Chapter 4 Nonlinear Diagnostics Nonlinear Diagnostics Chapter Overview

Chapter 4 Nonlinear Diagnostics

Nonlinear Diagnostics Chapter Overview Training Manual • The following will be covered in this section: – Solver Output – Monitoring the Solution – Newton-Raphson Residuals • The capabilities described in this section are generally applicable to ANSYS Structural licenses and above. ANSYS Workbench – Simulation • Since some nonlinear structural analyses can be challenging to solve, understanding how to diagnose nonconvergence problems is critical in obtaining answers. – Exceptions will be noted accordingly February 4, 2005 Inventory #002177 4 -2

Nonlinear Diagnostics A. Solution Information – Recall that with the Solution Information branch, the detailed Solver Output from ANSYS can be reviewed, and convergence graphs, such as the Force Convergence behavior, can be plotted. Text Output Graphical Output ANSYS Workbench – Simulation • In Chapter 2 Section D, the Solution Information branch was introduced Training Manual February 4, 2005 Inventory #002177 4 -3

Nonlinear Diagnostics … Solver Output Overview Training Manual 1) The beginning of the Solver Output simply shows the ANSYS license used (in this case, ANSYS Multiphysics/LS-DYNA) and the version number. ANSYS Workbench – Simulation • The Solver Output can provide detailed text output about the solution. It is useful to become familiar with how to read this file. February 4, 2005 Inventory #002177 4 -4

Nonlinear Diagnostics … Solver Output Overview Training Manual This listing is useful, as will be shown later, because it not only provides information on how many parts are in the model, but the Contact Region ID numbers are listed here It is instructive to note that while Contact Regions can be given any name in Simulation, the ANSYS solver treats each Contact Region with a unique number (ID). For debugging purposes, it is useful to find out which Contact Region has which ID number. For example, in the above snippet, Contact Region “Teeth 3” is referenced by contact ID 9 and 10. ANSYS Workbench – Simulation 2) Upon scrolling down until a series of asterisks are encountered, the reading of the finite element data by the solver can be seen. February 4, 2005 Inventory #002177 4 -5

Nonlinear Diagnostics … Solver Output Overview Training Manual The useful things to review here are the equation solver used (if left at “Program Chosen” or manually specified), whether large deflection effects are on or off, whether nonlinear material effects are considered (if plasticity is present), and the number of substeps used. ANSYS Workbench – Simulation 3) When the equation solution is initiated, the section of the output will be shown as on the right The review of this section of the Solver Output is not critical, but it indicates when the matrices are being solved and what the solution options specified in Simulation were. February 4, 2005 Inventory #002177 4 -6

Nonlinear Diagnostics … Solver Output Overview Training Manual Here, various options related to contact elements, including the contact Normal Stiffness and Pinball Radius will be listed Any NOTE or WARNING messages printed in this section are useful to review. For example, initial penetration or gaps (in active unit length) will be shown in this area Recall from Solver Section 2 that the Contact Region name and the contact set ID are listed. From that example, we know that the above contact set 9 is part of “Teeth 3” region. ANSYS Workbench – Simulation 4) Details of contact elements are then printed next. February 4, 2005 Inventory #002177 4 -7

Nonlinear Diagnostics … Solver Output Overview Training Manual • Note that for each equilibrium iteration, the residual forces (FORCE CONVERGENCE VALUE) must be lower than the CRITERION • Ideally, the residual or out-of-balance forces should be zero for a system to be in equilibrium. However, because of machine precision and practical concerns, Simulation determines a value small enough to result in negligible error. This value is the CRITERION, and the FORCE CONVERGENCE VALUE must be smaller than the CRITERION for the substep to be converged. • In the example below, after 3 equilibrium iterations, the residual forces are lower than the criterion, so the solution is converged. • Informative messages (such as convergence or bisection) are noted with “>>>” and “<<<“ in the output. ANSYS Workbench – Simulation 5) As the nonlinear solution progresses, the equilibrium iteration information is shown at the bottom (sample below) February 4, 2005 Inventory #002177 4 -8

