Hello,
I've been trying to have simulation replicate a physical test I did on a drive shaft. The FEA stresses seem realistic, as it failed around 43,000 in-lb. But the deformation does not, as seen in the comparison of the FEA and physical torque vs. twist graph. I'm using a true stress and true strain curve obtained through lab testing. I can't figure out why these graphs differ so much. Any help would be greately appreciated.
As far as I know, everything is the same. The material curve I am using is from a direct sample test of the material the part was made of. The loading is fairly simple, just a ramped up torque on one end with the other fixed. I'm not worried about the linear portion of the angle of twist graph. What I want to match up is the region where the entire shaft starts to greately yield, from 20 degrees to 65.
I'd start doing some variance testing to check what the trends are when you change things. They should follow some patterns. If they don't, your setup isn't correct or you have a bad input. This one is going to require work on your end to figure out because only you know how everything is setup and tested.
The diconnect to me is that the strains are way too low compared to the stresses. Even though the stresses are quite high, above yield, nothing seems to have a yield strain (0.0075). In the real test, it can obviously be seen that it is entirely yielding.
Goes back to the question, how are you outputting the results? Are the stresses real? Are they converged? Are they an artifact of the loading or constraints that you applied?
I'm getting the torque twist readings in the FEA by taking the displacement of an endpoint and finding the equivalent angle by taking:
Angle = 2sin-1(d/(2r)). This is then compared with experimental results. Obviously there is good agreement with the linear portion of the torque twist graph, but not the nonlinear. I'm not sure what you mean by "Are the stresses real? Are they converged? Are they an artifact of the loading or constraints that you applied?". I was thinking of adding more time steps between 35,000 in-lb and 45,000 in-lb because that is more of where the action is.
additional timesteps are unlikely to fix the offset. this is likely due to an input or setup problem. I could be wrong, but I only have the information you've provided here to work with. you have the model the test data..etc.
regarding these comments: "Are the stresses real? Are they converged? Are they an artifact of the loading or constraints that you applied?".
what i'm getting at is that before you start going down the path of the problem being sovled incorrectly by the software, make sure that your results aren't affected by singularities and that the results have converged (you've tried different element sizes and the results don't change and that the stresses you're evaluating the results based on aren't just at infinite locations of stress) and also that if you change the boundary conditions to more closely match your setup (for example using contact) that the results don't change significantly.
here's what i'd suggest. build a simpler model that you can calculate by hand. twist it in the software with a linear material. make sure that you're good with the results. then switch to the nonlinear material and see if it matches your expectations. from there you should know a lot more about where the potential issue might be.
again my guesses:
1. material properties not input properly. a simulation of the way you obtained the material properties would be best to confirm these. if it doesn't match, your simulation won't match.
2. conversion error of some sort. the fact that there is an offset tells me that something isn't right somewhere.
3. setup problem.
What is the clamping method at each end on the real test? Obviously on the FE model any fixed/loaded faces will be perfectly evenly distributed as it is an idealised model. Could manufacturing tolerances between the shaft and clamp on the real parts be the difference?
The shaft was inserted into a coupling that had flats machined into it. Any "give" by the coupling would take place at the begining of the test. What yielded during the test was the large groove on the shaft. This largely accounts for most of the twist past 15 degrees.
First thoughts,
Check your material props with the same test that they were acquired with. That will give you confidence that you have selected the right material model and that it is working.
Then, loads and restraints. Are they exactly the same?
Similarly, how are you outputting the results? Are they exactly the same?
Have you checked all your units and conversions? It looks like fea is ok except that it is offset. But the curve is also cut off. Unless I'm not reading it right, is guess it is a setup or input problem.