View Full Version : Polyurethane Foam Modeling
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.
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?
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 many models that should be able to capture the experimental data for your material and the specified loading histories.
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, I'm currently facing these issues :
1. The poisson's 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 poisson's ratio for curve fitting. I'm 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 poisson's 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 Poisson's 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 I'm 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, it's 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 doesn't allow me to do that with a message indicating that it's 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 wasn't sure about what the parameters D1, D2 signify. The curve fitting tool in ABAQUS unlike Matlab doesn't 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,
P.S : I would like to let you know that I currently work with a coarse mesh of around 1000 nodes for saving time
Just a couple of things to check, to make sure you're 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 you're exp data
-What are you're 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 shouldn't 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 haven't 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?!
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 Ogden's model. This is the way it's 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 doesn't 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 poisson's 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.
I'm currently working on Mcalibration software, another tool for predicting input parameters based on Dr.Jorgen's 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 I'm getting kind of close there, but not sure where I'm wrong, maybe mesh size or boundary settings. Should be good if you share some inputs in loading conditions or Boundary settings.
I set up a quarter sized symmetry model in Ansys. I used symmetry on 2 sides to help reduce computational time. I applied a non zero displacement B.C on the top of the sample, i.e give the y co-ord a value of -25mm. And I constrained the bottom in all directions. Could you not apply a non zero displacment, to match your experimental displacement? And you definitely need your compression stress and strain data in negative form..just multiply all your positive values by -1. In my opinion your mesh shouldn't make too much of a difference (once its not too coarse), as long as you don't go past roughly 0.5 strain as which point the mesh begins to distort wildly..
I then entered my exp data into ansys curve-fitting tool and got out a picture of the curve fit and my values for alpha, mu and beta..and got a decent cure fit.
So basically Ansys allows you to put in data and shows you graphically what your curve fit is, and gives you your parameters which you then solve the model with. Abaqus allows you to enter your data, but doesnt show you the curve fir or paramters..but the results are the same.
Mcalibration was recommended to me before, it looks like a useful tool for finding model parameters.
So what I would like to know is if it is possible to find the material model parameters (not in the .DAT file) that Abaqus is using?
Thanks for the feedback. I did exactly work like the way you have explained with a quarter sized symmetrical model in ABAQUS. I have constrained the bottom in all directions in my case too. I believe you have defined the displacement the material i subjected instead of the load applied. When I tried to define the displacement the material is subjected (it's 80% in my case , so I tried to compress the foam block to 40mm from initial 50mm), my load is exceeding by 5 times at 80% strain. Instead of 0.01Mpa measured in the experiments for achieving this strain value, I'm getting around 0.05Mpa in simulation for the same strain. Did you have any problem like this before?
You're right, Ansys does show the material parameters after curve fitting but ABAQUS doesn't with the Hyperfoam model indicating that we can evaluate the parameters only for Hyperelastic and viscoelastic materials. My guess is that it might need some extra add-on or plug-in. However, I'm thinking to call ABAQUS support to check about this.
And was a bit curious, but not sure that I wanted to check with you if the governing equation in ANSYS for the Hyperfoam is the same as in ABAQUS? I remember having waded through the ANSYS theory manual and could recall that the material model defined by Hyperfoam in ANSYS is different from material model for Hyperfoam in ABAQUS. However, I'm not exactly sure about this but just wanted to check with you.
Yeah, Mcalibration is a tool for finding the material parameters for different polymers developed by Dr.Jorgen. It helps in finding these parameters by curve fit from experimental data and by optimizing the initial solution.
I'm still stuck with this problem, So if anyone have any suggestions, I do welcome them very much.
That seems a bit strange. Well if you're B.C's are right and assuming the mesh isn't putting you off and you are comparing values at the right locations then by the process of elimination there is a problem with your model or your units. Make sure your units are all standard either N/m or N/mm and use the same for the Displacement..also make sure you're not taking the highest stress values from the model at a singularity (corner node of the model).
And if all that all that its still not working maybe you could try sending the file onto support.
Ansys has the Material model explained in 126.96.36.199 in the help and Abaqus has the same in section 19.5.2-3 of the user manual. There are some difference in the functions but I'm not sure what effects they have on a simulation
Does Mcalibration have the hyperfoam model? And are the results from Mcal and the Ansys curve fitter the same can anyone tell me?
Yes, MCalibration supports the hyperfoam model. It is very easy to calibrate the hyperfoam model using MCalibration !
so i see nobody ever answered the question as to how to get the material parameters ABAQUS selects when you input the test data. It might seem trivial but I couldn't find the answer anywhere. So for those who have trawled the message board looking for the solution....
*Preprint, model=yes in your .inp file
this will output material details in the .dat file.
Powered by vBulletin® Version 4.2.0 Copyright © 2013 vBulletin Solutions, Inc. All rights reserved.