Error Running Non Linear Time History Analysis

[darmawan]

Dear STKO Team

I am dealing with nonlinear time history analysis of a pile supported slab. The pile is hollow concrete prestressed pile.

I try to set the dynamic analysis following the ASDEA webinar about NLTH analysis of bridge. But my analysis still don't work.
I think there are still some misstake I did, But i still cant recognize where is the problem and how to solve it.

Any recomendation / suggestion will be very appreciated. Thanks you in advance

[Horace Horsecollar]

Dear Darmawan,
your file was not meshed and partitioned. If you mesh and partition it, the gravity works.
In addition, you did not assign in analysis: push, mass mid and mass edge (they are black).
Regards

[darmawan]

Dear Horace Horsecollar

Thank you for the response and reply,

I have meshed the model. But the gravity and dynamic still not working. Is the meshing wrong?
I see in the ASDEA example (NLTH of bridge), the mass is "black" too. Where should be the mass assigned?

Best regards

[marafini.f]

Dear darmawan,
masses do not need to be assigned anywhere, you just need to make sure they are applied to the right node and they will be calculated by STKO automatically, they will stay black.
I did not have time to go in-depth in your model. But I think you have the wrong units for mass and load assignments.
I did some modifications to your model and it does run now, but it's not correct fully so I am not going to attach it for now.
If I manage I'll do it later today or on Monday. For the time being, I suggest you proceed like this.

- check your material properties (your concrete07 has not Ec defined, try to use the material tester to draw a monotonic curve to be sure you are using the right constitutive model)
- check the units, if your model is N mm, then you are applying 320 kN on each node, that sound a bit much to me;
- operate an eigenvalue and modal properties plot before any other analysis, to check if it works as you expect (i did it and the period of the first mode came out of 2s, that's also a bit much, maybe your masses are not in the right order of magnitude, I expect a frame structure to have 0.1-0.2 seconds for a first period)
you can check out this thread for how to do an eigenvalue analysis with the proper commands
viewtopic.php?f=33&t=1753&p=3490&hilit=mass#p3490
- given that you are applying an initial strain, try to run a linear analysis without any load, to see if the effect of such strain is accounted for in the section.fiber.strain results on the steel fibers.
- do a gravity analysis and check the localForce results if they are consistent with what you expect (for example if they are symmetric and there is no concentrated force/stress somewhere)
- then proceed as you already did with the rest of the analysis, adding the damping, the uniform excitation etc...

you do not need a push force if you are using a uniform excitation

if you want to run in parallel, use reverse parallel, mumps and partition your model before run, in at least 2 parts.
But I suggest you start by asking less results, just displacements, modesOfVibration, localForce and section.fiber.stress and strain on elements and run with a single processor, then if you want to ask your recorder for much more results just change the setup for a parallel analysis afterwards. Your model is not big, you can do it with just one processor.

Try all of the above and let me know.
Sorry if I did not provide a more detailed answer but I think you can figure something out with these suggestions.

Enjoy your modelling
Francesca

[darmawan]

Dear Francesca

First, thank you for your detailed explanation, it helps me a lot. I tried to modify my model following your suggestions.

I forget to input the Ec

I modify the self-weight and mass of the structural element using EdgeForce and EdgeMass, respectively, instead of using NodeForce and NodeMass. I attach the calculation of the self-weight of each structural element. I use N, mm units

I tried to modify the modal analysis following the thread you shared, but the modal analysis still not working, perhaps I made a mistake?

Thanks you in advance

Best Regards,
Darmawan

[marafini.f]

Dear darmawan,

if you have already a gravity analysis to run, you do not need to create a new dummy analysis before the eigen analysis.
Just place your eigen and modal properties command after your gravity and add a record to save the results in a separate stage.

Remember, do not flag the wipeAnalysis option, not only for the eigen but also for the next analysis. That command will erase everything you set up beforehand, therefore the analysis setup read by the eigen command will make reference to the analysis default setting that may not work with your constraints for example.

Anyway, here is a model with a functioning eigen and modal analysis. I ran in sequential, cause I think you do not need parallel computing, and also modal analysis and gravity can be run simply without multiprocessor computation.

Unbraced_1_edits.zip

(642.64 KiB) Downloaded 202 times

Great job with your units!

Let me know how it goes.
Francesca

[darmawan]

Dear Fransesca,

Big thanks for your explanation. Your explanations help me a lot. I am trying to understand.

• I try to run the modal analysis. The analysis works, but the result did not appear from the post-processing as the thread you shared to me. I have checked the modesOfVibration in the MPCO recorder.

• Then, I tried to run the dyanmic analysis. I tried to follow the Massimo's webinar about Non Linear Time History Analysis. I use the same acceleration x & y too. But the running still did not work. I did not flag the wipeAnalysis

• And still wondering, the internal forces diagram seems not make sense. they are not symmetric

I need to learn more about OpenSees & STKO indeed. Still always getting error in my analysis

Thank you in advanced,
Darmawan

[marafini.f]

Dear darmawan,
the modalProperties command was added to OpenSees not long ago.
I suggest you uninstall opensees on your machine, and reinstall, by following this procedure:

• OpenSees 3.2.2 compiled by prof. Nicola Tarque, Pontifical Catholic University of Peru (website https://www.pucp.edu.pe/profesor/sabino ... ducciones/)
Features: Sequential OpenSees, Parallel OpenSees, Continuous Updates

Download the precompiled version of OpenSees (sequential) and OpenSeesMP (parallel)
https://drive.google.com/file/d/1ETGQ3Y ... 5Mk7C/view
Install them in the folder C:\OpenSees-Solvers (Default location)

If you dowload this version, the modalProperties command will work and save the result. Remember to use a record command at the end of your eigen value analysis and modal characteristic extraction.

As for the asymmetric response of your structure, I had noticed that too. I think it's because of the local axes orientation in your model. Check out our latest webinar presentation and this thread too. viewtopic.php?f=27&t=1906#p3369

Keep me updated.
Enjoy your modeling
Francesca

[darmawan]

Dear Fransesca

I have update my OpenSees slover. It works now, The modal analysis result appeared. thank you!

I have checked out the thread & last webinar, I think the local axis does not problem. But, I found that there is a triple pile element in the same location. I fixed it and the internal forces got better.

But the dynamic nonlinear time history analysis still did not work. I don't capture where the problem is. I have set the dynamic analysis command following Massimo's webinar about NLTH.

Thank you in advance

[marafini.f]

If you run your analysis with opensees sequential you have to use a numberer that it's not parallel.

With you model as it is, if you just change the parallel reverse numberer to the reverse numberer the NLTH runs.

If you want to use openseesmp, you need to partition your model, use the parallel numberer and mumps as system command in all the analyses you are setting up.