pushover analysis

[allano89]

Dear STKO team
I'm working in pushover analysis, but when I match the results with ETABS, the PUSHOVER CURVE is different.
what will be the problem?
The difference is shown in the photo attached.

[marafini.f]

Dear allano89,

I quickly opened your model and the graph you are showing from STKO is plotting the shear and displacement in the x direction of the top node.
I do not know precisely how it is in ETABS, but from the label on the graph you posted, it looks like it's providing the BASE shear against the top displacement.
To compare the graphs you should be sure you are plotting the same results, and in general a pushover curve is providing the shear at base against the displacement at the top.
You can try extracting the displacement from the top node and reaction force from the base node, both in the x direction, as separate chart data, than click on the option linking the chart to the database, as shown in the picture below, and copy paste the values of displacement in the shear chart data.

Immagine 2021-03-29 103236.png (31.78 KiB) Viewed 4927 times

You will obtain a chart like the one below, that I mirrored for the sake of visualization.

Immagine 2021-03-29 110507.png (8.12 KiB) Viewed 4927 times

I suggest you also check if your units in STKO are consistant and operate the necessary conversion for the comparison with ETABS.

Let us know if you need more help.
Enjoy your modeling

Francesca

[allano89]

thanks a lot. i extracted two charts data and I was able to plot a better pushover curve.
In order to get more accuracy results, can you help me or explain me how to assign 3D nodal masses instead of element masses, but considering the slab?

[marafini.f]

Dear allano89,

Your question is a bit weird. The way you apply the masses will not impact the accuracy of the results in the pushover curve. Masses and loads are separate concepts in OpenSees.

We looked more closely at your model and we noticed the following:

• The loads that you applied are eleLoad_beamUniform, which provide the option to be applied both according to the global reference system or the local one. You picked the local, but your local axes orientation is not coherent (see Fig.1) in all the elements as shown below, therefore one of your loads is pointing upwards (see Fig.2). Moreover, one of your beams is not selected in the load application (see Fig.3).
  You can fix this by either use the Reverse command to apply the correct local axes orientation (but be careful, if you move your model you will need to repeat the operation), or by selecting the global orientation contextually to the load application and refer to the main UCS.

1.png (192.65 KiB) Viewed 4907 times

Fig.1

2.png (72.11 KiB) Viewed 4907 times

Fig.2

3.png (70.74 KiB) Viewed 4907 times

Fig.3

• As I mentioned in your other post, you need to make sure of what you are comparing between ETABS and STKO, both in terms of fiber section modeling and rigid diaphragm assumptions. For example in OpenSees, frame structures modeled with rigid diaphragms are subject to high axial forces, which affect the overall response (see Fig.4). This is normally solved with the introduction of axial releases, which allow the beams to slide in correspondence with the extremities of the structure. Dr Petracca talked about this in this webinar.
  https://www.youtube.com/watch?v=94g7uhiqJ1Y

4.png (192.89 KiB) Viewed 4907 times

Fig.4

• There were a few things you should change in the analysis setup:
  • You can choose a UmfPack SOE as system solver, instead of FullGeneral. Your option is not incorrect, because your model is small, you will not have a sparse matrix, but FullGeneral (as written in OpenSees documentation), should almost never be used! Because it requires a lot more memory than every other solver and takes more time solving the operation than any other solver. It is required only if you are interested in looking at the global system matrix.
  • You choose a Linear algorithm, but you have material nonlinearities in the fiber sections, so you should pick another option, Kryvlov-Newton with 30 maximum iterations for example.
  • You were using 0.0001 for the Norm Unbalance Test, given that your model is approached with distributed plasticity and you are modelling in meters you can choose a lower number, more like 1/100 of a millimeters, rather than half a millimeter
  • You need to reset the time to 0 after your gravity analysis. Keep in mind that the pseudoTime in OpenSees is the "real time" in dynamic analyses, and the "load factor" in static analyses. More specifically in your example, if you do not reset the pseudoTime to 0 after the gravity analysis, your DisplacementControl analysis will start with a pseudoTime = 1, which means that your horizontal load will start at 1*reference_value instead of 0

I attach you here the model corrected.

18-STKO 2 PISOS KN-M(gravitacional-pushover)_edited.zip

(157.1 KiB) Downloaded 269 times

Differently from the static analysis, for eigenvalue and modal properties calculation you need to have masses, but they will never be considered as loads in your static analysis (for nodal mass application, just divide your slab in areas of pertinence of each column and apply the corresponding mass).

Let me know if you need any more help.

Francesca

[allano89]

thanks for your advice, I really appreciate it.
My question was, how to use EdgeMass with the contribution of the slabs?

[STKO Team]

My question was, how to use EdgeMass with the contribution of the slabs?

As I mentioned in the previous answer, the mass will only change the results of your eigen-analysis.

That being said, If you want to consider the mass of the slab, without modeling the slab, you can simply apply an equivalent translational and rotational mass to the master nodes.

Translational mass = rho * thickness * slab_area (in X and Y)
Rotational mass = rho * thickness * slab_polar_moment_of_intertia (J = Ixx + Iyy) (only about Z axis)

Here you can find 2 examples:

• Slab modeled via rigidDiaphragm and equivalent nodal masses at the floor master nodes
• Slab modeled with shells with distributed translational masses.
  Note that here, to simulate only axial stiffness, I increased the Young's modulus of 3 order of magnitude, and decreased the thickness (0.15 m) by 3 order of magnitudes. In this way, E*A will be the same, but the flexural stiffness will be almost zero.

Notes:
1) I discretized your model otherwise the rotational effect of the slab translational mass will not be integrated accurately. In fact the polar moment of intertia (Ixx + Iyy) is exact in the rigidDiaphragm case, but will be approximated in the slab case, and will be more accurate as you refine the mesh.

2) I changed your interaction for the rigidDiaphragm: you used the corner vertices as slaves. This is fine, however, if you refine the mesh, the inner nodes of the beams will not be part of the rigidDiaphragm. So I used the beam edges as slaves.

allano.zip

(173.09 KiB) Downloaded 230 times

[akshaysomkuwar123]

Dear Team,

I am doing Pushover analysis of a spherical lattice dome of span 40 m and height 13.33 m. I checked the elastic pushover analysis first to make sure the model is fine. But when doing non linear pushover I am getting convergence issue. I have attached the graph drift of apex node (mm) vs base shear (kN). currently I am using newtonlinesearch algorithm with energy test. Any suggestions will be helpful.

Thank you

[STKO Team]

It's difficult to tell without the model.
Could you share the model?
What non-linearities are you using? only material or also geometric nonlinearity?
Are you using adaptive time step?

[akshaysomkuwar123]

Please find the attached model. Yes, I have material as well as geometrical nonlinearity in my model.

[STKO Team]

Your model is extremely unstable near the peak.
I tried to use the ArcLength (instead of the DispControl) with an adaptive time step (automation we have in STKO) to try to pass the unstable point.
I also added the MPCO Recorder to visualize the output in STKO.

This is the arc-length curve (load multiplier vs displacement). As you can see from the close-up, the instability is very severe near the peak showing several snap-backs that cannot be captured with disp-control:

Instability2.png (51.15 KiB) Viewed 3979 times

This is the output of fiber-strains. You can see how 3 beams are completely collapsed with 3 hinges:

Instability1.png (319.14 KiB) Viewed 3979 times