Coupled RC Core Wall with MVLEM-3D

[kolozvari]

Hello,

I am working on a 3D model of Coupled RC Core Wall building. My approach includes using MVLEM-3D for RC walls and lumped plasticity shear hinge for coupling beams (see screenshot).

I have two questions:
1) What physical property needs to be assigned to MVLEM-3D wall elements? All wall modeling parameters are defined within MVLEM-3D element (element property), so I am not sure what to assign as the physical property of these elements. If I don't assign anything I receive an error that something is missing in the model definition.
2) How would you go about modeling of coupling beams? Currently I have two elastic beams in my model with a node in the middle intended for a shear hinge. Do I just simply add a zero length element to the middle node? Any particular details I should pay attention to?

Please let me know.

Thank you

[STKO Team]

Actually in STKO we have 2 automation:

• The HingedBeam element, which automatically places zero-length hinges at both ends of an Edge. it automatically detaches the Edge from the 2 end-nodes and places zero length at the 2 ends
• The BeamWithShearHinge element, which automatically places a zero-length hinge in the middle of an Edge. It automatically splits the Edge into 2 pieces and puts the hinge in the middle

In the current version of STKO you cannot use them together, so I made a quick change to use them together.
Here's a modified version of the HingedBeam:

HingedBeam.zip

(3.48 KiB) Downloaded 15 times

You can extract it and place it in C:\Program Files\STKO\external_solvers\opensees\element_properties\special_purpose, replacing the existing one. it will be available for everyone in the next STKO version


And here is a simple example that shows you how to use it with MVLEM-3D:

MVLEM_CBEAm.zip

(139.62 KiB) Downloaded 17 times

As you can see you have a simple attached geometry (as if the beam were continuous and attached to the walls):

MVLEM_1.png (197.61 KiB) Viewed 1690 times

In the first stage you will see the 2 rotational hinges yielding, but still in strain hardening. So both moment and shear grow together:

MVLEM_2.png (100.61 KiB) Viewed 1690 times

In the second stage, since the shear strength in this example is smaller, you will see a shear failure (and subsequently an unloading in moment-rotation to keep equilibrium with shear-softening):

MVLEM_3.png (90.12 KiB) Viewed 1690 times

MVLEM_4.png (35.46 KiB) Viewed 1690 times

NOTES:
The hinges (rotational and shear) are actually zero-length elements, so you can see their results asking for material.strain and material.stress in the MPCORecorder.
Then in the Post Processor you will see a material.strain/stress with 2 components for the shear-hinges (Vy, Vz) and a material.strain/stress with 6 components for the end-hinges (P, Vy, Mz, Tx, My, Mz).
Note that in these automations, the zero-length have automatically the same local axes of the parent beam element!

[kolozvari]

Thank you for quick and detailed response.

Please note that I do not need to use both shear and flexural hinges. I only want to use shear hinge in the middle of the beam. Please see the attached model. I would really appreciate if you can help me with two things:
1) regarding MVLEM elements: currently they have assigned Physical Properties W_36, W_34, etc. (all except W_30 which is basement wall and it should be elastic). However, this doesnt make sense since they are MVLEM elements. When I remove mentioned Physical Properties, the model reports the error that something is not defined/assigned (it's not very clear).
2) Regarding coupling beam: I have already created nodes in the middle and I am hoping to only assign a vertical shear spring using ZeroLenght elements. Is that possible? The approach you suggested is fine but I dont want to recreate the model. Do you think you can create only one shear hinge as an example in the attached model and I can take it from there? Uniaxial materials Pinching4 that start with CB (still unassigned) are intended for coupling beams.

Looking forward to hearing from you.

Thank you

[STKO Team]

1) regarding MVLEM elements: currently they have assigned Physical Properties W_36, W_34, etc. (all except W_30 which is basement wall and it should be elastic). However, this doesnt make sense since they are MVLEM elements. When I remove mentioned Physical Properties, the model reports the error that something is not defined/assigned (it's not very clear).

Fixed like this:

1. Look at the complete Traceback of the error -> The error comes from the ASDShellQ4 Element property, therefore you probably assigned a shell element to what should have been a MVLEM

   

   error_1.png (229.65 KiB) Viewed 1670 times

2. Isolate the portion of the geometry with MVLEM and Shell(Wall) Element property to spot the issue (Select the target properties, then use the command "Show")

   

   error_2.png (88.33 KiB) Viewed 1670 times

3. Then I used the Label tool to understand what was the element property you wanted to use there

   

   error_3_fix.png (104.21 KiB) Viewed 1670 times

2) Regarding coupling beam: I have already created nodes in the middle and I am hoping to only assign a vertical shear spring using ZeroLenght elements. Is that possible? The approach you suggested is fine but I dont want to recreate the model. Do you think you can create only one shear hinge as an example in the attached model and I can take it from there? Uniaxial materials Pinching4 that start with CB (still unassigned) are intended for coupling beams.

