I can't get this model to converge in spite of having filleted the presumed-relevant corner to remove the potential singularity. It is shown here face-on to a symmetry cut after an h-adaptive loop of 8 cycles:

(The stress range for the plots was deliberately set to the yield level of the stud.) This is intended to model a bolt threaded into a pair of test blocks, using a shrink fit to simulate the threaded joints. A horizontal force is applied to the blocks, and vertical motion of the blocks is not allowed, so that the stud is bent into an "S" shape.. Only one quarter of the model is shown because I used symmetry across the X-Y plane and anti-symmetry across the middle of the stud to reduce the computational load. The full model (before the symmetry cuts) is shown here for clarity:

Here's what happens when the mesh resolution is increased using the h-adaptive default settings:

This behavior is not caused by some instability of the h-adaptive method but has been replicated with manual mesh resolutions set by mesh controls. It also has not improved by addition of the fillet; similar stress increases at the edge where the stud emerges from the block were observed without it. The stress increases without limit on the compressed side of the stud here:

...and on the upper edge of the fillet inside the hole in the block here:

These stress maxima are near the location where the interference ends between the two parts. Here are the study properties:

(I haven't tried fiddling with the "Accuracy bias" setting, nor have I tried the p-adaptive method.) Attached is a P&G in case you want to look in greater depth.

Can anyone suggest what I'm doing wrong? -- John Willett

I overlooked the fact that this was a threaded stud, I thought this was a press fit or shrink fit. Given this information, which going back I now see was in your OP, I can tell you with confidence that this stress you are calculating does not measure anything physical. you are not modeling a bolt. you are modeling a pin. And the local stresses in a pin are not related to the local stresses in a bolt in any interesting or predictable way. This should be a hand calculation. Calculate the moment in the bolt at the connection and check that it can resist the Moment as a circular beam with a cross section equal to the stress area or the bolt, which is available in

Machinery's Handbook, or Google. Then add some appropriate safety factor and ship it. if this is fatigue, add another safety factor of 3 or 4, OR if you are super-dedicated, look up the stress concentration factor based on treating the thread as a notch. This last is conservative, though, because multiple adjacent notches tend to dissipate stress concentration.I say this should be a hand calculation, because you are trying to extract something from FEA that it cannot give you.

If you are still interested, though, I'll go through you other questions.

"What do you mean by "discontinuous contact condition?" The shrink fit and/or the adjoining surfaces included in each half of that contact set? If so, does that inevitably produce unbounded stress as the mesh size decreases?"

Discontinuous contact condition, because one element is touching the metal surrounding the hole, and the next is in space touching nothing. I don't know whether it's inevitable, as in re-entrant corner inevitable, but it's the least surprising thing since a lying politician. I am always very skeptical of contact stress results from FEA unless I know the analyst very well. Also, if your stud is glued to the surrounding metal, the discontinuous Young's modulus

willcause a singularity.I thought I was already using that as the convergence criterion

You are and it converged. That's why the solver stopped. Strain energy will frequently or usually converge even when stress diverges, as infinite strain becomes packed into infinitesimal volume. If you showed successive stress plots leading up to the singularity vs. decreasing element size, you'd see the series superficially resembles Gibbs phenomenon plotted vs. increasing n. What that shows is that your solution is converging to a divergent answer. It's not getting any better: your solution has converged even while your stress hasn't. Again, you can't see into the singularity, so you have to apply judgment.

You can assume there will be some localized yielding in that small volume and, if that's acceptable, ignore it. If that's not acceptable, you can extract the linear portion of the stress there and apply the appropriate stress concentration factor

I'd be surprised if the screw were going to fail based on your results so far, assuming you've modeled the stress area or minor area and not the nominal area of the screw. If you are going to have more than, say, 100k cycles, though, look at fatigue.