Nonlinear Diagnostics … Solver Output Overview Training Manual • When contact status changes abruptly, this is just a warning indicating that the contact elements enter or exit the ‘pinball region’ drastically. This may be due to parts sliding or separating drastically if the load is too high. Simulation may automatically bisect the solution, if necessary. • Element distortion messages are usually severe problems due to excessive loading or over-constraints. Bisection of the load is automatically performed, but sometimes corrective measures may need to be taken to fix the problem. ANSYS Workbench – Simulation Warning and error messages will also be printed in the output February 4, 2005 Inventory #002177 4 -9

Nonlinear Diagnostics … Solver Output Overview Training Manual The percentage of solver time used for contact vs. other elements can be determined here, including equation solver time. The very end shows the CPU time and the total wall time. ANSYS Workbench – Simulation 6) Lastly, after the solution has completed, the very end of the Solver Output provides some statistics on the analysis run. • If wall time is much larger than CPU time (such as 2 x) for a single processor, then that shows that much of the computational time may have been affected by slow disk I/O. • If dual processors are used, the CPU time will not be as accurate, as it is the sum of the time used by both processors. February 4, 2005 Inventory #002177 4 -10

Nonlinear Diagnostics … Solver Output Summary Training Manual – Users can review the Solver Output during solution to find detailed information of the current equilibrium iteration – The Solver Output can be reviewed after solution to determine reasons for non-convergence (if the solution had failed), to obtain information on solver performance, and find out specifics of contact element settings – Detailed warnings or error messages (marked with ***), if present, will also be printed in the Solver Output. Also, during solution, review of the substep status (denoted with >>>) will show the reasons for bisection, if any. ANSYS Workbench – Simulation • Becoming familiar with the contents and structure of the Solver Output can be very useful in understanding the finite element solution February 4, 2005 Inventory #002177 4 -11

Nonlinear Diagnostics B. Monitoring the Solution Training Manual – If the solution seems to be behaving unexpectedly, the user can stop the analysis and investigate the problem rather than wait until the solution is complete. This helps to save time. – Monitoring the solution also helps the user gain an understanding into the response of the system • There are two ways in which users can monitor the solution in Simulation: – Solution Information branch to provide equation solver behavior ANSYS Workbench – Simulation • While solving a nonlinear model, because many iterations may be needed, it is useful to see what the nonlinear solution trends are – Results Tracker to provide response of system during the solution February 4, 2005 Inventory #002177 4 -12

Nonlinear Diagnostics … Force Convergence Training Manual – As shown in the previous section, the Force Convergence graph is available from the Solution Information branch Recall that, in the Newton-Raphson method, force equilibrium is sought. If the out-of-balance (residual) forces is below the force criterion, the substep is assumed to be converged. During solution, one can review the Force Convergence graph to monitor the progress. The top Force Convergence graph shows that a bisection occurred. This means that a smaller load increment needed to be applied. The bottom “TIME” graph represents the fraction of total load. Although Time has no significance in a static analysis, it is used as a counter where Time=1. 0 is the final solution. If the Time is currently 0. 2, that means that 20% of the load is being applied. ANSYS Workbench – Simulation • The most useful way to evaluate the solution convergence behavior is to view the Force Convergence graph: February 4, 2005 Inventory #002177 4 -13

Nonlinear Diagnostics … Force Convergence Training Manual – This usually indicates either that (a) a smaller increment of the load should be applied or (b) contact Normal Stiffness may be too high. – Simulation will take care of case (a) by bisecting the solution – If the reason is related to case (b), either bisection or manually lowering the contact Normal Stiffness will help. ANSYS Workbench – Simulation • One common item is when the force convergence starts to “plateau” during solution February 4, 2005 Inventory #002177 4 -14

