I often seem to wait a long time for an analysis, only for it to fail (with no clues as to why).
Is there any way to judge from convergence output in Monitor, whether a solution is probable, or if things are simply not converging. For example see convergence results from my current run…
convergence.zip (559 Bytes)
Based on the convergence criteria: Stacked flow plates - model simplification - #26 by FEAnalyst
But this case looks like a typical underconstrained model (initial rigid body motions). So I would just check the BCs, constraints and interactions as well as other connections (frequency analysis can be helpful) right away.
I’ve simplified model to 2 parts -
Is there any guidance on setting up contact conditions? My experience with another FEA system isn’t helping here.
It might be best to start from tie constraints and then replace them one by one with contact pairs. If necessary, use adjustment and make sure you have sufficient boundary conditions. Sometimes it’s also necessary to use prescribed displacement instead of force initially.
I’m also working on bolt investigations at the moment. As FEAnalyst mentioned I would first go with pure Tie in bolt head and connection between the parts. When this case is working switch one by one from Tie to contact (first start with the bolt head). From my experience it can be helpful to change Tie adjustment of the fixed bolt end from default to a defined position tolerance like > 0.1. Especially if you have a coarse mesh. Is your model compareable to this model approach here?: https://prepomax.discourse.group/t/bolt-pretension-model/2037/5
Sorry - I don’t understand the ‘defined position tolerance’ stuff. I don’t see anything in documentation explaining options for contacts. It’s very different from my previous system.
I’ve actually joined the bolt heads (19 off) to the part they contact (did that in CAD to reduce number of parts - all parts are steel). As soon as I add a second part which touches the first - things fail; either a reported failure or just multiple iterations with no sign of convergence.
60 iterations is the default maximum so getting to 60 like you have is a sign it’s either never going to succeed or will be unnecessarily slow. There also seems to be no progress on any of the other metrics here, which suggests it’s going nowhere.
No increments converged so start with very light loads - ramped up gently from zero just to get over the hump of the first iteration converging, then all the contacts are probably working and everything should hold itself together for subsequent increments unless you do something obvious like ripping it apart with a huge force that would break the real thing too.
How is the second plate restrained? Friction with the other plate? Are the bolts already put in tension to engage that friction before it’s loaded? Even if all that’s true, it can still be flakey if any part is only restrained by contacts, not tied to anything else or having any displacement BCs on it.
Another possibility, if you’re using Pastix without mixed precision turned off, it’s less robust. If you see in the output Pastix ending it’s set of iterations with a large error (more than 1e-10 or so?) and CCX continues with the next iteration, that means it’s using that bad solution everything can go to pot.
can iit provide a picture of problems? i guess a single bolt, if yes probably a rigid body motion occurs cause of bolt rotated around axis, modeling with symmetry can help maybe. Regarding converges criteria, it seems not easy to detect since the solution unknown. However, a residual force reported in logs can indicate when the value is reduced during iteration, but frequently in jump at case of large multipart contact.
@DavidJ I think some detailed information about your model would be helpful. Maybe add some images discribing your problem. In general the basic theory of contact modeling in FEA is almost nearly the same based on pressure overclosure model. Therefore you could check abaqus contact reference for detailed information.
Defined position tolerance I mentioned is an option in the tie constraint menu. You should check mesh coincidence of the mating parts whereas above option could help.
For picture see Stacked flow plates - model simplification - #5 by DavidJ
I’ve since removed some parts and combined others to get mesh manageable.
I think I must be missing some basic settings/options - my previous FEA system was very different from this. The names used in contact don’t mean much to me.
I’m very confused now - Tie constraints or Tie contacts ?? I have contacts between parts.
There was mention of applying loads ‘gently’ - what is procedure to do that?
Tried switching to Tie constraints - now get
*ERROR in e_c3d: nonpositive jacobian
determinant in element 585632
???
i seen too much detail in bolt heads may cause mesh problem even with tetrahedral. It’s commonly to simplify all detail of bolt including threads by equivalency in diameter of cylinder.
in some case, tie constraint getting conflict with contact when collided. Contact type tied is compatible with penalty, it’s available in PrePoMax menus to easily to switch.
Is there any output result at all? Any final picture that could give a clue of what is going on?
With adjustment enabled ? Try without it. Tie constraints are usually better than tied contact because they don’t increase the analysis time significantly (but won’t give you contact pressure if that’s what you need).
You may use the amplitude feature to vary loads in time (by default it’s linear ramp but you can change it).
I simplified the bolts weeks ago - now simple round heads, and also merged into a single part with the washers and the outer plate. Inboard end faces (actually half way through) of bolts are fixed.
Thanks - I think turning off Adjust has helped (no idea what it does).
Amplitude - I only see ‘Tabular’ type - I have no idea what the settings mean . Is there some other option I have to enable to make ‘linear’ available.
What about ‘incrementation’ in settings for the Step ?
When checking part I now get warnings such as
*WARNING in gentiedmpc: no tied MPC
generated for node 610137
no opposite master face
found; in-face tolerance: 2.1848522719187587E-002
Well - it does now complete analysis (in about a minute) - BUT results are clearly incorrect (zero stress everywhere).
Here is an idea of the attempted analysis
Run a Modal Analysis (Frequency Step) to see if you have any unconstrained components.
What about displacements?. Has the model explode with huge displacements in a particular direction?, lets say x, y or z. I agree with Arnie. The frequency analisys is an excelent sanity check.
