Nonlinear Diagnostics ANSYS Workbench

50 slides
4.8 MB
532 views

Presentation Transcript

1

Nonlinear DiagnosticsChapter 4

2

Chapter OverviewSince some nonlinear structural analyses can be challenging to solve, understanding how to diagnose non-convergence problems is critical in obtaining answers. 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. Exceptions will be noted accordingly

3

A. Solution InformationIn Chapter 2 Section D, the Solution Information branch was introduced 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.

4

… Solver Output OverviewThe Solver Output can provide detailed text output about the solution. It is useful to become familiar with how to read this file. 1) The beginning of the Solver Output simply shows the ANSYS license used (in this case, ANSYS Multiphysics/LS-DYNA) and the version number.

5

… Solver Output Overview2) Upon scrolling down until a series of asterisks are encountered, the reading of the finite element data by the solver can be seen. 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.

6

… Solver Output Overview3) When the equation solution is initiated, the section of the output will be shown as on the right 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. 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.

7

… Solver Output Overview4) Details of contact elements are then printed next. 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 areaRecall 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.

8

… Solver Output Overview5) As the nonlinear solution progresses, the equilibrium iteration information is shown at the bottom (sample below) 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.

9

… Solver Output Overview Warning and error messages will also be printed in the output 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.

10

… Solver Output Overview6) Lastly, after the solution has completed, the very end of the Solver Output provides some statistics on the analysis run. 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. If wall time is much larger than CPU time (such as 2x) 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.

11

… Solver Output SummaryBecoming familiar with the contents and structure of the Solver Output can be very useful in understanding the finite element solution 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.

12

B. Monitoring the SolutionWhile solving a nonlinear model, because many iterations may be needed, it is useful to see what the nonlinear solution trends are 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 Results Tracker to provide response of system during the solution

13

… Force ConvergenceThe most useful way to evaluate the solution convergence behavior is to view the Force Convergence graph: As shown in the previous section, the Force Convergence graph is available from the Solution Information branch

14

… Force ConvergenceOne common item is when the force convergence starts to “plateau” during solution 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.

15

… Results TrackerBesides monitoring the out-of-balance forces, a Results Tracker is available from the “Solution Information” branch 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.

16

… Results TrackerAfter the Results Tracker items are requested and solution initiated, users may “track” the deformation or contact results during the course of the solution.

17

… Results TrackerSeveral items (of a similar type) may also be selected and reviewed at once during solution

18

C. Newton-Raphson ResidualsSo far, obtaining detailed solver information (Section A) and monitoring the solution (Section B) have been discussed. 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.

19

… Newton-Raphson ResidualsIn 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.

20

… Newton-Raphson ResidualsAfter solution is stopped or fails to converge, residuals will be available under the “Solution Information” branch, as shown below.

21

… Newton-Raphson ResidualsAnother 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 In this case, the ‘ring’ of high residual forces is part of a contact region, so the user knows where to examine

22

D. Example CasesIn 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 It is impractical to cover all of the different causes for non-convergence. Instead, some common problems users encounter will be discussed.

23

… Rigid-Body MotionA common error message that may appear is “internal solution magnitude limit was exceeded.” Essentially, this means that rigid-body motion is encountered. 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

24

… Rigid-Body MotionTo 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. 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.

25

… Contact StiffnessSometimes, contact Normal Stiffness may be too high and contribute to non-convergence A threaded fastener solves the first substep until 20% of the load, but then diverges.

26

… Contact StiffnessBy 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 By lowering the contact Normal Stiffness and refining the mesh near regions of contact, the problem can be solved

Browse More Presentations

Last Updated: 8th March 2018