MNF GENERATION IN MSC NASTRAN Section 10 MNF GENERATION IN MSC NASTRAN

MNF GENERATION IN MSC NASTRAN What’s in this section MNF Generation in MSC Nastran Importance of FEM Reduction Objective Prerequisites Modal Neutral Files Superelement Definitions General Rules for FE Model Preparation Selecting Attachment Points What is a “Spider-Web?” ADAMSMNF Case Control Units ADMOUT = YES FLEXONLY = NO Residual Vectors Releasing DOF Common MSC DB

Importance of FEM Reduction The purpose of reduction methods is to transform a large sparse matrix via matrix operations into a magnitude smaller dense matrix that still represents the properties of the original matrix. The matrix properties of interest are typically eigenvalues and associated eigenvectors that come from a combination of stiffness [K] and mass [M] matrices. The reduction will be invoked using the MSC Nastran ASETi and QSETi entries. The reduced component modes are transferred from MSC Nastran to ADAMS via a MNF file. This technique reduces the amount of data that needs to be transferred from the FE Analysis to the ADAMS Solver.

Importance of FEM Reduction The Component Mode Synthesis (CMS) method, which is a combination of a constrained modal analysis and static correction mode analysis will be used by MSC Nastran. Only defining the master nodes (without defining the kind of connection or loads) MSC NASTRAN, automatically, applies a modal analysis to the structure. The user defines only the number of modes. Then MSC NASTRAN, automatically, applies a sequence of static analysis on the master nodes, applying a unit load in each direction and calculating the stiffness and mass matrix

Importance of FEM Reduction Objective and Prerequisites Objective Using an existing FEA model used to perform a modal analysis, capture and reduce the modes of the structure down to a set of boundary nodes (points) that can be transferred to ADAMS. The component modes are captured using the MSC Nastran Component Modal Synthesis (CMS) Technique. Prerequisites Mass and C.G. of the Finite Element Model should match actual structure. Stiffness should be accurately characterized in the Finite Element Model. Verify static deflection analysis predictions are within expectations from either test data or hand-calculated results. Verify Eigenvalues (modes), and mode shape predictions are within expected ranges from either test data or hand-calculated results. Review Modal effective mass to ensure all critical modes are captured and included in the Guyan Reduction. Use the MSC Nastran Case Control output request; ‘MEFFMASS (GRID=0)=YES’ output option. Example: If the first critical mode in the Z-direction is the 21st mode (i.e. 50% of modal effective mass), but the Guyan Reduction and subsequent creation of the ADAMS MNF file only extracts the first 20 modes, the first critical Z-direction mode will not be included in the ADAMS Flexible Body simulation. In the scenario above, the user should extract at least 21 modes for transfer to an ADAMS Flex Body simulation.

MODAL NEUTRAL FILES Are: Contain the following information: Binary files Platform independent Contain the following information: Generalized mass and stiffness matrices Nodal masses/inertias Nodal coordinates Inertia invariants Eigenvalues Mode shapes File comments and version information Modal loads/preloads Attachment points Element topology Units Stress/strain modes

SUPERELEMENT DEFINITIONS What is a Superelement? Physical and mathematical representation Physical - substructure: a finite element model of a portion of a structure Mathematical - boundary matrices: loads, mass, damping, and stiffness reduced from the interior points to the exterior or boundary points MSC Nastran allows the use of a residual structure only or any superelement or any part super element to be used as a component for an Adams/Flex flexible body. The user can define the attachment points in MSC Nastran by either defining the component as a superelement, in which case, the physical external (a-set) grids become the attachment points; or for a residual only type model, using standard MSC Nastran ASET Bulk entries to define the attachment points.

SUPERELEMENT DEFINITIONS Three small examples are discussed below that are intended to show salient features of the MSC Nastran/Adams interface. In all, the examples GRID_1, GRID_11, GRID_111, and GRID_121 are to be used as the attachment points for Adams.

