Learning Forum

[livemansleeping]

I'm experiencing an interesting issue that some one here might be able to help me with.  I am running an impact at 600m/s into a composite material consisting of plastic orthotropic models subject to strain failure, and a johnson cook ceramic model and failure model.  I am using the default explicit dynamics lead material under a strain failure model.

The model consists of layered pieces of polyethylene under orthotropic plastic deformation and failure, interspersed with a ceramic designed to shatter via the johnson cook model of failure.  

I've tried several meshes in order to achieve a mesh that will operate given the limitations of ANSYS/AUTODYNE.  This includes a body-cartesian mesh for the impacting lead object, and the default, tetrahedral mesh as well.  Nothing seems to assuage the error.  When attempting to solve the simulation the following errors pop up. In this order (top to bottom)

...

Warning: Current result file may not contain requested result data . Please clear the solution and solve again.

Warning: The result file  cannot be opened.

Error: An error occurred when the post processor attempted to load a specific result. Please review all messages.

Error:Solver initialization error - see log file for more details.

Warning: Pyramid elements not supported by the solver. 11309 pyramid elements split into tetrahedral elements.

...

 

The solution information log only has a very simplistic output of information.  The entire simulation consisting of the following statements;

...

License acquired!
Checking model setup.....Please wait
Generating External Faces ...... please wait
Initializing.....Please wait
Cannot run problem. Invalid equation of state with ANP tetrahedra.
 
Valid equations of state for ANP tetrahedra are:
 
Linear
Polynomial
Shock
Porous
Compaction
P alpha
Rigid
Hyperelastic
User EOS
Finished model setup with errors...

...

Here's what seems so strange to me.  If the error is caused by running a tetrahedral mesh simulation with the johnson-cook model, then the multizone Hexa mesh should be sufficient to assuage that problem.  The mesh itself seems to have few, if any tetrahedral elements, and yet I am seeing an error message indicating that there are more than eleven thousand pyramid elements in this system.  Any information on why this is happening would be appriciated.  Included is an image of the multizone meshing settings, and an image of the mesh i'm actually working with. nearly all the cells i'm working with in the mesh are cubic.  Is there some sort of error-state in ANSYS that's causing the failure in the initialization stage of running this simulation?

Multizone mesh settings

Image of the generated mesh

 

[livemansleeping]

Update. I have isolated the problem to the Orthotropic Polyethylene fiber material.  It's operating under a relatively standard orthotropic model.  The following are the material properties I'm working with in the orthotropic model that I'm using.  It's a relatively simple system, but whenever I use that material in the simulation, I get the solver initialization error as seen above.

I've used this model of polyethylene in other simulations without any problem.  All body interactions are frictionless in the simulation. 

 

Could some one tell me what is going on here?

 

 

As per this article; https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/wb_sim/exp_dyn_theory_solv_cont.html

Orthotropic models do not function in an ANP tetrahedral mesh.  A complete Hexa mesh should remedy the problem, then, but it doesn't seem to.

[livemansleeping]

Update; the only way I can get this to run is with a Cartesian mesh.  Which, as you might imagine, is far more time consuming than is necessary.

[jj77]

That is good. Can you expand a bit what you did, because I am not following 100% - this is very useful to other members so if you could expalin a bit that would be much appreciated by many.

 

As far as I can understand when meshing in a certain way you can run it?

The question is though in your properties (eng. data) as you show above the EOS is still crossed out ?

I assume that it is then not working fully then (material model since eos is not accounted for)?

 

many thanks

 

[jj77]

I have spoken to people that know autodyn and ansys very well, and you can do orthotropic elasticity in Engineering data for Explicit dynamics + orthotropic stress limits for failure but you can not use the nonlinear EOS options or the orthotropic plasticity as you can in Autodyn (as shown above). So unless you do high vel. impact or blast that should be OK. If you do blast or high vel. impact then use autodyn gui as mentioned.

[livemansleeping]

Thanks for your response.  The Orthotropic model I'm attempting to use is as defined in the image.  EOS and Shear modulus are suppressed in favor of the Orthotropic model.  When I attempt to use any mesh, besides a cartesian mesh, the solver error appears whenever I attempt to initialize a solution.  I am modeling a high velocity impact (600 m/s).  I've attempting to use a Hexa-dominant mesh, a prism mesh, default meshing, etc.  The only type of meshing that does not result in the solver initialization error causing the "Finished model setup with errors" message is a Cartesian mesh.  The prism type mesh causes the meshing to crash the Explicit Dynamics Mechanical design.

 

All other mesh combinations result in the same message in the solution information.

...

License acquired!
Checking model setup.....Please wait
Generating External Faces ...... please wait
Initializing.....Please wait
Cannot run problem. Invalid equation of state with ANP tetrahedra.
 
Valid equations of state for ANP tetrahedra are:
 
Linear
Polynomial
Shock
Porous
Compaction
P alpha
Rigid
Hyperelastic
User EOS
Finished model setup with errors...

...

 

I am using 3 different materials in the setup in addition to the orthotropic material imaged above.  If I remove the orthotropic material from the model, then the error message does not occur, and the simulation begins running.

 

Details on the other two materials I'm using that do not seem to cause this error are contained in the images below.

 

 

 

You suggest that I may be using the wrong GUI? I'm using Explicit Dynamics - Mechanical in order to perform the simulation.  Is there another system gui that I should be using instead? Can you explain to me what I am doing wrong in that regard? I'm also including an image of the analysis settings that I'm working with.

 

 

If I am, indeed, operating with the incorrect GUI for my impact, please describe what changes I should be making in order to get the material to run correctly with the meshes I have available to me.  I'll also include a link to the full project file, along with the geometry I am playing with.

https://mega.nz/#!BNhQSAqZ!YBmrcZqha6TnIjyFvaRy6Eu-pvNbRsfGTSvzk5Ro7Zg

 

I'm not sure what you mean by using the autodyn gui as opposed to the gui I'm currently operating wtih.

[jj77]

I should say I know very little and have not used ansys explicit dynamics much.

 

Now the kind people at Ansys Autodyn (which is the solver behind Ansys Explicit Dynamics system), provided some very good feedback.

 

They said that the orthotropic+EOS can not be used from Explicit Dynamics - this explains as you have seen that one can only have an orthotropic only and not together with EOS. This is perhaps ok for impacts and low velocity dynamics, since the equation of state is not that important (thus not big changes in pressure, density temp. relation).

 

Of course now if you have a blast where there will be changes to the state (thus big changes in pressure, density temp. relation), then one can not use the Explicit Dynamics system. We can though do all the meshing and loads and settings in Explicit Dynamics and then link that up to the Autodyn system that is available in the student version. See this post here on how to link the Explict Dynamic (so all meshing + BC + Loads+Analysis settings there) to the Autodyn, where one can change the material EOS to Ortho that includes a EOS and everything needed for blast. In this post I give a quick tip on how to change the material (I imported/load the material in Autodyn/Material section say material called KFRP, and then one can change it as needed. If you need more than you need to find things online because I do not have a clue about Autodyn,

 

https://forum.ansys.com/forums/topic/explicit-dynamics-87/

[livemansleeping]

Thank you, I will read it.