I am currently working on the FEA of a boom assembly of a crane. The modell consists of the boom, a sheet metal part at the end of the boom aswell as some bolts and pins that connect the parts. The boom is constrained by resting on a pin which has 5 fixed DOF’s (it can rotate along its axis). The rigid body rotation of the boom is restricted by a wire rope a the end of the boom (its a derrick crane), which I modeled using a rigid body constrain. Now the location of the point of the rigid body changes depending on the load case. I get good results for all load cases except for one, in which one of the connecting bolts just expands like it was spinning at a crazy RPM around its axis. This failure seems to depend on the location of the point of the rigid body and i cant figure out how to fix it. Pls help. (the Analysis were created using Prepomax ver 2.2.11 dev)
this is the result and setup of the not working Analysis
Ok, I can access it now. Apparently, automatic preview breaks links from this website. The < and > tags can prevent it: https://limewire.com/d/WUsrU#QeYlLDfJI0
Connections look good, I checked them by replacing contact pairs with tie constraints (using the automatic search tool) and running a frequency analysis (always recommended when analyzing assemblies). The bolts also don’t have disconnected meshes or anything like that.
The results with this spurious deformation in the Auslegerhaelfte2vV150A90elastisch.pmx file are from t=0.0501953 s while the previous frame with correct results is from t=0.05 s. So it’s likely just a failed increment. I assume it stopped converging at that point ? It might be good to enable Nlgeom to get more realistic results (even just for debugging), but it will probably take quite some time to run. If it doesn’t converge, try replacing individual contacts with tied contacts or tie constraints to see where the issue is located (typically somewhere within the contact regions).
I created a rigid body from the nodes of the bolt head and constrained the rotation about the z axis. After this the remaining two bolts of the connection showed the same behavior as the first one.
the von Mises stress in the fiber of the boom is about 20 MPa smaller than those i derived from Hand calculation. Maybe using a rigid body as a rope ist not the best approach.
The Analysis now stopped converging after a steptime of 0.1 s instead of 0.05. I had to kill it to work on something else but tomorrow i will run it again and see if the bolts show the same behavior.
I did that and I found that the problematic contact. Its the contact between the upper pin (the pin that connects the “wire rope” and the sheet metal part. Its enough to set only that contact as tied to get convergence.
How do I fix it now ? And how can a bad contact create weird behaviour in other contact regions ?
It would be good to identify the exact cause of non-convergence and locate the problematic nodes involved in that contact now. Perhaps just refining the mesh may help, or you may have to try different contact settings. Sometimes it’s even necessary to add soft springs to stabilize such problematic parts, but that’s the last resort.
