You could try using the pin/bolt connector to avoid a contact solution. It might be closer but it too may result in the large bore still being overly stiff. The bolt connector without contact might be slightly better as at least the pin material properties may play. The issue in making the root fillet hot but not too hot is getting the bending around the pin accurate. In approach 2 which pin bearing load distribution did you use? Did you try both - 1/2 sine and parabolic?
Thanks for your answer.
In approach 2 I tried both 1/2 sine and parabolic (1/2 sine in the presentation).
They both yield the same answers in stress and displacement, and I can't see any noticable difference in the plot with the current scale.
I add the pin/bolt connector approach to my "to-do list". I will also fiddle with remote load/displacement and see what this gives.
Mikael, interesting reference. Can you tell us what you're trying to learn with this analysis? All 3 are valid depending on the assumptions you're ok with making. BC3 is the best to match real life if you can assume the pins are rigidly connected to the part they are connected to. If that isn't a good assumption then you'd have to add the next components that are deformable.
Bolt/pins is the way I'd go. You still need to model a component to pin your part to and then you have to be ok with the assumption that the pin isn't deformable.
I'm just trying to understand how to properly use BC:s
This is not a real part, I just did it for the purpose of testing.
All solutions are valid based on the assumptions made, of course.
But it is interesting that the results can differ so much on one part with the same mesh and loads.
I started with the BC1 which basically is what you are taught when you attend on a SW simulation course.
I then tried BC3 with actual 3d models on the pins and found a stress concentration in the radius, where I'd expect it to be.
Finally I tried the BC2 with 3-2-1- miminum restraint, taught by Roshaz on their homepage, and once again found an even higher stress on the radius.
So the lowest stress on the radius, with the given mesh, is 438 MPa, with pin modelled 686 MPa, and with minimum restraint 805 MPa.
I think that it is interesting that you can get so totally different results on a simple part like this.
The final question is if there is a better solution to constrain the part, without adding other geometry, to get a result close to what you achieve with BC3.
How do you know answer 3 is right? It is closest to physical but you're assuming it is right without comparing it against a known solution. I suspect if you start changing the mesh, you'll see that you have another factor here you haven't considered.
Overall, the only other option is virtualized pins or some combination of the methods you've chosen. But you can only decide which one is best based on what the answer should be and what you want to learn. If you need an absolute answer, the contact version is the only option. If you're doing design studies , I'd argue that your first one have you a decent amount of data to understand trends for the initial design and to help you get to the final design where you apply the full contact setup.
That being said, the exercise you've gone through is a good one. Very similar to what I use to teach new simulation engineers and customers in our mentoring service.
Ok, then I now that the only other option is to add virtualized pins, similar to what Bill proposed earlier.
I wondered if there were an even more clever solution using 3-2-1 combined with some fixture to get closer to the contact result but without the added time needed to solve contacts.
No, answer 3 is probably not right either since i haven't considered stiffness on the other end of the pins nor defects or manufacturing flaws in the "real" part, e.tc. The mesh could probably be even more refined in the high stress area, even though the increase in stress was very low with the last settings with 5 elements thru the radius.
But that is not my point. FEA is always an approximation, no question about that.
I expected a stress concentration in the radius when I first modeled the part and set up the problem.
With the simple BC1 you will not see this concentration and that is what concerns me.
I agree that for a design study, BC1 is enough to decide the overall dimensions of the part.
The stress concentration could then be handled with a larger radius if you do the full contact simulation and recognize it in the end.
But if you don't go further and add pins and perhaps even more details and contacts, you could end up confused when the part fails due to fatigue in the radius.
from what i see, the 3-2-1 method is the starting point. they talk about the need to add other methods to get closer to reality. so to be true to the contact solution, you need to use contact. the other methods you've tried in this exercise are all valid depending on the assumptions you're ok with. but overall, for someone looking for an absolute answer, the exercises are necessary. There is no short-cut to getting absolute answers that match physical behavior.