3.3.2. Apply Large Numerical Damping Over a Short Interval This technique is of a more general nature and uses numerical damping to eliminate errors or numerical noise due to inconsistent initial conditions. After the noise has been damped out over several substeps, you can perform the actual transient analysis with smaller numerical damping. Some potential drawbacks exist in cases where high frequency content of flexible multibody systems is im- portant for analysis. Applying high numerical damping in the dummy analysis can affect the desired high- frequency response. ANSYS recommends using the HHT method for this technique because the integration scheme shows good dissipation properties with numerical damping. Example Consider a rigid-flexible double pendulum made up of a rigid and a flexible beam. One end of the rigid beam is pinned and the other end is hinged to the flexible beam. The other end of the flexible beam is free. The rigid beam is assumed to have all of its mass concentrated at the end that is hinged to the flexible beam. The system is given an initial velocity tangential to the flexible beam axis at its free end, as shown in the following input file: Transient Analysis of a Rigid-Flexible Double Pendulum /title,Transient analysis of a rigid-flexible double pendulum /prep7 et,1,mass21 keyopt,1,3,2 !3d mass without rotary inertia et,2,mpc184 keyopt,2,1,1 !rigid beam keyopt,2,2,1 !lagrange multiplier et,3,mpc184 keyopt,3,1,6 !revolute joint between rigid and flexible beam et,4,beam188 !flexible beam n,1,0.0,0.0 !pinned (supported) end of rigid beam n,2,1.0,0.0 !hinged end of rigid beam (node 2) n,3,1.0,0.0 !hinged end of flexible beam n,4,1.25,0.0 n,5,1.5,0.0 n,6,1.75,0.0 n,7,2.0,0.0 !free end of flexible beam (node 7) type,1 real,1 m = 390 r,1,m en,1,2 !3d mass at the end of rigid beam type,2 real,2 en,2,1,2 !rigid beam local, 11, 0, 0.0, 0.0, 0.0, , , 90 sectype, 3, JOIN, REVO, TESTREVO secjoin, , 11, 11 type,3 real,3 secnum,3 en,3,3,2 !revolute joint mp,ex,1,2e11 !material properties for flexible beam mp,nuxy,1,0.3 mp,density,1,7.8e3 sectype,4,beam,csolid secdata,1,0.1784124116 !c-s area is 0.1 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 36 Chapter 3: Performing a Multibody Analysis type,4 real,4 secnum,4 mat,1 en,4,3,4 !flexible beam elements en,5,4,5 en,6,5,6 en,7,6,7 d,1,all ddel,1,rotz finish /solu vel = 6.2831853072 !tangential velocity ic,7,uy,0.0,vel !initial condition for velocity antype,trans time,0.1 kbc,1 nlgeom,on nsub,50,50,50 !use multiple substeps trnopt,full, , , , ,HHT !use HHT time integration tintp,0.2 !use high numerical damping outres,all,all solve time,6.0 midtol,on,10 !automatic time stepping with MIDTOL nsub,100,1e6,100 trnopt,full, , , , ,HHT tintp,0.05 !small numerical damping for HHT outres,all,all solve finish /post26 nsol,2,7,u,x,ux !x displacement for node 7 nsol,3,7,u,y,uy !y displacement for node 7 nsol,4,2,u,x,ux1 !x displacement for node 2 nsol,5,2,u,y,uy1 !y displacement for node 2 nsol,4,3,v,x,vx !x velocity for node 7 nsol,5,3,v,y,vy !y velocity for node 7 nsol,6,7,a,x,ax !x acceleration for node 7 nsol,7,7,a,y,ay !y acceleration for node 7 /axlab,x,Time T /axlab,y,D/V/A /gropt,divx,10 /gropt,divy,10 /gthk,curve,2 /title,Transient analysis of a rigid-flexible double pendulum plvar,ux,uy,ux1,uy1,vx,vy,ax,ay finish 3.4. Damping You can specify two types of damping in ANSYS: 3.4.1. Numerical Damping 3.4.2. Structural Damping 37 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 3.4. Damping 3.4.1. Numerical Damping Numerical damping is associated with the time-stepping schemes used for integrating second-order systems of equations over time. ANSYS provides the Newmark method and the HHT method for transient dynamic analysis of structural systems. Numerical damping for these schemes is determined by the parameter values specified via the TINTP command. Numerical damping stabilizes the numerical integration scheme by damping out the unwanted high frequency modes. For the Newmark method, numerical damping also affects the lower modes and reduces the accuracy of integration scheme from second order to first order. For the HHT method, numerical damping affects only the higher modes and always maintains second-order accuracy. ANSYS uses a default value (TINTP,GAMMA) of 0.005. The value that you select should be based on the problem at hand. A sensible value to try initially is 0.1. Use the lowest possible value that damps out non- physical response without significantly affecting the final solution. Problems involving rigid body translational motion, other forms of damping, or dissipative mechanisms like plasticity or friction typically require smaller values for numerical damping. Larger numerical damping values are usually necessary for problems involving rigid body rotational motion, elastic collisions (dynamic contact/impact), and large deformations with frequent changes in substep size. 3.4.2. Structural Damping Structural damping refers to physical damping present in the system. You can specify the damping at the material level via viscous material models or dashpots (for example, COMBIN14 elements). At the structural level, you can specify it as modal damping or Rayleigh damping. For more information, see Damping in the Structural Analysis Guide. 