{"id":32010,"date":"2019-08-19T19:49:42","date_gmt":"2019-08-19T19:49:42","guid":{"rendered":"https:\/\/www.padtinc.com\/2019\/08\/19\/ansys-mechanical-overcoming-convergence-difficulties-with-automatic-remeshing-nonlinear-adaptive-region\/"},"modified":"2023-01-12T11:24:13","modified_gmt":"2023-01-12T18:24:13","slug":"ansys-mechanical-overcoming-convergence-difficulties-with-automatic-remeshing-nonlinear-adaptive-region","status":"publish","type":"post","link":"https:\/\/www.padtinc.com\/2019\/08\/19\/ansys-mechanical-overcoming-convergence-difficulties-with-automatic-remeshing-nonlinear-adaptive-region\/","title":{"rendered":"ANSYS Mechanical \u2013 Overcoming Convergence Difficulties with Automatic Remeshing (Nonlinear Adaptive Region)"},"content":{"rendered":"\n

One of the problems we can encounter in a nonlinear\nstructural analysis in ANSYS Mechanical is that elements become so distorted\nthat the solver cannot continue.  We get\nmessages saying the solver was unable to complete, and the solver output will\ncontain a message like this one:<\/p>\n\n\n\n

 *** ERROR ***                           CP =      37.969   TIME= 14:40:06
 Element 2988 (type = 1, SOLID187) (and maybe other elements) has become
 highly distorted.  Excessive distortion of elements is usually a       
 symptom indicating the need for corrective action elsewhere.  Try      
 incrementing the load more slowly (increase the number of substeps or  
 decrease the time step size).  You may need to improve your mesh to    
 obtain elements with better aspect ratios.  Also consider the behavior 
 of materials, contact pairs, and\/or constraint equations.  Please rule 
 out other root causes of this failure before attempting rezoning or    
 nonlinear adaptive solutions.  If this message appears in the first    
 iteration of first substep, be sure to perform element shape checking. <\/code><\/p>\n\n\n\n

The Solution branch will have the telltale red lightning\nbolts, indicating the solution was not able to complete due to nonconvergence.<\/p>\n\n\n

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

If you are not aware, one technique we can use to get past\nthis problem of excessive element distortion is to have ANSYS automatically\nremesh the model or a portion of the model while the solution is\nprogressing.  The current state of the\nmodel is then mapped onto the new mesh, in the currently deflected state.  In this manner we can automatically continue\nwith the solution after a slight pause for this remeshing to occur.  Minimally all we need to do as users is\ninsert a Nonlinear Adaptive Region under the Static Structural branch, and\nreview and specify a few settings (more on this later).<\/p>\n\n\n

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

Let\u2019s take a look at a simple example.  This is a wedge portion of a circular\nhyperelastic part, subject to a pressure load on the top surface.  Other boundary conditions include a fixed\nsupport on the bottom and frictionless supports on the two cut faces of the\nwedge.<\/p>\n\n\n\n

For this case, the nonlinear adaptive region is the entire\npart.  <\/p>\n\n\n

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

The initial mesh was setup as a default mesh, although note\nthat for 3D models the nonlinear adaptive capability requires a tetrahedral\nmesh up through the current version, 2019 R2.<\/p>\n\n\n

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

Prior to solving with the nonlinear adaptive region\nincluded, this model fails to converge at about 56% of the total load.  With the addition of the nonlinear adaptive\nregion, the model is automatically remeshed at the point of excessive element\ndistortion, and the solution is able to proceed until the full load is applied.  The force convergence graph has a solid\nvertical orange line at the point where remeshing occurred.  The method can result in multiple remeshing\nsteps although in the sample model shown here, only one remeshing was needed.<\/p>\n\n\n

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

The image on the left, below, shows the original mesh at the\nlast converged substep before remeshing occurred.  The image on the right is the first result\nset after remeshing was completed.<\/p>\n\n\n

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

The tabular view of a result item will show in the last\ncolumn if remeshing has occurred during the solution.<\/p>\n\n\n

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

Here is the final deformation, for the full amount of\npressure load applied on the top surface.<\/p>\n\n\n

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

Next, let\u2019s take a look at the nonlinear adaptive region\ncapability in more detail.<\/p>\n\n\n\n

