Meshing a human intervertebral disc in Ansys WB 13

[Schaerli]

Hello Everybody

I'm new in this Forum and I've read some very interesting threads in here. Therefore I thought someone could probably help me with a problem I have in meshing a human intervertebral disc (IVD) in Ansys WB 13.

First i might explain you some basics about an IVD (see picture). The Disc is composed of mainly 4 different structures. The cartilaginous endplates on the bottom and the top of the disc (green), the incompressible - jelly like "nucleus pulposus" in the center of de IVD (red) and the "anulus fibrosus" (orange). As you can see in the picture, the IVD has already been meshed with mostly Hex-Elements.

The materials of the nucleus and the endplates are represented by two different mostly incompressible, linear material laws.

The anulus fibrosus is based on a hyper-elastic mooney-rivlin material law. Because the ground substance of the anulus can't bearly take any tractive forces (in truth), the substance is reinfoced by tensional fibres in a criss-cross pattern of 30 resp. 150 degrees to the horizontal (transversal plane) (see picture above).

My problem ist now, that i want to implement this fibres all around the anulus fibrosus. This means that every orange Hex-Element needs to be reinforced by these fibres. For that reason I wrote some APDL Code (I'm just learning this script language and I'm still a beginner in writing this kind of code...):

----------
/prep7

!Materialmodell für die eingebetteten Fasern
MP,EX,1500,500
MP,PRXY,1500,0.3

!Reinf265 Elemente
SECTYPE,100,REINF,SMEAR

!Material ID 150, A = 0.03 , S = 0.2, KCN = 20, THETA = 30/150, PATT = ELEf
SECDATA,1500,0.03,0.2,20,30,ELEf,3,0.5
!SECDATA,1500,0.03,0.2,20,150,ELEf,3,0.5

!Fasern sollen nur Zugkraefte aufnehmen
SECCONTROLS,1

secn,100

*DO,i,1,48,1
esel,s,mat,,IVDL2L3_%i%
EREINF
*ENDDO

etlist,all
alls

/solu

----------

The code works and the Reinf265 elements will be created. But, the problem is now, that the "planes" in the HEX-Elements, where the reinf elements will be created in, are not alligned all the same. That means that some fibres lie in the horizontal plane, some in the side plan and so on (see picture above).

I think the problem can be solved by line up the Hex-Elements respectively the sides of the HEX-Elements all in the same direction. This must be done during or right before the meshing of the IVD I think.

Can somebody help me with that? I would appreciate every help, hint and comment .


Greetings from Switzerland,

Christian S.

 

[Schaerli]

Tensional fibres in the Anulus Fibrosus

 

[Schaerli]

Miss-alignment of the planes for the Reinf265

 

[flash3780]

I have to say, that's a really interesting, challenging problem, although it is a bit beyond my level of expertise (I don't work with anisotropic materials). There are some folks on here who work with composites and may be able to help you out. If not, the xansys.org forum has some power-users who could likely give some guidance.

Of course, if you have Ansys technical support available to you, the folks at Ansys will help you find a solution as well. Check the Ansys customer portal for possible solutions, as well.

All that said, have you looked into the LOCAL command? You may be able to develop a function to determine the fiber direction at a given the coordinates of a particular elements. I would (rightly or wrongly) probably attempt to step through all of the elements that I wished to reenforce with a *DO loop, assigning them local coordinate systems as I went based upon a function that returns the fiber direction for a given x, y, and z global coordinate.

Perhaps in this particular case, a function for the fiber orientation would best lend itself to a cylindrical coordinate system? If so, maybe the CLOCAL command would work better than the LOCAL command. I say this because you could likely define your fiber direction as a function of only THETA and Z for each layer if you were using a cylindrical coordinate system.

In order to determine the coordinates of each element centroid, I think you'll want to use the *GET command:

*get,elem_x,e_num,cent,x
*get,elem_y,e_num,cent,y
*get,elem_z,e_num,cent,z

And, I was thinking for each element you'd do something like this:

csys_num=csys_num+1
clocal,csys_num,0,elem_x,elem_y,elem_z,th_xy,th_yz,th_xz

Also, I wonder if there's any symmetry in your model that could be utilized.

I wish that I could be of more help. Good luck!

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio

 

[msquared48]

Kudos for your efforts here. It's way beyond me too. But as I get on in life, I find that there is more for me to learn all the time.

I wish you well.

Mike McCann
MMC Engineering

 

[S275]

Very interesting and wish you all the best
Yesterday I was searching for some sources for structural stel material properties and found myself in this Biomesh web site

http://www.biomesh.org/

I though of sharing in case you haven't been there before
Good luck

 

[Schaerli]

Hello Everybody

Thank you very much for your help to solve my problem.
I tried to use some other WorkBench mesh options as well. The Ansys support adviced me to use a multizone mesh. Because it is very important for the positioning of the reinforcement elements that the element connectivity is consistent...

This is by default ensured in ANSYS MAPDL (that is why the reinforcement elements technology is available for ANSYS Classic in first place).
One could however still achieve consistent element connectivity if using the MultiZone mesher.

With the multizone mesher I was able to align some of the base hex elements but not all of them unfortunately...

So the next step I go for, is to write some APDL or Matlab code like flash3780 wrote to generate my fibre elements.

If anybody of you have some other ideas, please let me know .

Greetings from Switzerland
Chris