Dar All
I have calculated part of real frame with bolted joints and I’m in doubts about results.
as you can see on screen shots I have modeled quite accurate bolts with washers and also contact between washer and nut /head also contact between washer and frame.(it took much time to solve this)
Results show that tension ressistance stress limit is exeeded in head round area. Is it ok ? Bolts are bended ( not all). Can stress in round area be neglected? I have also calculated this joint with beam elements and also by using fastener option as alternative solution in creo simulate , but resuls for each option were different
best regards
You should add plasticity (even just a simple bilinear model) to material definition to get realistic stress levels. Then you’ll see if you have local yielding and to what extent. Linear elasticity lets the stresses grow indefinitely.
1 Like
ok I’m aware of this but linear model shows where stress go peak and plastic material even hide this issue but is more accurate , also for bolts 10.9 diference in elastic and plastic is only 100 MPa
900 MPa elastic vs 1000 total tension strenght plastic
More realistic because it allows for the stress redistribution, eliminates singularities and other unrealistic stress peaks. Instead of them, you will just get small areas of local yielding that might be acceptable (and are easy to spot using PEEQ output). If you don’t have full tensile test data, you could use the bilinear model and cut off the stresses at UTS, for instance. After that, there would be plastic plateau. Or you can include hardening and just watch for too large yielding (the analysis will likely fail to converge at some point but it may just mean that the structure reached its capacity).
Still, you should check whether the stresses keep increasing with local mesh refinement in those critical areas.
plastic area in bolts ?
Maximum stress is at the sharp edge of the washer but the plates have a very coarse mesh. I would refine it there and in other locations that may need it (maybe a few times if necessary), add plasticity (I guess that Nlgeom is already enabled?) and only then proceed to the results interpretation. There are some other checks that should be made to verify the results (especially since you’ve mentioned differences with other models/solvers and it would be good to explain that) but that’s another topic.
and another question
I have used contact type hard and secon friction 0,3 is it ok for such calculations?
It depends on the case but such settings are usually sufficient. To verify if contact is working properly, you can request field outputs for it and check the maps of CPRESS, COPEN and CSLIP/CSHEAR in results. Contact stresses should be relatively uniform. Sometimes the default hard contact stiffness is not good and then the linear surface behavior with custom stiffness (based on the stiffnesses of underlying materials and characteristic length) can be used instead.
Friction is tricky. It should be avoided (to reduce the risk of convergence issues) if it’s not expected to have a significant impact on the results but there are also cases where it’s absolutely crucial for accurate results. However, its value is usually very approximate anyway.
Have you done any hand calculations for the loads on the bolts? For example, the VDI 2230 guideline or Eurocode 3 would give you some idea about the strength of the bolted joint.
Regarding the actual stresses on the bolts, I agree with @FEAnalyst in setting a simple bilinear model. I generally ignore those stresses at the fillet and care more about the section stresses at the shank. Then, I feed those values to my spreadsheets and calculate the safety factors depending on the guidelines used.