You can also try with the single element model from here: HYPERFOAM Model Issue - #10 by Calc_em
Now you have to fit your data with the hyperfoam model N=2 to identify the actual parameters that best fit your model.
For the moment thanks a lot to everybody. 
Using the N=1 parameters twice is a great idea but I would like to add an small correction. One would be doubling de energy U=U1+U2=U1+U1=2U1.
First parameter should be divided by 2.
u1/2, 3.0, u1/2, 3.0, 0.05, 0.05
2 Likes
you can check CCX results with the model and data provided here (is a model with N=3).
4.22. Hyperfoam Model — LAMÉ Manual
Bug reported: Hyperfoam material model showing incorrect deformation with no stresses · Issue #188 · Dhondtguido/CalculiX · GitHub
1 Like
There are some great resources for such material models within the Dassault Systemes SIMULIA community, but you need to register there to access them. This post summarizes resources for the hyperfoam model in Abaqus (of course, in addition to its documentation): 3DSwym
Btw. it also says there:
If you base a *Hyperfoam material model on only uniaxial compression test data, it is likely that the simple shear behavior of the material model will be very wrong - orders of magnitude wrong. The 2006 paper by Petre and Erdemir point this out very clearly.
And mentions the Kossa & Berezvai 2016 paper too.
Dassault offers a cloud app that can calibrate such materials.
And you may want to check this project too: SimTK: Determination of elastomeric foam parameters for simulations of complex loading: Project Home
Or this thesis:
Petre, M. T. Determining material parameters for multi-axial simulations of elastomeric foams, MSc Thesis, Department of Biomedical Engineering, Case Western Reserve University, Cleveland, OH, USA, 2005.
1 Like
If you want to use Transfinite Gmsh, make sure that you select the volumetric (solid) part, not the surface (shell) one. And import it in STEP, not STL format.
However, Transfinite Gmsh requires all subvolumes to have 5 or 6 faces with 3 or 4 edges each, so you would need to partition your part (split it into multiple subvolumes fulfilling this requirement) in CAD software first.
But here you could just use Extrude Mesh or Sweep Mesh instead to get a hex or hex-dominated mesh. Just select the top or bottom surface for the extrusion/sweep.
And first make sure that your material model works as expected though (single element test should suffice for that).
1 Like
You should also enable recombination because now you only have wedge elements. When you do it and obtain hexahedral elements, it’s important to choose their type (in the FE Model tab when you edit a part). Try with C3D8R for now.
1 Like
Because you have to enable Recombination for Extrude Gmsh first and remesh to get hex-dominated mesh.
1 Like
Yeah, but the mesh in the plane is very coarse. Try refining it now. The mesh must be dense enough, but also designed in such a way that the elements don’t distort excessively when subjected to deformation (especially compression).
Can you share the .pmx or .inp file to see what combination of features eventually worked ? I guess you had to play with the hyperfoam constants ? And it diverged only close to the end (before reaching the complete 10 mm) ?
My posts are hidden because of SPAM ???
@Durbul Can you fix it ? Sometimes threads like this one are getting unlisted for some reason:
Done. Sorry @Viertelstein, Discourse has some automatic spam detection that is sometimes triggered if the same user posts many images.
2 Likes