMATION MESSAGE 5010 (LNCILD) STURM SEQUENCE DATA FOR EIGENVALUE EXTRACTION. TRIAL EIGENVALUE = D+08, CYCLES = D+03 NUMBER OF EIGENVALUES BELOW THIS VALUE = 2 *** USER INFORMATION MESSAGE 5010 (LNCILD) STURM SEQUENCE DATA FOR EIGENVALUE EXTRACTION. TRIAL EIGENVALUE = D+10, CYCLES = D+04 NUMBER OF EIGENVALUES BELOW THIS VALUE = 6 R E A L E I G E N V A L U E S MODE EXTRACTION EIGENVALUE RADIANS CYCLES GENERALIZED GNERALIZED NO. ORDER MASS STIFFNESS E E E E E E E E E E E E E E E E E E E E E E E E E+10

27 S5-27NAS105, Section 5, May 2005 DESCRIPTION OF ground_check_1a OUTPUT n Grid Point Weight Output (GPWG module) u The scale factor entered with parameter WTMASS is applied to the assembled element mass before GPWG. The GPWG module, however, converts mass back to the original input units that existed prior to the scaling effect of the parameter WTMASS u GPWG is performed on the g-size mass matrix, which is the mass matrix prior to the processing of the rigid elements, MPCs, and SPCs u Any masses at scalar points and fluid-related masses are not included in the GPWG calculation u GPWG for a superelement does not include the mass form upstream superelements. Therefore, GPWG for the residual structure includes only the mass of the residual (not any upstream superelements). The center of gravity location is also based on the mass of the current superelement only u The output from the GPWG is for information purposes only and is not used in the analysis u The rigid-body mass matrix [MO] is computed with respect to the reference grid point in the basic coordinate system. The Grid point to be used is specified using PARAM, GNDPNT u For further information see the MSC.NASTRAN Linear Static Analysis Users Guide (V2001), Appendix B

28 S5-28NAS105, Section 5, May 2005 DESCRIPTION OF ground_check_1a OUTPUT (CONT) n Stiffness Check Output u These checks are performed by multiplying the stiffness matrix by a set of rigid-body vectors(R b ) which are based on the geometry (calculated about PARAM, GRDPNT) u The rigid-body strain energy checks are calculated as (note that the factor of ½ is not included in the calculation) u This check is performed on the G-, N-, A-set matrices (i in CHKii is the set being checked) u If any term in the resulting CHK matrix exceeds the value of PARAM, CHECKTOL (default value is calculated based in the stiffness of your model), the results of the check are printed u Reaction forces are calculated, normalized to a minimum of 1.0, filtered, and printed (if CHECKTOL is exceeded)

29 S5-29NAS105, Section 5, May 2005 DESCRIPTION OF ground_check_1a OUTPUT (CONT) n Stiffness Check Output (Cont.) u Note that full data recovery is not performed, and if a DOF which does not belong to the remaining set is constrained, the nearest point (by connection) in the remaining set is indicated. See results for CHKKAApoint 1 is constrained, but does not belong to the A- set, therefore, the constraint shows up at point 2 n Mass Check Output u These checks are performed by multiplying the mass matrix by a set of rigid-body vectors(R b ) which are based on the geometry (calculated about PARAM, GRDPNT) u The calculation is similar to that performed on the stiffness matrix u The results at the G-set should match Grid Point Weight Generator u The checks at the N- and A-set check if MPCs and constraints remove (or re-distribute) mass

30 S5-30NAS105, Section 5, May 2005 Ground_check_1b – MODEL WITH A BAD ELEMENT n Same model as before, only now connect a CELAS2 element between DOF 2 at Grid Points 2 and 3 (this will cause grounding), as the direction of the stiffness terms is not along the line connecting the GRID points) n Samples of CELASi elements which cause grounding Connected to Ground Geometric mismatch K to ground

31 S5-31NAS105, Section 5, May 2005 STIFFNESS CHECKS (CONT) SOL 103 CEND TITLE = Cantilever Beam with 8 CBAR + 1 CELAS2 GROUNDCHECK=YES SUBCASE 1 SUBTITLE=Default LABEL = Perform Model Checks METHOD = 1 SPC = 1 VECTOR(SORT1,REAL)=ALL BEGIN BULK MAT PBAR, 1, 1, 1., 10., 10., 5. CBAR, 1, 1, 1, 2, 0., 1., 0. CBAR, 2, 1, 2, 3, 0., 1., 0.. CBAR, 8, 1, 8, 9, 0., 1., 0. $ Add a CELAS2 incorrectly specified CELAS2, 99, 1000., 2, 2, 3, 2 GRID GRID GRID PARAM GRDPNT 0 PARAM WTMASS PARAM AUTOSPC YES SPC EIGRL 1 5 ENDDATA Input File – ground_check_1b.dat

