Time History Analysis(plastic model vs elastic model)

luckypants
Posts: 41
Joined: Wed Jun 17, 2020 6:07 pm

Time History Analysis(plastic model vs elastic model)

Post by luckypants » Sun Sep 06, 2020 7:31 am

Dear STKO Team:

Here are two models. One is plastic model(lumped plasticity), and the other is elastic model.

After I finished my analysis, I found the displacement time-history response of the model was almost same with elastic model. What is wrong with my plastic model?

Furthermore, I also built the same model in ETABS. After I finished my analysis, I found the displacement time-history response was same in elastic part, but there was great different in plastic part.

So, It seems that the plastic model built in STKO was still elastic. How could I solve this problem?

Any advices and helps that you provide are highly appreciated.

Best Regards
Attachments
displacement.jpg
displacement.jpg (46.38 KiB) Viewed 447 times
elastic.rar
(82.89 KiB) Downloaded 12 times
plastic hinge.rar
(94.72 KiB) Downloaded 11 times

STKO Team
Posts: 321
Joined: Tue Oct 29, 2019 8:45 am

Re: Time History Analysis(plastic model vs elastic model)

Post by STKO Team » Mon Sep 07, 2020 9:00 am

Dear user, probably the plastic hinge data in OpenSees do not coincide with the one in ETABS. In fact if you look at the moment-curvature (material.stress material.strain) of your plastic hinges, you will see that they remain elastic. They reach about 25000 N*m, while your yield moment is about 110000 N*m.

One thing I noticed is that you used a vertical load but then you fixed the top vertical displacement. In this way the vertical load is useless.
make sure in ETABS the plastic hinge is the same as the one you put in opensees

luckypants
Posts: 41
Joined: Wed Jun 17, 2020 6:07 pm

Re: Time History Analysis(plastic model vs elastic model)

Post by luckypants » Tue Sep 08, 2020 7:34 am

Dear STKO Team:

Thank you very much for your advice.

I have checked the plastic hinge in ETABS is the same as the one I put in OpenSees. You could see the following pictures.

Both of their yield moment are about 110000 N*m.

Furthermore, I also check base shear in STKO, and I find the maximum is about 100000N. The moment of the column should reach yield moment, but why the plastic hinges still remain elastic?

By the way, How could I look at the moment-curvature (material.stress material.strain) in STKO? How do you know the plastic hinges reach about 25000 N*m?

Any advice and helps that you provide are highly appreciated.

Best Regards
Attachments
ETABS.jpg
ETABS.jpg (207.88 KiB) Viewed 431 times
OpenSees.jpg
OpenSees.jpg (78.55 KiB) Viewed 431 times

STKO Team
Posts: 321
Joined: Tue Oct 29, 2019 8:45 am

Re: Time History Analysis(plastic model vs elastic model)

Post by STKO Team » Tue Sep 08, 2020 8:34 am

Furthermore, I also check base shear in STKO, and I find the maximum is about 100000N. The moment of the column should reach yield moment, but why the plastic hinges still remain elastic?
I had a look at the absolute maximum of reaction force along the X direction and it reaches about 90000N. The reaction moment about the global Y axis instead is much smaller than the yield moment. it is about 20000 Nm.
By the way, How could I look at the moment-curvature (material.stress material.strain) in STKO? How do you know the plastic hinges reach about 25000 N*m?
First you need to create a GaussPlot, so that you can select the gauss points of the plastic hinges.
Then, when you try to extract the results, choose to extract them from gauss points.
Then for both X and Y data, choose to use a result, (material.strain(S23) for X and material.stress(S23) for Y)
plastichinge.png
plastichinge.png (154.51 KiB) Viewed 425 times
In any case I think the difference from ETABS and OpenSees are elsewhere. for example, if you change the stiffness modifiers in the elastic section, the plastic response of the hinge will change. Then I would look into the boundary conditions.
Are you sure about the constraints you put on top? you fixed everything but UX.

luckypants
Posts: 41
Joined: Wed Jun 17, 2020 6:07 pm

Re: Time History Analysis(plastic model vs elastic model)

Post by luckypants » Tue Sep 08, 2020 10:16 am

Dear STKO Team:

Thank you very much. Your advice helps me a lot. :D :D

The following picture is my model and my setting in ETABS(C1H1 and C1H2 are the plastic hinges). There are the constraints on the top, because I want to simulate the experiment which has done by MATS(Multi-Axial Testing System).

If Base shear multiplied by H(The height of the column) equals moment. Why the value of the moment is smaller than the base shear?

