General Mechanical

General Mechanical

Vertebrae screw pullout analysis

    • Patryk Sienkiewicz
      Subscriber

      Hello,

      I am trying to check the type of thread I used for transpedicular screw - I want to determine the force needed to pull it out of the vertebrae. My vertebrae model is divided into 3 objects - cortical bone, cancellous bone and posterior elements with proper materials assigned and shared topology. The screw is inserted into the vertebral body through the pedicle.

      Upper and lower vertebral body surfaces are fixed and I apply displacement of 1mm on the screw head in the longitudinal direction, trying to pull the screw out of the vertebrae.

      At first I have tried frictional contact (Augmented Lagrange) with 0.01 stiffness and bilinear hardening properties applied to materials - solver was unable to converge on a solution. Now I try to solve it with frictionless contact and without bilinear hardening - same thing, solver isn't unable to converge, doesn't matter if I use large deflection or not. I can only solve it with bonded contact and program controlled stiffness - but it says the force reaction on displacement is around 14000 N, which is at least 100 times more than I expect. 

      Could anybody tell me, how should I set up this analysis and what are the possible reasons for it not to converge?

      I tried to attach .wbpz file, but it seems I can't, I don't know why.

      Thanks in advance.

    • SaiD
      Ansys Employee

      Hello,

      Could you share the Force Convergence plots (you can obtain them by going to Solution Information > Force Convergence in the details)? Another place to look at would be the Solution Information > Solver Output and search for any error or warning messages. The messages might provide some clue about what is causing the non-convergence.

      Bonded contact is a linear contact (meaning that the status of the contact remains unchanged throughout the simulation) and that is probably why the solver is able to solve it without any convergence issues. You should expect a very large large force reaction when using bonded contact (as you are seeing) since this simulates the case of no separation and no relative sliding of the screw wrt the vertebrae.

      Ansys employees are not allowed to download any attachments from the forum, but you can trying attaching an archived file without the results (so that the file size is smaller), in case someone else has some suggestions. To reach a wider audience, please add inline images to explain your model setup etc.

       

    • Bill Bulat
      Ansys Employee

      How are you representing this catastrophic material failure? Is it your expectation that the finite elements surrounding the screw will severely distort and "fail" (as the bone material would physically)? Or are you instead using equivalent friction model in the contact that behaves as failed bone would? If the former, it seems that NLAD (nonlinear adaptive feature) would be necessary. Mind you, NLAD might not be sufficiently robust to accomodate the mesh distortion that I imagine one might see in such a simulation. If the latter, it isn't immediately obvious to me how you might determine an equivalent contact friction. But for what it's worth, contact friction related constants, such as TAUMAX, can, with an APDL command object, be made a function of independent variables (e.g., sliding distance, contact pressure) by using a table. You might consider trying to locate the following Help sections for more details about this:

      Kind regards,

      Bill

    • peteroznewman
      Subscriber

      Hello Patryk,

      I see the threads on the screw. Was that screw solid body subtracted from all the bone materials to make a screw-shaped hole in the bone?  I assume that is what you have done, but I ask just to make sure.

      Cortical bone is a brittle material, it fractures, it does not deform the way a ductile metal would plastically deform. Therefore you should not use any material models from the plasticity section for cortical bone. Cancellous bone, since it is full of voids may behave differently.

      I assume metals used for medical screws have high strength, so when they pull out, it is the bone that fails, not the metal.

      What data do you know for the material properties of each type of bone? I assume you know at least the Young’s modulus (E) and Ultimate Tensile Strength (UTS). 

      Cortical bone is much stronger than cancellous bone.  The first few threads carry the majority of the stress in a screw and those are in the cortical bone, so when that fails, the screw pulls out. The contribution of the cancellous bone may be insignificant.

      You need a material failure model at least for the cortical bone. Explicit Dynamics has a fully automated means of deleting elements that have failed. The simplest method is to remove elements that have exceeded a failure strain, which could be simply computed as UTS/E but more sophisticated material failure models can be substituted. With Explicit Dynamics, you have to build a mesh that avoids elements with tiny element edge lengths to prevent the automatically calculated time step from becoming very, very small, which causes the computation time to become very, very long.

      If you stay with implicit solvers such as Static Structural, there is a command called EKILL that can remove the stiffness from failed elements during the solution, but this requires you to use APDL code in your model to remove failed elements after each load increment. There are some threads on this topic you can read.

    • Patryk Sienkiewicz
      Subscriber

       

      Peter,

      Yes, the screw is a solid body and it was subtracted from the vertebrae. I know the yield strength, Young’s modulus and Poisson’s ratio for each material.

      So your suggestion is to use Explicit Dynamics instead of the Static Structural?

      this is the force convergence plot of the analysis i'm currently trying to solve - unfortunately, it got stuck at 60 iterations and doesn't proceed for 3 hours now.

       

    • peteroznewman
      Subscriber

      The benefit of Explicit Dynamics is that it takes such tiny time steps that it is always in dynamic equilibrium and does not work like Static Structural (implicit solver) that has to search for equilibrium and may not find it. So yes, it is worth a try because of the simplicity of using it. No contacts need to be defined. It automatically finds the contact between bodies. It automatically removes failed elements.

    • Patryk Sienkiewicz
      Subscriber

      For now I want to try pulling the screw out of Sawbone material cylinder. I know the compressive strength of it - can I use it instead of UTS?

    • peteroznewman
      Subscriber

      Yes, you can use compressive strength instead of UTS.

      The best situation is if you have experimental data for screw pullout force and you tune the material properties until the pullout force in the model matches the experimental value.

Viewing 7 reply threads
  • You must be logged in to reply to this topic.