3.5.Time-Step Settings Transient dynamic analyses involving large deformations or large rotations exhibit significant changes in stiffness and inertia properties. The default response-frequency-based automatic time-stepping criterion may not be suitable for such nonlinear analyses. Use the MIDTOL command to automatically adjust the time increment based on convergence at the middle of the substep and convergence at the end of the substep. For more information, see "Nonlinear Structural Analysis" in the Structural Analysis Guide. 3.6. Solver Options Multibody analyses generally involve large rotations in static or transient dynamics analysis, so nonlinear geometric effects must be accounted for. To do so, issue the NLGEOM,ON command. For faster convergence in a full transient dynamic analysis where mass elements such as MASS21 are used, issue the NROPT,UNSYM command. The command activates the Newton-Raphson option for solving the nonlinear equations in the analysis, necessary due to the nonsymmetric stiffness contribution resulting from gyroscopic effects. Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 38 Chapter 3: Performing a Multibody Analysis Chapter 4: Reviewing Multibody Analysis Results Results from a flexible multibody analysis consist mainly of displacements, velocities, accelerations, stresses, strains, and reaction forces in structural components. Constraint forces, current relative positions, relative velocities, and relative accelerations in joint elements are also available. Results are available for viewing in POST1, the general postprocessor ( /POST1), or in POST26, the time-history postprocessor (/POST26). For a description of the available output components, see the Output Data sections of the element descriptions for any of the elements that model the flexible components, rigid components, and joint elements. The following topics concerning how to review flexible multibody analysis results are available: 4.1. Reviewing Results in POST1 4.2. Reviewing Results in POST26 4.3. Output of Joint Element Quantities 4.4. Energy Output 4.1. Reviewing Results in POST1 In the POST1 general postprocessor, only one substep at a time can be read, and the results from that substep must exist in the Jobname.RST file. The load step option command OUTRES controls which substep results are stored in Jobname.RST. To review results in POST1: • The database must contain the same model for which the solution was calculated. • The Jobname.RST results file must be available. A typical POST1 postprocessing sequence follows: CommandCommentsActionStep If not, you will likely not wish to postpro- cess the results, other than to determine Verify from your output file (Jobname.OUT) whether 1. why convergence failed. If your solution the analysis converged at all load steps. converged, then continue postpro- cessing. /POST1If your model is not currently in the data- base, first issue a RESUME command. Enter the POST1 postpro- cessor. 2. SETYou can identify them by load step and substep numbers or by time. Read the results for the de- sired load step and substep. 3. Use any of these options: View the results.4. PLDISPDisplay the deformed shape. PLNSOL or PLESOL Display contours of stresses, strains, or any other applicable item. 39 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. CommandCommentsActionStep Optional: Examine tabular listings. PRNSOL (nodal results), PRESOL (ele- ment-by-ele- ment results), PRRSOL (reac- tion data), PRITER (substep summary data, etc.) ANTIMEOptional: Animate the motion of the flexible multibody mechanism results over time. Many other postprocessing functions are available in POST1. For more information, see "The General Post- processor (POST1)" in the Basic Analysis Guide. Load case combinations are not usually applicable to nonlinear analyses. 4.2. Reviewing Results in POST26 You can review the load-history response of a nonlinear structure using POST26, the time-history postprocessor (/POST26). Use POST26 to compare one ANSYS variable to another. For example, you could graph the relative rotation of a joint element versus time or any other variable. A typical POST26 postprocessing sequence for a flexible multibody analysis is similar to the sequence for a typical nonlinear analysis, as follows: CommandCommentsActionStep Do not base design decisions on uncon- verged results. If your solution converged, continue postprocessing. Verify from your output file (Jobname.OUT) whether the analysis converged at all load steps. 1. /POST26If your model is not currently in the data- base, first issue a RESUME command. Enter the POST26 postpro- cessor. 2. The SOLU command causes various itera- tion and convergence parameters to be Define the variables to be used in your postprocessing session. 3. NSOL, ESOL, read into the database, where you can RFORCE incorporate them into your postpro- cessing. Graph or list the variables.4. PLVAR (graph), PRVAR (list), EXTREM (list) Many other postprocessing functions are available in POST26. For more information, see "The Time-History Postprocessor (POST26)" in the Basic Analysis Guide. Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 40 Chapter 4: Reviewing Multibody Analysis Results 4.3. Output of Joint Element Quantities Several joint element output quantities are available for review purposes. You can use either POST1 or POST26, or both, to review those results. The solution output associated with the element is in two forms: • Nodal displacements included in the overall nodal solution • Additional element output to the results file listed below The following output is available for joint elements as SMISC quantities: • Constraint forces and moments • Constraint forces (moments) if stop is specified • Constraint forces (moments) if lock is specified • Stop status • Lock status • Relative position • Constitutive displacements and rotations • Joint elastic forces (moments) • Joint damping forces (moments) • Joint friction forces (moments) • Relative displacement and rotations (cumulative) • Relative velocities • Relative accelerations • Average temperature in the element The following output is available for joint elements as NMISC quantities: • The components of the bases vectors at the two nodes in the deformed configuration. The bases vectors are specified as the local coordinate systems via the SECJOINT command and evolve with the rotation of the underlying nodes. • The constraint forces and moments in the evolved basis at the first node of the joint element. The ANSYS Workbench Products generally use NMISC output for postprocessing. See the MPC184 element documentation and the individual joint element descriptions for details about the SMISC component specification and the use of the ETABLE command. In POST1, you can print joint element output (such as relative reaction forces, relative displacements, relative rotations, etc.) at the free or unconstrained relative degree of freedom via the PRJSOL command. To obtain the nodal forces at the joint element nodes, issue the PRESOL,FORC command. In POST26, you can use the JSOL command to specify result items (such as relative displacements, velocities, accelerations, etc.) that must be stored for a joint element. Then, you can plot or print the stored items via the PLVAR or PRVAR command, respectively. 41 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 4.3. Output of Joint Element Quantities 4.4. Energy Output You can monitor the total energies of the entire model in POST1 via the PRENERGY command. The total energy consists of elastic, kinetic, artificial hourglass/drill stiffness energy, and so on. In POST26, you can use the ENERSOL command to store a specific energy item. Then, you can graph or list the specific energy item in the output file via the PLVAR or PRVAR command, respectively. Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 42 Chapter 4: Reviewing Multibody Analysis Results Chapter 5: Using Component Mode Synthesis Superelements in a Multibody Analysis Obtaining the flexible response of a body or bodies to a dynamic motion event typically involves solving hundreds or thousands of time points. If a flexible body has many degrees of freedom (DOFs), a multibody analysis can be time-consuming. To minimize the necessary computing resources, you can use component mode synthesis (CMS) superelements (substructures) to replace the many thousands of DOFs of the flexible body with tens of DOFs that represent the dynamic response, thereby significantly reducing the required multibody analysis run time. The following topics describe the approach required to perform a substructure-based multibody analysis, including recovering the time-dependent flexible response: 5.1. Applicability of CMS Superelements in a Multibody Analysis 5.2. Flexible Body Types 5.3. Substructuring Overview 5.4. Master Degrees of Freedom in a Substructured Multibody Simulation 5.5. Steps for Performing a Substructured Multibody Simulation For an example of how to set up and use a substructuring in a multibody analysis, see Chapter 6, Example Multibody Analysis: Crank Slot Mechanism (p. 53). 5.1. Applicability of CMS Superelements in a Multibody Analysis The flexible body to be substructured is assumed to behave in a linear elastic manner, as follows • Only linear materials are allowed. • Nonlinear elements within the body (such as gasket or contact elements) are treated as linear and in their initial state. • The body may consist only of 3-D structural elements. (You can use 2-D elements with care provided that you follow the guidelines given later, particularly with respect to the number of DOFs at the master DOFs.) • Element formulations using Lagrange multipliers are not allowed. • Density or mass of some form must be present in the body. The body may undergo large rotations, but the strains and relative rotations within the body are presumed to be small. 5.2. Flexible Body Types A multibody simulation supports two types of flexible bodies: • Bodies that are excited by the motion of other bodies (rigid or flexible) but do not themselves undergo large motions 43 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. An engine block is an example of this type, where the block is excited dynamically from the crankshaft, pistons, and other moving parts attached or linked to the block. This case is a straightforward application of traditional superelements. • Bodies that are undergoing large motions A piston rod is an example of a body undergoing large motions; this type also uses superelements but with the additional capability that the superelement can undergo large motions, and large rotations in particular. A large-rotation superelement involves additional considerations. 