Stress Concentration in Bolt Holes 6

huiying,

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

HUYING: My recommendation is against using FEA to do a bolt/thread analysis. There is too much going on in a amall space. Typically in a bolted connection, if it is properly designed, the bolt will break before the threads pull out. Typically in a bolted connection the bolt is torqued to the 80% yield strength of the bolt material. If the mating material is softer then there are other considerations. Studies have shown in a bolt that usually the bolt and threads deform slightly and most of the load is carried in the first few threads of the bolt. Other factors enter into it such as: are the threads rolled or cut, and how was the bolt preloaded. Torqueing is good for plus of minus about 30% of the preload. In critical applications the "turn of the nut" method is usually used and the stretch of the fastener is measured. It is better, in my humble opinion, to stick with the tried and true methods that have yielded good results for the last 150 years or so.

Regards
Dave

As CESSNA1 points out, it is extremely difficult that a structure fails in a bolt-jointed area if the junctions have been properly designed. Refer to VDI 2230 Norms, or EN-10 (formerly UNI/ISO 10011), or equivalent ones. It is common engineering practice not to model bolted joints in the FE structures, replacing them by "adequate" constraints or DOF couplings, and separately calculate the bolted joints analytically based on the resultant forces calculated by FEM (when these forces are not known "a priori").
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,...

I disagree with some of the points made here. In my experience (civil/nuclear structures), connections have always been the weak points in the structure, and in most cases this area has a tendency to fail initially all things being equal, because of the nature of the connection itself (one big stress raiser). This is unless you work in the nuclear industry, where I have always designed/analysed connections 1.5 times stronger than the member strength.

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

Usually bolt connections are designed to have the "load triangle" entirely within the elastic limit (yeld strength) both of the bolt and of the joined parts, but this is NOT an absolute presription. There are cases in which bolt preload is raisen up to 100% of the yeld, this requires another type of calculation however. A third case is when only overload exceeds the yeld, while the preload stays below.
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.

Generally stress concentrations contained within an elastic region won't cause the structure to fail in a single event. The stress at the point from the hole would be classified as a peak stress and as such may cause failure by fatigue. You need to look at the stress components without this peak component to see if the structure will fail.
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

There is an elastic-plastic correction method proposed in MSC.Fatigue documents. If you did a linear analysis and you got hot spots at the hole (stress raiser) of your structure then you can correct the stress value obtained from linear FEA. Since, your structure acts as a spring (linear behaviour) until proportional point of the stress-strain curve, as Garland (GBor) explained very well, the FEA results cannot be used for nonlinear behaviour of your structure. However, Mertens-Dittmann method may be used to calculate elastic-plastic stress and strain from their elastic linear FEA results. This method is a modification to the conventional Neuber approach. Mertens suggested that a better estimate of the local notch stress and strain. This method is explained in the Fatigue Theory chapter (chapter 14) of MSC documents.

pages.infinit.net/featek
AAY

Huiying,

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.

Thank you for all your replies.

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.

Huiying,
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).