If I were you, I would do the following:
- Model the bushing only. In other words, ignore the shaft. I assume the shaft is significantly stiffer than the 'plyable' bushing.
- Apply a fixed boundary condition on the inner surface of the bushing. (the surface that makes contact with the shaft)
- Apply a pressure across the bushing face of interest (or whatever loading condition you are interested in). Perhaps the loading conditon is like the one in the attached sketch.
- Use solid elements and overload the mesh (make it relatively dense) because you want the elements to be pretty small. By making the elements small, you are effectively minimizing the inaccuracies of the fixed boundary condition.
- When you look at the results, don't pay to much attention to the first layer of elements on the inside surface where the fixed BC is applied. Moving radially outward towards the outter diameter, the results should be pretty good. (the finer the mesh, the better the results will be next to the boundary condition). You could get fancy and do a mesh density as a function of radius with the inner radius having the highest density of elements and te outter diameter have less (probably overkill, but if you want to... go for it). You should run a mesh convergence too (which means just start coarse and work your way to a finer mesh until the delta of the the results is negligable).
- This analysis will tell you the stress in the bushing as a function of a pressure force (in this case a force trying to slide the bushing along the shaft).
- You can calculate the required force to break static friction and apply that force to the simulation. This would then tell you the peak stresses involved. All of these procedures are with the assumption that you are not interested in the effects on the shaft (just the bushing). Also, just to make things clear, the peak stress the bushing will see is the value right before static friciton is broken. Assuming you have a decent estimate for the force to break static fricition (which will be a function of surface area and the friciton coefficient) then you should use that value in your simulation to derive the peak stresses on the bushing.
I re-read your original post and perhaps I missed the scope of the problem. Are you interested in a whole assembly fea study or could you break down the components? As for the radial stress component due to the shrink fit, I'm not sure how you would handle that. You wouldn't be able to apply a radial pressure at the locaiton of the fixed bc (in my approach). Perhaps you could do 2 studies ((1) just like the simulation setup above and (2) with a fixed displacement on the inner surface and a fixed bc on the outter). You might be able to superimpose both solutions (add the different components of the stress to get a magnitude)?
Here's another approach I tested:
Assemble the shaft and bushing together keeping the bushing concentric with the shaft. The bushing should be able to slide along the shaft (you can kep the roational degree of freedom ..free or fixed depending on your interests). Apply 'contact set' between the inner surface of the bushing and the outter surface of the shaft. Apply the friction coefficient. Put a fixed boundary condition one end of the rod. Apply a 'advance fixture' to the outter surface of the bushing as a fixed translation. Enter in the appropriate translation magnitude and the appropriate reference geometry for the direction of travel. Mesh and Run. This will do the following:
- Moves the bushing along the shaft a specific distance. When the bushing reaches that final point the residual stresses are equivalent to the highest static stresses. In other words, the bushing is moved such that it breaks static friction, and then it enters static friction with residual stresses at the maximum.
- The contact covers the radial forces. I assume you mad the shaft slightly larger than the bushing or the bushing slightly smaller than the shaft to account for the shrink fit diameters.
I think this procedure might cover what you want to do. Let me know what you think. (Also the reason why your simulation was failing was because you were breaking static friction and the part was able to move along the shaft without any constraints). The predefined translation instead of a pressure force should fix the problem.
this solution requires contact elements and a nonlinaer solver. do you posses the license for these?
I was able to get the assembly to work using the friction setting only. So now in the assembly, everything is staying in place when the external loads are applied without extra constraints. My next step is to create an impact analysis, which of course is non-linear, and inspect the contact pressures on the pressfit joints to determine if the applied loads will overcome the forces of the pressfit and allow movement within the assembly. Thanks for all the help so far.
are you aware there are closed form solutions that can compute the frictional force of the shrink fit w/a lot less effort and faster than FEA?
look in roarks formulas for stress and strains for starters.
thesesolutions will solve faster and are accurate. you should do it anyways to validate your model.