5.3. Substructuring Overview Substructuring is a technique that condenses a group of finite elements into a single element represented as a matrix. The single-matrix element is called a superelement. You can use the superelement in an analysis as you would any other ANSYS element type. Substructuring requires three passes: • A generation pass, where the group of elements are condensed down to generate the superelement. • A use pass, where the superelement is used in the analysis. In our case, in the multibody analysis. • An expansion pass, where the results of the superelement in the use pass are expanded to the original group of elements so that their displacements, forces, strains, and stresses are recovered. In the use pass, ANSYS allows the superelement to rotate with arbitrarily large rotations. In the generation pass, you define master degrees of freedom (MDOFs). The MDOFs are the DOFs that the superelement uses to interface with, or connect to, the other bodies or joints. Because the flexible body analysis occurs within a dynamic analysis, you must include the dynamic (mass) effects. Use component mode synthesis (CMS) to augment the superelement static stiffness with mode shapes that characterize the dynamic behavior, much as you would when performing a mode-superposition transient dynamic analysis. CMS is a form of substructure analysis allowing you to derive the dynamic behavior of the entire assembly from its constituent components. For more information, see "Component Mode Synthesis" in the Advanced Analysis Techniques Guide. 5.4. Master Degrees of Freedom in a Substructured Multibody Simulation The master degrees of freedom (MDOFs) are the degrees of freedom (DOFs) of the superelement which you intend to use to connect to the DOFs of the remaining bodies and joints. Because you almost always use all the DOFs of a node in the definition of the MDOFs, you can think in terms of master “nodes”; that is, the MDOFs are the nodes of the superelement that connect to the nodes of the remaining joints and bodies. If the connection occurs at a joint at the center of a hole or slot, you must place a master node there. For more information, see Connecting Bodies to Joints (p. 28). Nonrotating Bodies For nonrotating bodies, master nodes are located at the points where the superelement connects with the other bodies and are typically located at the centers of bolts or other fasteners and bearings. Try to minimize the number of master nodes. Where appropriate, use the techniques presented in Connecting Bodies to Joints (p. 28) to create a single master node that connects to a number of nodes. Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 44 Chapter 5: Using Component Mode Synthesis Superelements in a Multibody Analysis Rotating Bodies For rotating bodies, the idea is to create a beam-like superelement, ideally with two master nodes (but never less than two). You can use more than two master nodes (for example, when modeling a lever or rocker plate), but ANSYS assumes that the rotation of the superelement is the average of the rotations of all master nodes. All master nodes of a rotating body must have six active structural DOFs: UX, UY, UZ, ROTX, ROTY, and ROTZ. If the master node does not have six DOFs for example, if it is the node of a 3-D solid element create a six-DOF node at that location and tie it to the rest of the body appropriately. You can use either of the fol- lowing techniques, both of which essentially place a six-DOF node connected to a patch of elements super- imposed on the existing solid elements. • MPC Contact Create a pilot node and link it to bonded contact elements overlaid on the patch. For more information, see Connecting Bodies to Joints (p. 28). • Beams Overlay beam elements or MPC184 Rigid Beam elements in a “spider web” fashion. The beams should have high stiffness and no mass. Following is an illustration of both methods: When “rotating” the created node, the body rotates accordingly. You can also define MDOFs where loads are to be applied as well as at any points where velocities or accel- erations are of interest. 5.5. Steps for Performing a Substructured Multibody Simulation The methodology for performing a substructured multibody simulation assumes that you have generated the entire finite element model of the multibodies including the joints using ANSYS Workbench, for example- -and want to take advantage of substructuring to reduce the solution time. ANSYS refers to this method as a top-down approach (as opposed to a bottom-up approach of defining the substructure first and then building the rest of the model around it). Using substructures to represent some or all of the flexible bodies in a completely defined multibody model requires the following steps: 5.5.1. Step 1: Prepare the Full Model for a Substructured Multibody Analysis 5.5.2. Step 2: Create the Substructures (Generation Pass) 5.5.3. Step 3: Build the CMS-based Model (Use Pass) 5.5.4. Step 4: Run the Multibody Analysis 5.5.5. Step 5: Expand all Solutions (Expansion Pass) 5.5.6. Step 6: Create the Merged Results File 5.5.7. Step 7: Postprocess the Results 45 Release 12.0 - © 2009 SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 5.5. Steps for Performing a Substructured Multibody Simulation . Pass) 5. 5.4. Step 4: Run the Multibody Analysis 5. 5 .5. Step 5: Expand all Solutions (Expansion Pass) 5. 5.6. Step 6: Create the Merged Results File 5. 5.7. Step 7: Postprocess the Results 45 Release. defined multibody model requires the following steps: 5. 5.1. Step 1: Prepare the Full Model for a Substructured Multibody Analysis 5. 5.2. Step 2: Create the Substructures (Generation Pass) 5. 5.3 response: 5. 1. Applicability of CMS Superelements in a Multibody Analysis 5. 2. Flexible Body Types 5. 3. Substructuring Overview 5. 4. Master Degrees of Freedom in a Substructured Multibody Simulation 5. 5.