I am currently modelling a load being applied in the joint zone of a hemipelvis, which correspond to a person while one leg standing.
Previously, I validated my model with an already existent one from the literature by focusing on the contact area and contact pressure parameters. Nevertheless, when it comes to comparing Von Mises stress between both models, the result variance has increased.
I have asked myself this variance question without yet confirming which is the cause.
Both models have the same boundary conditions and the same magnitude of load. Additionally, they also use the same elements and order of elements(C3D4).
After comparing displacement between them, it seems to be a slight difference (higher in the literature validated model) between them. I attribute this difference to the fact that the already validated model has a smaller thickness than mine in the zone of interest where the load is being transmitted..
Since von Mises stress is calculated from displacement in nodes, it seems plausible to me that the differences in stress between my constructed and the already validated model is due to thickness difference ergo displacement and stress.
Can somebody aid me on this matter?
Hello Jose Gaxiola
Can you provide the Abaqus model (.inp)?
How did you define the contact?
Are there penetrations in the model?
You should use C3D10 elements. https://ww3.cad.de/foren/ubb/Forum254/HTML/003707.shtml
Also be aware that contour plots always need inter- and extrapolation to the nodes, so what you see in the plot may not be what happens at the integrations points. Try using the quilt option and/or use probe values to see what actually happens at IPs
The two different versions of software may also vary the results. It depends on the accuracy of the software. Please check once with the versions.
Hi Nils Wagner ,
Thank you for the advice. I am currently using a surface to surface contact with frictionless tangential behavior. I am not using quadratic elements(C3D10) in my model because I'm trying to validate my methodology compared to an already existent model which used linear. Hence, that's why I am not using them.
Unfortunately, because of the current remote work circumstances I cannot have access to the .inp. Nevertheless, I have hypothesized that difference in stress is given by the difference in displacement, which I attribute to the thickness difference among geometries. Therefore, this is what I am currently trying to prove.
Hi Martin Baeker ,
Thank you for the advice. In fact I know that interpolation first happen from nodes to IP to calculate stress and then projection is calculated for stress to be determined in nodes.
I have used the quilt contour option to see element behavior instead of as banded contour and have an idea on what's the difference, which I have mention in my previous comment.
When comparing von Mises stress values, I am exporting a rpt file based on integration points because extrapolation of values in nodes might cloud the actual result.
It seems as if your model is stiffer, look at the properties, DOF 3or 6 ?. How is your model fixed at the lower bone section? do you allow any motion? Number of elements in your model the same? is load applied to the same geometrical point or location in the two models?
Hi Nicolaos Kokavesis
Both models use the same young modulus and poisson ratio for the materials involved. Also, because in both models there are linear elements, DOF is subjected to 3 only per node.
In the lower bone section, the boundary is fixed for them (i.e. no displacement or rotation allowed). The motion of the pelvis is directed towards the femur as it should be while performing a one leg stance activity.
The number of elements vary because the geometries are different; nevertheless, the seed size used in both is the same in order to abolish this element difference.
Last, the load is being applied at the same point in both models because point's coordinates are the same.
I built a new model(second) with a similar thickness in the zone of contact as the model that already has been validated and I found that the difference of magnitude of stress in the zone of interest between the newly built model and the already validated is really similar. Thus, I strongly believe that this might be a good reason for the difference between my first model and the already validated one.
For sure sectional properties such as thickness is a factor as stresses are distributed in more material and stresses should be lower in thicker model. Regarding the fixing of the model I think it would be more realistic to allow for some displacement at fix point instead of 0's. There is some elastic energy stored in the system that should be accounted for. Else you will have higher forces at the femur head. Then it all depends on what you want show.
Hi Nicolaos Kokavesis
Thank you for the response and advice. I agree that displacement should be allowed ideally. Nevertheless, the purpose of this exercise is to model a person that is standing on one leg. Therefore, the condition analyzed is static. In reality, this doesn't happen as ideal and the joint experience a dynamic movement instead.
However, because my focus is not in the femoral neck, which is where stress concentration occurs normally, I am pursuing the aforementioned boundary conditions.
I compared overclosures between both models in the contact zone and was able to spot the differences in cartilage thickness before load was applied. To my understanding, this enabled more displacement in the validated model with lesser thickness in the zone of contact and interest. Hence, this displacement contributed to a higher peak value in Von Mises stress. Would you agree on this reasoning?
- Badges
- Science topic
- Similar topics
- Biological Science
- Physiology
- Physiological Processes
- Stress