32 S5-32NAS105, Section 5, May 2005 OUTPUT FROM ground_check_1b CANTILEVER BEAM WITH 8 CBAR + 1 CELAS2 *** USER INFORMATION MESSAGE 7570 (GPWG1D) RESULTS OF RIGID BODY CHECKS OF MATRIX KGG (G-SET) FOLLOW: PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF E-01 DIRECTION STRAIN ENERGY PASS/FAIL E-09 PASS E-08 PASS E-08 PASS E-10 PASS E-06 PASS E+02 FAIL SOME POSSIBLE REASONS MAY LEAD TO THE FAILURE: 1. CELASI ELEMENTS CONNECTING TO ONLY ONE GRID POINT; 2. CELASI ELEMENTS CONNECTING TO NON-COINCIDENT POINTS; 3. CELASI ELEMENTS CONNECTING TO NON-COLINEAR DOF; 4. IMPROPERLY DEFINED DMIG MATRICES; R E A L E I G E N V A L U E S MODE EXTRACTION EIGENVALUE RADIANS CYCLES GENERALIZED GNERALIZED NO. ORDER MASS STIFFNESS E E E E E E E E E E E E E E E E E E E E E E E E E+10

33 S5-33NAS105, Section 5, May 2005 RESULTS OF ground_check_1b n At the G-set, the structural matrices are grounded when the alter attempts to rotate the model about the z-axis n This is indicated by the large term in the CHKKGG matrix for DOF 6 n By looking at the REACGNRM matrix – this matrix represents the forces (normalized to a maximum of 1.0) preventing the model from moving as a rigid body. The column associated with DOF 6 (z-rotation) contains terms for DOF 2 of grid points 2 and 3, indicating that a modeling error exists in that area n This is the location of the CELAS2

34 S5-34NAS105, Section 5, May 2005 Ground_check_1c – MODEL WITH A BAD MPC n Same model as before, only now connect an MPC between DOF 2 at Grid Points 2 and 3 (since the points are not coincident, this will cause grounding) n The MPC states that the y-direction translation of the Grid Point 2 must equal the y-direction translation of Grid Point 3

35 S5-35NAS105, Section 5, May 2005 Ground_check_1c – IMPROPER MPC SOL 103 CEND TITLE = Cantilever Beam with 8 CBAR, and 1 MPC GROUNDCHECK(SET=(G,N))=YES SUBCASE 1 SUBTITLE=Default LABEL = Perform Model Checks METHOD = 1 MPC = 1 SPC = 1 VECTOR(SORT1,REAL)=ALL BEGIN BULK MAT PBAR, 1, 1, 1., 10., 10., 5. CBAR, 1, 1, 1, 2, 0., 1., 0. CBAR, 2, 1, 2, 3, 0., 1., 0.. CBAR, 8, 1, 8, 9, 0., 1., 0. $ Add an MPC Equation (incorrectly specified) MPC, 1, 2,2,1., 3, 2, -1. GRID GRID GRID PARAM GRDPNT 0 PARAM WTMASS PARAM AUTOSPC YES SPC EIGRL 1 5 ENDDATA Input File: ground_check_1c.dat

36 S5-36NAS105, Section 5, May 2005 OUTPUT FORM ground_check_1c CANTILEVER BEAM WITH 8 CBAR, AND 1 MPC *** USER INFORMATION MESSAGE 7570 (GPWG1D) RESULTS OF RIGID BODY CHECKS OF MATRIX KGG (G-SET) FOLLOW: PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF E-01 DIRECTION STRAIN ENERGY PASS/FAIL E-09 PASS E-08 PASS E-08 PASS E-10 PASS E-06 PASS E-06 PASS *** USER INFORMATION MESSAGE 7570 (GPWG1D) RESULTS OF RIGID BODY CHECKS OF MATRIX KNN (N-SET) FOLLOW: PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF E-01 DIRECTION STRAIN ENERGY PASS/FAIL E-09 PASS E-08 PASS E-08 PASS E-10 PASS E-06 PASS E+08 FAIL SOME POSSIBLE REASONS MAY LEAD TO THE FAILURE: 1. MULTIPOINT CONSTRAINT EQUATIONS WHICH DO NOT SATISFY RIGID-BODY MOTION; 2. RBE3 ELEMENTS FOR WHICH THE INDEPENDENT DEGREE-OF-FREEDOM CANNOT DESCRIBE ALL POSSIBLE RIGID-BODY MOTIONS.

