Isotropic elastic material to model fascia

[Antoine]

Hello FEBio Forum,

We are trying to model fascia as an isotropic elastic material, Young's modulus: 350 MPa, Poisson's ratio: 0.4. We expect the material to undergo large deformation with approx. 1000 N loading. We understand that isotropic elastic material may not be the correct definition to use in FEBio, as seen from an earlier thread (Link), when large deformation is expected; however, we are trying to recreate a model previously built in Abaqus using the biological definition (though super-simplified) given by Wright et al., (Wright et al., 1964. J bone joint surg).

When running the model in abaqus with the isotropic elastic material definition we do see large material deformation (see images attached) yet the part is able to complete its task (i.e. pulling on one bone to bring the articulating cartilage into contact with an opposing surface). Yet in FEBio the fascia exhibits large deformation but does not bring the two surfaces into contact. We are currently using a pressure load to apply the 1000 N, is it possible that nodal force would be more appropriate or is the material definition the factor of grievance?

Toe1.JPGtoe2.JPG

Any help would be much appreciated!

Many Thanks,

Oliver

[maas]

Hi Oliver,

I assume the images show the Abaqus models? Can you show us what the FEBio result looks like?

It could be the material. I suspect Abaqus' model uses linear elasticity. FEBio does not have a linear elastic model. The "isotropic elastic" is in fact a St.Venant-Kirchhoff material, which can be used for small strains and large rotations. However, for large strains this material behaves unrealistic. Of course, a linear elastic material behaves unrealistic for large strains as well, put the two materials will react differently.

It could also be the boundary conditions. I'm curious, how are you applying a 1000N load with a pressure load? You must have the area in order to apply a pressure. But the area can change as a result of the deformation. Does the approach you used in FEBio differ from the one you used in Abaqus? In any case, I do not recommend nodal forces. Finding the correct nodal forces to apply a distributed load is quite tricky as it requires taking into account connectivity and element size. (you can't just take 1000N and divide by the number of nodes.) An alternative is to connect your surface to a rigid body and then apply the 1000N load directly to that rigid body.

Cheers,

Steve

[Antoine]

Hi Steeve, thank you for your answer, and sorry for the long time in replying.

It's the FEBio model but we can provide pictures of the Abaqus model if you're interested.

In order to apply the pressure load on the two plantar fascia, we measured the surface of application of the pressure (using the position of the nodes). Then we fixed these two surfaces so they can only move according to the direction of the load, so we minimised the geometric change of this area during the deformation.
Then, by using P=F/S we deduced which pressure to apply to model the correct force.
We have changed the Poisson's ratio so it represents an incompressible material, which we assume, fascia and ligament behaviour reacts in a similar way.

The behaviour of the plantar fascia seems to be more compliant, but then, we are facing another issue: the sliding contacts on our model are not working properly. Instead of sliding against each other, the surfaces are going into each other.
We worked on the relation slave/master and on the penalty factor but we reported no change in the results.
As we are relatively new user of this software, would you kindly indicate which factor or parameter could be linked with this abnormal behaviour?

Many thanks,

Oliver&Antoine

[maas]

Hi,

Would it be possible to send me the model? If I can look at the model I might be able to provide better feedback.
You can also try the following. Try turning on the auto-penalty flag. That calculates an initial penalty parameter based on element size and material stiffness. With this flag on, the penalty factor is still used, but as a scale factor for the auto-penalty value. You can also turn on the augmented lagrangian flag (set laugon to 1 in feb input file). If none of this works, I'll need to see the actual feb input file to see what could be the issue.

Cheers,

Steve

[OJMorgan]

Hi Steve,

Pairing the auto-penalty and augmented lagrangian contact worked! Thanks for your help on this. We've moved to modelling the biphasic properties of cartilage now but when I try and edit the FEBio script I find that a large portion is missing. It's strange as the only change I've made to the model is to add a biphasic material. At first I thought it may have been a problem with the original model but when I revert the material properties back to isotropic elastic the script is complete and the model runs. I've looked through the forum and not found this problem (though I may have typed in the wrong keywords). Is this a problem you've experienced?

Thanks,

Oliver

[OJMorgan]

I've figured out the problem. Thanks again Steve.

Many Thanks and Kind Regards,

Oliver