Crushable foam

[VaidehiChennubhotla]

Hi,

A Crushable foam material model was used for compression test on a 50x50x50 mm block. The compression test data (FS curve) was overlaid on the CAE data. The test data seems a little softer as it we go down the curve, compared to what I am getting in the analysis. I have played around with parameters like K, Kt and poisson ratio and adjusted the test data to have more spacing. It didnt help. Then I tried using a single element mesh for the foam block, it made the curve stiffer. When I removed the indenter and removed global stabilize from my model it became softer. Either way, I am having difficulty to match the CAE data to Test data. What more can be done to the Crushable foam material card, to make it match with test data ?

Any help would be greatly appreciated.
Here is a picture showing test vs CAE data.

Thanks,
Vaidehi

 

[FEA way]

In such cases the most important factors, apart from material model, are element type and mesh density/quality. It is important to select elements and control their behavior (including control of undesirable effects such as element locking). So the question is which element type do you use and did you try other types ? Are you sure there’s no volumetric locking ?

 

[VaidehiChennubhotla]

Hi FEA way,

I used C3D8R for foam. I have played around with mesh density(Single element vs 6 elements along length). In above graph, yellow and blue curves are 6 elements along length. The rest are single element. I do not see any volumetric locking in the .dat or .msg files. However, I see these warnings in the .msg file.

***WARNING: THE PLASTICITY/CREEP/CONNECTOR FRICTION ALGORITHM DID NOT CONVERGE
AT 4 POINTS
***NOTE: MATERIAL CALCULATIONS FAILED TO CONVERGE OR WERE NOT ATTEMPTED AT ONE
OR MORE POINTS. CONVERGENCE IS JUDGED UNLIKELY.
Regards,
Vaidehi

 

[FEA way]

To check for volumetric locking you can compare deformations with stresses.
Maybe you will have to change some settings of the material to calibrate it so that it fits experimental results. Remember that input test data should be defined in terms of nominal stress-strain for hyperelastic materials.

 

[VaidehiChennubhotla]

Hi FEA way,

I didnt understand what you meant by comparing deformations with stresses. I have tried with different element types like C3D8, C3D8S, C3DI, C3D8H, C3D8HS, C3D8RH, C3D8IH, C3D20R, C3D20RH, C3D20, C3D20H. But it didnt help much.

As you can see, I have played around with material settings / parameters like k, kt, Nu etc what more can be done ?

I believe Abaqus requires true stress/strain. The compression test data which I got from Zwick machine was force-deflection data. I have calculated True stress as force/Area of cross section . And true strain as change in deflection/original length.

And calculated the plastic strain = Total strain - Elastic strain. Here I am using Crushable foam material card and not hyperelastic material card.

 

[FEA way]

What I meant is that you should compare overall levels of stresses and deformations. Volumetric locking would result in high stresses but low deformations (overly stiff behavior - that's why it's important to check it in this case).

Right, I forgot it's not hyperelastic material but crushable foam.

I see that single element didn't help much so far but generally it's a very good idea to calibrate material using single element test - remove indenter, apply compression as boundary condition instead (be careful with BCs) and try to match the response with actual behavior. You can use "Simple tests on a crushable foam specimen" chapter of Abaqus documentation as a reference.

 

[VaidehiChennubhotla]

Hi FEA way,

Yes I looked at the Stresses and deformations. At a small deformation of 0.88mm there is a large force of 1397 N. There seems to be volumetric locking. What could be done to prevent volumetric locking ?

Thanks,
Vaidehi

 

[FEA way]

Volumetric locking usually occurs in fully integrated elements but it can happen in reduced integration elements too. In such case one should use hybrid elements. But maybe in your case something else is causing the problem. If you perform single element test with proper BCs (as those in the documentation problem I mentioned before) then pretty much only possible reason left will be an error in material definition.

 

[VaidehiChennubhotla]

Hi FEA way,

Are you referring to

https://classes.engineering.wustl.e...ks/bmk/default.htm?startat=ch03s02ach161.html

documentation problem? There is no reference to Boundary conditions ... Could you let me know?

Thanks,
Vaidehi

 

[FEA way]

Yes, that's the chapter I was talking about (Benchmarks Guide --> Material Tests --> Plasticity and creep --> Simple tests on a crushable foam specimen). They don't describe boundary conditions in the text but you can download .inp files from there and review their content then run in Abaqus and open in CAE to see how they applied BCs.

 

[VaidehiChennubhotla]

Hi FEA way,

I have gone through the Boundary conditions mentioned in the chapter. Volumetric or Isotropic hardening didnt make much difference. Removing global stabilization didnt make much difference.

Single element mesh model for foam seems to make a lot of difference. It made the F-S curve very softer.

There is not much information on what kind of testing need to be done on hydrostatic compression? And how to get crushable foam coefficient (k). Would you be knowing this hydrostatic compression testing is done?

I have calculated kt=tensile yield stress/ compression yield stress = 1.7
Thanks,
Vaidehi

 

[VaidehiChennubhotla]

Hi FEA way,

Sorry for the late reply. So far I think volumetric locking is the main reason as you have mentioned. I increased the strain values in the plastic stress strain material curve of the Crushable foam. And CAE correlates very well with the Test data (compression test). But changes strain values upto 1.24 is very unrealistic in compression test and I think this is not the correct way. I shouldnt be manipulating the material as I did, its not the same material anymore. I think it is very random to change the strain values.

Stress Strain
0.2991 0
0.31 0.0107028
0.463943 0.0192756
0.522228 0.65
0.613645 0.9
0.729848 1.07
0.829368 1.19
0.915861 1.26
1.24306 1.4


Any help would be greatly appreciated.
Thanks,
Vaidehi

 

[FEA way]

I think that in this case it’s best to follow the procedure described in the documentation chapter that we were previously talking about in context of BCs (Simple tests on a crushable foam specimen). There you can find a paragraph titled Calibration of material parameters where they describe the way they calibrated crushable foam material model based on experiments. They used both hydrostatic and uniaxial compression test data (so you may need to perform additional physical testing on your material). Parameter k was calculated based on initial yield stress obtained in uniaxial test and initial yield pressure obtained in hydrostatic test. The choice of remaining parameters is also described there. Then they performed single element tests in Abaqus for both uniaxial and hydrostatic compression and found good agreement with experiment. Try the same. If you still have some mismatch at this stage then you can slightly modify the parameters but, as you said, too big changes forcing agreement shouldn’t be done. Instead make sure that you have correct test data and that parameters based on this data are also properly determined.