MES of Tensile Specimen Pronounced Necking... Axial Ridges??

Anonymous

MES of Tensile Specimen Pronounced Necking... Axial Ridges??

Anonymous
Not applicable

56 sec Video (below):  An R&D project featuring a 3D 1/8-model of a standard tensile test specimen having a minimum axial h-value of 0.001" at the failure plane.  YouTube Link:  https://youtu.be/j6j8C-iEQhY   What do you think this numerical behavior represents? 

 

Notes:
1. Low strain hardening coefficient
2. Lower order (linear) bricks
3. No geometric protuberance
4. AutoDesk Simulation Mechanical

 

The surface crinkling may be a valid phenomenon. A circumferential set of axial stripes or ridges is evidenced in lab tensile-testing of some metallic specimens. These ridges are probably all or mostly due to microstructural dislocation slip, which is beyond the capability of the FE model's isotropic material model used. Or, could it be that prior to (or without) microvoid nucleation, which is an MES impossibility, in this ductile sample the axial ridges are true "crinkling" but their rather large size is caused by the 8-node brick mesh limiting the model's sensitivity to manifest a much smaller and more numerous set of axial ridges.

 

Besides that material model being a limit to the nature of this model behavior, the 1/8 symmetry of the model negates simulation of a true cup-cone failure mode.  But,  imagine just prior to such a failure mode, except we have a symmetric, "cup-bullet" failure mode... the "bullet" being a "symmetric cup" of-sorts, and each side of the specimen forms a "symmetric cone" to match it.

 

 So, what do you think this numerical behavior represents? 

www.OrgeronEngineering.com

 

Tensile_Test_RndBar v0 Updated.png

VIDEO LINK:  

Reply
Reply
0 Likes
Reply
Accepted solutions (1)
863 Views
6 Replies
Replies (6)

KubliJ
Alumni
Alumni

Hi Keith,

 

Sorry for the delay.  I've done some research on this and unfortunately do not have much of an idea of what is going on.  Visually speaking it looks like the elements are buckling or something similar to the hourglass effect of reduced integration order.  If it is an hourglass effect, increasing the integration order could help.

 

Can I ask what the intent of this test analysis is for?

 

Thanks,

James

 

 



James Kubli, P.E.


Please marked this as solved if your question has been answered.
Reply
Reply
0 Likes

Anonymous
Not applicable

James,

 

I appreciate your efforts.  Relative to your suggestion of an hourglass effect, which is always possible with reduced integration linear bricks, I don't see how this less-sensitive element feature (in an "hourglass" configuration) could contribute to the generation of such axial ridges... below, I note that each ridge is comprised of about 10 elements!

 

I believe that this question is primarily one of results interpretation... 

 

Does the numerical behavior presented match any known physical phenomenon (albeit uncommon phenomenon... like the one I mentioned)?  Relative to mechanics of materials research using FE methods, I'm not sure that the objectives/features of this project have been duplicated prior to this.  Unless we can get enough interest by the community of experts, researchers, professors, etc. we could be missing an opportunity to contribute to this area of knowledge.  Below I list what may be the collection of unique model features that allowed such an interesting result:

 

  1. Objective 1: Simulate tensile test specimen pronounced necking with NO geometric perturbance (vs. use of geometry to perturb)
    • Purposeful inclusion of geometric anomalies to perturb initiation of pronounced necking can skew results 
    • Unknowingly, many researchers include mesh-related geometric anomalies and accidentally perturb the solution
      • A carefully designed 2D cross-sectional Sim-Mech auto-mesh was copy-joined manually, including scaling for the radius
      • Thus, a 100% set of high-quality hexahedra comprised the model's mesh
  2. Objective 2: Develop an efficient model for educational uses incorporating linear brick elements (vs. quadratic)
    • A patch of kinematic elements was used to buffer the application of prescribed displacements for optional conversion to quadratic 
  3. Objective 3: Use 1/8 triple-mirror symmetry model (3 symmetry planes) to visualize depth & allow 3D CAD use (vs. 2D axisymmetric)
    • Use of 3D elements over 1/4 of the cross-section allowed these results to manifest
    • I predict that use of a more refined mesh at the surface will allow more ridges to develop
      • At this time there are about 10 elements for each of the 16 ridges (over 360 degrees)
      • It is also possible that use quadratic elements vs. refining the mesh
Reply
Reply
0 Likes

KubliJ
Alumni
Alumni

Hi Keith,

 

Sorry for the delay.  I apologize, I do not have an explanation of the issue.  As you pointed out, it is not hourglass because it spans several elements.  It is possible rounding error.  You could try a nonlinear static analysis with Nastran, see if the effect is the same.  Fusion 360 has an explicit solver which should easily handle this level of deformation.

 

Thanks,

James

 

 



James Kubli, P.E.


Please marked this as solved if your question has been answered.
Reply
Reply
0 Likes

Anonymous
Not applicable
Accepted solution

James,

 

I believe that I have accidentally solved the puzzle...  Recently, I performed an MES including a cylinder's volume of fluid modeled with hydrodynamic elements and witnessed a very similar behavior, where the circular cross section morphed into having multiple lobes or ridges!  Thus, the cylindrical volume of steel at the pronounced neck of my tensile test model, having 100% of the elements experiencing axial stress beyond yield, behaved much like a fluid due to the Poisson ratio being set to 0.5 (constant volume strain, incompressible) during the post-yield straining according to the bilinear Von Mises plasticity material model deployed.

 

This explanation together with my prefaced statements about the absence of microvoid damage mechanisms within the simple material model's formulation indicates to me at least that the analysis had probably progressed beyond the point of a realistic damaged, tensile test failure and had begun synthesizing fantastical or at least extreme behavior.

 

So, how does this explanation stack up? @KubliJ @John_Holtz 

Reply
Reply
0 Likes

KubliJ
Alumni
Alumni

Hi Keith,

 

I would agree that the results are not likely correct.  Generally speaking with stiff materials like steel, the Algor solvers are good up to about 16% strain.  Softer materials can get better maximum strain. However, 300% strain would be outside the solvers capability. 

 

Thanks,

James



James Kubli, P.E.


Please marked this as solved if your question has been answered.
Reply
Reply

Anonymous
Not applicable

James,

 

Thanks for your feedback.  Yes, I introduced this model with an extremely low value for the strain hardening exponent.  This could have allowed more of the localized plastic material to be of nearly equal stiffness and behave more like a fluid.

 

All the best,

Keith.

Reply
Reply
0 Likes