Stress Concentration in Bolt Holes
Stress Concentration in Bolt Holes
(OP)
Hi,
We usually get stress concentations in bolt holes. If the FE result shows that the stress at these holes is greater than the UTS of the material, does it mean that the whole structural will fail?
Sometimes, bolt holes are ignored during simplification of the models, so how to know whether the stress concentrations at these points will cause the structural to fail?
Regards.
We usually get stress concentations in bolt holes. If the FE result shows that the stress at these holes is greater than the UTS of the material, does it mean that the whole structural will fail?
Sometimes, bolt holes are ignored during simplification of the models, so how to know whether the stress concentrations at these points will cause the structural to fail?
Regards.





RE: Stress Concentration in Bolt Holes
Are you running a linear analysis? If you are, then the answer is that you probably can't tell anything about the failure. If you recall a material's stress-strain curve (at least for most metals) starts to go non-linear as it approaches the yield strength. Linear FEA doesn't account for this, nor does it account for stress redistribution as the material yields at a particular location.
If you are running a non-linear analysis, then other questions would be: How did you model the bolts? How many elements do you have at the perimeter of the bolt hole? Is your model at the bolt holes made of plates or bricks? Does your FEA software output strain energy densities? Or perform fracture mechanics?
Specifically about the bolt hole stress: Is the high stress due to bearing? shear? pull-through?
The short answer to your question would be, "no", but if you can fill in some of the questions above, the forum may be able to give a pretty good answer.
Garland E. Borowski, PE
RE: Stress Concentration in Bolt Holes
Regards
Dave
www.wsec1.com
RE: Stress Concentration in Bolt Holes
If you DO want to simulate a bolted joint in FEM, you have to incorporate ALL the pertaining factors in your model: very fine mesh, pre-load, non-linear material properties, proper friction coefficients, proper settings for the contacts,...
RE: Stress Concentration in Bolt Holes
If you want to model a simple bolted joint, the level of complexity depends on the results you need. Bolts are *normally* only ever used within their elastic limit, hence you only need to analyse them elastically. If you need the forces in the bolt, then a simple hand calc will do -- if the connection is assembled correctly, and has the correct level of pre-load (~80% of yield as above is a recognised figure), then the bolt will see very little external load (usually less than 20%) and you need not worry about the bolt. Most of the external load will be taken by the members. If you want information on the deformation of your bolted connection (of the members say) then you need to introduce the stiffness of the bolt somehow, as well as the correct contact conditions at the interface, but you don't need to consider non-linear materials in my opinion (if it does go non-linear then you need to redesign the joint).
Going back to your original question, your analysis is picking up on a geometric discontinuity (the bolt hole). This is entirely correct, and should normally be a stress raiser. However, by assuming that the bolt or the hole does not exist will massively affect your results, since the stiffness locally will change. Usual disclaimer regarding the type of structure, load paths and the loads you put into it etc. If your analysis is linear, then forget trying to guess whether your structure will fail -- design/analyse it elastically to ensure it won't fail. Although you do get some redistribution of the load, a non-linear analysis will tell a different story altogether -- and why would you want to make your bolt/connection go to that level of plasticity anyway?
Cheers,
-- drej --
------------
See FAQ569-1083 for details on how to make best use of Eng-Tips.com
RE: Stress Concentration in Bolt Holes
The original question seems to have been posted because stresses have been calculated which are higher than yeld limit in a non-negligible zone of the joint. The post says "higher than ULTIMATE tensile strength". So non-linearity IS a concern in this case. Should these stresses be only a calculation hot-spot, of course Drej is perfectly right and nobody wants to go non-linear if it isn't absolutely needed...
IMO this has little to do with the fact that a bolted joint really is a weak-point of a structure: if the bolted joint is correctly calculated, its strength is adequate with respect to the overall design, and the raisen local stresses are not a concern if the rest of the parts have been already designed "safely". IMO, if one is trying to design "at limit" (extreme-performance design, no safety, one-shot use...), then the incursions in the plastic zone of the material are part of the design itself and the non-linear effects do have to be taken into account from the start.
RE: Stress Concentration in Bolt Holes
For the combined stress at the hole, design standards will tell you to use the elastic calculated stress and compare against SN curves for that material, using the number of cycles, N, you want the structure to survive given a certain probablity.
corus
RE: Stress Concentration in Bolt Holes
pages.infinit.net/featek
AAY
RE: Stress Concentration in Bolt Holes
What you are looking for is "Stress Categorization" -details may be found under Pressure Vessel Directives - sorry no link. The thrust of the argument, as others on this site have mentioned is that a local stress hot spot in a ductile material WILL NOT cause failure of the whole structure. You must look at the "overall section stresses" for failure of the whole structure. Local stress hot spots in ductile materials are sources for fatigue failure only.
I agree with other posts that the best way to calculate bolt loads is using classical methods based on loads derived from FE models.
The only times I have ever really looked deeply at bolt hole stresses is when examining thermal stresses in flange packs of different materials. I would use ABAQUS to do this with a full friction and 3D bolt head contact model.
RE: Stress Concentration in Bolt Holes
First, I would like to answer Garland's question to make myself more clear.
I'm using Patran/Nastran Linear Static for my FE analysis. I model the screws as bar elements and connect them to the holes on the solid body(Hex elements with holes between them) using MPCs.
The result I got is a stress concentration on the bolt holes as expected. These stress are higher than the UTS of the solid material. The stress on the screws(bar elements) are lower than the UTS of the bolt material.
From the discussions from the various members of this forum, can I conclude that:
-stress concentration more than UTS of the material does not necessary means failure, a non-linear analysis must be done
-as long as the bolts are designed and torque correctly, it will take up most of the load in the bolt area.
Some questions:
-It was mentioned that forces from FE can be used to design the bolt, in my case, are the forces the constraint forces, the MPC forces or the element forces?
-If the material around the bolt hole is weaker than the bolt itself (eg. steel screws used to hold one piece of Aluminium plate against the other) and if linear analysis shows that the area around the screw hole has stresses higher than UTS, this does not mean it will fail? Means that I have to do a non-linear analysis?
Thanks & Regards.
RE: Stress Concentration in Bolt Holes
1) as I don't know Nastran, I'm figuring out what your model would be in ANSYS. If I understood well, then the high stresses you are getting on the holes ARE calculation hot-spots.
2) if you want to examine the bolted joint with FE, build a "full-geometry" model where the bolt itself is also a meshed solid. Then, apply "contacts" btw bolthead lower surf and part surf, btw nut surf and part surf, and btw cyl surf of bolt and cyl surf of holes. In order to simulate pretension, a number of solution exist (in ANSYS you have a special option for this), but the most straightforward is to apply a negative thermal load to the bolt only, so that it shrinks down (but you have to define anisotropig thermal expansion coefficients, because you want the bolt to shrink only in the axial direction...)
3) if you have a complex interconnected structure, and you want to calculate analytically a joint but you don't know the forces on the connected members, then these forces will be the elem nodal forces (summed or integrated in some way depending on how your model is made, of course) that the two members share at their "interface" in the FE model
4) in the "weak members' material" you describe, VDI norms would have you redesign the joint (more bolts, lower pretension, bigger diameters,...) so that the ultimate strength (lowered by the safety factor, of course) is NOT reached for ANY of the components. If you are making a design "pushed to the limit", then you may want to account for the stress redistribution, local plastic deformation, and so on. In order to do that, the same kind of FE model described above is needed, with the difference that the solver wil be set to non-linear and all the material properties will include the non-linear part (which way depends on the constitutive laws that you can define within your FEA).