SUPERELEMENT DEFINITIONS 1. Flexible body component as a superelement The SPOINT and SEQSET1 bulk entries are used to define the component modes. These entries must specify enough degrees of freedom or modal amplitudes to capture the shape of the component and residual flexibility for any loading conditions. $ The corner grids 1, 11, 111, 121 are the exterior or attachment point grids $ SESET,200,2,THRU,10 SESET,200,12,THRU,110 SESET,200,112,THRU,120 $ SCALAR Point and SEQSET1 to define DOFs to use for component Modes SPOINT,80001,THRU,80010 SEQSET1,200,0,80001,THRU,80010

SUPERELEMENT DEFINITIONS 2. Flexible body component as a residual only run This example represents a MSC Nastran/Adams interface run with the component modeled residual only structure. This is accomplished by use of the ASET1 bulk entry. $ The corner grids 1, 11, 111, 121 are the exterior or attachment point grids $ ASET1,123456,1,11,111,121 $$ $ SCALAR Point and QSET1 to define DOFs to use for component modes $ Include enough for structure shape and capture of residual flexiblity SPOINT,80001,THRU,80050 QSET1,0,80001,THRU,80050

SUPERELEMENT DEFINITIONS 3. Flexible body component as a part superelement This example represents a MSC Nastran/Adams interface run with the component modeled as part super element 200 as defined by the BEGIN BULK SUPER = 200 entry. Grids listed in this section represent the complete component as a substructure. $ $ The corner grids 1, 11, 111, 121 are the exterior or attachment point grids GRID 1 0.0 0.0 0.0 GRID 11 0.0 1.0 0.0 GRID 111 1.0 0.0 0.0 GRID 121 1.0 1.0 0.0 $$ $ SENQSET to define DOFs to use for component modes - must be in main Bulk Data Section. Include enough for structure shape and capture of residual Flexiblity SENQSET 200 50 BEGIN BULK SUPER = 200 $ This PART defines interior grids as superelement 200

General Rules for FE Model Preparation Identify the component of the ADAMS multibody system to be modeled as FLEXIBLE BODY Prepare a single and unique FEM model of it. If many FLEXIBLE BODIES constitute ADAMS multibody system, a single and unique FEM model must be prepared for them. So, for each FLEXIBLE BODY a single and dedicated FEM run must be given. Don’t use FEM model constituted by assembly; each FLEXIBLE BODY must be a single FEM model.

General Rules for FE Model Preparation All of the typical elements of FEM code used for structural analysis model can be used. See the following list for an example: CBAR, CBEAM CQUAD4, CQUADR, CQUAD4FD, CQUAD8 CTRIA3, CTRIAR, CTRIARG, CTRIA6, CTRIM6 CTRIAX6, CTRIAX, CTRIX3FD, CTRIX6FD CONM2 CELAS1, CELAS2 CPENTA, CHEX8, CHEXA, CHEXAFD, CHEXA20F, CHEXAPR, CTUBE, CTETRA CTETPR, CTETR4FD, CTETR10F RBAR, RBE2, RBE3 It’s fundamental to define mass property (density) and material for each of the structural elements. Do NOT define null mass or density element.

General Rules for FE Model Preparation Don’t define Boundary Constraints or Loading condition in the FEM model (do FREE–FREE analysis); they will be completely and freely defined into ADAMS. Define all of interface nodes (MASTER nodes) for boundary constraints or loading condition. It can NOT be possible to define an interface node after that FEM analysis has been performed. It is GOOD to define constraint in an ADAMS model on nodes that are defined as interface node for better accuracy. It is recommended to define a force in an ADAMS model on nodes that are defined as interface node. However it is possible to define force in an Adams model on nodes that are NOT defined as interface nodes. This is particularly useful during early design stage.

General Rules for FE Model Preparation It’s fundamental to define interface nodes ONLY on FEM elements with 6 degrees of freedom. In fact, due to the orthogonalisation procedure of Stiffness and Mass matrices after a modal analysis (Component Mode Synthesis), the MATSER NODES must belong ONLY to the following elements CBEAM don’t use CBAR (only 5 DOFs) CQUADR don’t use CQUAD4 (only 5 DOFs) CTRIAR don’t use CTRIA3 (only 5 DOFs) RBAR and/or RBE2 Each violation at the above rule determines the creation of mnf file TOTALLY UNUSABLE because it doesn’t contain all the needed information.  We suggest using RBAR and/or RBE2 elements. Eventually, define a new node very close to the node of the element that it has been considered as MASTER node; connect this new node with the nodes of the near element using RBAR and/or RBE2 elements. With this workaround, the new node becomes a node with 6 DOFs. Example: Suppose that the MASTER node must belong to solid element. This is not possible (in fact, a solid element has only 3 DOFs): so, create a new node very close to the node of the solid element and connect the new node with three or four nodes of the solid element through RBAR or RBE2. Then define the new node as MASTER node, because now it has 6 DOFs.

