Hello, I’m new to finite elements and i would like to model a rubber diaphragm deformation. The material is a hyperelastic with the polynomial N=1 method.
But I’m facing serveral problems :
1- The model is not converging, but “failed with results”, and the result obtained is close to what is happening in the real diaphragm.
2- To help the model converge i refined the meshes, this didn’t help the simulation to converge, and gave me less realistic results.
I don’t know what this part looks like initially but the deformation seems to be large (what is the level of strain at the end of what converged?). It can be hard to achieve convergence in CalculiX in such cases.
It’s pretty much impossible to tell what caused non-convergence without knowing more about your model (boundary conditions, loads, interactions, constraints and so on) and possibly having access to the file with its setup, also to be able to run some tests. First of all, what are the constants of that material model and where did you get them from ? Also, why are you using this particular hyperelastic model ?
If I were you I would build a computational test bench for new material models.
Before going to the real model, you can test there your combination of coefficients and see how the material responds and its limitations.
For hyperplastic materials three types of tests are usually defined.
Uniaxial, biaxial, and planar.
Your model will be standard, and you can reuse it as many times as you want. From it you can extract very valuable information such as Stress Strain curves of your material and detect which are the limitations of the material and the coefficients you have defined…
Try to represent it for your material and post it and see what the curves look like.
Apart from my recommendation, your problem seems to be one of boundary conditions. ¿Do you have any symmetry conditions established?
You see some discontinuities in your model. ¿Is that intentional?
To reduce the computation time, I cutted the diaphragm to 1/4 and putted a boundary condition on the free sides. I also fixed the bottom edge.
For the load : it’s a uniform pressure at the top of the diaphragm.
For the material, I tried several ones (Odgen, Mooney-Rivlin, Neo-Hook), but none of them converged for my targeted displacement (15mm), and the one I’m using now is one that i took from a tutorial (*HYPERELASTIC,POLYNOMIAL,N=1
0.596207632,1.18322862, 17.7884311) . It gave me good results with my first meshing but i’m not sure of how reliable this result are since it didn’t converge
Thanks for your answer !
I’m not sure of what you mean by computational test bench : Is it for exemple building a cylindrical sample with my material and applying several contrains (Uniaxial, biaxial, planar) and following his behavior/reactions for each ?
And if this is what you mean, can i do it with prepomax or do you recommend me another free software ? also do you have maybe a source that I could rely on for this tests ?
For the discontinuity, I guess it was just a post processing error, because I cutted my diaphragm to 1/4 to reduce the computation time and then respresented the whole diaphragm via circular symmetry, but if i do the same with X and Y symmetry, i don’t have the discontinuity anymore
I would refine the mesh also away from the region of load applications, it’s really coarse there (just 1 tetra element through thickness). Also, try using prescribed displacement, maybe even applied via a rigid tool for more realistic analysis. The point is that load control may cause non-convergence in such highly nonlinear analyses.
Furthermore, decrease the initial increment size.
And the question is whether those hyperelasticity constants make sense here. They should be taken from experiments or literature discussing a similar type of rubber.
Wow. You are very brave. jajajaj. Welcome to Nonlinear buckling analysis of thin shells.
Check min 28:00 of the atteched vid. This is a very interesting and complex subject.
Thank your for mentioning this. I would also recommend the videos and blog posts by Łukasz Skotny from Enterfea. He’s a specialist in the area of FEA of nonlinear buckling of shells but uses different software.
Material model under compression is non convergent and provides uneven behavior depending on the Stress state. (It’s predictable due to the degree of the polynomial.). In any case, some right values would have provided acceptable solution.
Evaluation in Abaqus shows that this material is stable for strain range -0.5 to 0.5 but it still can be wrong. Like I said before, hyperelastic constants should come from physical tests or literature.
Prepomax could directly provide this curves in an easy way if the user could request custom formulas in the history output. This could be a nice improvement.
These constants seem to be a source of errors for most users. They are not really that complex to understand. I think the problem is that one wants to do a simple test and is used to take values that one finds out there. These constants must fulfill a series of requirements such that the energy density function is always positive. Some constants can be correct within a range of stretching and not be correct a few mm outside it. It is well understood if one thinks of them as the coefficients that arise from a polynomial regression such as those seen in Excel curve fit . Outside , the aproximation can diverge very quickly (see Graph). Draw a curve between some points and move the center ones slightly. The ends get crazy very easily. Now imagine that this curve is the elastic energy of the system!!!. You have to adjust the coefficients very well and not to go out of the range of validity. And especially the D1 coefficient. Abaqus formulates D1 with units of energy density ^-1. This causes errors systematically if values are taken from other formulations.
An important consideration in judging the quality of the fit to experimental data is the concept of material or Drucker stability. Abaqus checks the Drucker stability of the material for the first three deformation modes described above (Uniaxial, Biaxial and Planar).
This is no more no less than checking in the Stress-Strain curve that the slope is always possitive. A negative slope (Negative “local Young Modulus”) would produce large strains for an small load increment. This stability check could also be performed a priori for any hyperelastic material in Prepomax if one plots and inspect those deformation modes.
So, regarding my previous post, I should suggest not only to keep inside the Strain Range used to obtain the coefficients, but also check the slope in the Stress Strain curve for each deformation mode is always possitive in that range.
Hi @Yass9,
I have followed the thread here very closely and now have a few questions about your diaphragm. I myself have been in the product development of elastomer components for 25 years. I am not a FEA specialist, but I always have a lot to do with these colleagues. The subject of FEA and elastomer is definitely a very difficult one, but my approach was true and is more of a pragmatic approach. You have to be careful with all the theory and derivation that you do not lose the reference to the real components, but of course this is only my personal opinion and of course I appreciate very much here in the forum to learn a lot about the theory of FEA.
But now to my questions:
I assume that the component (diaphragm) is made of a silicone material with a shore hardness of about 50-60Sh(A), correct?
It seems that there is a second “hard” part in the central hole, or overmolded, correct?
Why did you put a load of 8MPa if you are going to inspect 15mm of deformation?
I just did a non-linear calculation with a hyperelastic material.
The “buckling” of the diaphragm can and will be a little off, because
pragmatic approach with the material model
the production can have an influence on the buckling behavior
the vulcanization tool may differ from the ideal model
there may be differences in wall thickness
the gating point and process parameters can have a significant influence.
Nice !!. That after buckling inscribed hexagon can be clearly recognized.
I would like to ask you about those Stress and Strain values shown on the graphs.
Are you representing values extracted from the analysis or did you plot the function?
What do the values shown on the graph represent (True, Engineering, Lagrange Strains, Von Misses, Principal Stress, …?)
Uniaxial Stress Stretch formula from Wiki is different and I’m worry if mine could be wrong too. Stresses are not close at all.
Where Stress is the First principal Stress which in this case (S2= S3 =0) is the same as VM, True Stress and Cauchi Stress. Lambda represents the Stretch ratio measured as L/L0.
According to the formula value should be 80MPa. I’m obtaining 77 MPa without too much refinement.
You really have to be careful with the true strains or engineering strains and stresses. If I had to take responsibility for the component, then the values would be realistic for me for the time being (max. 20% strain and approx. 1MPa stress). In the end, the real trick is to know the limits of the material used. Of course, other factors play a role here, such as whether the component is only loaded statically or also dynamically.
If this component were to be subjected to a fatigue test, I can well imagine that where the greatest stresses are, the component would also fail. But the regions between tensile (green) and compressive stress (cyan) are also susceptible to failure.
I hope that’s okay that I’m taking a pragmatic approach here rather than a highly scientific one, as I mentioned earlier.