Nonlinear Diagnostics … Results Tracker – The Results Tracker enables users to monitor deformation at a vertex and/or contact region information during the solution. – For “Results Tracker > Deformation, ” select a vertex of interest and specify whether x, y, or z deformation is to be monitored. – For “Results Tracker > Contact, ” a pull-down menu enables users to select a contact region. Then, the quantity to track (such as number of contacting elements) can be displayed. ANSYS Workbench – Simulation • Besides monitoring the out-of-balance forces, a Results Tracker is available from the “Solution Information” branch Training Manual February 4, 2005 Inventory #002177 4 -15

Nonlinear Diagnostics … Results Tracker Training Manual In this example, the number of contacting elements is monitored for a particular contact region. As is apparent in the graph on right, between Time=1. 4 and 1. 7, the number of contacting elements jumps from zero to 29. Since “Time” is a “placeholder” in a nonlinear static analysis, this means that, after the first load step (Time=1. 0), between 40% and 70% of the load, contact is established. ANSYS Workbench – Simulation • After the Results Tracker items are requested and solution initiated, users may “track” the deformation or contact results during the course of the solution. February 4, 2005 Inventory #002177 4 -16

Nonlinear Diagnostics … Results Tracker Training Manual In this case, the penetration of eight Contact Regions is shown One can review whether maximum penetration is too great – if so, the solution can prematurely be stopped, and the Normal Stiffness of the appropriate Contact Region increased since the user knows which Contact Region has too much penetration. Also, from this, if the user expects the Contact Region “Radial” to come into contact, but that is not reflected while monitoring, the user will also know what results to review after solution is complete. In this example, Contact Regions “Teeth 1 -4” are in contact by the second substep. “Teeth 7” doesn’t seem to come into contact until the fourth substep. This shows the user during solution what Contact Regions are engaging and when. ANSYS Workbench – Simulation • Several items (of a similar type) may also be selected and reviewed at once during solution February 4, 2005 Inventory #002177 4 -17

Nonlinear Diagnostics C. Newton-Raphson Residuals Training Manual • In the event that non-convergence is encountered, the Newton-Raphson Residuals are very useful in locating possible problem areas – If the solution does not converge because of force equilibrium, this will be reflected in the Solver Output and Force Convergence graph. The Force Convergence (residuals) will be greater than the Force Criterion. – In this situation of non-convergence, the Newton-Raphson Residuals (if requested) will show which areas had high force residuals. This usually helps to pinpoint what locations prevented force equilibrium, usually either because of the Load and Supports at that location or because of Contact Region settings. ANSYS Workbench – Simulation • So far, obtaining detailed solver information (Section A) and monitoring the solution (Section B) have been discussed. February 4, 2005 Inventory #002177 4 -18

Nonlinear Diagnostics … Newton-Raphson Residuals Training Manual ANSYS Workbench – Simulation – In the “Solution Information” details view, enter the number of equilibrium iterations to retrieve Newton-Raphson Residuals. For example, if “ 4” is entered, the residual forces from the last four iterations will be returned if the solution is aborted or does not converge. February 4, 2005 Inventory #002177 4 -19

Nonlinear Diagnostics … Newton-Raphson Residuals Training Manual If a solution fails to converge or is aborted by the user, the requested number of residuals will be available. By looking at the residuals, one can example at which locations out-of-balance forces are high. This helps users identify possible problematic locations, so that corrective action may be taken. ANSYS Workbench – Simulation – After solution is stopped or fails to converge, residuals will be available under the “Solution Information” branch, as shown below. February 4, 2005 Inventory #002177 4 -20

Nonlinear Diagnostics … Newton-Raphson Residuals Training Manual – In this case, the ‘ring’ of high residual forces is part of a contact region, so the user knows where to examine ANSYS Workbench – Simulation • Another example is shown below. The force residuals are high (not in equilibrium), and the Newton-Raphson Residuals allow the user to see what areas may contribute to the high out-of-balance forces February 4, 2005 Inventory #002177 4 -21

