True stress/strain data for PEEK polymer
I am working on a small FEM project involving PEEK interfacing with UHMWPE using a software package from ADINA. We are testing this construct on an MTS machine at a displacement rate of 2mm/min in our testing lab. Does anyone have any stress/strain data (curves), either uniaxial, biaxial, triaxial and in compression for PEEK at a similar loading rate that I can use as input data for material parameters? Where can I find this same data for conventional (non-irradiated) UHWMPE?
You can download stress-strain data from victrex.com, a PEEK manufacturer. Due to copyright restrictions I cannot post that data on this website without their permission (which I don't have yet). Note, in order to download the technical data you need go through a free registration.
You can also download stress-strain data for conventional UHMWPE from this page.
How are you planning on modeling the PEEK and UHMWPE?
Thank you for your reply. I have since registered at the website and have incorporated their stress/strain data into my model, along with UHMWPE data supplied by one of your papers on this website.
In regards to modeling the PEEK and UHWMPE:
1.) For element formulation, I am using 8 node elements since 10 nodes is computationally expensive at this point. I do have a thin PEEK section that for all intents and purposes can be described as a cantilever beam loaded at its end in my construct, so I have used an incompatible mode formulation to hopefully account for any significant bending. This is also a static analysis.
2.) For material formulation, at first I used a linear material formulation, however I felt this was not capturing what was occuring at this thin section, so now I am using an multilinear material formulation without large displacements/strains to see if I can capture what is occuring at this thin section.
The issue that I am having at this point is this: in the test lab, this thin PEEK section is not undergoing any plastic deformation but my FE model is predicting yield at loads smaller than in the test lab. Also, the UHMWPE is in contact with and bending this thin PEEK section. I am not sure if I am capturing what is occuring with the UHMWPE since I can see the deformation due to contact with the PEEK on the UHMWPE peice and not in the FE model. Since both of these materials exhibit some viscoelasticity, due you think the loading rates given for the published material properties has a great effect on the results or should I start to think about a more advanced material formulation?
Sorry for the long explanation, I hope I did not confuse the subject. Your help is greatly appreciated.
Overall, your approach sounds OK. It seems, however, that your material model representation might not be completely accurate. From your description it is not clear if it is the PEEK or the UHMWPE model that is off.
I have a few questions: what strain magnitudes do you expect to see in the two materials? how fast is the load applied? is it mostly bending (i.e. uniaxial loading) or is it a multiaxial deformation state? How long is the load applied on the specimen?
Also, do you have more information about the PEEK or the UHMWPE. As I am sure you know, these materials are sometimes particle or fiber filled.
The choice of material model and material model calibration will strongly influence the simulation response. There are a few good material models that can be used for these materials.
Both materials are unfilled.
The construct is statically uniaxially loaded at 2mm/min to a specified load (e.g. 1000N) on a MTS machine and then immediately released. A UHMWPE post is attached to the machine actuator and this in turn is axially compressed against the PEEK. The PEEK piece is attached to the load cell.
I would expect to see a strain magnitude of at least 2% or greater. It all depends on the final load chosen. The reason why I say it all depends on the load chosen is because it is difficult to pinpoint when the PEEK will plastically deform in this construct, hence the FE model.
Hope this helps,
It sounds like that the strains are relatively small. What I would try is to first run a simulation using linear elastic materials, and then extract the maximum stresses and strains in the system. The magnitude of the resulting stresses and strain from this simulation will indictate what material model is appropriate: if the max stress is "below yield" then linear elasticity will do; if the max stress is slightly below the yield stress then I would use linear viscoelasticity; if the max stress is larger than the yield stress than I would use a more advanced material model suitable for semicrystalline polymers (e.g. the Hybrid Model).
The choice of material model also will depend on how accurate you need your results to be, and how much effort you are willing to spend on the analysis.
Best of luck,