SELECTING ATTACHMENT POINTS Attachment points are idealized for attachment by preserving all six DOFs. An attachment point is equivalent to a superelement exterior grid point. Each attachment point normally contributes six modal DOF. A large number of attachment points can result in a large MNF. Example: If you have 50 attachment points you would have 300 additional modes (6 modes/attachment point) in your MNF. If you have 50,000 nodes in your model, the resulting MNF would be approximately 720 MB. 8bytes/DOF * 6 DOFs/node * 50,000 nodes/mode * 300 modes = 720 MB You can always apply joints and forces to any node without it having been identified as an attachment point during the FEA. The nodes with the greatest force interaction should be chosen as attachment points.

WHAT IS A “SPIDER WEB?” Elements surrounding the attachment point. Solid elements require a spider web that connects at least three nodes of the mesh because solid elements have no rotational DOFS. Use spider webs to give the attachment point a full set of stiffnesses. Think of a cylinder with the nodes on the circumference at one end all connected to a single centerline node. RBE3 “spider-web" - The independent nodes are the circumference nodes and are free to move elastically while the centerline dependent node is the average of all of the motions of the circumference. RBE2 “spider-web” - The independent node is the centerline node and the dependent circumference nodes are fixed to it with the same motions. The RBE3 retains the circumferential wave modes at the end whereas the RBE2 will not. RBE3 vs RBE2 What is the difference between using RBE3 and RBE2 elements in MSC NASTRAN? http://simcompanion.mscsoftware.com/infocenter/index?page=content&id=KB8015450

ADAMSMNF CASE CONTROL Starting with v2004 of MSC Nastran, a new ADAMSMNF Case Control command is now available for requesting the MNF file directly in MSC Nastran for Adams/Flex. The MSC Nastran/Adams integration provides an easy method to move from a FE analysis to a system analysis study by providing the direct generation within MSC Nastran of the Adams Modal Neutral File (MNF) required for the Adams/Flex solver. The interface is initiated by the simple MSC Nastran Case Control command ADAMSMNF FLEXBODY=YES and the addition of a Bulk Data entry, DTI,UNITS. DTI,UNITS used to specify the unit system to be used by Adams/Flex.

ADAMSMNF CASE CONTROL ADAMSMNF {FLEXBODY = [NO/YES]} Note: The underlined text indicates default values {FLEXBODY = [NO/YES]} Requests that the MSC Nastran/Adams interface be run. {FLEXONLY = [YES/NO]} Requests data recovery be run or not run after standard DMAP solution. {ADMCHECK = [NO/YES]} Requests diagnostics print {ADMOUT = [NO/YES]} Requests that the FLEXBODY run outputs MSC Nastran OP2 files. {OUTGSTR = [YES/NO]} Controls grid point stress output to OP2 file or MNF or both.

ADAMSMNF CASE CONTROL {OUTGSTRN = [YES/NO]} {OUTSTRS = [NO/YES]} Controls grid point strain output to OP2 file or MNF or both. {OUTSTRS = [NO/YES]} Controls element stress output to OP2 file. {OUTSTRN = [NO/YES]} Controls element strain output to OP2 file. {V1ORTHO = [-1.0/value1]} Lower frequency bound of the Craig-Bampton modes (cycles/unit time) value1 = User specified value of lower bound. {V2ORTHO = [1.0e8/value2]} Higher frequency bound of the Craig-Bampton modes (cycles/unit time) value2 = User specified value of upper bound.

