Beam-to-Solid-Bar-Slip

cqf_2232
Posts: 64
Joined: Fri Dec 10, 2021 1:00 am

Re: Beam-to-Solid-Bar-Slip

Post by cqf_2232 » Fri Apr 29, 2022 2:22 am

For example, I have defined the mechanical parameters of concrete in DamageTC3D. When cracks appear in the concrete, it shows the damage? Or does the damage appear only when the ultimate strain is exceeded?

STKO Team
Posts: 1346
Joined: Tue Oct 29, 2019 8:45 am

Re: Beam-to-Solid-Bar-Slip

Post by STKO Team » Fri Apr 29, 2022 8:28 am

You can refer to this paper for more details on the DamageTC3D model:
https://www.researchgate.net/publicatio ... hear_walls
When cracks appear in the concrete, does it show the damage? Or does the damage appear only when the ultimate strain is exceeded?
Damage appears when a crack appears, not when they are fully open. Damage is a measure of how much of the material is cracked. 0 means elastic. 1 means the crack is fully open, and the material does not give any stress. When the value is less than 1 but larger than 0, it means that the crack is developing
damage_1.png
damage_1.png (47.84 KiB) Viewed 744 times
Attachments
damage_0.png
damage_0.png (69.88 KiB) Viewed 744 times

cqf_2232
Posts: 64
Joined: Fri Dec 10, 2021 1:00 am

Re: Beam-to-Solid-Bar-Slip

Post by cqf_2232 » Wed Jun 15, 2022 8:49 am

Dear STKO Team,
I built a three-point bending beam model based on experiments. For some reason, the convergence is poor. Can you help me check if it is related to improper parameter settings. Some details of the model are described below:
1. Only the four longitudinal rebars at the bottom consider the bond slip. Due to the difference in stirrup spacing, I used two uniaxial materials with different parameters to simulate bond slip.
2. The previous three steel plates and concrete were connected by the merge command, and the convergence was good. Frictional contact is now used between the three steel plates (slave solids) and the concrete (master solid).
3. The top steel plate and the loading control point are connected using 'beamsolidcoupling’.
Attachments
beam.rar
(961.27 KiB) Downloaded 10 times

STKO Team
Posts: 1346
Joined: Tue Oct 29, 2019 8:45 am

Re: Beam-to-Solid-Bar-Slip

Post by STKO Team » Tue Jun 21, 2022 10:53 am

Your model is fine. I just noticed that you are using the Surface to surface contact.
You selected the "FromElement" option with a node-to-element interaction because the geometries of the master/slave pairs are not conforming.
This is what I explained in the webinar, and should work in theory. What we do behind the scenes, is to create an auxiliary node for the contact master, and this node is attached to the master surface with an embedded condition, whose penalty stiffness is equal to the contact stiffness.
However we noticed that this approach can give numerical instabilities, and we are working on a cleaner implementation.
In the meantime, you can use the node-to-node contact.

What I did, is to simply add a central line to the beam faces so that they match the faces of the steel plate, making sure their mesh nodes are coinciding.
Have a look at the attached file.
beam.zip
(1.45 MiB) Downloaded 12 times
I also changed from Displacement control to load control with imposed displacement. It's easier to handle in this kind of problem.

Now it seems to work, but it fails earlier, probably because the mesh is quite coarse.
DAMAGE.png
DAMAGE.png (172.89 KiB) Viewed 599 times
DMAAGE_2.png
DMAAGE_2.png (32.66 KiB) Viewed 599 times

cqf_2232
Posts: 64
Joined: Fri Dec 10, 2021 1:00 am

Re: Beam-to-Solid-Bar-Slip

Post by cqf_2232 » Tue Jun 21, 2022 2:10 pm

Thank you very much! As you mentioned the mesh is rough, probably due to the rebar holes being dug in the solid elements. I tried adding auxiliary lines to delineate hexahedral elements, but it turned out to be tetrahedral elements. How can I optimize the mesh?

STKO Team
Posts: 1346
Joined: Tue Oct 29, 2019 8:45 am

Re: Beam-to-Solid-Bar-Slip

Post by STKO Team » Tue Jun 21, 2022 3:54 pm

You can just use a smaller global mesh seed.
For this model, you should use a tetra mesh anyway

cqf_2232
Posts: 64
Joined: Fri Dec 10, 2021 1:00 am

Re: Beam-to-Solid-Bar-Slip

Post by cqf_2232 » Wed Jun 22, 2022 2:24 pm

Thank you again!I also noticed that you scaled down the values of Kn and Kt. How should these two parameters be set? Does it have an effect on convergence?
Attachments
value.png
value.png (300.24 KiB) Viewed 588 times

STKO Team
Posts: 1346
Joined: Tue Oct 29, 2019 8:45 am

Re: Beam-to-Solid-Bar-Slip

Post by STKO Team » Wed Jun 22, 2022 2:46 pm

They are penalty parameters. If you make the too large you will have numerical errors. I just made them few order of magnitude larger than the typical stiffness of your model

cqf_2232
Posts: 64
Joined: Fri Dec 10, 2021 1:00 am

Re: Beam-to-Solid-Bar-Slip

Post by cqf_2232 » Sun Jul 17, 2022 12:44 pm

Dear STKO Team,
I applied cyclic loads to the bridge pier, and the hysteresis curve obtained by the simulation is quite different from the test. Due to the defects of the test equipment, the vertical load of the bridge pier may not reach the design value of 310 kN. I tried reducing the vertical load to 245 kN and could get a similar bearing capacity to the test.
Q1. As shown in the figure, the simulated hysteresis curve has a lower unload stiffness compared to the test. I still can't get a proper curve by adjusting the pdf_c parameter of DamageTC3D. How to solve this problem?
Q2. Do I need to replace MultiLinear material with Pinching4 material to simulate bond performance degradation when cyclic loads are applied to bridge piers?
Q3. I learned that a new version coming out next week can simulate slip with embedded reinforcement. Will the results be better when I divide the hexahedral elements?
Attachments
Model.rar
(1.49 MiB) Downloaded 11 times
image.png
image.png (338.86 KiB) Viewed 466 times

STKO Team
Posts: 1346
Joined: Tue Oct 29, 2019 8:45 am

Re: Beam-to-Solid-Bar-Slip

Post by STKO Team » Mon Jul 18, 2022 2:41 pm

Q1. As shown in the figure, the simulated hysteresis curve has a lower unload stiffness compared to the test. I still can't get a proper curve by adjusting the pdf_c parameter of DamageTC3D. How to solve this problem?
Try to increase both pdf_t and pdf_c to 0.6. They are more appropriate for concrete.
Then you can keep on increasing the pdf_c if needed.

Q2. Do I need to replace MultiLinear material with Pinching4 material to simulate bond performance degradation when cyclic loads are applied to bridge piers?
Sure, the Multilinear is not meant to be used for softening

Q3. I learned that a new version coming out next week can simulate slip with embedded reinforcement. Will the results be better when I divide the hexahedral elements?
It will be for sure faster to implement in your model since you can avoid doing the holes in concrete.
Probably it will be also more accurate due to the use of Hexa elements

Post Reply