{"id":32223,"date":"2019-10-09T15:25:32","date_gmt":"2019-10-09T15:25:32","guid":{"rendered":"https:\/\/www.padtinc.com\/2019\/10\/09\/ansys-mechanical-semi-implicit\/"},"modified":"2022-12-07T15:44:24","modified_gmt":"2022-12-07T22:44:24","slug":"ansys-mechanical-semi-implicit","status":"publish","type":"post","link":"https:\/\/www.padtinc.com\/2019\/10\/09\/ansys-mechanical-semi-implicit\/","title":{"rendered":"ANSYS Mechanical \u2013 Overcoming Convergence Difficulties with the Semi-Implicit Method"},"content":{"rendered":"\n

In our last blog, we discussed using Nonlinear Adaptive\nRegion to overcome convergence difficulties by having the solver automatically\ntrigger a remesh when elements have become excessively distorted.  You can read it here:  http:\/\/www.padtinc.com\/blog\/ansys-mechanical-overcoming-convergence-difficulties-with-automatic-remeshing-nonlinear-adaptive-region\/<\/a><\/p>\n\n\n\n

This time we look at another tool for overcoming convergence\ndifficulties, the Semi-Implicit method. \nANSYS, Inc. describes the semi-implicit method as a hybrid, combining\nfeatures of both implicit and explicit finite element methods.<\/p>\n\n\n\n

In highly nonlinear problems involving significant deformations we may get a solver error like this one:  <\/p>\n\n\n\n

*** ERROR ***                           CP =   18110.688   TIME= 11:58:42
Solution not converged at time 0.921 (load step 1 substep 185).           Run terminated.  <\/p>\n\n\n\n

Like it does with other problems that lead to convergence\nfailures, the Solution branch will have telltale red lightning bolts,\nindicating the solution was not able to complete due to nonconvergence.<\/p>\n\n\n

\n
\"\" <\/picture><\/figure><\/div>\n\n\n

In this case, it can be difficult to determine from the error message in the solution output exactly what the problem is.  Plotting the Newton-Raphson residuals can be a good starting point.  In order to plot the Newton-Raphson residuals, though, we need to turn them on prior to solving.  See this older Focus blog for instructions on how to do that:<\/p>\n\n\n\n

http:\/\/www.padtinc.com\/blog\/overcoming-convergence-difficulties-in-ansys-workbench-mechanical-part-i-using-newton-raphson-residual-information\/<\/a><\/p>\n\n\n\n

A plot of the Newton-Raphson residuals shows us where the\nhighest force imbalance is in the model:<\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

That\u2019s a nice looking plot, but doesn\u2019t tell us much without\nknowing more about the simulation.  The\nmodel is of a plastic bottle, subject to a force load tending to \u2018crush\u2019 the\nbottle from top to bottom.  There is a\nslight off center load as well, so that the force is not purely in the downward\ndirection.  <\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

The bottle is constrained with a fixed support on the bottom\nflat surface, and contact elements between the outer surface of the bottle and\na fixed surface representing a table or floor. \nThis is to prevent the bottle from deflecting below the plane of that\nsurface.<\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

The material used is a polyethylene plastic, from the ANSYS Granta\nMaterials Data for Simulation add-on, which is a great tool to get access to\nhundreds of materials for ANSYS simulations. \nThe geometry of the bottle was created in SpaceClaim as a surface body and\nmeshed with shell elements in ANSYS Mechanical. \n<\/p>\n\n\n\n

The solution was run as nonlinear static, with large\ndeflection effects turned on.  Automatic\nTime Stepping was manually activated with a starting and minimum number of\nsubsteps set to 200 and a maximum number of substeps set to 1000.<\/p>\n\n\n\n

With these settings, the solution ran to about 92% of the\nfull load, where it failed to solve after bisecting to the maximum number of\nsubsteps (minimum \u2018time\u2019 step).  The\nforce convergence plots showed the bisections and failed convergence attempts\nstarted at about iteration 230 and \u2018time\u2019 0.92. \n(If you are not familiar with the convergence plots from a\nNewton-Raphson method solution, please see our Focus archives for an article on\nthe topic \u2013 look for the link to the GST Plot: \nhttp:\/\/www.padtinc.com\/blog2\/wp-content\/uploads\/oldblog\/PADT_TheFocus_08.pdf<\/a>).<\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