I also check the reaction moment in ETABS. The moment is about 120000 N*m. It is very different from the result in STKO.

What is the reason make them different? Does the location of plastic hinge make them different?

Because I set the plastic hinge both ends of the column in OpenSees. I don't set plastic hinge at the same location in ETABS.

By the way, what do the component of S11 or S23 mean? What do the number 1 or 2 mean ?

Any advice and helps that you provide are highly appreciated.

Best Regards
Attachments
My.jpg
My.jpg (197.27 KiB) Viewed 423 times
ETABScon.jpg
ETABScon.jpg (144.32 KiB) Viewed 423 times

STKO Team
Posts: 321
Joined: Tue Oct 29, 2019 8:45 am

Re: Time History Analysis(plastic model vs elastic model)

Post by STKO Team » Tue Sep 08, 2020 3:51 pm

If Base shear multiplied by H(The height of the column) equals moment. Why the value of the moment is smaller than the base shear?
Yes here you should have that RMy = L/2 * RFx. But you don't. This happens because the the beam is taking all the rotation while the zerolength takes almost nothing. In fact what happens is that the moment in the beam is correct, but it is not in equilibrium with the momemnt on the zerolength, and this is also related to the fact that you don't see any plasticity in the hinge.
Why?
The reason is simple. You are accepting a non-converged solution. Even if you have chooses 1.0e-6 as a tolerance, it is a tolerance on the displacement field, that also contains rotations. now the yield rotation in your hinge is in the order of 1.0e-11, that is much much smaller than your tolerance. That is, you are accepting any rotation in your hinges. And that's why the forces are not in equilibrium.
This happens also because you used a too large value for the initial stiffness of the hinge (1.0e+15) while the elastic bending stiffness of the beam is about 1.0e+9.
Adding stiffness values that are too high with respect to the rest of the model, just makes your model ill-posed. I typically choose at most 2 or 3 order of magnitude more. So I changed your intial stiffness of the hinge and of the stiff matrerial to 1.0e+11.

Another important change is that I used here the test normUnbalance. When you have a stiff problem (like in this case) it's better to test the residual rather then the solution vector.

Finally I changed the algorithm to krylov, that is much more stable for this kind of problems.
It seems to be working now...
PH_1.png
PH_1.png (27.66 KiB) Viewed 409 times
Attachments
plastic hinge.zip
(128.7 KiB) Downloaded 11 times

luckypants
Posts: 41
Joined: Wed Jun 17, 2020 6:07 pm

Re: Time History Analysis(plastic model vs elastic model)

Post by luckypants » Wed Sep 09, 2020 12:10 pm

Dear STKO Team:

You solve the problem. Thank you so much.

Then, I still want to ask some questions.

1. Sorry, I don't fully understand the first paragraph. What dose "the beam is taking all the rotation" mean ?

I also confuse that the moment in the beam is correct and it is not in equilibrium with the momemnt on the zerolength.

2. The reason that the yield rotation in my hinge is so small(The correct value is about 0.03.) is I used a too large value for the initial stiffness of the hinge. Is it right?

3. What does the component of S11 or S23 in Gauss point plot mean? What does the number 1 or 2 mean ?

4. If we analyze the plastic hinge, it will be better to choose the following setting. Is it right?

algorithm → Krylov-Newton

Test→normUnbalance

Because I don't really understand different kinds of algorithm and test and what is the best choice for us when we analyze.

Best Regards

STKO Team
Posts: 321
Joined: Tue Oct 29, 2019 8:45 am

Re: Time History Analysis(plastic model vs elastic model)

