My question is if the increase of incomprehensibility parameter d1 of hyperelastic materials will result in less resistance to deformation of the material.
The incompressibility parameter d1 defines the bulk modulus K as K = 2/d. So as d increases, K decreases and the material becomes less incompressible (i.e. more compressible!). So yes, if the expected deformation is volumetric (i.e. change in volume), then reducing d1 will result in less resistance to that mode of deformation. But if the expected deformation has a deviatoric part (which controls change in "shape" and not the change in "volume") then resistance to that component of deformation will not be affected by d1.
You can go through the following section in Ansys Help and click on the specific material model that you are using, for more information:
Hop this helps,
Thank you for the response!
I am not sure about the change in "shape". To be more specific, I am trying to expand a stent inside an artery and the problem I am facing is that the artery compresses the stent in to a smaller diameter when the balloon deflates. Normally the stent should keep the artery open.
I am using a Mooney-Rivlin 5 parameter hyperelastic for the artery and I don't know which parameter should I alter. The goal is to make an artery more compliant to deformation and that will apply less pressure to the stent when deformed.
Is there any suggestion?
When the balloon expands, plastic deformation is accumulated in the stent but the artery remains elastic. When the balloon deflates, the elastic forces in the artery push the stent, which will reduce in diameter slightly, but the forces from the artery should not be high enough to plastically deform the stent.
Do you have plasticity defined for the stent material?
Hi Mr. Newman,
I believe the problem was not on the material properties.I was used shared topology between the artery and the plaque mutual surface. As a result, there were high stresses at the edges of the plaque on the left and right part, causing the irregular compression of the stent, as shown in the images below. I think I have to share less faces of the artery-plaque assemblage.
Shared topology is good if the plaque remains connected to the artery during stent inflation. Are you saying the plaque is sheared or torn from the artery during stent inflation?
No. What I am saying is that as the plaque is pushed down and its edges remain in the same place, because of the mutual nodes with the artery, there is a high tension in those edges (as shown in the figure below), that force this deformation on the side of the stent.If I free the edges of the plaque, they will be allowed to move downwards and the stress concentration in that area will be reduced. As a result, there will be less pressure to the stent.
Are you saying that plaque is not physically connected to an artery? I thought they were basically interconnected. What you are saying is you want to cut them apart.
It is normal for high stress to develop at the interface between two materials with different stiffness values. If the stress gets high enough, it can exceed the strength of the bond between the tissues. Do you have data on the strength of the bond between plaque and artery? If so, you can model the tearing at the interface with Cohesive Zone Elements.
Yes you are right about the connection between the artery and the plaque! Unfortunately I have no relevant data and this exceeds my capabilities.
However, I would like to thank you for your suggestions once again!
There is one more question that I would like to ask you and if needed I will create a new discussion.
In an already converged analysis of the artery-stent assembly, when I try to add a new connection and run another simulation, there seems to be an unjustified event.
While the new connection is between the balloon and the stent, the artery is also deforming when the balloon is moving, without even touching the geometry of the stent or the balloon. This "remote" movement seems to appear only at steps where the new connection is alive. Even if I remove any relation between the balloon and the artery, the "remote" deformation still occurs.
I have faced this kind of problem several times and it would be valuable of you had any idea about the nature of the problem.
You cannot add new contacts to a simulation that is solved without solving it over again.
You must put all the contacts you will eventually need into the model before you start, then use Contact Step Controls, where the contact is Inactive (dead) in Step 1 and Active (alive) in Step 2.
I would have to see the model or get a much more detailed explanation with images to comment on why something is moving when a contact comes alive.
Thank you for the advice Mr. Peter!
I think there was a problem with the geometry.
I appreciate your help!
Ansys customers with active commercial software licenses can access the
customer portal and submit support questions. You will need your active account number to register.