Learning Forum

[PPosabella]

Hello everybody,

I am trying to simulate a compression test (static analysis) of a porous structure to validate results over experimental data. Samples are 3D printed through SLA (Formlabs 3B, Flexible 80A resin).

First, I experimentally characterised the material properties in compression, then obtained a material model in Workbench (Ogden 1st Order). 

My geometry is a porous structure with a spherical unit cell (full structure, first picture), the simulation is performed using symmetries in the x- and z- directions (second picture).

BCs. Upper surface: uY ≠ 0; uX = uZ = 0; lower surface: fixed support (I tried just uY = 0 but had convergence issues).

The engineering stresses and strains are obtained from FE results (stress = reaction force / initial cross section; strain = displacement / initial length) and compared to the ones obtained from the testing machine. Here is the simluation results compared to the experimental ones.

Two questions arise:

1) The first regions overlap with good agreement, until buckling of the structure occurs - which is not detected in the simulation. Is there anything missing in the model? Maybe the printed structure has many imperfections due to the printing process so buckling occurs much before than if considering the designed (then "perfect") one? (I ran a different simulation on the same structure without symmetries, obtaining a buckled curve, maybe confirming my thought?)

2) Depending on the used geometry (the picture above shows 1/14 symmetric region) simulations don't always converge for high strains, due to highly distorted elements. I know this is a very frequent matter with hyperelastic materials and I have tried to solve by reading/watching videos: I tried (local) remeshing, NLAD, etc but apparently I cannot overcome this problem right now.

Here is the link to the archived project https://drive.google.com/file/d/1JHpWhteu_Wn1ZezxKyFEAj8fhTru21VL/view?usp=drive_link.

Thanks in advance, any suggestions would be highly appreciated :)

 

[John Doyle]

What happens when you unload the test structure?  Does it permanently deform, after buckling, or does it spring back to its original shape?    If there is local damage (or yielding) occurring in the resin, the hyperelastic material model is not going to capture that.   Perhaps a Three Network Model would be a better material option.  If it is purely hyperelastic, with no local damage, perhaps the 1st order Ogden is just insufficient to fully capture the stiffness response in the 3D stress state.   If that is the case, can you generate material test data in tension, shear and compression; and curve fit this to a higher order Ogden model? 

Also, what about self-contact between the surfaces on the interior of the structure?  Do the surfaces remain separated, or do they collapse onto each other?  If there is nonlinear contact between internal surfaces, perhaps that explains the sharp increase in stiffness response at larger strains.

[Bill Bulat]

Another (maybe remote) possibility is that physically (during testing), multiple side-by-side columns of the porous structure (such as the one represented with your 1/4 symmetry model) deflect laterally as a group when the structure is compressed (with each individual column deforming in much the same way beam buckling is depicted in engineering textbooks (Buckling - Wikipedia):

With symmetry models, we usually constrain the normal component of displacement on the symmetry surfaces. You didn't mention doing this yourself, but if you did, that would prevent the model from exhibiting the deformation mode that I'm describing.

I am a little confused by the image of your model (which appears to be 1/4 symmetry of the geometry of a single "column") and your reference to "1/14 symmetry" - I may be missing something that renders my discussion inapplicable.

Is the model that Mechanical creates for you meshed with SOLID285?:

Given your use of an Ogden material model, I suspect this is the case, but if not, these do tend to be less susceptible to mesh entanglement problems such as the one you're experiencing.

Best,

Bill

[PPosabella]

@John: The structure recovers its shape after compression is released, this is why I'm considering it as hyperelastic. I updated the material model adding the tensile testing data, the best fit was with 5 parameters-Mooney-Rivlin model (Ogden models did not fit properly), but still experiencing the same issues.

In any case, the structure does not bend on itself during simulations, so there are no self contacts at all.

 

@Bill: What I'm trying to simulate is the compression of the whole structure which has a 10x10 mm base dimension. The picture above show an element with edge of 1/14th of the entire structure (i.e., 0.714 mm). If we talk about single "column" then yes, you are right, it is one half of its edge (1/4th considering the cross-sectional area). In any case, both simulating the behaviour of a single column with or without simmetries still show no buckling. 

Also, switching to SOLID187 to SOLID285 elements didn't improve the solution.

[John Doyle]

Thanks for the confirmation.

Perhaps your first instinct was right (i.e. localized buckling).  Could you run an linear eignevalue buckling analysis to get an approximate idea as to what physical anomoly (perterbation) would be needed to induce local buckling and then introduce that perturbation into the geometry for the structural nonlinear analysis?  Also, try a displacement based load (for stability).