ADAMSMNF CASE CONTROL {MINVAR = [FULL/CONSTANT/PARTIAL/NONE]} Requests the type of mass invariants to be computed. FULL : all nine mass invariants will be calculated. CONSTANT : mass invariants 1, 2, , 6, and 7 will be calculated. PARTIAL : mass invariants 5 and 9 will NOT be calculated. NONE : the ADAMSMNF module outputs ONLY modal data. {PSETID = [NONE, setidplotel, ALL]} Selects a set of elements (including PLOTEL) whose grids are retained in the MNF. Setidplotel : specified in the OUTPUT(PLOT) section of MSC Nastran. ALL : select all the sets defined in the OUTPUT(PLOT) section.

ADAMSMNF CASE CONTROL

UNITS Units must be defined using the DTI entry when generating the MNF file. Adams/View and Solver require units Example:

UNITS

ADMOUT = YES The ADMOUT=YES option is intended for users who plan to import ADAMS results into MSC Fatigue. ASSIGN OUTPUT2=’name.out’ STATUS=UNKNOWN UNIT=20 FORM=UNFORM. To insure compatibility with the Adams OP2-to-MNF translator the MSC Nastran SYSTEM word OP2NEW is automatically set to OP2NEW = 0. This means that any OP2 files generated will have a pre-MSC Nastran 2004 format.

FLEXONLY = NO For PARAM,POST,0 Orthonormalized modes used by Adams available for display in PATRAN and SimXpert. Solution modes computed by MSC Nastran available for display in PATRAN and SimXpert.

RESIDUAL VECTORS Concept of Modal approach { U } = [ f ] {x } Assume response can be represented as a linear combination of calculated modes { U } = [ f ] {x } Number of possible modes = number of degrees of freedom with mass on them Same results as direct if all modes are retained Not practical Defeats purpose of modal approach

RESIDUAL VECTORS where [ f ]r = modes that are retained { U } = [ f ] {x } = [ f ]r {x }r + [ f ]n {x }n where [ f ]r = modes that are retained [ f ]n = modes not retained [ f ]r is usually a small subset of [ f ] Quality of modal solution depends on how well a linear combination of [ f ]r can represent the actual solution due to the applied loads. To compensate for the missing modal content the method of Residual Vectors is recommended and is turned ON by default for most modal solutions

RESIDUAL VECTORS Augment modes with static vectors obtained from static loading The response of the neglected modes tends to be static if these frequencies are high as compared to the excitation frequency As (w/wn) << 1 Excellent approximation of missing modes if the above condition is satisfied Improves modal solutions in all cases Recommended to be included for all response analysis using the modal approach (the default) Supports Superelement Analysis Two eigenvalue tables printed Original eigenvalue table Second eigenvalue table with the additional eigenvalues appended at the end—one for each additional residual vector.

RESIDUAL VECTORS Re-orthogonalization is performed to ensure that linearly dependent vectors are removed Residual vectors can come from the following sources Inertial forces due to rigid body motion Applied loads Structural, viscous, and inertial forces due to enforced motion Forces at user specified discrete degrees of freedom Discrete damping forces due to viscous elements

RESIDUAL VECTORS Residual Vectors can be requested with RESVEC Case Control command Note: By default RESVEC is turned ON

RELEASING DOF Using the RELEASE card in the Bulk Data section you can define degrees-of-freedom for superelement exterior grid points that are not connected to the superelement. SEID Superelement identification number. (Integer > 0) C Component number. (Any unique combination of Integers 1 through 6) Gi Grid point identification numbers. Example: The following statement will remove rotational DOF of attachment grid point 1 $ SESET,200,2,thru,8 RELEASE,200,456,1

COMMON MSC DB Flexible bodies can now be imported directly from an MSC Nastran database without creating an MNF. Advantages: Create several flexible bodies from one MSC DB. Read access time for mode data is quicker than from an MNF. No need for MNF creation. ADAMSMNF case control command is still required. For more information, refer to MSC Simcompanion KB article#KB8018149… AFL-009: MSC Database (MSC DB) for Adams Flexible Body http://simcompanion.mscsoftware.com/infocenter/index?page=content&id=KB8018149

exercises Perform Workshop 10 “Procedure to Create a Flex Body with MSC Nastran” in your exercise workbook.