Hello Everyone
Thanks for both the excellent software and the interesting discussions.
I am running an FEA of an orthopaedic construct (plate + screws + two bones) in PrePoMax/CalculiX.
The implant and screws are separate parts connected with fixed (tied) constraints, as the screws lock tightly into the plate. Each bone has 4 screws that go straight through both sides of the hollow bones, as there is no contact between the bones, so the only load path is:
loaded bone → 4 screws → implant → 4 screws → other bone.
The model converges reliably with nonlinear geometry. I do have some issues however, these are
-
With tied screw–bone interfaces, the model is very stiff and gives unrealistically high stresses (up to ~1 GPa) at the bone–screw interface.
-
With hard contact + friction (μ ≈ 0.3), convergence is still good and the displacements are more reasonable, but bone stresses are still very high (several GPa).
-
Stress is concentrated in the cortical bone around the screws and in the implant, but the stresses are, I think, unrealistically high.
Model details:
-
Screws are partitioned to match cortical regions, so essentially the screws are divided into three sections connected by tied constraints, with the upper surfaces of these sectioned screws connecting to the implant, the middle section connecting to the first cortex and the lower part connecting to the second cortex
-
Contact is defined between the screw shaft and the cortical bone (inner/outer)
-
Screw shaft is longer than the cortical thickness
Main question:
What is the best way to model the screw–bone interface in this type of analysis (without explicitly modelling threads)? Should this be tied, frictional, or something else to get realistic load transfer without artificial stress concentrations?
Based on the literature, the most common approach for this interface is tied contact. Is there supposed to be any osseointegration there ?
Too large stresses mean that you may have to simplify the geometry of the screws, correct/refine the mesh or adjust the contact definition.
Thanks for the reply. In the model that I am currently wrestling with, all of the geometry is very simplified but matches (kind of) the real geometry. For example, the real implant is a complex free-form shape, and the one I have here is merely a rectangular prism; similarly, the bones are represented by hollow cylinders. I have modelled the screw bone interfaces as tied, but the stresses were even worse than they are with “Hard” and friction
To clarify, there’s no osseointegration; the screws are modelled as cylinders. In the real case, there might be some bone growth onto the surface of the screw.
Here’s one interesting example: Numerical Simulation of Bone Plate with Fatigue Crack and Investigation of Attraction Hole for Retarding Crack Growth
But then I guess it’s a meshing issue. Did you try refining the mesh significantly there ? Perhaps there’s just some nasty edge that needs a fillet or something. Make sure the standard rules for contact definition are followed - the master surface should have a coarser mesh and belong to the stiffer part.
Btw. some time ago there was a thread about femur torsion modeling (including both cortical and cancellous bone). Simplifying this problem to just two tied cylinders clearly showed how these meshing and contact/constraint assignment rules affect the results. Mismatched tetrahedral meshes can provide really bad stress results, while well-matched hexahedral meshes easily resolve such issues (also with contact pressure distribution - btw. you should check CPRESS to make sure that contact is properly established). Of course, it’s not always possible to use hex elements, especially in biomedical problems, but even there, it’s highly desired, and there are tools supporting that.
I think that I have pretty much the same set-up as that shown in the paper, even down to the number of screws! I have just tried a smaller mesh but I haven’t remeshed with hexahedral elements…I’ll have to work out how to do that.
If you are able to apply hex mesh to your geometry (so basically, if it can be extruded, revolved, swept, thickened from a surface in its local normal directions, or divided into subvolumes having 5 or 6 faces with 3 or 4 edges each), then it would be the best option. It makes modeling such interfaces (especially cylindrical) so much easier - smooths the contact pressure, facilitates contact or tie constraint establishment, and so on. Usually, first-order elements are better for contact, too, and linear hexes are perfectly usable if there are enough of them. Such meshes are pretty much a must in interference fit modeling (which might be applicable to such biomedical problems as well).
This thread describes hex meshing in PrePoMax: Summary of Gmsh hex meshing rules
But the same rules are also listed in the user manual. There are some YouTube tutorials about these meshing algorithms, too (linked in the manual).
TIE will give you unrealistic stress at the interface due to non coincidence of the nodes, if you need realistic stress there, you need to model the phisical thread. But we are taking about bones, where the mechanical properties are not constant along the depth, and even change according the the state (aging, is not the same if you test inmediatelly fresh or is a dry sample) of the bone, the donor, even the health conditions of the donor. So if you are modeling your thread as simple cilinders and using “bone”, in my humild opinion getting “accurate” stress at the interface is not possibe with such level of variables.
You can try meshing with coincident nodes and avoid the TIE, but again, in the interface there will be a lot of incertainities. And if you mesh with coincident nodes if I remember well the stress at the interface will be mixed, so if the two materials has very different young modulus as in your case, then the results will not be valid as well.
Well-matched hex meshes can mitigate stress discontinuity issues even when tie constraints are used. Of course, ensuring proper master-slave assignment, as mentioned previously, also helps. And using tied contact if necessary. Of course, simply merging (compounding) both parts is also an option, but it often prevents hex meshing.
Screw threads are rarely taken into account in the literature on the subject (unless dental implants are considered, of course), but some studies indeed include them, especially if they focus mostly on the screw-bone interface, such as this paper: https://www.mdpi.com/2073-8994/10/8/335