I’m interested if this kind of split sprocket can be simulated from assembly and what do I need to take in consideration?
Rim is S355 and hubs are also S355. Hexagonal screws are M16x70 10.9 DIN 931 and Nuts M16 DIN 985. Hubs are welded to the side of rims all the way around on outside. This sprocket is for M160-A-160 conveyor chain and Ø80mm axle with 22mm keyway.
Split Sprocket.pmx (302.6 KB)
I have once seen a situtation, where the 30mm free hole had caused a crack due to it being positioned too close to the sprocket teeth surface.
It’s important to connect all the parts properly. You could start with tie constraints and thus assume perfect bonding between the parts, then you may replace it with contact where needed.
Pre-tension can be applied to the screws if you want to takie it into account. Then you can apply the actual load which has to approximate the way in which the chain subjects the sprocket to torsion. Of course, you will also have to fix the hub.
Try to perform nonlinear analysis - with plasticity and geometric nonlinearity included. It will be much more realistic.
1 Like
By nonlinear analysis, I believe you mean NlGeom setting? (geometric nonlinearity – large deformations and large displacements)
How is the plasticity defined to the simulation?
Usually this area holds the bush or roller while sprocket rolls, so it probably should be uniform pressure?
There are three main types of nonlinearities in FEA - geometric (Nlgeom), material (i.a. plasticity) and boundary (mainly contact). It’s best to include all of them to obtain realistic results. Of course, contact is not always necessary. To include plasticity you just have to add Plastic behavior to the material definition and specify yield stress - plastic strain data points. If you don’t have the whole curve for the multilinear model, you can use the bilinear one and specify just one point (yield stress with 0 plastic strain) or, better, two points (the previous one plus another one with nonzero plastic strain to define hardening).
Yes, uniform pressure should be fine. It would be best to partition the surfaces in CAD software before importing the model to PrePoMax so that you can easily apply loads to the proper regions.
1 Like
Are you talking about fatigue or static analysis. This sounds like a fatigue issue as only a really poorly designed part would fail statically under normal use. Also rotational loading is the classic root of fatigue analysis (rail road wheels breaking off their axels) Fatigue analysis can make use of FEA to determine stresses but it is by no means a direct result. (and extracting stresses from FEA is not something one should do without great care) I suppose you can model fracture mechanics but that would not be justified here (and I don’t think Calculix can do that). You can do models with that delete elements based on max strain criteria or a simple quasi-plastic failure which will provide an idea of the ultimate capacity of a structure but again I don’t see the need.
Luke