First, multiple substeps must be used for the solution.  If we are performing a nonlinear analysis,\nthis will be the case anyway.  Second,\nLarge Deflection needs to be turned on in the Analysis Settings branch.  Also, results must be stored at all time\npoints (note that time is a tracking parameter in a static analysis, but all\nstatic as well as transient results in ANSYS Mechanical are associated with a\nvalue of \u2018time\u2019).<\/p>\n\n\n\n

There are several restrictions on features that CAN\u2019T be in\nthe model, such as cyclic symmetry (hence the frictionless support BC\u2019s on the\nsimple model shown above), Auto Asymmetric Contact, Joints, Springs, Remote\nForces and Displacements, etc.  Also\ncertain material properties are excluded, such as Cast Iron plasticity and\nShape Memory Alloy.  Also, as mentioned\nabove, for 3D models, the mesh must be tetrahedral.  For a full listing of these restrictions,\nrefer to the ANSYS Mechanical User\u2019s Guide. \nA search on \u2018nonlinear adaptive\u2019 will take you to the right location in\nthe Help.<\/p>\n\n\n\n

Nonlinear Adaptive Regions can be scoped to 3D solid and 2D\nbodies, or to elements via a Named Selection. \n<\/p>\n\n\n\n

In the Details view for the Nonlinear Adaptive Region, the\nmain option to be defined is the Criterion by which remeshing will be\ninitiated.  There are three options\navailable in Mechanical:  Energy, Box,\nand Mesh.<\/p>\n\n\n\n

The Energy criterion checks the strain energy of each\nelement within the Nonlinear Adaptive Region. \nIf the strain energy is above a criterion, remeshing is triggered.  The input is an energy coefficient between\nzero and one, and is a multiplier on the ratio of total strain energy of the\ncomponent divided by the number of elements of the component.  Recommended values are 0.85-0.9.  A lower coefficient will tend to cause\nremeshing to be more likely.<\/p>\n\n\n\n

The Box criterion defines a geometry region based on a\ncoordinate system and bounds relative to that coordinate system.  Elements in the Nonlinear Adaptive Region\nwhose nodes have all moved within the box will be remeshed.  The idea is that if it\u2019s known that elements\nwill be highly distorted as they move into a certain region, we can ensure that\nremeshing will occur there.<\/p>\n\n\n\n

The Mesh criterion allows us to specify that remeshing will\noccur if mesh quality measures drop below certain levels as the mesh\ndistorts.  For 3D models, the available\nmeasures are Jacobian Ratio and Skewness. \nThese are described in the Mechanical User\u2019s Guide in the section on\nNonlinear Adaptive Region.<\/p>\n\n\n\n

In the example shown above, the Energy criterion was used\nwith an energy coefficient of 0.85.<\/p>\n\n\n\n

There are some things to be aware of when you are trying to\nimplement a Nonlinear Adaptive Region to help overcome convergence\ndifficulties.  First, if any of the\nrestricted features mentioned above are included in the model, such as remote\ndisplacements, it\u2019s not going to work. \nTherefore, it\u2019s important to review the list of restrictions in the Help\nand make sure none of those are applied in your model.  Second, \u2018buckling\u2019 or element distortion due\nto an unstable structure is not a behavior that Nonlinear Adaptive Regions can\nhelp with.  The Nonlinear Adaptive Region\ncapability is more suited to problems like hyperelastic seals being compressed\nor objects that are undergoing a high degree of bending (but not snapping\nthrough).  <\/p>\n\n\n\n

Also, a coarse mesh that distorts may not produce a usable\nremesh.  The remeshing step may occur,\nbut the simulation may not be able to proceed beyond that and stops with an\nerror in element formulation error.  More\nmesh refinement may be needed in this case.<\/p>\n\n\n\n

As a further word of caution, self contact problems may not\nwork very well within the context of Nonlinear Adaptive Regions.  If self contact is needed, consider splitting\nthe bodies into multiple parts to avoid self contact.  <\/p>\n\n\n\n

There are some other considerations for the method as\ndiscussed in the Help, but hopefully the guidelines and recommendations\npresented here will allow you to filter potential applications appropriately\nand setup models that can take advantage of the Nonlinear Adaptive Region\ncapability.  We have a short animation\nwhich shows the remeshing step in the sample model.  <\/p>\n\n\n\n

If you have nonlinear static structural models with convergence difficulties due to excessive element distortion, please consider using this method to help you get a fully converged solution.<\/p>\n\n\n\n

Here is a video to help everyone visualize:<\/p>\n\n\n\n

\n