37 S5-37NAS105, Section 5, May 2005 OUTPUT FORM ground_check_1c (Contd.) CANTILEVER BEAM WITH 8 CBAR, AND 1 MPC R E A L E I G E N V A L U E S MODE EXTRACTION EIGENVALUE RADIANS CYCLES GENERALIZED GNERALIZED NO. ORDER MASS STIFFNESS E E E E E E E E E E E E E E E E E E E E E E E E E+10

38 S5-38NAS105, Section 5, May 2005 Discussion of ground_check_1c Results n At the G-set, the structural matrices pas the rigid-body tests, since the CELAS2 which caused the problem in ground_check_1b has been removed. n Matrix KNN fails the rigid-body test due to the incorrectly- specified MPC equation. This is indicated by the large term in the CHKKNN matrix at DOF 6. n By looking at the REACNCOL matrix – this matrix represents the forces (normalized to a maximum of 1.0) preventing the model from moving as a rigid body. The 6 th column contains terms for GRID points 1 and 3, indicating that a modeling error exists in that area. n This is the location of MPC (NOTE – since the test is performed on the N-set, GRID 2 DOF 2 no longer exists, since it is in the M-set and has been removed).

39 S5-39NAS105, Section 5, May 2005 Ground_check_2a – MODEL ERROR SOL 101 CEND TITLE = Groundcheck for an Inclined Rod ECHO = SORT GROUNDCHECK(GRID=1, SET=(G,N+AUTOSPC))=YES SUBCASE 1 SUBTITLE=Default SPC = 1 LOAD = 1 DISPLACEMENT(SORT1,REAL)=ALL SPCFORCES(SORT1,REAL)=ALL STRESS(SORT1,REAL,VONMISES,BILIN)=ALL BEGIN BULK MAT PROD CROD CROD FORCE, 1, 3, 0, 1000., , 0.5, 0. GRID GRID GRID PARAM AUTOSPC YES PARAM GRDPNT 0 SPC SPC ENDDATA Input File: ground_check_2a.dat Question: What is wrong with this rod model?

40 S5-40NAS105, Section 5, May 2005 HOW TO AVOID SERIOUS MODELING MISTAKES n Take the time to understand the structure and how it behaves under load. Perform hand analysis or use a simple model first. n Take the time to understand MSC.NASTRAN (particularly the elements). Run small samples each time you try something new. n Use independent checks (if available). n Estimate the cost (labor and computer costs) before you start.

41 S5-41NAS105, Section 5, May 2005 CHECK FOR BAD MODES n Identify your modes using one or more of the following: u Plot your eigenvectors (either using the MSC.NASTRAN plotter or MSC.PATRAN) and identify them u Try setting NORM=MAX on EIGRL entry and look at modal masses. Small values may indicate singularities or local modes (not recommended). u Use Case Control Commands EKE, and MEFFMASS to print kinetic energy and modal effective mass. n Watch for warnings on orthogonality checks n Look for extraneous low frequency modes – these often indicate incorrect modeling (for example plate elements without MID2 on the PSHELL entry)

42 S5-42NAS105, Section 5, May 2005 SOME ADDITIONAL DEBUGS FOR DYNAMICS n In dynamic analysis, use normal modes as a diagnostic tool n Simulate statics in modal dynamic solutions and compare the results to a static solution (this is a way to determine if your nodes are capable of representing the solution) u In Transient analysis, apply a constant loading, and damping u In frequency response, apply the load at 0.0 Hz, and remove structural damping n Use sssalter modevala.vxx to see if your modes can represent the solution if the loads are applied statically (although you are looking at a dynamic solution, it is hard for the modes to represent the dynamic solution under loading if they cannot represent the static solution) n Selecting time or frequency set selection can have a major impact on the solution accuracy u In Transient response, the accuracy is directly related to the integration time step (A central difference is used to calculate the velocity and acceleration). If you are using a direct solution, run using different integration time steps to see if the answers change u In Frequency Response, the peak responses normally at or near occur at resonance. Use a modal solution with FREQ3, FREQ4, and/or FREQ5 entries to guarantee that the solution is obtained with reasonable accuracy near the resonance frequencies.

43 S5-43NAS105, Section 5, May 2005 SAMPLE OF SHRINK PLOTS Stiffened Plate with Error in Modeling

44 S5-44NAS105, Section 5, May 2005 SOME RECOMMENDATIONS n Understand the important things BEFORE you get into trouble!!! u Understand your structure and how you expect it to perform u Understand your loading u Understand your model u Understand how to use the program u Understand the limitations of the method u Use simple sample problems (preferably with known solutions) to understand the MSC.Nastran solution. n ALWAYS perform a static solution first, then progress to the more complicated solutions.

Еще похожие презентации в нашем архиве:

Готово:

WS2-1 WORKSHOP 2 NORMAL MODES ANALYSIS OF A 2 DOF STRUCTURE NAS122, Workshop 2, August 2005 Copyright 2005 MSC.Software Corporation.

WS2-1 WORKSHOP 2 NORMAL MODES ANALYSIS OF A 2 DOF STRUCTURE NAS122, Workshop 2, August 2005 Copyright 2005 MSC.Software Corporation.

© 2017 MyShared Inc.

All rights reserved.