Search
Close this search box.
Notifications
Clear all

2D Fung Hyperelastic material in Abaqus

8 Posts
3 Users
0 Reactions
2,369 Views
Posts: 5
Topic starter
(@Radwa)
Active Member
Joined: 9 years ago

Hi!

Im quite new to modeling hyperelastic materials. Im trying to model aorta using built-in orthotropic Fung model in Abaqus, needing 11 constants:

b1111 b2222 b3333 b1122 b1133 b2233 b1212 b1313 b2323 c D

In the literature, a 2D fung model is assumed and b2222, b2233, b3333 and c are calculated where 1,2 and 3 axes are for radial, circumferential, and axial, respectively.

I am modeling a cylinder for aorta and using Fung model for the material section, using the data from literature for material constants b2222, b2233, b3333 and c. I assigned 0 for the rest of the constants. However, job is terminated with the error indicating the stiffness matrix is not positive definite. Knowing that I dont have the data for b1111,... what do you recommend? Should I put a small value like 1e-10 for the rest of the constants? BTW, I use D=0.

thanks for your help

Nima

7 Replies
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

First I would check the stability of your Fung model by simulating a single element under displacement boundary conditions. If that works then I would do the same thing using force boundary conditions.

I dont recall the exact definition of the different terms, but b1111 seems like an important term that should not be zero. Can you find suitable parameters in the literature?

-Jorgen

7 Replies
Posts: 5
Topic starter
(@Radwa)
Active Member
Joined: 9 years ago

Thank you very much Dr. Jorgen
In the literature, there are several people worked on this type of hyperelasticity. You suggested using a single element, but the problem is material properties. In one of the literatures I read, the parameters are as follows:
c=5 kPa, b2222=14.5, b3333=7, and b2233=0.1.
I tried modeling a cylinder, using shell, extrusion for the aorta. Then in the material properties I used these values for fung orthotropic:
c=5 kPa, b2222=14.5, b3333=7, b2233=0.1, and 1e-10 for the rest of the b, because the literature didnt have any values corresponding them, and also D=0.
I used shell membrane section with membrane elements (M3D4R) using an explicit step.
As the boundary condition I pinned one end of the cylinde and restricted radial displacement in the other. I used displacement to maintain l/l_0=1.1 to have pre-strain in the model. So far, my model works well, either assuming material properties are defined well or not. but as soon as I use another explicit step to impose mean pressure to the aorta, which is a linear pressure increase from zero to 11kPa, in the first increments of the job, it will be terminated with the excessive element distortion in some elements.
The question is, is there any way i could simplify fung model from 3D to 2D? this will ease modeling and the need for knowing b1111, ... .
And is there a way to prevent excessive element distortion? because I use small and fine mesh and still the job terminates.
Thank you very much for helping 🙂 ,)
and sorry for the length of my msg!

Reply
Posts: 3
(@kimkrogh)
New Member
Joined: 9 years ago

Hello Nima,

I am working on a problem very similar to yours. I have the 2D Fung material constants (3) plus c only. Is your model stable when you run FEA assuming the rest of the constants are 1e-10? Is there a way to verify if the results obtained with these values are correct?

I know that when 3D Fung model is used, the shear parameters in the 3rd direction is assumed to be a high value (such as 10) to assume high stiffness in that direction.

I also have a question about assigning the material orientation. My artery is not a perfect cylinder. So I am not able to create a cylindrical coordinate system with a single center. Since I am using 2D Fung model, should I stick to using a rectangular coordinate system (or just the global coordinate system)? My concern is, would this not lead to different fiber directions in every elements local coordinate system? How did you apply the material orientation to your model?

Thanks

Mirunalini

[QUOTE=Nima.,12856]Thank you very much Dr. Jorgen

In the literature, there are several people worked on this type of hyperelasticity. You suggested using a single element, but the problem is material properties. In one of the literatures I read, the parameters are as follows:

c=5 kPa, b2222=14.5, b3333=7, and b2233=0.1.

I tried modeling a cylinder, using shell, extrusion for the aorta. Then in the material properties I used these values for fung orthotropic:

c=5 kPa, b2222=14.5, b3333=7, b2233=0.1, and 1e-10 for the rest of the b, because the literature didnt have any values corresponding them, and also D=0.