Nonlinear Diagnostics D. Example Cases Training Manual – It is impractical to cover all of the different causes for nonconvergence. Instead, some common problems users encounter will be discussed. ANSYS Workbench – Simulation • In the present section, some different scenarios will be briefly covered. Reviewing Solver Output, monitoring the solution, and performing nonlinear diagnostics will be discussed for the different cases February 4, 2005 Inventory #002177 4 -22

Nonlinear Diagnostics … Rigid-Body Motion Training Manual – Insufficient constraints, either with Supports or Contact Regions, may allow for parts to ‘fly off’ into space – The Solver Output may also provide the rigid-body direction ANSYS Workbench – Simulation • A common error message that may appear is “internal solution magnitude limit was exceeded. ” Essentially, this means that rigid-body motion is encountered. February 4, 2005 Inventory #002177 4 -23

Nonlinear Diagnostics … Rigid-Body Motion Training Manual – Another method is to look at contact pairs to see which ones are initially open. Recall that the first part of the Solver Output relates contact ID with Contact Region name. In this example, “contact offset block-2 To contact offset bolt-1” contact region (set #10 and 11) has an initial gap. One can check the model to see whether or not the gap should be there and if it may be causing the rigid-body motion because of lack of initial contact being established. ANSYS Workbench – Simulation – To check what parts are undergoing rigid-body motion, one can perform a free vibration analysis and look for near-zero frequency modes. This can be computationally expensive. February 4, 2005 Inventory #002177 4 -24

Nonlinear Diagnostics … Contact Stiffness Training Manual – A threaded fastener solves the first substep until 20% of the load, but then diverges. ANSYS Workbench – Simulation • Sometimes, contact Normal Stiffness may be too high and contribute to non-convergence February 4, 2005 Inventory #002177 4 -25

Nonlinear Diagnostics … Contact Stiffness Training Manual – By lowering the contact Normal Stiffness and refining the mesh near regions of contact, the problem can be solved Unconverged Newton-Raphson Residuals Converged Solution after Adjustments ANSYS Workbench – Simulation – By looking at the Newton-Raphson residuals, it seems that force balance could not be achieved at areas of Contact Regions. The mesh also looks very coarse February 4, 2005 Inventory #002177 4 -26

Nonlinear Diagnostics … Model Setup Training Manual In this model, Pretension Bolt Loads are present, so there are two load steps. The first load step (preload) converged without problems. The second load step, however, had problems where not even one substep converged. ANSYS Workbench – Simulation • The error message “solver engine was unable to converge on a solution for the nonlinear problem as constrained” can be due to several factors, although it is often a good idea to double-check the model setup if this message is encountered. February 4, 2005 Inventory #002177 4 -27

Nonlinear Diagnostics … Model Setup Training Manual – During the first load step, only one Contact Region is holding the parts together, as shown in the Results Tracker on left. – From the Solver Output on right, the Contact Region holding the parts together has lost contact. This indicates that, most likely, the Loads applied have made the parts lose contact. Things to check: Were other Contact Regions supposed to be in initial contact? Was load magnitude incorrectly applied? Were any other sources of constraint omitted? ANSYS Workbench – Simulation • By examining the Results Tracker and Solver Output, one can determine the cause of nonconergence: February 4, 2005 Inventory #002177 4 -28

Nonlinear Diagnostics E. Tips on Solving the Model Training Manual – Look at Force Convergence graph to see how solution is behaving – Check Solver Output for contact information (are Contact Regions initially in contact? What is the initial gap/penetration, if any? ) and any warnings or errors during solution. – Use Results Tracker to monitor contact information or deformation at vertex. Is the model behaving as expected? – If non-convergence occurs, check Newton-Raphson Residuals to find locations of high residuals, which reflect possible problem areas. Are there Loads or Supports applied in those problem areas, or are the areas part of a Contact Region? Double-check model setup. ANSYS Workbench – Simulation • As shown in the previous section, the following combination of steps help to pinpoint possible sources of non-convergence: February 4, 2005 Inventory #002177 4 -29

