Hi all. I’m getting fairly desperate here. I’ve got about 60 hours spent working on a few different kinds of bolted connections and I can’t seem to get the analysis to solve. I’ve tried to simplify it to the connection shown below but I just can’t get it to solve.
For now I’m just trying to get the pretension step to solve but I can’t seem to even get to work.
A quick rundown:
Modelled in FreeCAD as sold parts (part workbench). Fasteners in screw maker. Import and meshing are working great. No issues there.
Bolts are sliced in XZ-plane and XY-plane. Washer, nut and half-bolt are union parts.
The flange and “leg” are merged in the FE-Model tab.
A Single material property and section for all solids.
Bolt is tied to top flange (tried contact with friction - same issue) - also added point springs with no joy.
Same for nut/washer side
Flange/flange is a contact pair.
BCs:
Fixed at leg bottom surface
half symmetry (0 mm Y-direction, rest unconstrained. Also tried UR1 and UR2 0 rad)
Pretension set on boundary layer on the top bolt mating surface.
Once I get the pretension to solve I aim to add tensile forces in the Z-direction only.
I’ve used FEAnalysts and Andreas Baer’s videos as inspiration (can’t post multiple links)
The only thing I haven’t been able to replicate is the surface/line at the washer contact point in Anders’ video. But I don’t think that’s the issue.
I’m really motivated and excited to use prepomax but it’s really throwing hurdles my way. I’d love some advice if anyone can help. I’m new and I’m not allowed to upload here so I’ve thrown the file into my onedrive (no removed) - hopefully I’m not breaking any rules.
It’s important to follow these steps as shown there - create a compound from two halves of the bolt, create a prismatic boundary layer and then define the pre-tension on one of the internal surfaces. Finally, remember to freeze the preload in the second step when applying the operational load.
In practice, bolts are usually modeled using 1D element approach when there’s more of them but you can start from a solid bolt model if you are only interested in the connection itself.
You have to create a compound from the bolt halves. Currently, you have the top and bottom half of the rest of the model compounded but no connection between them. You can see how it’s free to move in a frequency analysis.
Then add the boundary layer. Displacement-controlled preload is indeed good to aid convergence in the initial testing/debugging phases.
Thanks FEAnalyst and Gunnar! Finally making some progress! Compound part seems to have done the trick - I must have watched those youtube videos 20 times but I didn’t spot that for some reason.
I can’t quite wrap my head around the compound part. Is it just the modelling process? Split to get end surfaces to apply boundary layer to and pretension? Other than those end surfaces it behaves as a single part after the fact?
Compound creation results in a continuous mesh so selected parts indeed behave like a single part. You can easily check that by running a frequency analysis. Here, it’s also necessary to have interior surfaces for pre-tension so you need two separate halves of each bolt (but then you merge them so that they behave like a single bolt again).
Both behaviours are possible and depend on the selected mesh settings. These can be found in the global settings and locally under Advanced Mesh Settings:
To determine whether the meshed parts are connected at the end, you can activate the Exploded view or preview “Merge Coincident Nodes”. In the case of the bolts, the halves should neither “fly apart” nor should any coincident nodes be found.
I’m working on my next problem that has multiple pretensioned bolts. I’m having issues again with the pretension step.
The solver has a bunch of these warnings:
*WARNING in gentiedmpc:
DOF 2 of node 1377660 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 2 of node 1377708 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
DOF 2 of node 1377710 is not active;
no tied constraint is generated
*WARNING in gentiedmpc:
These nodes are all at the surfaces between the fastener and plate face.
I let it run over night and the iterations basically repeat:
I’ve tried letting the contact/tie adjust the mesh and not adjust the mesh. @FEAnalyst You mentioned in your video that you prepared the surface under the bolt/nut heads. I suspect this could help. How did you prepare it? Or am I completely off on this theory?
I made those surface partitions using the Boolean fragments tool in FreeCAD. The goal was to limit tie constraint to those small surfaces instead of the whole top/bottom faces of the plates. But this won’t help much with convergence. If you check other threads about preload here, you will see that non-convergence is very common with such models. You should simplify the model and try with tie constraints everywhere and displacement-controlled preload first. Then, if it works, add more advanced features (including contact) gradually.
Thanks FEAnalyst. I’ll study those other threads. My model is already tie-constrained at the nut/plate interfaces. I’ve also tried contacts with point springs at the nuts and bolt heads. And I’ve set it to displacement controlled. I’ll see if I can find other ways to simplify it further!
