I can confirm the crash. It seems to be caused by compression-only constraints (it works if you deactivate them). But if you change the solver to PaStiX or Spooles, you will see that it fails:
Solution contains NaN!
PaStiX could not converge to a valid result
Job failed - no results exist.
Quick debugging showed that this was caused by 0 spring stiffness and tensile force specified for both compression-only constraints:
Set them to Default instead and it will work.
You’re restricting BC too much. Solids don’t have rotational degrees of freedom. A surface moving vertically changes the X and Y distances, so you can’t set the movement Z=-0.05mm and X=Y=0. There must only be a Z displacement,
I would avoid tie constraints here. Instead, with a few simple partitions, you can use Transfinite Gmsh on a compound:
Yes, I pointed it out at the beginning of the thread. BCs on rotational DOFs have no effect here.
Applying BCs to the whole part is risky too. When there are tie constraints, compression-only constraints and BCs (also in local CSYS) close to each other (or even overlapping partially), it’s easy to get an overconstraint.
The idea behind constraining X and Y displacement comes from the presence of the bolt head and nut. As an approximation i assume no relative displacement between the metal and the G10 washers, as if they were glued together.
We’re talking about axial displacements of 0.1 mm, i guess that the radial displacement in a real case between bolt head and washer, considering friction, is much smaller than 0.1 mm. That’s why i constrained the in plane displacements of the 2 contact surfaces.
I can also try the transfinite mesh then, the other analysis are quite complicated because of the numerosity of contact surfaces… The main aim was to understand how an isolating member (G10 chosen to isolate aluminium and stainless steel in a marine environment) mush softer than the surrounding ones, would absorb the bolt preload.
179
In my opinion, the mesh is too thick in the maximum stretch zone. There’s very significant nonlinear deformation. In this zone, instead of two elements, I’d try to use eight elements for the clearance width.
I have this transfinite hex-only mesh of 10416 C3D20R elements (note that the element type is also very important):
But a mesh convergence study is definitely always recommended.
Thicken Shell Mesh may sometimes have some issues, especially for complex geometries, inconsistent normals and at the corners. But it’s not necessary to use it in this case.
In fact, even transfinite mesh is not necessarily needed here if you just model it as a single part with partitions on the face:
I wanted to experiment with other ways to build the mesh. I noticed that offsets <0 can cause unexpected problems with thick plates and small curvatures.
Might be good to report a bug in the Bug Reports subforum then. Also to avoid going off-topic in the OP’s thread.
I’ve run the analysis using a transfinite mesh leveraging the subdivisions as suggested by @FEAnalyst .
Both use linear brick elements.
Regarding Von Mises stress:
The first mesh has size 0.5mm and shows a max Von Mises of 55 MPa:
The second mesh has size 0.25mm and shows a max Von Mises of 51 MPa:
Both maximum are located where the shearing action of the imposed displacement is highest.
Regarding displacemnts:
The first mesh has size 0.5mm and shows a max displ of 0.103 mm:
The second mesh has size 0.25mm and shows a max displ of 0.106 mm:
Qaulitatively speaking the finer mesh is better at showing the presence of a toroidal region in the washers where the “ALL” displacement is almost null, in practice it is the neutral axis region.
Results speaking, linear elements of size 0,5 and 0,25 mm cast the same values.
Default C3D8 ? It’s usually best to switch to C3D8R if you have enough of them. And of course, second-order elements (C3D20 and C3D20R) can provide even better results.
You divided a problematic area of 1mm width into four 0.25mm elements. I had two 0.25mm elements, and the result was 63.81 MPa, or 15% larger. In my opinion, the minimum area size is at least four elements; making smaller elements is imprecise.
Wouldn’t it be good to add a fillet there as well to avoid unrealistic stress concentrations ?