Nonlinear Diagnostics … Tips on Solving the Model Training Manual – If plasticity is present and excessive element distortion occurs, try running the model without plasticity first to determine if the material model is the cause of the problem. • If the problem can be isolated to the plasticity material, check the plasticity definition. Does it become perfectly plastic? If so, can a plastic hinge (mechanism) form? Is it possible that elements have such little stiffness that they can distort too much? – For contact problems, duplicate the branch and run the model with Bonded Type contact first to see if the problem can be isolated to the contact definition. ANSYS Workbench – Simulation • If those steps still don’t provide enough information on what the problem is, there are other things that can be done: • If it is contact causing problems and force residuals are too high, change all contact to Pure Penalty and enter a low Normal Stiffness (0. 01 to 0. 1). Try solving the model then – there may be excessive penetration, but if results are obtained, the user can get a sense of how the parts are interacting with contact. February 4, 2005 Inventory #002177 4 -30

Nonlinear Diagnostics … Tips on Solving the Model Training Manual • Chattering information is printed during solution as well as at the end if non-convergence is met – the user can also request Contact Chattering in the Results Tracker. If there is too much chattering, one can switch to Augmented Lagrange method or use the Preprocessing Commands Branch to access chattering controls (FTOLN) for Normal Lagrange contact. ANSYS Workbench – Simulation – If Normal Lagrange Formulation is used for contact, check chattering status. February 4, 2005 Inventory #002177 4 -31

Nonlinear Diagnostics … Summary Training Manual – Oftentimes, it may be better to start simple and add complexity as you go, so that sources of problems can be isolated more readily. Adding lots of complexity to the first analysis can result in wasted time down the road. – Do not randomly change settings. Use recommended settings first, then change contact or solver settings only if there is clear reason to do so, as illustrated in the Solver Output, Results Tracker, or Newton-Raphson Residuals. – Although Contact Regions are automatically created, always verify all Contact/Target surfaces and contact settings to ensure that Contact Regions are defined as expected. Review the detailed contact output in the Solver Output to verify the initial contact status of Contact Regions and what value of the penetration or gap is, if present. ANSYS Workbench – Simulation • Simulation provides many tools in helping users to monitor nonlinear analyses as well as diagnose any problems. February 4, 2005 Inventory #002177 4 -32

Workshop 4 Nonlinear Diagnostics General Troubleshooting

Nonlinear Diagnostics F. Workshop 4 - Nonlinear Diagnostics Goal – In this workshop, our goal is to use the nonlinear diagnostics tools available in Solution Information branch to troubleshoot an advanced nonlinear application. • Model Description 3 D large deflection of spring plate using a frictionless contact pair: – Spring plate – Flat rigid plate – One frictionless contact pair Loads and Boundary Conditions: – Fixed support – Displacement of flat surface into Spring 8 mm ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -34

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Training Manual • Start an ANSYS Workbench session. Browse for and open “Spring_ws 04 A. wbdb” project file. – This project contains a Design Modeler (DM) geometry file “Spring_ws 04 A. agdb” and a Simulation (S) file “Spring_ws 04 A. dsdb”. • Highlight the Model, Spring_ws 04 A. dsdb file and open a Simulation Session. ANSYS Workbench – Simulation Steps to Follow: February 4, 2005 Inventory #002177 4 -35

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Insert a manual contact region (RMB on Contact folder) between curved surface of spring and adjacent flat plate. In Details of Contact Region Window, defining Contact and Target surfaces, choose Frictionless type, Asymmetric behavior and Augmented Lagrange algorithm. Take the defaults for all other options. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -36

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Under the Solution Folder, insert – – – Total Deformation Equivalent Stress Contact Tool (Status, Pressure) • Turn off Weak Springs option • Activate Large Deflection. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -37

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Insert a Solution Information branch which includes – Newton-Raphson Residual feedback on the last three iterations of the run – Results tracker feedback on the contact status (Number of Contacting… and Penetration…) Note: Items in the Solution Information Branch can be monitored during the solution run • Execute SOLVE. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -38

