asdeasoft.net

Hello STKO Team!

I have a problem with progressive collapse analysis of a frame system. This is a non-physical growth in the total vertical load during analysis time. The analysis includes two stages:(1) calculation of intial stresses and displacements (0-1 sec); (2)calculation of progressive collapse after one of the reactions is removed (1-2.5sec) . No aaditional force is applied at the second stage although, the total sum of the reactions/internal axial force in the colomns and, most probably, total vertical load increases up to the collapse (see in the attached figure from the first second). As a result no stabilization is observed although bearing capacity of the beam is not exceeded. What can be the reason for that problem? The model can be downloaded using the attached link (https://drive.google.com/file/d/1Gqk0ad ... sp=sharing).

Best Regards,
Aleksandr

It's simply due to the fact that the vertical loads are increasing linearly during the transient analysis.
Why?
You are using a Linear time series in the loadPattern. the first static analysis goes from 0 to 1, so the load factor goes from 0 to 100%. Then the transient analysis starts and goes from 1 sec. to 2 sec., so the load factor grows to 200 %.

In the first analysis, you should:
1) check the loadConst option. It will tell the previously defined loads, to remain contant, despite of what the time series says.
2) reset the time to 0. so the transient analysis will go from 0 to 1 (instead of 1 to 2)

Here is the fixed file:
I just reduced the number of elements to speed up the test. I also used adaptive time stepping, that will increase convergence if you decide to push the analysis further.
And I also used the new monitor feature. Have a look.

Dear STKO Team,

thank you for your response and model correction. Actually, I detected the problem in the amplitude, but wipe command and other amplitude variants did not help me because of convergence problems. Are there any other additional way to stop loading change after analysis step according to previously defined amplitudes?

Best Regards,
Aleksandr

Actually, I detected the problem in the amplitude, but wipe command and other amplitude variants did not help me because of convergence problems

Sorry but I did not understand what the problem is. Now when you use the loadConst option, the previously defined load should remain constant, and they won't follow the associated time series.

Are there any other additional way to stop loading change after analysis step according to previously defined amplitudes?

If you use the linear time series for the first analysis, you MUST use the loadConst command. otherwise, as soon as the time becomes larger then 1, the time series will keep growing (it won't stop at 1, it will always grow linearly with time).
Then there is a second note: When you use the loadConst command, there is a second option to reset the time to 0. This is not mandatory, it's up to you. For example, if the timeSeries for your second step, starts at 0, then you need to reset the time to 0, otherwise it will get the timeSeries value at the current time (say 1 for example).

The other option is to avoid using the loadConst + reset time to 0. But in this case you need to pay attantion to the timeSeries you use.
Assuming your first step starts a t = 0, and ends at t = 1.
Then your second step starts at t = 1, and ends at t = 2.
You must define 2 Path time series,
the first one will be X = [0 1 2], Y = [0 1 1]. SO basically grows from 0 to 1 in the first step and remains constant in the second.
the second one will be X = [0 1 2], Y = [0 0 1]. So basically remains at 0 in the first step and grows in the second step.
A side note: due to round-off errors, it may happen that the last step will be slightly larger then your last time t = 2 (for example it could be t = 2.0000000000001). In those cases the timeSeries will give you a 0 load factor because the t is out of range. In this case I always put an extra point in the Path timeSeries just to keep the last value constant:
Just to follow the previous example:
Step 1: X = [0 1 2 2.1], Y = [0 1 1 1]
Step 2: X = [0 1 2 2.1], Y = [0 0 1 1]

If you have other iussues please send us your SCD file with a detailed description of what is going on.

Dear STKO Team,

that is what I actually wanted to know.
Thank you for your answer.

Best Regards,
Aleksandr

Dear STKO Team,

I am sorry to trouble you but I have discovered a strange effect in a similar 2d-frame model of progressive collapse.
After colomn removing, an additional "strange" compressive force appeared in the girger beam above the removed colomn (I have not observed it in linear analysis and non-linear analysis with lumped plasticity.) Could you please explain what can be the reason of such effect. Axial force diagram and the model are attached. There is no horizontal loading in the model, therefore, the reaction at the end of the initial static step is virtually 0.

Best Regards,
Aleksandr

Dear Aleksandr,

It is perfectly normal that you see compressive forces growing where the beams are going into a nonlinear stage. It happens because when the beams (with fiber cross-sections) start failing, the neutral axis would like to shift upward due to cracking, thus showing an expansion (positive axial strain) in the beam central axis. However the beams in the center of the building are somehow confined by the rest of the building, and this confinement results into compressive stresses in the beams.

This is correct. You did not see it in the elastic model and in the nonlinear model with lumped plasticity because:
1) the elastic section does not go into nonlinear stage obviously
2) the lumped plasticity does not have any P-My-Mz coupling, thus it will never be able to represent the shifting of the neutral axis...

A side note: You see zig-zag diagram for normal forces just because you are using displacement-based elements.

Dear STKO Team,

thank you for your response. We'd been looking for an experimental work confirming the conclusion and finally, we found a good experiment directly related to that issue:
https://ascelibrary.org/doi/abs/10.1061 ... 1X.0001938
Similar effect was observed there experimentally. Thank you for your answer.

Best Rgards,
Aleksandr

Nice reference.
Yes this behavior happens quite often in beams.

It is physical, but sometimes it is seen as an un-realistic behavior because one does not expect compressive axial forces on beams.
However, when an RC beam goes into the nonlinear stage, the neutral axis shifts towards the top, and the center-line of the beam would show positive deformation, which in fact represents the opening of the crack. When a beam is constrained by other beams (as in your case) or is involved in rigid diaphragm constraints, the axial deformation is constrained, and so it will develop compressive axial forces.

In your example, it is physical (correct) because the central beams are constrained by a finite (real) value of stiffness, i.e. the EA of the neighboring beams.
Instead, pay attention to rigid diaphragms, as they impose a zero axial deformation. In fact, they emulate a rigid membrane for the slab. However, in real life, the slab is not at the center-line of the beam, and it is not infinitely rigid, so the resulting axial forces in the beam will be too high and unrealistic, and it may overestimate the real bending capacity of your beams.

Of course this happens only when your beam has P-M-M interaction. So only with fiber sections

STKO Team wrote: ↑

Fri Nov 13, 2020 12:40 pm

It's simply due to the fact that the vertical loads are increasing linearly during the transient analysis.
Why?
You are using a Linear time series in the loadPattern. the first static analysis goes from 0 to 1, so the load factor goes from 0 to 100%. Then the transient analysis starts and goes from 1 sec. to 2 sec., so the load factor grows to 200 %.

In the first analysis, you should:
1) check the loadConst option. It will tell the previously defined loads, to remain contant, despite of what the time series says.
2) reset the time to 0. so the transient analysis will go from 0 to 1 (instead of 1 to 2)

Here is the fixed file:
I just reduced the number of elements to speed up the test. I also used adaptive time stepping, that will increase convergence if you decide to push the analysis further.
And I also used the new monitor feature. Have a look.
FrameDistr_v1-7SP_d32-A600.zip

Dear STKO
I downloaded the attached file and the file posted below. However, I cannot perform the calculations. I have version 3.1.0 of STKO and have not modified anything. I just wanted to learn from the posted example.