I used shell membrane section with membrane elements (M3D4R) using an explicit step.

As the boundary condition I pinned one end of the cylinde and restricted radial displacement in the other. I used displacement to maintain l/l_0=1.1 to have pre-strain in the model. So far, my model works well, either assuming material properties are defined well or not. but as soon as I use another explicit step to impose mean pressure to the aorta, which is a linear pressure increase from zero to 11kPa, in the first increments of the job, it will be terminated with the excessive element distortion in some elements.

The question is, is there any way i could simplify fung model from 3D to 2D? this will ease modeling and the need for knowing b1111, ... .

And is there a way to prevent excessive element distortion? because I use small and fine mesh and still the job terminates.

Thank you very much for helping 🙂 ,)

and sorry for the length of my msg!

Reply
Posts: 5
Topic starter
(@Radwa)
Active Member
Joined: 9 years ago

[QUOTE=mirukpt,12858]Hello Nima,

I am working on a problem very similar to yours. I have the 2D Fung material constants (3) plus c only. Is your model stable when you run FEA assuming the rest of the constants are 1e-10? Is there a way to verify if the results obtained with these values are correct?
I know that when 3D Fung model is used, the shear parameters in the 3rd direction is assumed to be a high value (such as 10) to assume high stiffness in that direction.

I also have a question about assigning the material orientation. My artery is not a perfect cylinder. So I am not able to create a cylindrical coordinate system with a single center. Since I am using 2D Fung model, should I stick to using a rectangular coordinate system (or just the global coordinate system)? My concern is, would this not lead to different fiber directions in every elements local coordinate system? How did you apply the material orientation to your model?

Thanks
Mirunalini

Hi Mirunalini
Unfortunately, my model is not stable. Even with no applied forces or displacements, and only with clamped BC, I still get my model distorted!
Im sure the problem is because of the parameters b_ijkl. Im still working on it but yet couldnt find any literature using the 3D fung model.
And about the orientation, I suggest partitioning your model and assigning orientation to each partition. However, Im not sure this works!

Are you using solid or shell for modeling the geometry? and what are the material constants you are currently using? which part of the aorta are you modeling?

Reply
Posts: 3
(@kimkrogh)
New Member
Joined: 9 years ago

I cannot partition my model easily since it is not axisymmetric and is derived from CT scans. so it is subject specific. I am using solid tetrahedral elements for my model, although someone recently suggested using hex elements. I havent tried it yet. I am working with rat abdominal aortas, so the material constants vary from those of human AA.

Let me know if you make any progress with respect to the 3D to 2D reduction. I will keep you updated too.

[QUOTE=Nima.,12860]Hi Mirunalini

Unfortunately, my model is not stable. Even with no applied forces or displacements, and only with clamped BC, I still get my model distorted!

Im sure the problem is because of the parameters b_ijkl. Im still working on it but yet couldnt find any literature using the 3D fung model.

And about the orientation, I suggest partitioning your model and assigning orientation to each partition. However, Im not sure this works!

Are you using solid or shell for modeling the geometry? and what are the material constants you are currently using? which part of the aorta are you modeling?

Reply
Posts: 5
Topic starter
(@Radwa)
Active Member
Joined: 9 years ago

I finally managed to model ascending aorta using material constants from a paper, as here:
b1111=14.5 b1122=0.1 b2222=7 b1133=b2233=b3333=0.0001 b1212=0.05 b1313=b2323=0.0001 c=5000 D=0.1
I used M3D4R membrane elements on a fairly straight segment of an ascending aorta (shell cylinder)
I used 3 steps, first and second steps were static, general, for stretch=1.1 and mean aortic pressure of 9000 Pa, respectively. Then I used an implicit scheme for the time-varying pressure during a 0.8 seconds cardiac cycle.

Now, I want to model a thick 5mm glue on it. Knowing that the aorta is modeled as shell with 1.3 mm thickness, should I use solid or shell for modeling the glue on it? The glue is a 1 mm length and 5 mm thickness cylinder. I myself think that since the thickness is 5 times bigger than the length and is about 1/2 of the radius of the aorta, it should be modeled as solid.
I appreciate any suggestions on this matter.

Reply
Page 1 / 2
Share: