# Thread: Modelling Aluminium Foam in ABAQUS using crushable foam model

1. Junior Member
Join Date
2009-09
Posts
4

## Modelling Aluminium Foam in ABAQUS using crushable foam model

Hi guys,

I am having some isses with modelling the uniaxial compression of an aluminium foam using the CRUSHABLE FOAM model in ABAQUS.

I have an nominal stress-strain curve for the foam, which I converted to a true stress-true strain curve using the following formulae:

1. true stress = nom. stress*(1+ nom. strain)
2. true strain = ln(1+ nom. strain)
[NB: I assume nominal strain is negative for uniaxial compression for the above]

I then calculate plastic strain by using the formula:

3. True Plastic Strain = true strain - (true stress/modulus)

After running the analysis (using NLGEOM option ON), I plot S22, NE22, LE22 (stresses and strains in compression direction), and I get the results that i expect (i.e., true stresses, nominal strains, and logarithmic strains that I expect). The problem is that if I try to calculate nominal stress via the sum of reaction forces on the top or bottom row of nodes in my mesh, I get RF's which decrease with displacement (like my true stress-strain curve). I've been trying to figure out where I'm going wrong, but no avail.

I'd like to sort this out because I need to calculate load vs displacement graphs for spherical indentation analysis, but the loads that I am getting out of the model seem to be incorrect. I have a feeling I'm missing out on something fundamental, and I haven't been able to crack it. Any help would be greatly appreciated!

Thanks,
chris-av

P.S. I've attached my input file so that any errors can be pointed out to me.

2. Your expression for the true stress is only valid for incompressible materials, and will not be accurate for foams.

Can you explain why you are trying to determine the true stress?

-Jorgen

3. Junior Member
Join Date
2009-09
Posts
4
Jorgen,

I thought that ABAQUS requires the CRUSHABLE FOAM HARDENING data in the form of true stress and true plastic strain? I figured that stress output (S) would be true stress also.

If the expression for true stress is invalid, do I assume that the true stress is approximately equal to the nominal stress?

4. I don't recall if you should use engineering or true values - the manuals will specify that.

Typically, foam data is presented as engineering stress and strain since that is easier to obtain. If you need to determine the true stress then you need to know the Poisson's ratio as a function of applied strain. The Poisson's ratio is material specific and is typically not equal to 0.0.

-Jorgen

5. Junior Member
Join Date
2009-09
Posts
4
Thanks for your help so far.

I have had some success by assuming that true stress is approximately equal to engineering stress, and using the true strain data as the input as well.

This seems to have resolved most of the problems. However, the nominal stress from the FEM model are just a touch higher than expected. I have found that by setting the plastic poisson's ratio = 0, the results are spot on.

This leads me to believe that engineering stress is not equal to true stress, and that the Poisson's ratio needs to be taken into account when inputting true stress into the model. Does anyone know the relationship between true stress and eng. stress for a metal foam?

Chris

6. The "correct" way of doing it is to measure not only the uniaxial stress and strain, but also the Poisson's ratio and the volumentric response.

You can then easily convert between true stress and eng. stress since (in uniaxial loading) true stress is simply force divided by current area, and the engineering stress is the force divided by the original area.

-Jorgen

7. Junior Member
Join Date
2009-09
Posts
4
Thanks Jorgen for your help. It's greatly appreciated.

I'm running into some other troubles now with regard to solving problems in shear and tension. When using the crushable foam model, I get convergenece errors, and ABAQUS abandons the simulation.

I have tried the shear case with a variety of mesh configurations. What is interesting to note is that ABAQUS has no problems solving the problem when it contains a single element, but as I refine the mesh I get the aforementioned convergenece errors. Any ideas as to why this is occurring?

Thanks,
Chris

8. Some FE simulations that involve non-linear materials, or contact, etc, can give convergence issues. Often a single element case is easier to solve since the displacements are all prescribed.

-Jorgen

9. Junior Member
Join Date
2009-05
Posts
13
i could not understand the crushable foam harding data in your txt file:
the yield stress getting smaller and smaller as strain goes up?why?

*CRUSHABLE FOAM HARDENING
1.228624636,0
0.82781349,0.509956883
0.79713732,0.590656559
0.781275376,0.662709546
0.795485886,0.734108063
0.813777358,0.810104554
0.816812063,0.924868275
0.818125902,1.054248536
0.839043918,1.131467806
0.779384564,1.38558583
0.705066732,1.608796943
0.438636523,2.302186333
0.241553864,2.995512679

#### Posting Permissions

• You may not post new threads
• You may not post replies
• You may not post attachments
• You may not edit your posts
•