If you don't want to change the geometry (next time it's easier if you use a unique edge, and then the BeamWithShearHinge), now you can use the HingedBeam, only on the first half of each edge, and using a hinge only on the node J (send node), which will correspond to the middle node:

1. First I created a selection set with all the first-half parts of the edges of the coupling beams (luckily all the coupling beams were built with a counter - clockwise local X axis)

   

   hinge_first_half.png (75.7 KiB) Viewed 1668 times

2. Then I created a template physical property for the first half of the coupling beams. I used a elastic (E = 0) NULL material just to emphasize the shear hinge in the output, then you will change it with the Pinching you want.
   Note that you have to do it for each type of beam (for simplicity I used the same property on all the beams)

   

   hinge_first_half_phys_prop.png (49.81 KiB) Viewed 1668 times

3. This is what you get

   

   results.png (68.2 KiB) Viewed 1668 times

Here's the file:

[kolozvari]

Thank you very much for your detailed response!

Two follow up questions:
1)

Then I used the Label tool to understand what was the element property you wanted to use there

Where is this tool? I wished so many times that there is something that can tell you what is assigned to what. I didnt know it even exists.

2)

If you don't want to change the geometry (next time it's easier if you use a unique edge, and then the BeamWithShearHinge)

I would actually prefer to use only one edge and BeamWithShearHinge, but I got a bit confused about this. In my understanding, BeamWithShearHinge is a Property, correct? If that is the case, what element type should be assigned to the BeamWithShearHinge? I looked at your MVLEM example, but in that one you are combining HingedBeam and BeamWithShearHinge, and I couldnt really figure out how it works.

Looking forward, I have a few one more questions:
1) Eventually, I will have to process drifts, coupling beam rotations, and other EDPs along the height of the building. Selecting nodes manually each time after the analysis would be very time consuming and it would be very easy to make an error. Any advice on how to create groups of nodes/element so I can easily post-process results later?
2) How do you assign OpenSees drift recorder in STKO?

Thank you so much. Looking forward to hearing from you!

[STKO Team]

Where is this tool? I wished so many times that there is something that can tell you what is assigned to what. I didnt know it even exists.

labels.png (63.79 KiB) Viewed 1656 times

I would actually prefer to use only one edge and BeamWithShearHinge, but I got a bit confused about this. In my understanding, BeamWithShearHinge is a Property, correct? If that is the case, what element type should be assigned to the BeamWithShearHinge? I looked at your MVLEM example, but in that one you are combining HingedBeam and BeamWithShearHinge, and I couldnt really figure out how it works.

• Physical Property
  
  • Define any physical property for a beam, for example a Section->Elastic (P1)
  • Define a uniaxial material for shear Vy (P2)
  • Define a uniaxial material for shear Vz (3P)
  • Create a special_purpose->Beam-Column->BeamWithShearHingeProperty
    
    • Beam Property = P1
    • Vy Material = P2
    • Vz Material = P3
    • K = a penalty > GA/L, for example GA/L*100
• Element Property
• Define a base element property compatible with the Physical property P1, for example beam_column_elements->elasticBeamColumn (E1)
• Create a special_purpose->BeamWithShearHinge (E2)
  
  • Beam Element = E1

1) Eventually, I will have to process drifts, coupling beam rotations, and other EDPs along the height of the building. Selecting nodes manually each time after the analysis would be very time consuming and it would be very easy to make an error. Any advice on how to create groups of nodes/element so I can easily post-process results later?

Expand the Database node in the post-processor WorkTree, and have fun with what you find inside!!!

MetaDataInOutputDataBase.png (398.52 KiB) Viewed 1656 times

Or have a look here for custom extraction using the Python API:
viewtopic.php?f=46&t=2439

2) How do you assign OpenSees drift recorder in STKO?

You can use a customCommand (Tcl script with the opensees command for that recorder). Note however that it won't work in parallel:
viewtopic.php?f=46&t=2410

[kolozvari]

Hello,

Thank you for detailed response. I have re-did the model with BeamWShearHinge property (it is much cleaner that way) and I assigned actual properties of all coupling beams (model is attached). However, unfortunately, the model is not converging at about 30% of the ground motion. I have tried several things such as using linear materials for coupling beams and changed a bit penalty parameter for BeamWShearHinge (10^9, 10^10, 10^12), but I couldn't fix the convergence issue. I am using Concrete02 and Steel02 materials for MVLEM_3D elements and Pinching4 materials for coupling beams. I have use this combination of materials and models on large building models and didnt have any convergence issues.

