Pushing the Limits of Nonlinear Deformation?

[markdeckerZBQL7]

Looking for general feedback on how far nonlinear deformation and plasticity can be pushed in Sim Mechanical for this type of application.

Tensile testing of very thin copper plate to understand strength and eventual location of breaking point for various geometry configurations.  Not trying to even get out anywhere near the ultimate stress.  Due to stability issues, I have throttled it back to only displace the thickness of the plate.

When I run this in 2D, it is quite unstable with the time step level fluctuating wildly and it is very sensitive to mesh (the sharp corners certainly don't help here).  Varying mesh (both discrete and non-discrete), using mid-side nodes, Rayleigh damping, Updated Lagrangian and 4th order integration don't seem to help much here.

Force displacement curve seems pretty choppy.

I also ran this in Abaqus (currently evaluating it using the SE version) and the run behavior seems much more stable and the output more plausible.  I could also deform it to a much a greater extent in Abaqus than Sim Mechanical before it also eventually diverges.

[John_Holtz]

Hi @markdeckerZBQL7

That is an interesting problem. It is hard to tell what is causing the convergence difficulties, but it could be:

• the singularity at the corners, or
• the horizontal portions (the "arms") are in bending. So one side of the top arm is in tension, and one side is in compression. When it goes fully plastic, along the centerline of the arm see a gradient from +yield strength to -yield strength. Is this causing convergence problems? (See attached image). I tried creating a really fine mesh along the centerline of each arm, but it did not help much.

I wonder if @Keith.Orgeron (Keith Orgeron) has some ideas on this. He's a nonlinear/elastic-plastic expert.

[Keith.Orgeron]

John, Mark,

I ran a similar model using bronze and with the SimMech defaults and the bilinear plasticity model the results matched Mark's.  However, it was simple to fix using the following to reduce the dynamics and plastic flow initiation effects of the simulated event:

1. Smaller time steps of 0.010 sec vs. 0.050 sec (default)
2. Longer time of 10 sec vs 1 sec (default)
3. Curve plasticity model vs. bilinear (default)

Will upload graphic tomorrow... 

Keith

[Keith.Orgeron]

Well, this worked but only for displacement of 100% of the thickness, then something else blew up.  The reaction force plot represents a single node.  Just realized I didn't show the mesh... but, it is a default mesh size and looks similar to the others in this thread (coarse mesh).

[Keith.Orgeron]

@John_Holtz, I considered Mark's posted words in greater detail and attempt here to support his effort directly with these comments:

@markdeckerZBQL7:  "Tensile testing of very thin copper plate to understand strength and eventual location of breaking point for various geometry configurations.  Not trying to even get out anywhere near the ultimate stress.  Due to stability issues, I have throttled it back to only displace the thickness of the plate. 

When I run this in 2D, it is quite unstable with the time step level fluctuating wildly and it is very sensitive to mesh (the sharp corners certainly don't help here).  Varying mesh (both discrete and non-discrete), using mid-side nodes, Rayleigh damping, Updated Lagrangian and 4th order integration don't seem to help much here. 

Force displacement curve seems pretty choppy."

kjo's REPLY:

• Note that I am new to this forum's posting app, so, my content and threading may not be orthodox... apologies!
• Do not have enough data to reproduce all critical input... so this effort is all qualitative and speculative

1. Revised model to 0.100" thick plate, approximating copper (could not readily find plastic mechanical properties)
2. To understand "... strength... and breaking point" the local geometry would need the radii shown for appropriate accuracy
3. Great width assumed, relative to thickness, so this 3D brick model (imported from SW) uses plane-strain BC's
4. Molded S-shape assumed otherwise residual stresses are significant due to forging process
5. Shell elements could be used but cannot reflect the nonlinear through-thickness stress-strain profiles accurately
6. The source of the "choppy" force-displ. curve is due to the sequential tangent modulus stiffness reductions per element integration point
7. An MES dynamic solution adds vibratory responses to be navigated by the solver adding to the total error norm per step
8. Use of a Nonlinear static solution removes dynamic accelerations but the solver parameter defaults are not as well refined as for MES
9. I suspect the use of an Abaqus explicit solution?  Hence the selection of 1 sec event?... or is this the true event time?
10. If the event occurs over 1 second, then the straining could require higher strain rate material properties too
11. SimMech's explicit solver for an MES solution which should be attempted

Other model, material and solution parameters:

• Straight lengths are less than Mark's
• Mesh is only slightly finer but more uniform
• Material is probably still too stiff... picking up more load (if load units are lbs-force?)
• VM bilinear isotropic hardening model used
• Very small time steps used
• Updated lagrangian formulation used
• MES & other modeling defaults accepted (if I recall them all)

[Keith.Orgeron]

@markdeckerZBQL7,

I believe that I understand the source of the solution instability.  It stems from the unconstrained motion of the Pulled-End in the vertical direction (Y), normal to the pull direction (X).  The plot below shows the derivative of this motion or dY/dt of the y-displacement.  It accelerates as more of the model yields and continues to plastically flow.  The population and frequency of the many plastic integration points incrementally flowing for each time step increase and cause the Pulled-End to fall for a left-side dominated flow and to rise for a right-side dominated flow... all the while stiffening and raising the natural frequency closer to the rather random set of exciting frequencies.  

 

Thus, given the stiffness assumed and the resulting frequency content of our models some level of resonance and solution failure is imminent unless a vertical constraint of some kind can be justifiably included.  The Abacus solution could have included a smoother yielding element formulation or a smoothing algorithm for this microscopic level of vertical motion...?  The pulling machine will probably have a vertical constraint capability, as it will probably not be capable of vertically floating with no resistance.  What do you think?  And you @John_Holtz?

[Keith.Orgeron · Accepted solution]

Mark,

Finally took time to test my conclusion... and yes, it does make a huge difference!  However, it is not easy to guide it downwards without introducing some vertical shear and challenging the solution's convergence.  But, using a high-speed batch-file solve that I learned from @John_Holtz and a few iterations, the embedded image shows the results than can be obtained. 

[markdeckerZBQL7]

Appreciate the input here Keith and John.  Looks like we will be winding down on using Ted Lin's original Accupak code.

This is all great feedback.  Curious how well it would translate over to NIC or Fusion solutions?

• The copper is only 1 mil thick and is electroplated, so there are no initial residual stresses.
• Since it is electroplated and ultra thin, I do not know what kind of radii they could control.
• I also used a VM isotropic bilinear for all solutions in both Algor and Abaqus.
• The Abaqus run I did was an implicit solution.  Still impressed on how it could handle it using default settings.