Bolted Joint Prying Stresses of the Clamped Member

[1980c3]

Howdy folks,

In my FEA, I am encountering a scenario in which the bolted-on assembly is experiencing lateral load due to vibrations (should be a screenshot). As the top box tips over, the bolt head essentially "digs in" on one side and pries at clamped material. The peak principal stresses are found near the edge of the bolt's contact. Would you expect this to be singular? In changing the density of the inflation region around the bolt hole, it for sure does NOT seem strongly mesh dependent (meaning I change the mesh and the results change by 5% at the most). Thoughts?


The bolt to plate contacts are all frictional. And, for clarity sake, I am dedicating a time step to applying the bolt clamp, and locking the bolt for the remaining steps.

 

[centondollar]

Hi folks, for what it's worth, the linear FEM stresses are intended to be corrected for plasticity using Neuber's rule (and eventually strain levels used in strain life assessments).

That doesn't make the FE model correct. If you want to model plasticity, you need to model it.

And truthfully, since the FEM is reporting a positive principal stress, there is certainly a direction that is experiencing tensile stresses.

Your model shows that. If your model is wrong (analysis with frictional contact with some generic coefficients does not properly capture interaction of bolt and base plate), your conclusion is also wrong.

Make a free body diagram. What you will immediately notice is that shear and bending of the bolt nut causes local compression between nut and plate - it does not typically lift up the plate. You will also notice that bending of the bolt causes tensile stresses in the bolt, and that these interact with shear. Finally, by applying engineering judgement to evaluate the nut-plate contact area (it is small) and force (it may be large or small, depending on bending in the bolt), you will see that linear analysis is insufficient.

PS. You seem to be using shell elements, which will not accurately describe interaction of bolt, nut, bolt hole and the remaining plate, since the entire hole and its edges is described by only shell bending, shear and membrane stresses.

 

[1980c3]

Hi centondollar,

Sure I can try a nonlinear FEM then.. just leverage bilinear isotropic hardening? (I.e, one stiffness up to yielding, then a different one after yielding).

Just so we are clear, the model is 3D, I just have the results scopes to the top face of the bottom box flange (where the bolt is clamping).

I’ll keep you all updated on the NL analysis.

 

[centondollar]

I'm no expert on analysis of bolted joints with non-linear FEA, but there should be a lot of publications available on this subject. Try skimming through those before you continue with this model. Typically, one would use solid elements, material non-linearity (bilinear isotropic as described in e.g., AISC or Eurocode is the simplest model for steel), a realistic contact formulation (this is among the most difficult steps) and a suitable time-stepping scheme if the load is dynamic. The solver should be able to handle any force-displacement paths (displacement controlled Newton iteration cannot handle snap-back) - arc length methods are often robust.

Basically, unless you devote a lot of time to modelling everything correctly (including the supporting structure), use a robust solver and evaluate both plasticity and contact with the most accurate models, you'll have a difficult time getting realistic results. If this is to be mass-produced, just test it instead. The phenomena you encounter in FEA might not actually occur in reality.