Displacement Control for two nodes

[Syun]

Dear STKO Team,

Hi, I am a beginner for both OPENSEES and STKO. Recently, I am currently attempting to use rcjoint3D to simulate the experimental results of a beam-column joint. However, I have encountered an issue where I cannot apply displacement control to both beams simultaneously at their ends. As shown in the first figure, I need to perform displacement control at both points A and B simultaneously (but in opposite direction), following the displacement pattern in the second figure.

However, when I try to set the selection sets, it is not possible to select two selection sets at the same time or to select a single selection set containing two points.

Could you please advise if there is a solution to this issue? I look forward to your response.
Here is my STKO file. If you have time, I would appreciate it if you could take a look. Thank you!
https://drive.google.com/file/d/1YXxuuT ... sp=sharing

[STKO Team]

In this case, don't do and "indirect displacement control analysis" (i.e. impose load and do a DisplacementControl integrator).
Instead, you can do a "direct displacement control analysis" (i.e. impose a displacement via the load->sp, and do a load control analysis)

[Syun]

Dear STKO Team,

Thank you for your response! This has resolved my previous issue.

However, I now face a different problem. I am conducting a simulation of an external joint with a height of 3.7 m and a length of 4.1 m, applying both axial force and displacement control at the column base (as shown in the first figure). I used rcjoint3D combined with pinching4 to simulate the joint deformation.

After completing the simulation and plotting the hysteresis loop of the joint, I noticed that the initial stiffness of the joint significantly differs from the experimental values (as shown in the second figure, where the blue line represents the experimental results, and the red line represents my simulation results).

To address this, I temporarily excluded the joint deformation and considered only the beam-column deformation using the fiber section. The results showed a much more reasonable stiffness (as shown in the third figure).

Based on this, I believe the issue lies in the joint simulation. I have repeatedly adjusted the pinching4 parameters, such as increasing the stress on the backbone curve to a very high value for observation. However, the results have not changed significantly, and the simulated joint stiffness remains much smaller than the experimental values.

At this point, I am unsure how to resolve the issue. Could you please take a look at my rcjoint3D settings to check if something is incorrect? My STKO file is attached at the bottom. I look forward to your response.

[STKO Team]

The Penalty stiffness in your RCJoint Physical property is too low.
It should be 3-4 orders of magnitude higher than your model's representative stiffness (EA/L). In this way, it approximates a rigid connection in the DOFs not involved in the RCJoint.

Another suggestion:
In a disp control analysis it's better to set the reference load close to the expected value (in this way the lambda, which is an unknown in the DisplacementControl method, is close to 1)

Check this:

M6.zip

(157.19 KiB) Downloaded 78 times

I also put a monitor. You can put your experimental data as background if you want

[Syun]

Thank you so much for taking the time to assist me with my problem!
While the stiffness value still differs slightly from the experimental results (it now appears to be somewhat higher than the experimental value), your guidance has greatly improved the situation compared to before. Truly appreciate your valuable suggestions and I will continue fine-tuning the parameters. If I encounter any further challenges, I hope I may seek your advice again.

[STKO Team]

You're welcome

[Syun]

Dear STKO Team,

After completing the joint simulation tests, I proceeded with modeling a 10-story RC structure using the same approach. The beam and column elements are modeled with fiber sections, and the joints are implemented using rcJoint3D. However, upon completing the modeling and performing a modal analysis, I encountered some unexpected results. Specifically, the initial natural periods are predominantly controlled by RMz (as shown in Figure 1).

Figure 1

1.PNG (44.45 KiB) Viewed 1769 times

Additionally, I conducted a dynamic analysis, but the results appear abnormal in the post-processing software. Essentially, the structure exhibits almost no displacement (as shown in Figure 2), which suggests that the overall stiffness in the x and y directions might be excessively high.

Figure 2

messageImage_1741754509320.jpg (123.75 KiB) Viewed 1769 times

To troubleshoot this issue, I tested a model without rcJoint3D, considering only fiber sections. In this case, the analysis results were as expected and appeared normal (as shown in Figure 3).

Figure 3

2.PNG (27.09 KiB) Viewed 1769 times

For the modeling process, I closely followed the tutorials and example files provided by your team (specifically, Week 18 - Example 33). After thoroughly reviewing my model, I couldn't identify any inconsistencies in the setup. At this point, I am uncertain about what might be causing the issue.

Would you be able to take a look and provide any insights on potential aspects I may have overlooked? I have attached my structural model for your reference.

I sincerely appreciate your time and assistance and look forward to your response.

[STKO Team]

The Joint Model doesn't work with the transformation method (due to overlapping constraints, as explained in the webinar).
You should use the penalty handler, or the new Auto handler (which uses an automatic penalty for overlapping MP constraints, and transformation for the SP constraints, it will be the topic of our next webinar)

Also, don't use -fullGenlapack, it's really slow (useful only for small models).

One last note: If there's no previous analysis settings before the eigen command, the eigen command will create some default settings (and for the constraint handler the default is Transformation, which doesn't work with the RCJoint model).
Therefore I put a fake (0 steps, no wipeAnalysis) analysis command before the eigen

[Syun]

Dear STKO Team,

Thank you very much for your help! Thanks to your guidance, I successfully conducted the simulation using fiber elements with rcJoint3D joints.

However, when I tried to analyze the failure modes of the joints on each floor, I realized that I am unsure how to select the appropriate nodes to extract the relevant joint data. This data is necessary for plotting the hysteresis loops of the joints (as illustrated in Figure 1). Alternatively, if plotting based on moment and rotation instead of the format in Figure 2 is more suitable, that would also be fine.

Figure 1

圖片1.png (137.56 KiB) Viewed 1721 times

Would you be able to provide some guidance on how to extract the necessary data for this purpose?

For your reference, I have attached the completed MPCO file in case it is needed.

I sincerely appreciate your time and assistance and look forward to your response.

[STKO Team]

Unfortunately you attached only the CDATA file which does not contain the results.
Anyways, you can get the behavior of the joint:

• record material.strain and material.stress (the joint is build as a zerolength element, so those results will contain your join model data)
• Use a gauss plot to visualize them and select them to extract chart data

See the end of this webinar to see how to do it:
https://www.youtube.com/watch?v=l6ZIhiROfLU