I have a few questions/requests if you dont mind:
1) Can you please give me some advice how can I figure out what is causing the convergence problems? Is there any tool in STKO that can say which element is the problem?
2) Can you please scan through the attached model and let me know if there any issues with it, particularly in terms of definition of nonlinear materials/elements?
3) Can you please tell me how can I implement an alternative nonlinear solution strategy that will be executed in case the analysis fails with the current nonlinear solution algorithm? For example, if analysis doesn't converge with current stiffness to switch to initial stiffness. This is possible in OpenSees with some coding, but I am not sure how to do that in STKO.
4) Can you please remove all files you sent me in this thread from the forum? I have noticed there are few files still lingering in previous messages?

Looking forward to hearing from you. Thank you.

[STKO Team]

Here's a working file:

• The analysis starts to have convergence issues at about 30% probably due to softening in some walls. It stops because you selected Fixed Time Step. I switched to Adaptive Time Step
• At this point It was converging thanks to the adaptive time step, but the convergence was very poor, so I stopped it to have a look at the results. It appeared that at about 30% of the analysis, the acceleration in one corner of a wall was blowing up to unreasonable values (1.2e4 m/s^2!!!!).
• So there was clearly something with the dynamic analysis. I noticed that you used the Tangent Stiffness in the Rayleigh Damping. I switched to Initial Stiffness and it runs fine now.
  Why?
  Making damping relative to the tangent stiffness is not a good choice. What happens when you have softening? Negative eigenvalues on the tangent stiffness, hence negative damping forces... Just think that, even though we call it "stiffness", the tangent matrix just contains numbers (components of the gradient of unbalance forces) that may not have any physical meaning.
  Furthermore, damping is a way to include nonlinearities that we did not include via non-linear constitutive models, so it seems reasonable to make it relative only to the elastic stiffness

1) Can you please give me some advice how can I figure out what is causing the convergence problems? Is there any tool in STKO that can say which element is the problem?

There is not such a tool in STKO. What I typically do is to look at the output and try to understand what is going on from the results.

3) Can you please tell me how can I implement an alternative nonlinear solution strategy that will be executed in case the analysis fails with the current nonlinear solution algorithm? For example, if analysis doesn't converge with current stiffness to switch to initial stiffness. This is possible in OpenSees with some coding, but I am not sure how to do that in STKO.

It can be done using custom functions that can be called before and/or after the current analysis step is solved. It's a new feature that is not yet documented because we will do a webinar about it. But if you need it let us know, and we will try to explain it here.
Anyway, most of the times I solve convergence issues just by using adaptive time step. The type of solver should be decided based on the type of problem you have.

4) Can you please remove all files you sent me in this thread from the forum? I have noticed there are few files still lingering in previous messages?

Done

[kolozvari]

This is great, thank you! Can you please remove the model for the forum?

The analysis starts to have convergence issues at about 30% probably due to softening in some walls. It stops because you selected Fixed Time Step. I switched to Adaptive Time Step

I have noticed you changed the number of numIncr in the "analyze" command to about a half of what was there originally. Can you please explain why is that? Is this how it should be done with Adaptive Time Step is used?

Regarding post-processing, what response do I need to select to obtain force and deformation of coupling beams if they are modeled as BeamwithShearHinge STKO automation? Would this give me deformations at the shear hinge only or total beam rotation?

Thank you

[STKO Team]

Can you please remove the model for the forum?

Done

I have noticed you changed the number of numIncr in the "analyze" command to about a half of what was there originally. Can you please explain why is that? Is this how it should be done with Adaptive Time Step is used?

Originally there were (if I remember correctly) 1000 iterations.
It's too much. Keep in mind that a standard Newton method should have a (almost) quadratic convergence, so if it does not converge in max 10 or 20 iterations (depending on how strict is your tolerance), it's useless to keep on trying, instead, it's better to reduce the time step, so that the prediction of the Newton method will be closer to the solution.
Since I used the Krylov-Newton, it does not have an exact quadratic convergence so I typically choose about 30 iterations.
Only when I need (very rarely) ModifiedNewton with initial tangent, then I allow 100 iterations.

Regarding post-processing, what response do I need to select to obtain force and deformation of coupling beams if they are modeled as BeamwithShearHinge STKO automation? Would this give me deformations at the shear hinge only or total beam rotation?

You can ask for whatever results is provided by the Beam Element type used in the BeamWithShearHinge.
Instead, to record the response of the shear hinge in the middle just ask for material.strain and material.stress.
Keep in mind that BeamWithShearHinge is not a new element, it's just an STKO automation that builds a compound of beam elements (whatever you choose) and a zero-length element in the middle