Even though our solution has not converged, it is probably\nhelpful to view the deformation results for substeps which did converge (at\npartial load) as well as the unconverged results which will be written as the\nlast set of results.<\/p>\n\n\n\n

This plot shows the total deformation at the last converged\nsubstep (time value 0.92):<\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

This plot shows the unconverged solution, \u2018extrapolated\u2019 to\ntime 1.0: <\/p>\n\n\n\n

\"\" <\/picture><\/figure>\n\n\n\n

From the unconverged\ndeformation plot we can see that the top of the bottle is tending to experience\nvery large deformations.  It\u2019s not\nsurprizing that convergence difficulties are being encountered.<\/p>\n\n\n\n

One of the techniques we can utilize to get past this\nproblem is the Semi-Implicit method in ANSYS Mechanical.  As of 2019 R2, this needs to be activated\nusing a Mechanical APDL command object, but it can be as simple as adding a\nsingle word within the Static Structural branch:<\/p>\n\n\n\n

SEMIIMPLICIT<\/strong><\/p>\n\n\n\n

There are some optional fields on that command, but\nminimally just the one word command is needed.<\/p>\n\n\n\n

Once the semi-implicit method is activated, if the solver\ndetects the default implicit solver is having trouble, it automatically\nswitches to the semi-implicit solving scheme. \nLike a traditional explicit solver, the semi-implicit method can better\nhandle very large deformation, transitory-like effects.  The method can switch back to implicit if\nconditions warrant for a more efficient solution and in fact can switch back\nand forth between the two schemes.<\/p>\n\n\n\n

The solver output will tell us if the semi-implicit scheme has been activated:<\/p>\n\n\n

EQUIL ITER  26 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.9526   

     NONLINEAR DIAGNOSTIC DATA HAS BEEN WRITTEN TO  FILE: file.nd004

     DISP CONVERGENCE VALUE   =  0.3918      CRITERION=   1.448     <<< CONVERGED

     LINE SEARCH PARAMETER =  0.4113     SCALED MAX DOF INC =  0.3918   

     FORCE CONVERGENCE VALUE  =   44.44      CRITERION=  0.9960   

     MOMENT CONVERGENCE VALUE =   3.263      CRITERION=  0.1423   

    Writing NEWTON-RAPHSON residual forces to file: file.nr001

    >>> TRANSITIONING TO SEMI-IMPLICIT METHOD

     NONLINEAR DIAGNOSTIC DATA HAS BEEN WRITTEN TO  FILE: file.nd001


    EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC=  0.8788E-04

     NONLINEAR DIAGNOSTIC DATA HAS BEEN WRITTEN TO  FILE: file.nd002

 *** LOAD STEP     1   SUBSTEP   185  COMPLETED.    CUM ITER =    284

 *** TIME =  0.920010         TIME INC =  0.100000E-04

    Kinetic Energy = 0.2157        Potential Energy =  60.59   

 *** AUTO STEP TIME:  NEXT TIME INC = 0.10000E-04  UNCHANGED

     NONLINEAR DIAGNOSTIC DATA HAS BEEN WRITTEN TO  FILE: file.nd003<\/pre>\n\n\n
There are some \u2018symptoms\u2019 of the switch from implicit to\nexplicit.  The most obvious is probably\nthat the force convergence plot will stop updating.  <\/p>\n\n\n\n
\"\" <\/picture><\/figure>\n\n\n\n
Changing the Solution Output to the Solver Output will show\nthe explicit scheme being used in that case. \nThe telltale is the information on Response Frequency and Period (the\nexample shown is a static structural solution).<\/p>\n\n\n\n
\"\" <\/picture><\/figure>\n\n\n\n
Deformation plot trackers and contact trackers continue to\nwork as expected during the solution, however.<\/p>\n\n\n\n
\"\" <\/picture><\/figure>\n\n\n\n
Using the semi-implicit method, the solution was able to\nsuccessfully converge to the full load, and converged results are available at\nthe last time point:<\/p>\n\n\n\n
\"\" <\/picture><\/figure>\n\n\n\n
We also used the new keyframe animation technique to animate the results time history.<\/p>\n\n\n\n
\n