Soft Material- Jacobian Error

swarajswaraj
Hey,
SoI finally bought Mecway and started working on a dental project. This project is about estimating teeth movement due to the aligner. The teeth root is surrounded by a soft material which is called Periodontal Ligament. Please take a look at the attached picture, the image on the right is the isolated view of the PDL. The thing is I am getting jacobian error and I cant do anything about it. The Youngs Modulus of PDL is 1 MPa. Please tell me hw to fix it

Comments

  • swarajswaraj
    Boundary Conditions,
    Force is applied to one node of the teeth above the PDL, and the teeth root is bOnded with PDL
  • SergioSergio
    edited March 2018
    Hi Swaraj, welcome then! I'm working on a similar project. Have sense to include in the model such a soft tissue? I meant, jaw bone will be several orders of magnitud stiffer than the PDL.

    Check this article about Jacobian error, maybe you could try to use a different kind of mesh (hexas)

    https://knowledge.autodesk.com/support/simulation-mechanical/troubleshooting/caas/sfdcarticles/sfdcarticles/Error-Non-positive-Jacobian-in-Simulation-Mechanical.html


    Regards
  • swarajswaraj
    Hey Sergio,
    The thing is when I am trying analysis for each separately, Its working. I have a stl of teeth. So my choice is to make tet 10 element. I am refining my model in meshmixer and making it a solid by using freecad then going to Salome and meshing it. The number of faces i had in stl IS STILL THE SAME WHEN I DO VOLUME MESH IN SALOME. Its just a random informaton i wanted to throw. I have so many doubts and nobody to clear so i vomitted it all out
  • VictorVictor
    It's supposed to mean the element is so badly shaped that it's not really a solid anymore - eg partly inside-out.

    It sounds like you're near to solving it if it works for each part separately. That indicates the mesh isn't faulty. Are you using *TIE to join them? That deforms elements if they're not perfectly aligned, and could lead to this error.

    CCX also generates that error for very small elements in a very big mesh. I think if the length of the smallest element is maybe 5 or so orders of magnitude smaller than that of the overall structure, it can happen.

    For nonlinear, it might be too soft and deforming to an inside-out or other impossible shape. That might require finer mesh or correcting a boundary conditions mistake, or a better material model (linear elastic materials can't be compressed too far in non-linear analysis or they reach an instability). Try simply a fixed support with no loads to eliminate the possibility of this kind of problem.
  • swarajswaraj
    Yes, I am using tie to join them. I will try out your advice and will give you an update.
  • swarajswaraj
    Hey Victor, I unchecked the tie check box but in doing so bonded contact is not taken into account.
  • VictorVictor
    It sounds like that means you should make the surfaces closer to the same shape as each other, so they don't need to be deformed by *TIE. Have you looked at the elements identified in the error message to see how they might be deforming?

    I notice the surfaces seem to be faceted. You should usually get the mesher to place the midside nodes on the geometry surface so they're smooth curves. That may help the two parts to fit together more accurately.
  • SergioSergio
    To replace the TIE you can try to mesh with coincident nodes in Salome, but for that you need the geometry in stp format.
  • swarajswaraj
    edited March 2018
    Hey,
    I am making my mesh more fine and I will see if tie is causing any problem. I am not going into Salome becaue mine geometry is complex and selection of nodes in Salome is tough. Thanks to mecway paint tool it made my job easy, Now I tried to simulate hyperelastic model of PDL so i used Mooney Rivelin MOdel. But I am getting this error "ALLOCATE failure : bytes 2053082832, line 517, file DV.c". Should I post this query as a new topic?
  • SergioSergio
    If you will use hyperelastic materials then will be a no lineal analysis, with several (lots) increments. Pay attention to create the more efficient mesh in order to have a model that can be solved in a short time. With that you can make several tries with differents boundary conditions in a razonable time, and lern in the process (and can be "fun"), otherwise you'll finish ofuscated by not having a solution at all in a long running.

    You can start replacing the hyperelastic behavieur with just a lineal material with Poisson 0.49 and very soft Young modulus, and keep your analysis lineal for initial tests.
  • swarajswaraj
    Ok Sergio,
    But what the Allocation Failure signifies
    and as I am analysing tooth movement, it is very important for me to get deformation in occlusal axis i.e (facial/lingual,mesial/distal) rather than X,Y,Z is there any way I can get component along the above mentioned references
    PS: Jacobian Error is solved
  • SergioSergio
    I would reorient the geometry in the CAD program to the real position before meshing in order to avoid such problem.
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register