Post by STKO Team » Thu Sep 10, 2020 5:04 pm

1. Sorry, I don't fully understand the first paragraph. What dose "the beam is taking all the rotation" mean ?
I also confuse that the moment in the beam is correct and it is not in equilibrium with the momemnt on the zerolength.
The zero-length elements and the beam are connected in series. For equilibrium they should have the same bending moment (bottom-end of the beam should have the same moment as the bottom hinge, and the top-end of the beam should have the same moment as the top hinge).
However in a nonlinear analysis you try to reach equilibrium convergence by iterations... And the solvers "thinks" that it found equilibrium when the error is smaller than the tolerance you provided in the test command.
But what happens if your tolerance is too high? OpenSees will accept an error that is not negligible, and so the equilibrium is not fullfilled. That's why in your previous (wrong) model, the beam had a correct momemnt, while the zero-length element had a much smaller momement.
2. The reason that the yield rotation in my hinge is so small(The correct value is about 0.03.) is I used a too large value for the initial stiffness of the hinge. Is it right?
Yes, of course the yield rotation is the yield momement / K0. In the image you provided, also the ETABS hinge has a very small yield rotation. Instead a value of 0.03 radians is reached only when the M-R curve drops to a residual value.
Don't be confused however! keep in mind that the ETABS is plotting Moment vs Plastic Rotaiton (not full rotation). That's why the initial stiffness is so high and the yield rotation is almost zero. In theory they should be K0 = inf, YieldPlasticRot = 0. But this is not possible due to numerical errors, so you use a large value as K0, and an almost 0 value for yield rotation.
But this is fine, because the zero-length element has a length = 0, so it should represent only the plastic part, since the elastic rotation is taken by the beam.
3. What does the component of S11 or S23 in Gauss point plot mean? What does the number 1 or 2 mean ?
That is just a side-effect of the fact that STKO and OpenSees are two distinct applications with different conventions. The zero-length element, when all 6 DOFs are used, gives an output called "stress". And it contains the following results:
  1. Fx
  2. Fy
  3. Fz
  4. Mx
  5. My
  6. Mz
However STKO assumes that a result called "stress" with 6 components is a 3D Stress Tensor in Voigt notation:
  1. S11
  2. S22
  3. S33
  4. S12
  5. S23
  6. S13
But you know that it is not a stress tensor but just the forces and moments of a 6-DOF spring, so the 5th (S23) and 6th (S13) components are actually My and Mz
4. If we analyze the plastic hinge, it will be better to choose the following setting. Is it right?
algorithm → Krylov-Newton
Test→normUnbalance
Because I don't really understand different kinds of algorithm and test and what is the best choice for us when we analyze
No, it is true only in this specific problem. The choise of the analysis settings depends on the problem type. This is quite complex to explain here. However our next free e-learning course will deal exactly with these kind of issues. I highly suggest you to attend it.
Here is the link to our webinar page:
https://asdeasoft.net/?stkowebinars-for-opensees
If you want I can take this one as an example and explain in details the steps I took to solve it.

luckypants
Posts: 41
Joined: Wed Jun 17, 2020 6:07 pm

Re: Time History Analysis(plastic model vs elastic model)

Post by luckypants » Fri Sep 11, 2020 2:52 pm

Dear STKO Team:

Thank you so much for teaching me. I learn a lot. I will also attend the course. :D :D

Then, there are three questions I want to ask.

1. What does "ETABS do not plot full rotation" mean? Do you mean ETABS present only the plastic part? Because the initial stiffness is so high. It can't present the elastic part due to x-axis scale(the elastic rotation is too small). Is it right?

2. After I checked the result, I found the period of the column changed at 1.2 sec(The original period is 0.6 sec).

Does this change influence the result? It seems that the column is different from the original one.

3. Why is the cyclic deterioration parameter changed at 1000? Is it the default value for Modified Ibarra-Medina-Krawinkler Deterioration Model?

Yes, I do. You can take this one as an example. I really want to know the steps you took to solve it.

Best Regards

STKO Team
Posts: 321
Joined: Tue Oct 29, 2019 8:45 am

Re: Time History Analysis(plastic model vs elastic model)

Post by STKO Team » Mon Sep 14, 2020 8:39 am

1. What does "ETABS do not plot full rotation" mean? Do you mean ETABS present only the plastic part? Because the initial stiffness is so high. It can't present the elastic part due to x-axis scale(the elastic rotation is too small). Is it right?
If you look at the figure you posted of the ETABS hinge plot, you can see that the X-axis labels says "Plastic Rotation". As you know, the total rotation is Elastic Rotation + Plastic Rotation. Keep in mind that the elastic rotation is NOT the first part of the graph!!! I've seen people assuming that was the elastic part of the deformation, but it is not true, only in perfect plasticity it is true. I will explain this topic in the webinar in more detail.
2. After I checked the result, I found the period of the column changed at 1.2 sec(The original period is 0.6 sec)
It depends on when you check the eigevalues. I remember that you put the EIGEN command at the end. However the eigen command uses the current stiffness. You previous model remained elastic. But now it went into plastic regime, so it make sense that the eigevalues changed. Try to use an eigen command also before the analysis. You will see how the eigenvalues change from one analysis to the other

3. Why is the cyclic deterioration parameter changed at 1000? Is it the default value for Modified Ibarra-Medina-Krawinkler Deterioration Model?
I just used a high value to suppress cyclic deterioration since in your ETABS model there was none.. just to make a fair comparison.

Post Reply