I am trying to model a sandwich panel with a polyurethane foam using ANSYS. I am unfamiliar with the modeling of foam and was hoping for a recommendation on what types of tests would give me the data I need and also what material models would be the best to use. The type of foam is ELASTOPOR P 15390R Resin/ELASTOPOR P 1001U Isocyanate. It is a two component polymeric MDI based system utilizing water and HFC-245fa as blowing agents. Any information at all would be appreciated.

# Polyurethane Foam Modeling

Foams are typically characterized by a combination of uniaxial tension, uniaxial compression, and confined compression experiments. As an alternative to the uniaxial experiments, you can also use shear experiments. Note that for foams it is important to perform some kind of confined compression or triaxial compression experiments.

The best choice of material model will depend on the strain levels and degree of accuracy that you need from your simulations. What strain levels do you need to simulate, and what temperature and strain histories are you interested in?

Jorgen

The sandwich panels are panels for air handlers. The amount of strain is fairly small. In flexure tests of the panels so far it is less than .5 for a 96 long panel. Temperature is not too important for this application. The temperature the foam will experience does not vary too far from room temperature.

It sounds like you are mostly interested in small strains, and that the deformation state is mostly tension, compression, and perhaps some shear.

Based on that I would start by performing exactly those experiments: uniaxial tension, uniaxial compression, and simple shear. I would then initially attempt to fit a hyperfoam model (*Hyperfoam in ABAQUS) to the data. Note, there are [b]many[/b] models that should be able to capture the experimental data for your material and the specified loading histories.

Hello All,

For some reason, I am not able to start a new thread and hence posting my query here as the subject was more relevant!

I am trying to model uniaxial compression of low denisty polyurethane foam in ABAQUS. For doing this, I have carried out a uniaxial compression test of a solid foam block in Instron and with the experimental data, I have found the values of Myu1, alpha1, Myu2 and alpha2 by curve fitting in Matlab. When I tried to incorporate these values into ABAQUS and run a simulation on a same sized foam block, Im currently facing these issues :

1. The poissons ratio was assumed to be zero as suggested in the Polymer Foams Handbook by N.J.Mills citing couple of references who have used zero poissons ratio for curve fitting. Im able to run the simulation with this case, but the load at 80% of strain in experiments (10N) is achieved at 20% of strain in Simulation.

2. This made me to search for some more references as I speculated poissons ratio for low density foams might be significant and came across the classic paper of Mr. Roderic Lakes in 1988 Science journal titled Foam structures with a negative Poissons ratio. A detailed study from other papers helped me in understanding that the P.R for low density polyurethane foams with density of 24Kg/cu.m varied from -0.28 at 2% compresion to -0.03 at 45% strain. As the density of the foam that Im trying to model is around the same range, I used these values of -0.28 and -0.03 in the Nu1, Nu2 input parameters of Hyperfoam model in ABAQUS. But still, its the same result and no improvement is obtained in the curve.

3. Alternatively, I tried using the uniaxial test data directly with the Hyperfoam model in ABAQUS and tried to evaluate the curve fit parameters, but it doesnt allow me to do that with a message indicating that its possible only for Hyperelastic and viscoelastic models. I then tried using the Hyperelastic material model and tried to fit the curve with Ogden model, but I am obtaining a Negative Shear modulus (Myu1) value when I did so. I believe though it says Ogden fit, it has a different governing equation and wasnt sure about what the parameters D1, D2 signify. The curve fitting tool in ABAQUS unlike Matlab doesnt allow user to customize limits to which the values need to be restricted . But I was able to get some improvisation with the maximum load being achieved at 30% strain in this case.

1. Is there some improvement that I can work in my model to overcome this problem. Can anyone suggest me the correct apporach for modeling a problem like this?

2. Have anyone tried fitting the experimental data with Hyperfoam model in ABAQUS and achieved the material constants? If so, can someone suggest on where I should look on for this?

