Learning Forum

[langlinator]

Hi

I am using a Nonlinear Adaptive Region in a static structural analysis, to re-mesh as a response to large strains. I need to model very large strains (for steel), up to around a value of 1.

Known limitations of Ansys nonlinear adaptivity that I have already worked around:

• Not compatible with weak springs (I had to use just 1 plane of symmetry instead of 2)


• Only supports tetrahedral elements (I would have preferred a structured hex mesh for my problem)

I have attached an image of my geometry and boundary conditions.

The problem I encounter is blank areas of results (I think due to poor mesh).

I have tried changing a variety of nonlinear adaptivity parameters in the Energy and Mesh criteria. I've also tried adjusting options in the nonlinear adaptive Analysis settings, including NSL & aggressive remeshing. Everything I have tried, in line with what I've read in the Mechanical help literature, seems to make the problem worse - with larger areas of results missing. And that's if it works at all - two subsequent problems are (1) problem size limit (32k nodes) exceeded (I guess due to a significant increase in nodes after remeshing, which doesn't actually make sense based on the geometry and deformation) or (2) "Internal solution magnitude exceeded".

In the case of subsequent error (2) I check the file0.err and fine the text below, relating to a number of nodes. I don't understand, why I'm getting an error that elements are highly distorted, when that should have triggered remeshing.

Does anyone have experience with nonlinear adaptivity and have advice on how to overcome these issues?

 *** ERROR ***                           CP =     110.516   TIME= 21:59:28
 Element 9519 (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.  

[langlinator]

[langlinator]

Actually there is a third error

(3) The result cannot be evaluated because it has (1) an invalid scoping on a body with a changing mesh or (2) an invalid scoping when the result file is the mesh source. Body scoping is required for the result.

Which is not at all convenient because I have results in the form of Probes and Paths that are essential to my analysis. This can't be the source of the problem as it only occurs intermittently.

[langlinator]

I should probably also note the plasticity model I am using; Multinear Isotropic Hardening. Assumption that this takes TRUE STRESS values in the table, with plastic strain values.

[peteroznewman]

In my opinion, the optimal approach to the Nonlinear Adaptive Region is to not use it.

I have successfully reached strains of 1.0 with a structured mesh and a plasticity material model. Were you unable to get to that point? There are some element keyops that help you get there such as reduced integration and mixed u-P formulation. Another helpful strategy is to make the initial mesh have the aspect ratio such that as the solution progresses, the aspect ratio improves instead of gets worse. For example, if the elements are going to be distorted and become short and wide, don't start with a square element, start with a tall and narrow element and let it deform into a square.

[langlinator]

Interesting, thank you. Are there tools in Ansys student edition for creation of a structured mesh? I haven’t found them yet, if there are.

[peteroznewman]

On the geometry you show, apply a Mesh Control Method = Sweep to the body. That should create a structured mesh. You get to specify how many elements along the sweep direction. This is one control on the element aspect ratio of depth.  Then you can add a sizing control on the circular edge, that is another control on the element aspect ratio on width. Finally, you split the center out and apply sizing on those new edges and apply Face Meshing to get the structured mesh shown below to control the element aspect ratio on height.

[langlinator]

Thank you for the advice, and attaching the wbpz, that has answered a lot of my questions about the meshing options.

 

 

[langlinator]

Only further question - When I solve the project, I get error:

The maximum contact stiffness is too big. This may affect the accuracy of the results. You may need to sale the force unit in the model.

I don't have any experience with modelling contacts so this is a new area for me. I can read the Ansys documentation to work it out. However, I noticed that your Mechanical model doesn't have contacts - but has three solid bodies - how have you achieved this?

[peteroznewman]

By using Shared Topology. In SpaceClaim, after using Slice Body to divide the solid, click on the Workbench tab then click on the Share button.

Coincident surfaces are identified and only one set of nodes are meshed on those two surfaces so that the elements touching that coincident surface from each side end up holding on to a shared node, thereby creating a continuous mesh.

[langlinator]

Great, thank you.

[langlinator]

Hi Peter, I have tried this using both Spaceclaim and Design Modeller. I still have contact regions in my mechanical model. Did you do anything else differently?

Worked it out in SpaceClaim. I'm unfamiliar with SpaceClaim, prefer Design Modeller.

[langlinator]

For anyone reading this trying to use Shared Topology in Design Modeller:

• Click "share topology" before making slices etc


• You won't be able to apply symmetry in Design Modeller. You have to do it in mechanical by insert>symmetry on the Tree instead

[peteroznewman]

In DesignModeler, create Planes and Slice bodies. When done, select all the bodies at the bottom of the outline, right click and Form New Part. That will create a multibody part that has Shared Topology turned on by default.