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics The run converges without error. A plot of Total Deformation, however, indicates that results are not correct. – • Review Solution Output Information, Number contacting and Penetration. The Contact has obviously failed to engage, but why? ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -39

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics The run converged in one iteration!. The calculated force convergence value was essentially zero. The maximum DOF increment equals the full displacement applied under “Given Displacement” branch ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -40

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Return to the Solution Information worksheet and examine the contact specifications closely. The most useful feedback in this output is the note about an initial gap existing between the contact and target elements. The contact is initially “Open” Scrolling up the worksheet further, notice that the initial substep size is “ 1”, maximum of “ 10”. This means that the total displacement (8 mm) of the flat plate is applied at the first substep! With the initially open contact status and this large initial displacement, the contact jumps over the target from the start and is never detected. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -41

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Training Manual Return to the Details of Contact Region window and specify the Interface Treatment to “Adjust to Touch”. This option is very useful for small adjustments to close gaps and force a closed contact status at the start of the analysis. • Without changing any other specifications, execute another SOLVE. • Solution now begins a long iteration process. Notice in the updated Solution Information Worksheet that the initial contact adjustment was made to close the gap as expected. ANSYS Workbench – Simulation • February 4, 2005 Inventory #002177 4 -42

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics After numerous iterations which include three bisections to try to overcome converge difficulties, the solution ultimately fails to converge. The feedback from this output indicates a very high calculated Force residual as compared with criteria. • ANSYS Workbench – Simulation • Training Manual In the interest of time, stop the solution prior to this failure. February 4, 2005 Inventory #002177 4 -43

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics In order to achieve a successful convergence, it is necessary to determine the cause of the high residual. One troubleshooting technique that can be useful (especially in very complex models with multiple sources of nonlinearities) is a plot of the Newton. Raphson residual data. In this case, we saved the last three iterations. This plot indicates that the highest Newton-Raphson residual is located at the contact interface. The cause of the convergence difficulty is a contact normal stiffness which is excessive relative to the stiffness of the underlying geometry. This makes the model too sensitive to changes in contact status at this location. A smaller factor on contact stiffness combined with a refined timestep size will prove to be very helpful in reducing this residual force and thereby enhancing convergence. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -44

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Training Manual Return to the Details of Contact window and set a manual stiffness to 1 e-4 • Highlight the Solution Branch and in the Details of Solution window, redefine time step specifications: – – • Turn Auto Time Stepping On Initial Substeps = 10 Minimum Substeps = 5 Maximum Substeps = 25 ANSYS Workbench – Simulation • This will force ANSYS to start initially with 10 substeps and allowing auto time stepping to use a maximum 25 if necessary. February 4, 2005 Inventory #002177 4 -45

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Furthermore, a closer inspection of this region indicates that contact may only be engaging at a relatively few gauss points, aggravating convergence and, if nonlinear materials were active, causing excessive element distortion errors in this location. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -46

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Training Manual To address this, insert strategic mesh sizing of 0. 5 mm to the curved surfaces associated with the contact region (six faces total). The localized mesh refinement adds more contact gauss point in this critical area thereby reducing the iterations to convergence. It also enhances quality of results. • After making these changes, re-execute SOLVE … ANSYS Workbench – Simulation • February 4, 2005 Inventory #002177 4 -47

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Solution now converges in 30 iterations without error and without any bisections. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -48

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Post process results. . . ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -49

Nonlinear Diagnostics … Workshop 4 - Nonlinear Diagnostics Note: Had we not refined the mesh and not included stiffness updating between iterations, the solution would still have converged, but it would have taken 90 iterations and required two bisections toward the end of the given displacement. Also, because of the crude mesh, results at the contacting surface would not have been as accurate. ANSYS Workbench – Simulation • Training Manual February 4, 2005 Inventory #002177 4 -50