Thanks very much to whosoever in advance,

Enticer

P.S : I would like to let you know that I currently work with a coarse mesh of around 1000 nodes for saving time

Hi,

Just a couple of things to check, to make sure youre modeling the foam correctly..

-Is it a static model and are you just applying a non-zero B.C to the top of the sample?

-Have you inputted your compression data (both stress and strain) in negative form, this is the form abaqus requires

-How are you measuring the stresses in the simulation, to compare with experiment? Maybe if you could measure the overall reaction of the nodes/elements under the plate, and then compare these to youre exp data

-What are youre paramters gotten from your matlab program, and how did you get them..are you sure they are correct?

I think it is standard enough to assume 0 poissons ratio, so that shouldnt have a huge effect. I have successfully input data into the abaqus material section for a hyperfoam model in the GUI, and have gotten good results but I havent been able to view the parameters in Abaqus so if anyone knows how to find the parameters after inputting experimental data that would be very useful to me?!

Polyu

Hi Polyu,

Many thanks for your rpely.

1. Yeah, mine is a static model with a cubical block of 50 x 50 x 50 (all in mm) and I apply a load of 10Kpa on the top of the sample. Only BC that I apply is to the base which is prevented from all translations and rotations. So, I guess this is pretty much simpler in setting the model.

2. I remember having tried once but I have working mostly with positive values. I probably will have to rework on inputting the stress and strain as negative values and will revert on this.

3. I measure the cauchy(true) stress vs logarithmic strain at a particular node by selecting a node. And then I convert these true stress vs logarithmic strain data to nominal stress vs nominal strain to compare with my experimental data which is of the same form using the general engineering formula ,

True stress, e = ln(1+E) E, E being engineering strain that needs to be found

True strain, s = S (1+E) S, S being engineering stress that needs to be found

4. The parameters in Matlab have been found by curve fitting of experimental data to Ogdens model. This is the way its been discussed in Polymer foams handbook by N.J.Mills which I believe is probably one of the versatile book on foam mechanics. From my understanding, these values seemed to be right when I compared the values with works of other researchers in this area. For instance, My foam blocks weight density is 17.84kg/m3 and the parameters that I have obtained from Matlab are

Mu1 = 0.105 Kpa

Alpha1 = 11.19

Mu2 = 18.04Kpa

Alpha2 = -7.492

Polymer foams handbook discuss the parameters obtained for a 41kg/m3 foam by Setyabudhy et al (1997) as Mu1 = 18.3kpa, Alpha1 = 17.4, Mu2=0.21kpa and Alpha2= -2 with Poissons ratio = 0. Here the values of Mu1 and Mu2 seemed to be inverted but that doesnt affect the curve fit. I have obtained a curve fit with almost same goodness level when Mu1 and Mu2 values are swapped.

My speculation is the foam that I work with is a softer one when compared to the 41kg/m3 foam discussed in Polymer foams handbook. And hence, there should be a significant effect of poissons ratio in my case. I tried working on the curve fit again considering P.R but with these values, my model is showing me an error code 144. There has been no proper documentation that I have come across for this problem. And when I assume nil P.R, I face the problem mentioned in my initial post.

Im currently working on Mcalibration software, another tool for predicting input parameters based on Dr.Jorgens suggestion (owner of Polymerfem)

Just was a bit curious, did you work on something for the getting these input parameter values from any other curve fitting procedure. I guess Im getting kind of close there, but not sure where Im wrong, maybe mesh size or boundary settings. Should be good if you share some inputs in loading conditions or Boundary settings.

Thanks,

Enticer

- Simulation of soft open foam8 years ago
- Crushable foam Simulation inAbaqus8 years ago
- Thermoforming Simulation of Polymeric Foam Materials9 years ago
- Experimental Data for Foams10 years ago
- Hyperfoam vs. Ogden Foam10 years ago

- 21 Forums
- 3,923 Topics
- 13.3 K Posts
- 7 Online
- 29.7 K Members